Solid Works 2004 Reference Guide Eng
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SolidWorks 2004 Reference Guide
© 1995-2004, SolidWorks Corporation 300 Baker Avenue Concord, Massachusetts 01742 USA All Rights Reserved U.S. Patents 5,815,154; 6,219,049; 6,219,055; 6,603,486; 6,611,725 and certain foreign patents. U.S. and foreign patents pending. SolidWorks Corporation is a Dassault Systemes S.A. (Nasdaq:DASTY) company. The information and the software discussed in this document are subject to change without notice and should not be considered commitments by SolidWorks Corporation. No material may be reproduced or transmitted in any form or by any means, electronic or mechanical, for any purpose without the express written permission of SolidWorks Corporation. The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of this license. All warranties given by SolidWorks Corporation as to the software and documentation are set forth in the SolidWorks Corporation License and Subscription Service Agreement, and nothing stated in, or implied by, this document or its contents shall be considered or deemed a modification or amendment of such warranties. SolidWorks® is a registered trademark of SolidWorks Corporation. SolidWorks 2004 is a product name of SolidWorks Corporation. FeatureManager® is a jointly owned registered trademark of SolidWorks Corporation. Feature Palette™, PhotoWorks™, and PDMWorks™ are trademarks of SolidWorks Corporation. ACIS® is a registered trademark of Spatial Corporation. FeatureWorks® is a registered trademark of Geometric Software Solutions Co. Limited. GLOBEtrotter® and FLEXlm® are registered trademarks of Globetrotter Software, Inc. Other brand or product names are trademarks or registered trademarks of their respective holders.
COMMERCIAL COMPUTER SOFTWARE - PROPRIETARY U.S. Government Restricted Rights. Use, duplication, or disclosure by the government is subject to restrictions as set forth in FAR 52.227-19 (Commercial Computer Software - Restricted Rights), DFARS 227.7202 (Commercial Computer Software and Commercial Computer Software Documentation), and in the license agreement, as applicable. Contractor/Manufacturer: SolidWorks Corporation, 300 Baker Avenue, Concord, Massachusetts 01742 USA Portions of this software are copyrighted by and are the property of Electronic Data Systems Corporation or its subsidiaries, copyright© 2004 Portions of this software © 1988, 2000 Aladdin Enterprises. Portions of this software © 1996, 2001 Artifex Software, Inc. Portions of this software © 2001 artofcode LLC. Portions of this software © 2004 Bluebeam Software, Inc. Portions of this software © 1999, 2002-2004 ComponentOne Portions of this software © 1990-2004 D-Cubed Limited. Portions of this product are distributed under license from DC Micro Development, Copyright © 1994-2002 DC Micro Development, Inc. All rights reserved Portions © eHelp Corporation. All rights reserved. Portions of this software © 1998-2004 Geometric Software Solutions Co. Limited. Portions of this software © 1986-2004 mental images GmbH & Co. KG Portions of this software © 1996 Microsoft Corporation. All Rights Reserved. Portions of this software © 2001, SIMULOG. Portions of this software © 1995-2004 Spatial Corporation. Portions of this software © 2003-2004, Structural Research & Analysis Corp. Portions of this software © 1997-2004 Tech Soft America. Portions of this software © 1999-2004 Viewpoint Corporation. Portions of this software © 1994-2004, Visual Kinematics, Inc. This software is based in part on the work of the Independent JPEG group. All Rights Reserved
Contents
Chapter 1
SolidWorks 2004 Reference Guide
Scope ................................................................................................................................................................................. 1-1 Discounted Printing Offer ................................................................................................................................................. 1-1 Conventions ....................................................................................................................................................................... 1-1 Resources ........................................................................................................................................................................... 1-2
Chapter 2
SolidWorks Fundamentals
SolidWorks Fundamentals ................................................................................................................................................. 2-1 Basic Concepts .................................................................................................................................................................. 2-2 Document Windows .......................................................................................................................................................... 2-2 Cascade ....................................................................................................................................................................... 2-3 Tile Horizontally - Tile Vertically ............................................................................................................................. 2-3 Arrange Icons ............................................................................................................................................................. 2-3 Close All ..................................................................................................................................................................... 2-3 New Window .............................................................................................................................................................. 2-3 PropertyManager Overview .............................................................................................................................................. 2-4 Callouts and Handles ......................................................................................................................................................... 2-6 Drag and Drop ................................................................................................................................................................... 2-7 Shortcut Menu ................................................................................................................................................................... 2-8 Accepting Features ............................................................................................................................................................ 2-9 Pop-up Tooltips ............................................................................................................................................................... 2-10 Help ................................................................................................................................................................................. 2-10 What's Wrong? ................................................................................................................................................................ 2-12 Print ................................................................................................................................................................................. 2-13 Page Setup ................................................................................................................................................................ 2-13 Line Weights ............................................................................................................................................................ 2-14 Margins ..................................................................................................................................................................... 2-15 Printing Drawings .................................................................................................................................................... 2-15 Print Selection .......................................................................................................................................................... 2-16 Custom Scale Examples ........................................................................................................................................... 2-17 Print Preview ............................................................................................................................................................ 2-18 Keyboard Shortcuts ......................................................................................................................................................... 2-18 Send Mail ......................................................................................................................................................................... 2-20 Toolbars ........................................................................................................................................................................... 2-21 Toolbars .................................................................................................................................................................... 2-21 2D to 3D Toolbar ..................................................................................................................................................... 2-22 Align Toolbar ........................................................................................................................................................... 2-22 Annotations Toolbar ................................................................................................................................................. 2-23 Assembly Toolbar .................................................................................................................................................... 2-24 CommandManager ................................................................................................................................................... 2-24 Curves Toolbar ......................................................................................................................................................... 2-25 Dimensions/Relations Toolbar and Menus .............................................................................................................. 2-26
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Drawing Toolbar ......................................................................................................................................................2-26 Explode Sketch Toolbar ...........................................................................................................................................2-27 Features Toolbar .......................................................................................................................................................2-27 Font Toolbar .............................................................................................................................................................2-29 Layer Toolbar ...........................................................................................................................................................2-29 Line Format Toolbar .................................................................................................................................................2-29 Macro Toolbar ..........................................................................................................................................................2-30 Mold Tools Toolbar ..................................................................................................................................................2-30 Reference Geometry Toolbar ...................................................................................................................................2-31 Sheet Metal Toolbar .................................................................................................................................................2-31 Simulation Toolbar ...................................................................................................................................................2-32 Sketch Toolbar ..........................................................................................................................................................2-32 SolidWorks Office Toolbar ......................................................................................................................................2-33 Spline Tools Toolbar ................................................................................................................................................2-33 Standard Toolbar ......................................................................................................................................................2-33 Save ...................................................................................................................................................................2-34 Save As ..............................................................................................................................................................2-34 Cut .....................................................................................................................................................................2-35 Copy ..................................................................................................................................................................2-35 Paste ..................................................................................................................................................................2-35 Delete ................................................................................................................................................................2-35 Undo ..................................................................................................................................................................2-36 Redo ..................................................................................................................................................................2-36 Rebuild ..............................................................................................................................................................2-36 Redraw ..............................................................................................................................................................2-36 Color And Optics PropertyManager .................................................................................................................2-37 Materials Editor PropertyManager ....................................................................................................................2-38 Texture PropertyManager .................................................................................................................................2-39 Show Web Toolbar ............................................................................................................................................2-39 Standard Views Toolbar ...........................................................................................................................................2-40 Surfaces Toolbar .......................................................................................................................................................2-40 Tools Toolbar ...........................................................................................................................................................2-41 View Toolbar ............................................................................................................................................................2-41 Web Toolbar .............................................................................................................................................................2-41 Stop Current Jump .............................................................................................................................................2-41 Reload Documents ............................................................................................................................................2-42 Insert Hyperlink .................................................................................................................................................2-42 Open Internet Address .......................................................................................................................................2-42 Weldments Toolbar ..................................................................................................................................................2-43 FeatureManager Design Tree ..........................................................................................................................................2-43 FeatureManager Design Tree ...................................................................................................................................2-43 Show Feature's Description ...............................................................................................................................2-44 Show Component's Description ........................................................................................................................2-44 Show Component's Configuration Name ..........................................................................................................2-45 Show Component's Configuration Description .................................................................................................2-45 Show Configuration's Description ....................................................................................................................2-45 FeatureManager Design Tree Conventions ..............................................................................................................2-46 Parent/Child Relationships .......................................................................................................................................2-46 Rollback Bar .............................................................................................................................................................2-47 Split Panel Display ...................................................................................................................................................2-48 Flyout FeatureManager Design Tree ........................................................................................................................2-49 FeatureManager Options ..........................................................................................................................................2-49 Selecting from the FeatureManager Design Tree .....................................................................................................2-50 Find in FeatureManager Design Tree .......................................................................................................................2-50 Add Folders ..............................................................................................................................................................2-50 Opening New and Existing Documents in SolidWorks ..................................................................................................2-51 New SolidWorks Document .....................................................................................................................................2-51
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Default Templates .....................................................................................................................................................2-52 Creating Additional Template Tabs ..........................................................................................................................2-52 Setting Default Material Properties ..........................................................................................................................2-53 Open ..........................................................................................................................................................................2-53 Opening Documents from Part or Assembly Windows ...........................................................................................2-54 Multi-Threaded Retrieval .........................................................................................................................................2-55 SolidWorks Documents in Windows Explorer .........................................................................................................2-55 Drag and Drop Files to a SolidWorks Document .....................................................................................................2-56 Web Folders Overview ....................................................................................................................................................2-57 Web Folders Overview .............................................................................................................................................2-57 Web Folders - Saving and Opening Files .................................................................................................................2-57 Change URL .............................................................................................................................................................2-58 Copy Referenced Files to Server ..............................................................................................................................2-58 Selection ...........................................................................................................................................................................2-59 Highlighting ..............................................................................................................................................................2-59 Select .........................................................................................................................................................................2-60 Select Partial Loop ....................................................................................................................................................2-61 Select Chain ..............................................................................................................................................................2-62 Select Other ..............................................................................................................................................................2-63 Midpoint Selection ....................................................................................................................................................2-63 Selection Filter ..........................................................................................................................................................2-63 Selection Filter Hot Keys ..........................................................................................................................................2-63 Box Selection ............................................................................................................................................................2-64 Loop Selection ..........................................................................................................................................................2-65 Tangent Selection .....................................................................................................................................................2-65 Select through Transparency ....................................................................................................................................2-66 Viewing Models ...............................................................................................................................................................2-67 Applying Color and Optic Properties .......................................................................................................................2-67 Draft Quality HLR/HLV ...........................................................................................................................................2-68 Shaded and Dynamic Previews ................................................................................................................................2-68 Hidden Lines Removed ............................................................................................................................................2-69 Hidden Lines Visible ................................................................................................................................................2-69 Applying, Creating, and Editing Materials ...............................................................................................................2-69 Materials - Supported Graphics Cards ..............................................................................................................2-71 Materials - General Information ........................................................................................................................2-71 Materials - Visual Properties .............................................................................................................................2-71 Materials - Physical Properties ..........................................................................................................................2-72 Materials - Crosshatch .......................................................................................................................................2-72 RealView Graphics ............................................................................................................................................2-72 Perspective ................................................................................................................................................................2-72 Modify Perspective ...................................................................................................................................................2-73 Creating a Section View ...........................................................................................................................................2-73 Section View PropertyManager ................................................................................................................................2-74 Shaded .......................................................................................................................................................................2-74 Shaded With Edges ...................................................................................................................................................2-75 Shadows ....................................................................................................................................................................2-75 Orientation ................................................................................................................................................................2-75 Add a Named View ..................................................................................................................................................2-77 Textures ....................................................................................................................................................................2-77 Wireframe .................................................................................................................................................................2-78 Manipulating Models .......................................................................................................................................................2-78 Middle Mouse Button Functions ..............................................................................................................................2-78 Pan ............................................................................................................................................................................2-79 Rotate View ..............................................................................................................................................................2-79 Previous View ...........................................................................................................................................................2-80 Zoom to Fit ...............................................................................................................................................................2-80 Zoom to Area ............................................................................................................................................................2-80
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Zoom In/Out .............................................................................................................................................................2-81 Zoom to Selection .....................................................................................................................................................2-81 Customizing SolidWorks .................................................................................................................................................2-81 Overview of SolidWorks Options ............................................................................................................................2-81 Document Templates ................................................................................................................................................2-82 Customize Commands ..............................................................................................................................................2-83 Customize Headers and Footers ...............................................................................................................................2-83 Customize Keyboard ................................................................................................................................................2-84 Customize Macro Button ..........................................................................................................................................2-84 Customize Menus .....................................................................................................................................................2-85 Customize Options ...................................................................................................................................................2-86 Customize Toolbars ..................................................................................................................................................2-86 Skins .........................................................................................................................................................................2-87 SolidWorks Tools ............................................................................................................................................................2-89 Add-Ins .....................................................................................................................................................................2-89 Conversion Wizard ...................................................................................................................................................2-89 Copy Options Wizard ...............................................................................................................................................2-90 Manufacturing Network ...........................................................................................................................................2-90 Moving from AutoCAD ...........................................................................................................................................2-91 Quick Tips ................................................................................................................................................................2-91 SolidWorks API ........................................................................................................................................................2-91 SolidWorks Service Packs ........................................................................................................................................2-91 SolidWorks Web Site ...............................................................................................................................................2-92 Recording and Playing Macros ........................................................................................................................................2-92 New Macro ...............................................................................................................................................................2-92 Record/Pause Macro .................................................................................................................................................2-92 Edit Macro ................................................................................................................................................................2-93 Run Macro ................................................................................................................................................................2-93 Stop Macro ...............................................................................................................................................................2-93 Assign a Macro to a Shortcut Key or Menu .............................................................................................................2-93 VBA ..........................................................................................................................................................................2-94 Object Linking and Embedding - OLE ............................................................................................................................2-95 Object Linking vs. Embedding .................................................................................................................................2-95 Object .......................................................................................................................................................................2-95 Display Content .................................................................................................................................................2-96 Display as Icon ..................................................................................................................................................2-96 Reset Size ..........................................................................................................................................................2-97 Inserting SolidWorks Data in Other Applications ....................................................................................................2-97 OLE Object Property ................................................................................................................................................2-97
Chapter 3
Sketching
Sketching in SolidWorks ...................................................................................................................................................3-1 Sketch ................................................................................................................................................................................3-2 Sketch on the Face of a Part ..............................................................................................................................................3-3 Starting a New 2D Sketch ..................................................................................................................................................3-3 Starting the Sketch .............................................................................................................................................................3-4 Starting the Sketch .............................................................................................................................................................3-5 Working in a Sketch ..........................................................................................................................................................3-5 Opening a New Sketch ......................................................................................................................................................3-6 Inferencing Pointers and Lines ..........................................................................................................................................3-6 Sketch Modes .....................................................................................................................................................................3-7 Autotransitioning ...............................................................................................................................................................3-8 Silhouettes ..........................................................................................................................................................................3-8 Cutting, Copying, and Pasting in Sketches ........................................................................................................................3-8 Modify Sketch ...................................................................................................................................................................3-9 Edit Sketch .......................................................................................................................................................................3-10 Exit Sketch .......................................................................................................................................................................3-11
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Derived Sketch .................................................................................................................................................................3-11 Sketch Plane References ..................................................................................................................................................3-12 Edit Sketch Plane .............................................................................................................................................................3-12 Shaded Sketch Plane ........................................................................................................................................................3-12 Reference Plane Normal to Edge .....................................................................................................................................3-13 Sketch Tools .....................................................................................................................................................................3-13 Align Grid .................................................................................................................................................................3-13 Automatic Inferencing Lines ....................................................................................................................................3-14 Automatic Solve .......................................................................................................................................................3-14 No Solve Move .........................................................................................................................................................3-15 Move or Copy PropertyManager ..............................................................................................................................3-15 Check Sketch for Feature Usage ...............................................................................................................................3-16 Allowed Contour Types ............................................................................................................................................3-16 Circular Sketch Step and Repeat ..............................................................................................................................3-17 Constrain Spacing and Fixed Options ......................................................................................................................3-19 Constrain All .............................................................................................................................................................3-19 Contour Selection .....................................................................................................................................................3-19 Close Sketch to Model ..............................................................................................................................................3-21 Construction Geometry .............................................................................................................................................3-21 Convert Entities ........................................................................................................................................................3-22 Detach Segment on Drag ..........................................................................................................................................3-22 Extend Entities ..........................................................................................................................................................3-22 Face Curves ..............................................................................................................................................................3-23 Intersection Curve .....................................................................................................................................................3-24 Linear Sketch Step and Repeat .................................................................................................................................3-25 Fixed Spacing in Linear Sketch Step and Repeat .....................................................................................................3-26 Constrain Angle in Linear Sketch Step and Repeat ..................................................................................................3-26 Mirror Entities ..........................................................................................................................................................3-27 Move, Rotate, Scale, or Copy ...................................................................................................................................3-27 Offset Entities ...........................................................................................................................................................3-30 Override Dims on Drag/Move ..................................................................................................................................3-30 Sketch Chamfer ........................................................................................................................................................3-31 Sketch Fillet ..............................................................................................................................................................3-31 Sketch Fillet PropertyManager .................................................................................................................................3-32 Split Entities ..............................................................................................................................................................3-32 Trim Entities .............................................................................................................................................................3-32 Dimensions and Relations ................................................................................................................................................3-33 Dimensions ...............................................................................................................................................................3-33 Horizontal Dimension .......................................................................................................................................3-34 Vertical Dimension ............................................................................................................................................3-34 Lock Dimensions ...............................................................................................................................................3-34 Point-to-Point Dimensions ................................................................................................................................3-35 Point-to-Point Dimensions ................................................................................................................................3-35 Arc Dimensions .................................................................................................................................................3-35 Arc Dimensions .................................................................................................................................................3-35 Circular Dimensions ..........................................................................................................................................3-36 Circular Dimensions ..........................................................................................................................................3-36 Angular Dimensions Between Two Lines .........................................................................................................3-37 Angular Dimensions ..........................................................................................................................................3-37 Angular Dimensions Between Three Points ......................................................................................................3-37 Dimensions Between Arcs or Circles ................................................................................................................3-38 Autodimension ..........................................................................................................................................................3-39 Geometric Relations .................................................................................................................................................3-40 Automatic Relations .................................................................................................................................................3-40 Add Relations/Properties PropertyManager .............................................................................................................3-41 Sketch Relations .......................................................................................................................................................3-42 Sketch Relations Callouts .........................................................................................................................................3-43
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Sketch Geometry Status ...........................................................................................................................................3-43 Sketch Status Conventions .......................................................................................................................................3-43 Display/Delete Relations PropertyManager .............................................................................................................3-44 Scan Equal ................................................................................................................................................................3-45 External vs. Defined in Context ...............................................................................................................................3-45 Splines ..............................................................................................................................................................................3-46 Splines ......................................................................................................................................................................3-46 Proportional Splines .................................................................................................................................................3-47 Spline PropertyManager ...........................................................................................................................................3-47 Fit Spline ..................................................................................................................................................................3-48 Simplify Spline .........................................................................................................................................................3-49 Insert Spline Point ....................................................................................................................................................3-49 Moving Frame ..........................................................................................................................................................3-49 Frame Point PropertyManager .................................................................................................................................3-50 3D Frame Point PropertyManager ............................................................................................................................3-51 Curvature Combs ......................................................................................................................................................3-52 Curvature Scale ........................................................................................................................................................3-52 Inflection Points ........................................................................................................................................................3-52 Minimum Radius ......................................................................................................................................................3-53 2D Sketching ...................................................................................................................................................................3-53 Line ...........................................................................................................................................................................3-53 Line PropertyManager ..............................................................................................................................................3-54 Points ........................................................................................................................................................................3-55 Point PropertyManager .............................................................................................................................................3-55 Circle ........................................................................................................................................................................3-55 Circle PropertyManager ...........................................................................................................................................3-56 Ellipse .......................................................................................................................................................................3-57 Partial Ellipse ............................................................................................................................................................3-57 Ellipse PropertyManager ..........................................................................................................................................3-57 Centerlines ................................................................................................................................................................3-58 Virtual Sharp ............................................................................................................................................................3-58 Centerpoint Arc ........................................................................................................................................................3-59 Tangent Arcs ............................................................................................................................................................3-59 3 Point Arc ................................................................................................................................................................3-59 Arc PropertyManager ...............................................................................................................................................3-60 Parabolas ...................................................................................................................................................................3-61 Parabola PropertyManager .......................................................................................................................................3-62 Polygons ...................................................................................................................................................................3-63 Polygon PropertyManager ........................................................................................................................................3-63 Rectangles .................................................................................................................................................................3-64 Parallelograms ..........................................................................................................................................................3-65 Text ...........................................................................................................................................................................3-65 Sketch Text PropertyManager ..................................................................................................................................3-66 Sketch Picture ...........................................................................................................................................................3-67 Sketch Picture PropertyManager ..............................................................................................................................3-68 3D Sketching ...................................................................................................................................................................3-68 3D Sketching ............................................................................................................................................................3-68 Line Snap ..................................................................................................................................................................3-69 3D Lines ...................................................................................................................................................................3-70 3D Line PropertyManager ........................................................................................................................................3-70 3D Splines ................................................................................................................................................................3-71 3D Spline PropertyManager .....................................................................................................................................3-72 3D Points ..................................................................................................................................................................3-73 3D Point PropertyManager .......................................................................................................................................3-73 3D Circle PropertyManager .....................................................................................................................................3-74 Coordinate System - 3D Sketching ..........................................................................................................................3-74 Space Handle ............................................................................................................................................................3-75
vi
Dimensioning a 3D Sketch .......................................................................................................................................3-75 Virtual Sharps - 3D Sketch .......................................................................................................................................3-75 3D Arc PropertyManager .........................................................................................................................................3-75
Chapter 4
2D to 3D Conversion
2D to 3D Conversion Overview ........................................................................................................................................4-1 2D to 3D Toolbar ...............................................................................................................................................................4-4 Importing Drawings into Part Documents .........................................................................................................................4-4 Extracting Sketches ............................................................................................................................................................4-5 Aligning Sketches ..............................................................................................................................................................4-6 Extruding in 2D to 3D ........................................................................................................................................................4-7 Cutting in 2D to 3D ............................................................................................................................................................4-8 Additional Conversion Tools ...........................................................................................................................................4-10 Repair Sketch ............................................................................................................................................................4-10 Create Sketch from Selections ..................................................................................................................................4-10
Chapter 5
Reference Geometry
Reference Geometry Overview ..........................................................................................................................................5-1 Updating Reference Geometry in Document Templates ...................................................................................................5-1 Planes .................................................................................................................................................................................5-2 Creating Planes ...........................................................................................................................................................5-2 Changing Plane Names ...............................................................................................................................................5-8 Plane Display ..............................................................................................................................................................5-8 Hiding or Showing Planes ........................................................................................................................................5-10 Moving, Resizing, and Copying Planes ....................................................................................................................5-10 Automatic Sizing of Planes and Axes ......................................................................................................................5-10 Axis Overview .................................................................................................................................................................5-12 Reference Axis .................................................................................................................................................................5-12 Reference Axis .................................................................................................................................................................5-13 Coordinate System ...........................................................................................................................................................5-13 Coordinate System PropertyManager ..............................................................................................................................5-14 Origin ...............................................................................................................................................................................5-14 Centroid ............................................................................................................................................................................5-14 Converting Sketch Lines to Construction Geometry .......................................................................................................5-15 Curve Overview ...............................................................................................................................................................5-15 Curve Through XYZ Points ......................................................................................................................................5-16 Curve Through Reference Points ..............................................................................................................................5-16 Curve from File .........................................................................................................................................................5-17 Helix and Spiral ........................................................................................................................................................5-17 Helix/Spiral PropertyManager ..................................................................................................................................5-18 Projecting Sketched Curves ......................................................................................................................................5-18 Replacing a Sketch of a Projected Curve .................................................................................................................5-19 Split Lines .................................................................................................................................................................5-20 Composite Curve ......................................................................................................................................................5-21 Reference Points ..............................................................................................................................................................5-22 Point PropertyManager ....................................................................................................................................................5-22
Chapter 6
Features
Features Overview .............................................................................................................................................................6-1 Features Toolbar ................................................................................................................................................................6-2 Feature Previews ................................................................................................................................................................6-4 Chamfers ............................................................................................................................................................................6-7 Deform ...............................................................................................................................................................................6-8 Deform ........................................................................................................................................................................6-8 Deform Curve to Curve ..............................................................................................................................................6-9 Deform Feature Using Curve to Curve ...............................................................................................................6-9 Deform Feature Curve to Curve Options ..........................................................................................................6-12
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Deform Point ............................................................................................................................................................6-19 Deform Feature Using Point .............................................................................................................................6-19 Deform Feature Point Options ..........................................................................................................................6-21 Domes ..............................................................................................................................................................................6-30 Drafts ...............................................................................................................................................................................6-32 Draft Overview .........................................................................................................................................................6-32 Draft Feature .............................................................................................................................................................6-32 Draft with Neutral Plane ...........................................................................................................................................6-33 Parting Line Draft .....................................................................................................................................................6-35 Allow Reduced Angle Option ..................................................................................................................................6-36 Parting Line with Step Draft .....................................................................................................................................6-37 Tapered and Perpendicular Draft Steps ....................................................................................................................6-38 Extrudes ...........................................................................................................................................................................6-38 Extrude Feature ........................................................................................................................................................6-38 Extrude Feature Overview ........................................................................................................................................6-39 Extruded Boss/Base ..................................................................................................................................................6-44 Boss/Base-Extrude ...................................................................................................................................................6-45 Extrude Thin Feature ................................................................................................................................................6-46 Cut Feature ...............................................................................................................................................................6-47 Cutting Tools ............................................................................................................................................................6-47 Surface Cut ...............................................................................................................................................................6-49 Extruded Cut .............................................................................................................................................................6-50 Fillets ...............................................................................................................................................................................6-53 Fillet ..........................................................................................................................................................................6-53 Fillet Overview .........................................................................................................................................................6-57 Constant Radius Fillet ..............................................................................................................................................6-58 Multiple Radius Fillet ...............................................................................................................................................6-60 Round Corner Fillet ..................................................................................................................................................6-61 Setback Fillet ............................................................................................................................................................6-62 Variable Radius Fillet ...............................................................................................................................................6-64 Using Variable Radius Control Points .....................................................................................................................6-67 Full Round Fillet .......................................................................................................................................................6-69 Face Fillet .................................................................................................................................................................6-70 Face Fillet with Hold Line ........................................................................................................................................6-71 Face Fillet with Split Line ........................................................................................................................................6-73 Holes ................................................................................................................................................................................6-74 Simple Hole ..............................................................................................................................................................6-74 Creating a Simple Hole ............................................................................................................................................6-76 End Condition Types ................................................................................................................................................6-76 Hole Wizard ..............................................................................................................................................................6-77 Hole Wizard Overview ......................................................................................................................................6-77 Hole Wizard on a Plane .....................................................................................................................................6-78 Hole Wizard Hole Placement ............................................................................................................................6-79 Favorite Hole Types ..........................................................................................................................................6-80 Property ......................................................................................................................................................6-80 Parameters ..................................................................................................................................................6-80 Delete Favorite Hole .........................................................................................................................................6-81 Retrieve Favorite Hole ......................................................................................................................................6-81 Update Favorite Hole ........................................................................................................................................6-81 New Favorite Name ..........................................................................................................................................6-81 Hole Series ........................................................................................................................................................6-81 Hole Wizard Holes ............................................................................................................................................6-83 Hole Wizard Custom Standards .................................................................................................................6-83 Edit Hole Wizard Standards .......................................................................................................................6-83 Hole Wizard - Edit Standards Data ............................................................................................................6-84 Counterbore ................................................................................................................................................6-84 Dynamic Changes with Counterbore Holes ...............................................................................................6-85
viii
Countersink ................................................................................................................................................6-85 Dynamic Changes with Countersink Holes ...............................................................................................6-86 Hole ............................................................................................................................................................6-86 Dynamic Changes with Regular Holes ......................................................................................................6-87 Tap ..............................................................................................................................................................6-87 Dynamic Changes with Tap Holes .............................................................................................................6-88 Pipe Tap ......................................................................................................................................................6-88 Dynamic Changes with Pipe Tap Holes .....................................................................................................6-89 Legacy ........................................................................................................................................................6-89 Lofts .................................................................................................................................................................................6-90 Loft Overview ...........................................................................................................................................................6-90 Loft Features .............................................................................................................................................................6-91 Loft with Thin Feature ..............................................................................................................................................6-94 Loft Thin Feature Samples .......................................................................................................................................6-95 Loft with Non-Planar Profile ....................................................................................................................................6-95 Loft with Split Line ..................................................................................................................................................6-96 Loft with Guide Curve and Planar Profile ................................................................................................................6-97 Loft with Guide Curve and non-Planar Profile .........................................................................................................6-99 Recommendations for Lofts with Guide Curves ....................................................................................................6-101 Loft Side Tangency .................................................................................................................................................6-101 Loft with Centerline ................................................................................................................................................6-101 Loft with Start and End Tangency Control .............................................................................................................6-103 Add Loft Section .....................................................................................................................................................6-104 Loft Synchronization ..............................................................................................................................................6-106 Patterns and Mirroring ...................................................................................................................................................6-108 Pattern and Mirror Overview ..................................................................................................................................6-108 Patterns of Patterns .................................................................................................................................................6-109 Curve Driven Pattern Overview .............................................................................................................................6-110 Curve Driven Pattern ..............................................................................................................................................6-110 Linear Pattern ..........................................................................................................................................................6-114 Circular Pattern .......................................................................................................................................................6-119 Sketch Driven Patterns ...........................................................................................................................................6-121 Table Driven Patterns .............................................................................................................................................6-123 Save Table Pattern Coordinates .......................................................................................................................6-125 Load Table Pattern Coordinates ......................................................................................................................6-125 Mirror Pattern .........................................................................................................................................................6-125 Control and Modify Patterns ..................................................................................................................................6-126 Geometry Pattern .............................................................................................................................................6-127 Vary Sketch .....................................................................................................................................................6-128 Pattern Deletion ...............................................................................................................................................6-128 Seed Feature ....................................................................................................................................................6-129 Mirror Feature .........................................................................................................................................................6-129 Revolves .........................................................................................................................................................................6-132 Revolved Boss/Base ...............................................................................................................................................6-132 Revolve Features ....................................................................................................................................................6-132 Ribs ................................................................................................................................................................................6-135 Rib Overview ..........................................................................................................................................................6-135 Rib - Linear and Natural Type ................................................................................................................................6-138 Rib Feature ..............................................................................................................................................................6-139 Scaling ............................................................................................................................................................................6-141 Shapes ............................................................................................................................................................................6-142 Shape Feature ..........................................................................................................................................................6-142 Shape Feature Controls Tab ....................................................................................................................................6-144 Shells ..............................................................................................................................................................................6-145 Shell Features ..........................................................................................................................................................6-145 Shell with Multi-Thickness Faces ..........................................................................................................................6-146 Shell Feature Diagnostics .......................................................................................................................................6-147
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Surfaces ..........................................................................................................................................................................6-148 Surfaces Overview ..................................................................................................................................................6-148 Surfaces Toolbar .....................................................................................................................................................6-148 Surface Bodies ........................................................................................................................................................6-149 Surface Features .....................................................................................................................................................6-149 Planar Surface .................................................................................................................................................6-149 Extruded Surface .............................................................................................................................................6-150 Revolved Surface ............................................................................................................................................6-151 Swept Surface ..................................................................................................................................................6-152 Lofted Surface .................................................................................................................................................6-153 Offset Surface ..................................................................................................................................................6-154 Radiating a Surface from a Parting Line .........................................................................................................6-155 Surface Face Blend Fillet ................................................................................................................................6-156 Surface Controls .....................................................................................................................................................6-157 Extend Surface ................................................................................................................................................6-157 Fillet Surface ...................................................................................................................................................6-159 Knit Surface .....................................................................................................................................................6-161 Mid Surface .....................................................................................................................................................6-162 Fill Surface ......................................................................................................................................................6-164 Trim Surface ....................................................................................................................................................6-170 Untrim Surface ................................................................................................................................................6-172 Radiate Surface ...............................................................................................................................................6-175 Hide and Show Bodies ....................................................................................................................................6-175 Delete Face ......................................................................................................................................................6-177 Delete Hole ......................................................................................................................................................6-179 Replace Face ...................................................................................................................................................6-180 Sweeps ...........................................................................................................................................................................6-182 Sweep Overview .....................................................................................................................................................6-182 Simple Sweep .........................................................................................................................................................6-183 Sweeps Feature .......................................................................................................................................................6-185 Sweeps with Mulltiple Profiles ..............................................................................................................................6-187 Sweeps with Guide Curves .....................................................................................................................................6-187 Recommendations for Sweeps with Guide Curves ................................................................................................6-189 Preview Intermediate Sweep Sections ....................................................................................................................6-189 Sweeps Options ......................................................................................................................................................6-190 Sweep Options .................................................................................................................................................6-190 Sweep Options Align with End Faces .............................................................................................................6-190 Example of Sweep with Thin Features ...........................................................................................................6-191 Example of Merge Smooth Faces Option in Sweeps ......................................................................................6-191 Sweep Options Advanced Smoothing .............................................................................................................6-191 Sweep Options Maintain Tangency ................................................................................................................6-191 Loft Tangency Options ....................................................................................................................................6-192 Start and End Tangency Options for Sweeps ..................................................................................................6-193 Orientation/Twist Control Option ...................................................................................................................6-193 Orientation/Twist Type - Follow Path ............................................................................................................6-194 Thicken ..........................................................................................................................................................................6-195 Tools for Features ..........................................................................................................................................................6-198 Analysis of Features ...............................................................................................................................................6-198 Draft Analysis Overview .................................................................................................................................6-198 Draft Analysis .................................................................................................................................................6-201 Deviation Analysis ..........................................................................................................................................6-205 Manipulation of Features ........................................................................................................................................6-208 Move/Size Features with Feature Handles ......................................................................................................6-208 Move/Copy Bodies ..........................................................................................................................................6-209 Combine Bodies ..............................................................................................................................................6-213 Delete Body .....................................................................................................................................................6-214 Choose Option .................................................................................................................................................6-214
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Select Detailed Preview ...................................................................................................................................6-215 Wrap ...............................................................................................................................................................................6-216
Chapter 7
Parts
Overview and Editing Parts ...............................................................................................................................................7-1 Parts Overview ............................................................................................................................................................7-1 Edit Definition ............................................................................................................................................................7-1 Properties of Features and Faces ................................................................................................................................7-2 Dynamic Feature Editing ............................................................................................................................................7-3 Copying Features ........................................................................................................................................................7-4 Color of Parts ..............................................................................................................................................................7-4 Material Properties and Appearance of Parts .............................................................................................................7-5 Appearance and Material Properties ...........................................................................................................................7-6 Edit Color ....................................................................................................................................................................7-7 Entity Property ............................................................................................................................................................7-8 Advanced Properties ...................................................................................................................................................7-9 Multibody Parts ................................................................................................................................................................7-10 Multibody Overview .................................................................................................................................................7-10 Multibody Parts Versus Assemblies .........................................................................................................................7-10 Modeling Techniques ...............................................................................................................................................7-11 Body Intersection ...............................................................................................................................................7-11 Bridging .............................................................................................................................................................7-12 Local Operations ...............................................................................................................................................7-12 Symmetry Modeling ..........................................................................................................................................7-13 Tool Body Modeling .........................................................................................................................................7-14 Controlling Parts ..............................................................................................................................................................7-14 Parent and Child Relations .......................................................................................................................................7-14 Equations ..................................................................................................................................................................7-14 Edit and Delete Equations .................................................................................................................................7-15 Operators and Constants ....................................................................................................................................7-16 Equation Comments and Status .........................................................................................................................7-16 Shared Values ...........................................................................................................................................................7-17 Measure .....................................................................................................................................................................7-18 Measurement Options ...............................................................................................................................................7-19 Dependency Editing ..................................................................................................................................................7-20 Suppress and Unsuppress Features ...........................................................................................................................7-21 Derived Parts ............................................................................................................................................................7-21 Insert Part ..................................................................................................................................................................7-22 Mirror Part ................................................................................................................................................................7-22 Derive Component Part ............................................................................................................................................7-23 Split and Save Bodies ...............................................................................................................................................7-23 Edit Derived Parts .....................................................................................................................................................7-26 Create Assembly .......................................................................................................................................................7-27 Resolve Ambiguity ...................................................................................................................................................7-27 File Management with External References .............................................................................................................7-28 Feature Statistics .......................................................................................................................................................7-28 Model Geometry Overview ......................................................................................................................................7-29 Selected Items Check Entity .....................................................................................................................................7-29 Checking Model Geometry .......................................................................................................................................7-30 Checking a Planar Surface ........................................................................................................................................7-30 Checking Part Faces or Edges ..................................................................................................................................7-31 Check Entity .............................................................................................................................................................7-31 Finding the Minimum Radius of Curvature ..............................................................................................................7-31 Interrupt Regeneration ..............................................................................................................................................7-32 Send To .....................................................................................................................................................................7-32
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Displaying Parts Information ...........................................................................................................................................7-32 Displaying Annotations in Parts ...............................................................................................................................7-32 Summary Information ..............................................................................................................................................7-33 Summary Info – Custom and Configuration Specific ..............................................................................................7-33 Edit List ....................................................................................................................................................................7-35 Section Views Overview ..........................................................................................................................................7-35 Section View Selection .............................................................................................................................................7-36 Section Views in Models ..........................................................................................................................................7-37 Using Viewing Planes for Section Views ................................................................................................................7-37 Mass Properties and Section Properties ...................................................................................................................7-38 Curvature ..................................................................................................................................................................7-39 Curvature Options ....................................................................................................................................................7-41 Curvature Display .....................................................................................................................................................7-41 Zebra Stripes .............................................................................................................................................................7-42 Zebra Stripes on Boundaries ....................................................................................................................................7-44 Lighting ............................................................................................................................................................................7-45 Lighting Overview ....................................................................................................................................................7-45 Basic Lighting Controls ............................................................................................................................................7-45 Ambient Light ..........................................................................................................................................................7-46 Directional Light Properties .....................................................................................................................................7-47 Point Light Properties ...............................................................................................................................................7-48 Spot Light Properties ................................................................................................................................................7-49 Lighting - Basic ........................................................................................................................................................7-50 Lighting - Advanced .................................................................................................................................................7-50 Lighting - Position and Direction .............................................................................................................................7-51
Chapter 8
Mold Design
Mold Tools Toolbar ...........................................................................................................................................................8-1 Understanding Mold Design ..............................................................................................................................................8-2 Mold Tools - Undercut Detection ......................................................................................................................................8-3 Scaling Factor and Draft in Mold Design ..........................................................................................................................8-4 Mold Tools - Parting Lines ................................................................................................................................................8-4 Mold Tools - Ruled Surfaces .............................................................................................................................................8-6 Mold Tools - Shut Off Surfaces .........................................................................................................................................8-6 Mold Tools - Parting Surfaces ...........................................................................................................................................8-7 Mold Tools - Tooling Split ................................................................................................................................................8-9 Interlock Surface ..............................................................................................................................................................8-10 Finishing the Interlock Surface ........................................................................................................................................8-10 Mold Tools - Insert Cavity ..............................................................................................................................................8-11
Chapter 9
Assemblies
Assemblies .........................................................................................................................................................................9-1 Design Methods .................................................................................................................................................................9-1 The FeatureManager Design Tree in an Assembly ...........................................................................................................9-2 Component Icons in the FeatureManager Design Tree .....................................................................................................9-3 Viewing Mates ...................................................................................................................................................................9-3 Adding Components to an Assembly ................................................................................................................................9-4 Insert Components ......................................................................................................................................................9-4 Adding Components from an Open Document Window ...........................................................................................9-5 Adding Components from Windows Explorer ...........................................................................................................9-5 Adding Components from Internet Explorer ..............................................................................................................9-5 Adding Components by Dragging and Dropping .......................................................................................................9-5 Inferencing to the Assembly Origin ...........................................................................................................................9-6 Deleting Components from an Assembly ..........................................................................................................................9-6 Saving an Assembly and Its Components .........................................................................................................................9-6 Saving an Assembly in Various Ways ...............................................................................................................................9-7 Replace Components .........................................................................................................................................................9-7
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Reload Documents .............................................................................................................................................................9-8 Edit Referenced File Locations ..........................................................................................................................................9-8 Replace Mated Entities ......................................................................................................................................................9-8 Assembly Statistics ............................................................................................................................................................9-9 Component Properties ........................................................................................................................................................9-9 Assembly Instance Color .................................................................................................................................................9-10 Arranging Components ....................................................................................................................................................9-10 Assembly PropertyManager .....................................................................................................................................9-10 Positioning Components in an Assembly .................................................................................................................9-10 Fixing the Position of a Component .........................................................................................................................9-11 Moving a Component ...............................................................................................................................................9-11 Rotating a Component ..............................................................................................................................................9-12 Assembly Mates ........................................................................................................................................................9-13 Mate PropertyManager ......................................................................................................................................9-13 Standard Mates ..................................................................................................................................................9-14 Standard Mates by Entity ..................................................................................................................................9-15 Mate Alignment .................................................................................................................................................9-17 Mate Reference ..................................................................................................................................................9-17 Mategroups ........................................................................................................................................................9-18 Modifying a Mating Relationship .....................................................................................................................9-19 Angle Mate ........................................................................................................................................................9-19 Coincident Mate ................................................................................................................................................9-20 Concentric Mate ................................................................................................................................................9-20 Distance Mate ....................................................................................................................................................9-21 Parallel and Perpendicular Mates ......................................................................................................................9-21 Tangent Mate .....................................................................................................................................................9-22 Cam-Follower Mates .........................................................................................................................................9-22 Gear Mates .........................................................................................................................................................9-23 Limit Mates .......................................................................................................................................................9-23 Symmetry Mate .................................................................................................................................................9-24 SmartMates ...............................................................................................................................................................9-25 Geometry-Based Mates .....................................................................................................................................9-25 Feature-Based Mates .........................................................................................................................................9-26 Pattern-Based Mates ..........................................................................................................................................9-26 Adding SmartMates While Moving Components .............................................................................................9-27 Deleting a Mating Relationship ................................................................................................................................9-28 Suppressing a Mating Relationship ..........................................................................................................................9-28 Mate Diagnostics ......................................................................................................................................................9-28 Conflicting Mates ..............................................................................................................................................9-29 Design Errors and Mating .................................................................................................................................9-30 Errors in Solving Mates .....................................................................................................................................9-31 In-Context Mating Conflicts ..............................................................................................................................9-31 Mates to Dangling Geometry ............................................................................................................................9-31 Mating Conflicts with Sketch Relations ............................................................................................................9-32 Physical Simulation ..................................................................................................................................................9-33 Linear or Rotary Motors ....................................................................................................................................9-33 Linear Springs ...................................................................................................................................................9-34 Gravity ...............................................................................................................................................................9-35 Recording and Replaying a Simulation .............................................................................................................9-35 Sub-assemblies .................................................................................................................................................................9-36 Working with Sub-assemblies ..................................................................................................................................9-36 Forming a New Assembly from Existing Components ............................................................................................9-37 Dragging Components to Edit the Assembly Structure ............................................................................................9-37 Assembly Structure Editing ......................................................................................................................................9-38 Changing the Order of Components .........................................................................................................................9-39 Inserting a New Sub-assembly .................................................................................................................................9-39 Dissolving a Sub-assembly .......................................................................................................................................9-39
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Changing the Editing Focus Manually .....................................................................................................................9-40 Automatic Change of Editing Focus ........................................................................................................................9-41 Limitations in Sub-assembly Editing .......................................................................................................................9-41 Flexible Sub-Assemblies ..........................................................................................................................................9-41 Working with Parts Within an Assembly ........................................................................................................................9-42 Working with Parts within an Assembly ..................................................................................................................9-42 External References ..................................................................................................................................................9-42 Understanding the Update Path ................................................................................................................................9-43 Locking and Breaking External References .............................................................................................................9-43 Rules for External References ..................................................................................................................................9-43 List External References ...........................................................................................................................................9-44 Searching for Referenced Documents ......................................................................................................................9-44 Search Results ..........................................................................................................................................................9-46 Saving Assemblies with In-context Features ...........................................................................................................9-46 Editing Parts in the Assembly Context .....................................................................................................................9-47 Creating a Part in an Assembly ................................................................................................................................9-47 Editing a Part in an Assembly ..................................................................................................................................9-48 Transparency During Part Editing ............................................................................................................................9-48 Time-Dependent Features ........................................................................................................................................9-49 Tips for Mating with Time-Dependent Features ......................................................................................................9-49 Adding a Component Pattern ...................................................................................................................................9-49 Linear Component Pattern ................................................................................................................................9-50 Circular Component Pattern ..............................................................................................................................9-50 Feature Driven Pattern ......................................................................................................................................9-51 Mirror Components - Overview ...............................................................................................................................9-51 Mirror Components Step 1: Selections .............................................................................................................9-52 Mirror Components Step 2: Filenames .............................................................................................................9-53 Mirror Components Step 3: Orientation ............................................................................................................9-53 Reorder and Roll Back in Assemblies ......................................................................................................................9-53 Assembly Layout Sketch ..........................................................................................................................................9-54 Example of Using an Assembly Layout Sketch .......................................................................................................9-54 Assembly Features ....................................................................................................................................................9-55 Creating an Assembly Feature ..................................................................................................................................9-55 Feature Scope ...........................................................................................................................................................9-56 Joining Parts .............................................................................................................................................................9-56 Creating a Joined Part .......................................................................................................................................9-56 Editing a Joined Part .........................................................................................................................................9-57 Identifying the Parts in a Joined Part ................................................................................................................9-58 Weld Beads ...............................................................................................................................................................9-58 Weld Types .......................................................................................................................................................9-58 Creating and Editing Weld Beads .....................................................................................................................9-58 Surface Delta and Radius ..................................................................................................................................9-59 Weld Face Selection Tips ..................................................................................................................................9-60 Automatic Weld Symbols .................................................................................................................................9-60 Simplifying Assemblies ...................................................................................................................................................9-61 Simplifying Large Assemblies .................................................................................................................................9-61 Large Assembly Mode .............................................................................................................................................9-61 Lightweight Components .........................................................................................................................................9-61 Toggling the Visibility .............................................................................................................................................9-62 Component Suppression States ................................................................................................................................9-63 Loading Additional Model Data ...............................................................................................................................9-64 Comparison of Components Suppression States ......................................................................................................9-64 Assembly Envelopes ................................................................................................................................................9-65 Apply Envelope ........................................................................................................................................................9-65 Creating Assembly Envelopes ..................................................................................................................................9-66 Removing Assembly Envelopes ...............................................................................................................................9-66 Select Using Envelope ..............................................................................................................................................9-66
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Component Selection by Properties ..........................................................................................................................9-67 Advanced Hide/Show Components ..........................................................................................................................9-67 Advanced Component Selection ...............................................................................................................................9-68 Saving and Reloading Selection Criteria ..................................................................................................................9-68 Displaying Assemblies .....................................................................................................................................................9-69 Exploding an Assembly View ..................................................................................................................................9-69 Assembly Exploder ...........................................................................................................................................9-69 Exploding and Collapsing an Exploded View ...................................................................................................9-70 Alternative Method for Editing an Exploded View ..........................................................................................9-71 Explode Line Sketch ..........................................................................................................................................9-71 Jog Line .............................................................................................................................................................9-71 Image Quality in Assemblies ....................................................................................................................................9-72 Color and Appearance in Assemblies .......................................................................................................................9-72 Annotations in Assemblies .......................................................................................................................................9-73 Preventing Interference Between Components ................................................................................................................9-74 Interference Detection ..............................................................................................................................................9-74 Collision Detection ...................................................................................................................................................9-74 Physical Dynamics ....................................................................................................................................................9-75 Dynamic Clearance ...................................................................................................................................................9-76 Smart Fasteners ................................................................................................................................................................9-77 Smart Fasteners Overview ........................................................................................................................................9-77 Smart Fasteners PropertyManager ............................................................................................................................9-78 Smart Fasteners Bolts and Screws ............................................................................................................................9-79 Smart Fasteners Nuts ................................................................................................................................................9-81 Smart Fasteners Washers ..........................................................................................................................................9-82 Unsupported Hole Types ..........................................................................................................................................9-83 Editing Smart Fasteners ............................................................................................................................................9-85 Smart Fasteners Hardware Stacks ............................................................................................................................9-86 Drag-and-Drop Editing of Smart Fasteners ..............................................................................................................9-87 Smart Fasteners Part Numbers ..................................................................................................................................9-88 Mark Up-to-date .......................................................................................................................................................9-88 Configuring Bolt Patterns in Smart Fasteners ..........................................................................................................9-89 Smart Fasteners Defaults ..........................................................................................................................................9-90
Chapter 10 Configurations Configurations Overview .................................................................................................................................................10-1 ConfigurationManager .....................................................................................................................................................10-1 Show Preview ..................................................................................................................................................................10-2 Configurations and In-context Components ....................................................................................................................10-2 Configure Document ........................................................................................................................................................10-3 Configure Document for View / Configurations .............................................................................................................10-3 Manual Configurations ....................................................................................................................................................10-4 Creating a Configuration Manually ..........................................................................................................................10-4 Add Configuration/Configuration Properties ...........................................................................................................10-4 Properties for Newly Inserted Items .........................................................................................................................10-5 Derived Configurations ............................................................................................................................................10-6 Activating a Configuration .......................................................................................................................................10-8 Configurable Items for Parts .....................................................................................................................................10-8 Sketch Dimensions in Configurations ...............................................................................................................10-8 Sketch Planes in Configurations ........................................................................................................................10-9 Sketch Relations in Configurations ...................................................................................................................10-9 End Conditions in Configurations ...................................................................................................................10-10 Configurable Items for Assemblies ........................................................................................................................10-10 Modifying a Configuration Dimension ..................................................................................................................10-11 Editing a Configuration ..........................................................................................................................................10-11 Special Assembly Configurations ...........................................................................................................................10-12 Component Configurations in an Assembly ...........................................................................................................10-12
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Deleting a Configuration ........................................................................................................................................10-13 Design Table Configurations .........................................................................................................................................10-14 Creating a Design Table .........................................................................................................................................10-14 Creating a Design Table as a Separate Excel File ..................................................................................................10-14 Inserting a Design Table .........................................................................................................................................10-16 Design Table PropertyManager ..............................................................................................................................10-17 Add Rows and Columns .........................................................................................................................................10-18 Creating Configurations with a Design Table ........................................................................................................10-18 Formatting a Design Table .....................................................................................................................................10-19 Manually Add Parameters in a Design Table .........................................................................................................10-21 Numerical Configuration Name .............................................................................................................................10-21 Editing a Design Table ...........................................................................................................................................10-21 Deleting a Design Table .........................................................................................................................................10-21 Saving Design Tables .............................................................................................................................................10-22 Deleting a Configuration ........................................................................................................................................10-22 Specifying Design Table Parameters ......................................................................................................................10-23 Specifying Design Table Parameters ..............................................................................................................10-23 Summary of Design Table Parameters ............................................................................................................10-24 Dimensions in Design Tables ..........................................................................................................................10-25 Dimensions ......................................................................................................................................................10-26 Component Configuration ...............................................................................................................................10-26 Component Visibility ......................................................................................................................................10-26 Component Suppression State .........................................................................................................................10-27 Suppression of Features ..................................................................................................................................10-27 Base Parts ........................................................................................................................................................10-28 Component Part Number .................................................................................................................................10-28 Comment .........................................................................................................................................................10-29 Equations in Configurations ............................................................................................................................10-30 Expand in BOM ..............................................................................................................................................10-31 Lighting in Design Tables ...............................................................................................................................10-31 Split Parts ........................................................................................................................................................10-32 Custom Properties ...........................................................................................................................................10-32 User Notes .......................................................................................................................................................10-33 Color Parameter ...............................................................................................................................................10-33 Design Tables in Drawings ....................................................................................................................................10-35 Design Tables in Drawings .............................................................................................................................10-35 Displaying a Design Table in a Drawing ........................................................................................................10-35 Design Table in a Drawing ..............................................................................................................................10-36 Editing a Design Table in a Drawing ..............................................................................................................10-36
Chapter 11 Drawings Drawings Overview .........................................................................................................................................................11-1 Getting Started in Drawings ............................................................................................................................................11-2 Setting Options for Drawing Documents .................................................................................................................11-2 Creating a Drawing ...................................................................................................................................................11-3 Sheet Format/Size .....................................................................................................................................................11-3 Sheet Properties ........................................................................................................................................................11-4 Multiple Drawing Sheets ..........................................................................................................................................11-4 Sheet Formats, Sheets, and Views ............................................................................................................................11-5 Customizing Sheet Formats ......................................................................................................................................11-5 Saving Sheet Formats ...............................................................................................................................................11-6 Linking Notes to Document Properties ....................................................................................................................11-7 The Drawing Window ..............................................................................................................................................11-8 Views of Parts and Assemblies ................................................................................................................................11-8 View Boundaries ......................................................................................................................................................11-9 Scales in Drawings ...................................................................................................................................................11-9 Dimension Type .....................................................................................................................................................11-10
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Crosshatch in Drawings ..........................................................................................................................................11-10 2D Sketching in Drawings ......................................................................................................................................11-10 Quality in Drawings ................................................................................................................................................11-11 Convert to Draft Quality .........................................................................................................................................11-12 Sending Drawing Documents Electronically ..........................................................................................................11-12 Types of Drawing Documents .......................................................................................................................................11-13 Drawing Documents ...............................................................................................................................................11-13 Detached Drawings .................................................................................................................................................11-13 Working in Detached Drawings .............................................................................................................................11-14 Lightweight Drawings ............................................................................................................................................11-16 Standard Drawing Views ...............................................................................................................................................11-17 Standard Drawing Views ........................................................................................................................................11-17 Standard 3 View .....................................................................................................................................................11-17 Standard 3 View PropertyManager .................................................................................................................11-19 First Angle and Third Angle Projection ..........................................................................................................11-19 Model View ............................................................................................................................................................11-19 Model/Predefined/Empty View PropertyManager .................................................................................................11-21 Relative to Model View ..........................................................................................................................................11-22 Relative View PropertyManager in Drawings ................................................................................................11-23 Relative View PropertyManager in Models ....................................................................................................11-24 Drawing View Orientation ..............................................................................................................................11-24 Predefined Views ....................................................................................................................................................11-24 Empty Views ..........................................................................................................................................................11-25 Derived Drawing Views ................................................................................................................................................11-26 Derived Drawing Views .........................................................................................................................................11-26 Projected View ........................................................................................................................................................11-26 Projected View PropertyManager ...........................................................................................................................11-27 Auxiliary View .......................................................................................................................................................11-28 Auxiliary View PropertyManager ..........................................................................................................................11-29 Detail View .............................................................................................................................................................11-30 Detail View PropertyManager .........................................................................................................................11-31 Modifying a Detail View .................................................................................................................................11-32 Detail Circle Styles ..........................................................................................................................................11-33 Crop View ...............................................................................................................................................................11-33 Broken-out Section .................................................................................................................................................11-34 Broken-out Section PropertyManager ....................................................................................................................11-35 Broken View ...........................................................................................................................................................11-35 Broken View Break Line Styles .............................................................................................................................11-37 Section Views in Drawings ....................................................................................................................................11-37 Section View PropertyManager ......................................................................................................................11-38 Modifying Section Views ................................................................................................................................11-40 Section Views of Assemblies ..........................................................................................................................11-40 Section Scope ..................................................................................................................................................11-41 Troubleshooting Section Views ......................................................................................................................11-41 Modifying Section Line Properties .................................................................................................................11-42 Aligned Section View .............................................................................................................................................11-42 Alternate Position View ..........................................................................................................................................11-43 Alternate Position PropertyManager ......................................................................................................................11-44 Position Schematic PropertyManager .....................................................................................................................11-44 OLE Items in Drawings ..........................................................................................................................................11-45 Drawing View Update ............................................................................................................................................11-45 Drawing View Alignment and Display ..........................................................................................................................11-45 Drawing View Alignment and Display ..................................................................................................................11-45 Manipulating Views ................................................................................................................................................11-46 Drawing View Properties ................................................................................................................................11-46 Multiple Views PropertyManager ...................................................................................................................11-47 Updating Views ...............................................................................................................................................11-47
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Move Drawing .................................................................................................................................................11-48 Moving Drawing Views ..................................................................................................................................11-48 Aligning Views ...............................................................................................................................................11-49 Rotating Views ................................................................................................................................................11-49 Rotate Drawing View ......................................................................................................................................11-50 Copying and Pasting Views ............................................................................................................................11-50 Hiding and Showing ...............................................................................................................................................11-51 Hiding and Showing Views .............................................................................................................................11-51 Hiding and Showing Edges .............................................................................................................................11-51 Hiding and Showing Sketches .........................................................................................................................11-52 Show Hidden Edges ........................................................................................................................................11-52 Hide/Show Components ..................................................................................................................................11-53 Hide Behind Plane ...........................................................................................................................................11-53 Displaying ...............................................................................................................................................................11-55 Component Line Font ......................................................................................................................................11-55 Drawing View Display Modes ........................................................................................................................11-55 Line Format .....................................................................................................................................................11-56 Tangent Edge Display Overview ....................................................................................................................11-57 Tangent Edge Display .....................................................................................................................................11-57 Layers ..............................................................................................................................................................11-58
Chapter 12 Detailing Detailing Overview ..........................................................................................................................................................12-1 Detailing Overview ..................................................................................................................................................12-1 Setting Detailing Options .........................................................................................................................................12-1 Inserting Model Items ...............................................................................................................................................12-1 Insert Model Items ....................................................................................................................................................12-2 Inserting Annotations into Drawings ........................................................................................................................12-3 Inserting Dimensions into Drawings ........................................................................................................................12-3 Inserting Reference Geometry into Drawings ..........................................................................................................12-4 Favorites ...................................................................................................................................................................12-4 Add or Update a Favorite .........................................................................................................................................12-6 Dimensions in Drawings ..................................................................................................................................................12-6 Dimensions Overview ..............................................................................................................................................12-6 Setting Dimensions Options .....................................................................................................................................12-7 Dimension PropertyManager ....................................................................................................................................12-8 Symbol ....................................................................................................................................................................12-10 Dimension Properties .............................................................................................................................................12-10 Value ...............................................................................................................................................................12-11 Name ...............................................................................................................................................................12-11 Full Name ........................................................................................................................................................12-11 Units ................................................................................................................................................................12-11 Font ..................................................................................................................................................................12-12 Arrow Style .....................................................................................................................................................12-12 Arrows .............................................................................................................................................................12-12 Display as inspection dimension .....................................................................................................................12-12 Read only .........................................................................................................................................................12-12 Dimension Precision .......................................................................................................................................12-12 Dimension Display ..........................................................................................................................................12-13 Driven ..............................................................................................................................................................12-13 Display with parentheses .................................................................................................................................12-13 Display as dual dimension ...............................................................................................................................12-13 Display with solid leader .................................................................................................................................12-13 Use document's second arrow .........................................................................................................................12-13 Display second outside arrow .........................................................................................................................12-14 Display as chain dimension .............................................................................................................................12-14 Diameter dimension ........................................................................................................................................12-14
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Foreshortened radius .......................................................................................................................................12-14 Dimension to inside of arc ...............................................................................................................................12-15 Display as linear dimension .............................................................................................................................12-15 First arc condition, Second arc condition ........................................................................................................12-15 Layer ................................................................................................................................................................12-15 Dimension Units/Chamfer Dimension Units ..........................................................................................................12-16 Dimensioning to Midpoints ....................................................................................................................................12-16 Reference Dimensions ............................................................................................................................................12-16 Parentheses .............................................................................................................................................................12-17 Baseline Dimensions ..............................................................................................................................................12-17 Ordinate Dimensions ..............................................................................................................................................12-17 Horizontal Ordinate Dimensions ............................................................................................................................12-19 Vertical Ordinate Dimensions ................................................................................................................................12-19 Parallel Dimensions ................................................................................................................................................12-19 Chamfer Dimensions ..............................................................................................................................................12-20 Dimension Leaders/Text .........................................................................................................................................12-21 Leader/Text Display for Chamfer Dimensions .......................................................................................................12-21 Moving and Copying Dimensions ..........................................................................................................................12-22 Aligning Dimensions ..............................................................................................................................................12-22 Align Dimensions Parallel/Concentric ...................................................................................................................12-23 Align Collinear/Radial Dimensions ........................................................................................................................12-24 Dimension Extension Lines ....................................................................................................................................12-24 Modify Text of Dimension .....................................................................................................................................12-26 Modify Dimension ..................................................................................................................................................12-26 Specify Configurations ...........................................................................................................................................12-27 Increment ................................................................................................................................................................12-27 Hide/Show Annotations ..........................................................................................................................................12-27 Dimension Tolerance ..............................................................................................................................................12-28 Fit Tolerances .........................................................................................................................................................12-29 Annotations ....................................................................................................................................................................12-31 Annotations Overview ............................................................................................................................................12-31 Annotations Options Overview ..............................................................................................................................12-31 Annotation Properties .............................................................................................................................................12-32 Multiple Annotations ..............................................................................................................................................12-33 Aligning Annotations ..............................................................................................................................................12-34 Multi-jog Leaders ...................................................................................................................................................12-35 Notes .......................................................................................................................................................................12-36 Hyperlinks in Notes .........................................................................................................................................12-37 Note PropertyManager ....................................................................................................................................12-38 Note Properties ................................................................................................................................................12-39 Multiple Leaders .....................................................................................................................................................12-41 Link to Property ......................................................................................................................................................12-41 Balloons ..................................................................................................................................................................12-42 Balloon PropertyManager .......................................................................................................................................12-44 Stacked Balloons ....................................................................................................................................................12-44 Stacked Balloon PropertyManager .........................................................................................................................12-46 AutoBalloons ..........................................................................................................................................................12-46 AutoBalloon PropertyManager ...............................................................................................................................12-47 Center Marks ..........................................................................................................................................................12-48 Center Mark PropertyManager ...............................................................................................................................12-50 Centerline Annotations ...........................................................................................................................................12-51 Hole Callouts ..........................................................................................................................................................12-52 Hole Callout Variables ...........................................................................................................................................12-53 Cosmetic Threads ...................................................................................................................................................12-54 Cosmetic Thread PropertyManager ........................................................................................................................12-55 Surface Finish Symbols ..........................................................................................................................................12-56 Surface Finish PropertyManager ............................................................................................................................12-57
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Datum Feature Symbols .........................................................................................................................................12-58 Datum Feature PropertyManager ...........................................................................................................................12-59 Datum Targets ........................................................................................................................................................12-59 Datum Target PropertyManager .............................................................................................................................12-60 Geometric Tolerancing ...........................................................................................................................................12-60 Geometric Tolerance Properties ......................................................................................................................12-62 Geometric Tolerance Options .........................................................................................................................12-62 Dowel Pin Symbols ................................................................................................................................................12-63 Weld Symbols ........................................................................................................................................................12-64 Weld Symbol Properties ..................................................................................................................................12-64 ANSI Weld Symbol Properties .......................................................................................................................12-65 GOST Weld Symbol Properties ......................................................................................................................12-66 Area Hatch/Fill .......................................................................................................................................................12-66 Area Hatch/Fill Properties ......................................................................................................................................12-68 Blocks .....................................................................................................................................................................12-69 Insert Block PropertyManager ........................................................................................................................12-73 Block Instance PropertyManager ....................................................................................................................12-74 Attributes .........................................................................................................................................................12-74 Block Definition PropertyManager .................................................................................................................12-75 Tables .............................................................................................................................................................................12-76 Annotation Tables ..................................................................................................................................................12-76 Table Anchors ........................................................................................................................................................12-77 Table Templates .....................................................................................................................................................12-78 Custom Table Templates ........................................................................................................................................12-79 Table Format PropertyManager .............................................................................................................................12-79 Table Cell PropertyManager ..................................................................................................................................12-80 Bill of Materials ......................................................................................................................................................12-81 Bill of Materials PropertyManager .................................................................................................................12-83 Bill of Materials Contents ...............................................................................................................................12-84 Bill of Materials Column PropertyManager ....................................................................................................12-85 Bill of Materials Sort .......................................................................................................................................12-85 Hole Tables .............................................................................................................................................................12-86 Hole Table Add Holes .....................................................................................................................................12-88 Hole Table PropertyManager ..........................................................................................................................12-88 Hole Table Axis PropertyManager .................................................................................................................12-89 Hole Table Insert PropertyManager ................................................................................................................12-89 Hole Table Column PropertyManager ............................................................................................................12-90 Revision Tables ......................................................................................................................................................12-91 Revision Table PropertyManager ....................................................................................................................12-92 Revision Table Column PropertyManager ......................................................................................................12-93 Excel-based Bill of Materials ........................................................................................................................................12-94 Bill of Materials Overview .....................................................................................................................................12-94 Bill of Materials Templates ....................................................................................................................................12-94 Bill of Materials - Inserting ....................................................................................................................................12-95 Bill of Materials - Configuration ............................................................................................................................12-95 Bill of Materials - Contents ....................................................................................................................................12-96 Bill of Materials - Control ......................................................................................................................................12-96 Bill of Materials - Edit Text ...................................................................................................................................12-97 Bill of Materials - Part No. Column .......................................................................................................................12-98 Bill of Materials - Multiple Configurations ............................................................................................................12-98 Bill of Materials - Save as Excel File .....................................................................................................................12-99 Bill of Materials - Custom Properties ...................................................................................................................12-100
Chapter 13 Import/Export Importing and Exporting Files .........................................................................................................................................13-1 Importing/Exporting SolidWorks Documents .................................................................................................................13-2 Importing Documents ......................................................................................................................................................13-3
xx
Importing Geometry .........................................................................................................................................................13-3 Editing Imported Features ................................................................................................................................................13-4 Open - Match Faces and Edges of Imported Features .....................................................................................................13-5 Import Diagnosis ..............................................................................................................................................................13-5 Import Diagnosis PropertyManager .................................................................................................................................13-6 General Import Options ...................................................................................................................................................13-7 STL and VRML Import Options ......................................................................................................................................13-8 Exporting Documents and Setting Options ......................................................................................................................13-9 ACIS Export Options ................................................................................................................................................13-9 DXF/DWG Export Options ....................................................................................................................................13-10 eDrawings Export Options .....................................................................................................................................13-11 IGES Export Options ..............................................................................................................................................13-11 Surface Representation ...........................................................................................................................................13-12 Parasolid Export Options ........................................................................................................................................13-13 STEP Export Options .............................................................................................................................................13-13 STL Export Options ................................................................................................................................................13-14 TIFF Export Options ...............................................................................................................................................13-15 VRML Export Options ...........................................................................................................................................13-15 Exporting Multibody Documents ..................................................................................................................................13-16 Print3D ...........................................................................................................................................................................13-16 File Types .......................................................................................................................................................................13-17 ACIS Files (*.sat) ...................................................................................................................................................13-17 Autodesk Inventor Files ..........................................................................................................................................13-17 CADKEY Files .......................................................................................................................................................13-17 CATIA Graphics Files ............................................................................................................................................13-18 DXF 3D Files ..........................................................................................................................................................13-18 DXF/DWG Files (*.dxf, *.dwg) .............................................................................................................................13-19 DXF/DWG View Only ....................................................................................................................................13-20 DXF/DWG View Only PropertyManager .......................................................................................................13-21 Inserting DXF/DWG Files ..............................................................................................................................13-21 Copying and Pasting from AutoCAD to SolidWorks .....................................................................................13-22 Imported DXF/DWG Entities ..........................................................................................................................13-22 DXF/DWG Mapping .......................................................................................................................................13-23 eDrawings ...............................................................................................................................................................13-24 Saving Drawing Sheets in eDrawing Files .............................................................................................................13-25 Saving Configurations in eDrawing Files ...............................................................................................................13-26 Highly Compressed Graphics Files ........................................................................................................................13-26 HOOPS Files ..........................................................................................................................................................13-27 IGES Files (*.igs, *.iges) ........................................................................................................................................13-27 IGES Entity Types ..................................................................................................................................................13-28 IGES Levels ............................................................................................................................................................13-29 IGES 3D Curves .....................................................................................................................................................13-29 JPEG Files ..............................................................................................................................................................13-29 Mechanical Desktop Files .......................................................................................................................................13-29 Parasolid Files (*.x_t, *.x_b) ..................................................................................................................................13-33 PDF Files ................................................................................................................................................................13-33 Pro/ENGINEER Files .............................................................................................................................................13-33 Importing Pro/ENGINEER Part Files Into SolidWorks .........................................................................................13-34 Importing Pro/ENGINEER Assembly Files Into SolidWorks ...............................................................................13-35 Exporting SolidWorks Documents as Pro/ENGINEER Files ................................................................................13-36 Solid Edge Files ......................................................................................................................................................13-36 STEP Files (*.step) .................................................................................................................................................13-37 STL Files (*.stl) ......................................................................................................................................................13-37 TIFF Files (*.tif) .....................................................................................................................................................13-38 Inserting TIFF Files ................................................................................................................................................13-38 Unigraphics II Files ................................................................................................................................................13-39 VDAFS Files (*.vda) ..............................................................................................................................................13-39
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Viewpoint Files ......................................................................................................................................................13-39 VRML Files (*.wrl) ................................................................................................................................................13-40 ZGL Files ................................................................................................................................................................13-40
Chapter 14 Library Features and the Feature Palette Window Library Features and the Feature Palette Window ..........................................................................................................14-1 Palette Features and Library Features - Similarities and Differences .............................................................................14-1 Mandatory References .....................................................................................................................................................14-2 Library Features ...............................................................................................................................................................14-2 Library Features ........................................................................................................................................................14-2 Creating a Library Feature ........................................................................................................................................14-3 Adding a Library Feature to a Part ...........................................................................................................................14-4 Insert Library Feature Wizard ..................................................................................................................................14-5 Editing a Library Feature ..........................................................................................................................................14-5 Change Dimensions ..................................................................................................................................................14-5 Adding Color ............................................................................................................................................................14-5 Dissolving a Library Feature ....................................................................................................................................14-6 Feature Palette Window ...................................................................................................................................................14-6 Feature Palette Window ...........................................................................................................................................14-6 Feature Palette Window Overview ...........................................................................................................................14-6 Displaying the Feature Palette Window ...................................................................................................................14-7 Organizing Feature Palette Items .............................................................................................................................14-7 Creating a Palette Item .............................................................................................................................................14-8 Thumbnail Graphics .................................................................................................................................................14-9 Working with Palette Items and Folders ..................................................................................................................14-9 Palette Parts as Derived Parts .................................................................................................................................14-10 Adding Palette Items to Documents .......................................................................................................................14-10 Adding a Palette Feature to a Part ...................................................................................................................14-10 Edit This Sketch ..............................................................................................................................................14-11 Edit Dimension Access ...................................................................................................................................14-12 Internal Dimensions ........................................................................................................................................14-12 Adding a Palette Part to an Assembly .............................................................................................................14-12
Chapter 15 Sheet Metal Sheet Metal ......................................................................................................................................................................15-1 Designing Sheet Metal with Sheet Metal Features ..........................................................................................................15-2 Base Flange ..............................................................................................................................................................15-2 Examining the FeatureManager Design Tree ...........................................................................................................15-2 Edge Flange ..............................................................................................................................................................15-3 Profile Sketch ...........................................................................................................................................................15-4 Miter Flange .............................................................................................................................................................15-4 Miter Flange - Arc Sketches ..............................................................................................................................15-6 Miter Flange - Sketch Creation .........................................................................................................................15-6 Miter Flange - Edge Selection ...........................................................................................................................15-7 Bend Positions ..........................................................................................................................................................15-7 Trim Side Bends .......................................................................................................................................................15-8 Sheet Metal Tab ........................................................................................................................................................15-9 Sketched Bend ..........................................................................................................................................................15-9 Hem ........................................................................................................................................................................15-10 Closed Corner .........................................................................................................................................................15-12 Designing a Solid Body, then Converting it to Sheet Metal ..........................................................................................15-13 Bend Types .............................................................................................................................................................15-13 Creating a Sheet Metal Part Using Sharp Bends ....................................................................................................15-13 Creating a Sheet Metal Part Using Round Bends ...................................................................................................15-14 Creating Sheet Metal Parts with Conical Faces .....................................................................................................15-15 Adding Walls to a Sheet Metal Part .......................................................................................................................15-16 Sheet Metal Features ..............................................................................................................................................15-17
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Importing a Sheet Metal Part to SolidWorks ..........................................................................................................15-17 Comparing Sheet Metal Design Methods ......................................................................................................................15-18 Comparing Sheet Metal Design Methods ...............................................................................................................15-18 Design a Sheet Metal Part from a Solid ..................................................................................................................15-18 Design a Part from a Solid, Then Convert it to Sheet Metal ..................................................................................15-19 Design a Sheet Metal Part from the Flattened State ...............................................................................................15-20 Design a Part from the Flattened State, Then Convert it to Sheet Metal ................................................................15-20 Reasons to Build a Part, then Convert it to Sheet Metal ........................................................................................15-21 Combining the Different Sheet Metal Design Methods .........................................................................................15-21 Other Sheet Metal Topics ..............................................................................................................................................15-22 Bend Allowance and Bend Deduction ....................................................................................................................15-22 Bend Allowance and Bend Deduction Options ...............................................................................................15-22 Bend Allowance and Bend Deduction ............................................................................................................15-22 K-Factor ...........................................................................................................................................................15-23 Bend Table Overview ......................................................................................................................................15-23 Bend Table - Text File .....................................................................................................................................15-24 Bend Table - Excel Spreadsheet ......................................................................................................................15-24 Bend Allowance Value ....................................................................................................................................15-25 Bend Deduction Value ....................................................................................................................................15-25 Using Forming Tools with Sheet Metal ..................................................................................................................15-25 Forming Tools .................................................................................................................................................15-25 Creating Forming Tools ..................................................................................................................................15-25 Creating Openings on Forming Tools .............................................................................................................15-27 Create a Positioning Sketch for Forming Tool ................................................................................................15-27 Working with Palette Items and Folders .........................................................................................................15-27 Applying Forming Tools to Sheet Metal Parts ................................................................................................15-28 More Sheet Metal Topics ........................................................................................................................................15-28 Using Auto Reliefs ..........................................................................................................................................15-28 Changing Auto Reliefs ....................................................................................................................................15-29 Edit Auto Reliefs .............................................................................................................................................15-29 Edit All Auto Reliefs .......................................................................................................................................15-29 Rip ...................................................................................................................................................................15-30 Bends ...............................................................................................................................................................15-31 Edit Bends .......................................................................................................................................................15-31 Reorder Bends .................................................................................................................................................15-31 Flattening Sheet Metal Bends ..........................................................................................................................15-32 No Bends .........................................................................................................................................................15-32 Sheet Metal - Default Bend Parameters ..........................................................................................................15-32 Mirroring Sheet Metal Parts ............................................................................................................................15-33 Cut Across Sheet Metal Bends ........................................................................................................................15-34 Normal Cut ......................................................................................................................................................15-35 Break Corner/Corner-Trim ..............................................................................................................................15-35 Jog ....................................................................................................................................................................15-36 Lofted Bend .....................................................................................................................................................15-38 Bend Deviation ................................................................................................................................................15-39 Creating Sheet Metal Parts with Cylindrical Faces .........................................................................................15-40 Creating Drawings of Sheet Metal Parts .........................................................................................................15-41 Flat Pattern .......................................................................................................................................................15-42 Merge Faces .....................................................................................................................................................15-43 Simplify Bends ................................................................................................................................................15-43 Corner Treatment .............................................................................................................................................15-43 Add Corner-Trim .............................................................................................................................................15-44 Creating a Sheet Metal Flat Pattern Configuration .........................................................................................15-44 Unfold/Fold .....................................................................................................................................................15-45
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Chapter 16 Weldments Weldments Toolbar .........................................................................................................................................................16-1 Weldments - Structural Members ....................................................................................................................................16-1 Weldments - Pierce Points (Locate Profile) .............................................................................................................16-3 Weldments - Corner Treatments ..............................................................................................................................16-4 Weldments - Change Corner Treatment ...................................................................................................................16-4 Weldments - Trim and Extend .........................................................................................................................................16-5 Weldments - Adding Gussets ..........................................................................................................................................16-7 Weldments - Fillet Weld Beads .....................................................................................................................................16-10 Weldments - End Caps ..................................................................................................................................................16-13 Creating Sub-Weldments ...............................................................................................................................................16-14 Weldment Drawings ......................................................................................................................................................16-14 Weldment Cut Lists .......................................................................................................................................................16-15 Weldment Cut List PropertyManager ............................................................................................................................16-16 Weldment Cut List Column PropertyManager ..............................................................................................................16-17 Custom Properties in Weldments ..................................................................................................................................16-18
Chapter 17 SolidWorks Options Overview of SolidWorks Options ...................................................................................................................................17-1 System Options ................................................................................................................................................................17-2 General System Options ...........................................................................................................................................17-2 Drawings Options .....................................................................................................................................................17-4 Display Style Options ...............................................................................................................................................17-5 Area Hatch/Fill Options ...........................................................................................................................................17-6 System Colors ...........................................................................................................................................................17-6 Sketch Options ..........................................................................................................................................................17-7 Display and Selection Options .................................................................................................................................17-8 Performance Options ..............................................................................................................................................17-10 Performance Settings ..............................................................................................................................................17-13 Assembly Options ..................................................................................................................................................17-13 Large Assembly Mode Options ..............................................................................................................................17-13 External References - Options ................................................................................................................................17-15 Default Templates ..................................................................................................................................................17-16 File Locations .........................................................................................................................................................17-16 FeatureManager Options ........................................................................................................................................17-17 Spin Box Increments ..............................................................................................................................................17-18 View Rotation Options ...........................................................................................................................................17-18 Backup Options ......................................................................................................................................................17-19 Document Properties .....................................................................................................................................................17-19 Detailing Options ....................................................................................................................................................17-19 Dimensions Options ...............................................................................................................................................17-21 Notes Options .........................................................................................................................................................17-23 Balloons Options ....................................................................................................................................................17-23 Arrows Options ......................................................................................................................................................17-24 Virtual Sharp Display Options ...............................................................................................................................17-25 Annotations Display Options .................................................................................................................................17-25 Annotations Font Options .......................................................................................................................................17-26 Tables Options ........................................................................................................................................................17-26 View Labels Options ..............................................................................................................................................17-27 Grid and Snap Options ...........................................................................................................................................17-28 Units Options ..........................................................................................................................................................17-28 Document Colors ....................................................................................................................................................17-30 Material Properties Options ....................................................................................................................................17-30 Line Font Options ...................................................................................................................................................17-31 Image Quality .........................................................................................................................................................17-31 Plane Display ..........................................................................................................................................................17-32
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1 SolidWorks 2004 Reference Guide
Dear SolidWorks Customer, We are pleased to introduce the SolidWorks Reference Guide, a new publication available to SolidWorks Subscription Service members. This publication includes the entire contents of SolidWorks® 3D mechanical design software online help documentation in an easy-to-navigate Adobe® Acrobat® PDF format, making it easier for you to find the technical information you need quickly. In addition, we offer convenient printing options for any customer who wishes to obtain a printed version of this document, which is approximately 1,000 pages long. For details, please visit the “guides” section of the SolidWorks Support web site or click to http://www.solidworks.com/pages/services/subscription/ReferenceGuide.html. We welcome your feedback concerning the SolidWorks Reference Guide. Please send comments and suggestions via email to [email protected]. We appreciate your support as an active member of the SolidWorks community! Sincerely,
John J. McEleney CEO, SolidWorks Corporation
Scope The information in the Reference Guide comes from the SolidWorks Online Help for SolidWorks 2004 Service Pack 1. The Reference Guide does not include information on the add-ins such as the PhotoWorks software or the eDrawings software. The purpose of the Reference Guide is to provide a linear, easily printed version of the SolidWorks Online Help. SolidWorks Corporation is responding to your enhancement requests for a way to easily print the help, quickly return to previous topics, and mark pages for later reference. Please note: •
The text in the Reference Guide matches the text in the SolidWorks Online Help; it has not been rewritten for printed format. The text might seem awkward at times because it originates from context-sensitive help.
•
The order of the topics in the Reference Guide might seem awkward at times. SolidWorks Corporation made its best attempt to arrange the topics of the SolidWorks Online Help in the most logical order.
•
Some page breaks may come at awkward times. A decision was made to forfeit some ideal placement of page breaks in favor of fewer pages in the book.
•
All Related Topics buttons in the SolidWorks Online Help were deleted from the Reference Guide.
SolidWorks 2004 Reference Guide
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Chapter 1 SolidWorks 2004 Reference Guide
Conventions The Reference Guide uses the following font and icon conventions: •
bold - Indicates a user interface element such as a menu item, tooltip, title of a dialog box, and so on.
•
- Represents a note or a tip. It is not a link; the information follows the icon. Notes and tips provide timesaving steps and helpful hints.
•
hyperlinks - Indicates a hyperlink to another section of the Reference Guide. You can click hyperlinks in the .pdf file to be taken to another section. Hyperlinks do not change to cross-references with a page number in any printed versions of the book.
Resources Some of the resources provided by SolidWorks Corporation to aid you in learning the software are: •
Quick Tips - Pop-up messages that appear while you create SolidWorks documents. These messages give hints and options based on the current SolidWorks mode. Access: Click Help, Quick Tips.
•
Introducing SolidWorks book - Discusses basic concepts and terms used throughout SolidWorks. The book uses a bathroom vanity to illustrate various tools and functions in the software. Access: Click Help, Introducing SolidWorks, or read the printed manual that is shipped to new customers.
•
What's New book - Highlights the new functionality with step-by-step examples for many of the new functions. Access: Click Help, What's New Manual, or read the printed manual that is shipped to subscription customers.
•
Online Tutorial - Includes step-by-step examples that teach the functionality of the SolidWorks product and its add-ins. Access: Click Help, Online Tutorial.
•
Moving from AutoCAD - Assists AutoCAD users in learning some of the differences between SolidWorks and AutoCAD. Access: Click Help, Moving from AutoCAD.
•
Glossary - Contains definitions of solid modeling and SolidWorks-specific terms. Access: Click the Glossary tab in the SolidWorks Online Help.
•
Design Portfolio - Showcases parts created with SolidWorks, provides a high level overview of design intent, and presents potential design implementations. Access: Click Help, Design Portfolio.
•
Release Notes - Contains information about new and changed functionality at every Service Pack. Access: Click Help, SolidWorks Release Notes.
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2 SolidWorks Fundamentals
SolidWorks Fundamentals What is SolidWorks 2004? SolidWorks® 2004 is mechanical design automation software that takes advantage of the familiar Microsoft® Windows® graphical user interface. This easy-to-learn tool makes it possible for mechanical designers to quickly sketch ideas, experiment with features and dimensions, and produce models and detailed drawings. This chapter discusses some basic concepts and terminology used throughout the SolidWorks software. It provides an overview of the following topics:
•
Basic Concepts
•
The FeatureManager Design Tree
•
Opening New Documents and Using Templates
•
Opening Existing SolidWorks Documents
•
What's Wrong?
•
Shortcut Menus
•
View Modes
•
Selection Methods
•
Print and Print Preview
•
SolidWorks Service Packs
•
Converting Older SolidWorks Files to SolidWorks 2003
•
Getting Help and Visiting the SolidWorks Web Site
•
Using the Macro Tools
•
Object Linking and Embedding (OLE)
•
SolidWorks Application Programming Interface (API)
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Chapter 2 SolidWorks Fundamentals
Basic Concepts •
A SolidWorks model consists of parts, assemblies, and drawings.
•
Typically, you begin with a sketch, create a base feature, and then add more features to your model. (You can also begin with an imported surface or solid geometry.)
•
You are free to refine your design by adding, changing, or reordering features.
•
Associativity between parts, assemblies, and drawings assures that changes made to one view are automatically made to all other views.
•
You can generate drawings or assemblies at any time in the design process.
•
The SolidWorks software lets you customize functionality to suit your needs.
•
Click Tools, Options on the main menu to display the available System Options and Document Properties tabs.
•
The SolidWorks software saves your work for you. The auto recover option automatically saves information about your active part, assembly, or drawing document so you do not lose your work in case of a system crash. To set this option, click Tools, Options. On the System Options tab, click Backups and select Save auto recover info every changes. Specify the number of changes that should occur before information is automatically saved.
Document Windows In the SolidWorks application, each part, assembly, and drawing is referred to as a document, and each document is displayed in a separate window. (Each drawing document can contain multiple drawing sheets, though.)
2-2
•
You can have multiple part, assembly, and drawing document windows open at the same time. Also, you can have multiple views of the same document visible at the same time.
•
To arrange the windows, you can drag them by their title bars, and you can resize them by dragging a corner or border. Also, from the Window menu, you can select Cascade, Tile Vertically, or Tile Horizontally.
•
To organize your SolidWorks window, you can minimize open documents. Click Minimize in the upper right corner of the document border. An icon appears in the lower part of the SolidWorks window. If the icon is not visible, it may be behind another open document. Resize any open documents as necessary. Click Window, Arrange Icons to arrange them at the bottom of the SolidWorks window.
•
Click Window, Close All to close all open documents. You are prompted to save any unsaved documents.
Cascade Arranges all SolidWorks document windows so they overlap with all their title bars visible. To cascade document windows:
Click Window, Cascade.
Tile Horizontally - Tile Vertically Arranges and shrinks the open SolidWorks document windows so they are all visible. To tile the document windows:
•
Click Window, Tile Horizontally to display the windows horizontally on your screen.
•
Click Window, Tile Vertically to display the windows vertically on your screen.
NOTE: If you have many SolidWorks documents open, the display will be both vertical and horizontal.
Arrange Icons Lines up all minimized document icons in evenly spaced rows at the bottom of the SolidWorks window. To arrange minimized document icons:
Click Window, Arrange Icons.
Close All Closes all open documents. If a new or changed document has not been saved, the program asks you to confirm whether you want to save the document or rebuild the part. To close all documents:
1.
Click Window, Close All.
2.
Respond to confirmation requests from the SolidWorks application to save or not save documents when they are closed.
New Window Creates a new window for viewing the active part, assembly, or drawing. To open another view in a new window:
1.
Click Window, New Window.
2.
Adjust the size and location of the new window, as desired. (To hide the FeatureManager design tree in the new window, drag the right edge of the FeatureManager design tree to the left edge of the window.) NOTE: This window is just another view of the same document. You can set the zoom, rotation, and view mode (wireframe, hidden removed/gray, or shaded) for each window independently, but any changes you make to the model will be reflected simultaneously in both windows.
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Chapter 2 SolidWorks Fundamentals
PropertyManager Overview More functions now use the PropertyManager instead of dialog boxes, which allows your graphics to be displayed instead of hidden by dialog boxes. Description The PropertyManager contains the following items: •
PropertyManager Title Block. Contains the feature icon and feature name
•
OK
, Cancel
, Preview
(Not shown are Keep Visible Undo
, and Help , Back
buttons.
, Next
, and
buttons.)
•
Group Boxes. Contain Group Box title label icons
• •
Group Box Open and Group Box Closed icons Selection Boxes. Available for making selections in the graphics area or in the FeatureManager design tree. When active they are pink. When you click an item in the selection box, the selected item is easier to identify in the graphics area, because the highlighted edges are bolder:
Edge is selected in PropertyManager - easier to identify in graphics area
, buttons and
Edge is not selected in PropertyManager - harder to identify in graphics area
Color Schemes You can apply pre-defined color schemes to the PropertyManager. To apply a pre-defined color scheme to the PropertyManager:
1.
Click Tools, Options, System Options, Colors.
2.
Select None in PropertyManager Skin. Skins take precedence over a color scheme in the PropertyManager.
3.
Select a color in Current Color Scheme. The colors in PropertyManager Color and PropertyManager Skin may change according to the color you selected in Current Color Scheme.
4.
Click OK. When you display the PropertyManager, the new color scheme appears.
2-4
Entering Values and Accepting or Cancelling Commands When you have the PropertyManager displayed, there are several ways to enter values and accept commands. To enter values and accept commands:
Original part with Depth
1.
set to 10.
Set Depth to 30, but do not press Enter.
Press Enter and the preview updates.
In the Extrude PropertyManager, under Direction 1, set Depth
Press Enter again and the part updates to show the new value.
to 30, but do not press Enter.
The preview does not change because you have not yet accepted the new value. 2.
Press Enter. The preview now updates to show the new Depth
because you accepted the new value.
3.
At this point, if you want to cancel the Extrude command and retain the original depth, press Esc. However, you want to accept the new value.
4.
Press Enter again. The Extrude command is accepted. The part updates to show the new value, and the PropertyManager closes.
Deleting and Clearing Selections In the PropertyManager, you can right-click items in a list to delete them from the selection. For example, to delete a face selection from the Shell PropertyManager, right-click the name of the face in the list and select Delete. You can also right-click anywhere inside the list, and select Clear Selections to delete all of the items in the list. Split Bar The split bar separates the PropertyManager from the graphics area. If you drag the split bar back and forth, it snaps into position at the optimum width for displaying the PropertyManager. When you create new documents, the split bar opens at the optimum width. You can drag the split bar to resize the windows, as necessary.
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Chapter 2 SolidWorks Fundamentals
Callouts and Handles Callouts Callouts are text-filled boxes that appear in the graphics area when you use certain tools. Callouts help you easily distinguish between different entities. For example, these callouts show the sweep profile and the sweep path. You can drag these callouts to reposition them, but you cannot use them to change any properties of the entity to which they refer
Some callouts, such as those for chamfers, display figures that you can edit to manipulate the size of the entity.
In this example, you can edit the callout in the graphics area. Handles Handles allow you to dynamically click, move, and set certain parameters without leaving the graphics area. The handle color is set in Tools, Options, System Options, Colors, in the System colors box. Active handles are the Highlight color. Inactive handles are the Inactive Entities color. Handles span the length of extrusions. Drag the handle to the desired extrude depth, and the handle spans that length. You can also drag the pointer (instead of the handle) to the desired extrude depth. Click the handle, then drag the pointer in either direction
One handle has one arrow head, and the other handle has two arrow heads, to help you see which direction the handle applies to.
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Drag and Drop SolidWorks supports several drag and drop operations for features. •
Reordering features. You can change the order in which features are rebuilt by dragging them in the FeatureManager design tree. Place the pointer on a feature name, press the left mouse button, and drag the feature name to a new position in the list. (As you drag up or down the tree, each item that you drag over highlights. The feature name that you are moving drops immediately below the currently highlighted item when you release the mouse button.) If the reorder operation is legal, a
pointer appears; if it is not legal, a
pointer appears.
NOTE: A reorder operation is legal as long as the parent feature precedes its child feature. For more information, see Parent/Child Relationships. You can create folders in the FeatureManager design tree, and drag and drop features into the folders. Example: The Cut-Extrude feature was made before the Shell feature was added.
In the Feature Manager design tree, the Shell feature icon was dragged and dropped before Cut-Extrude icon.
•
Moving and copying features. You can move or copy features by dragging them in the model.
To move a feature to a new place on a model:
While holding down the Shift key, drag the feature to a different location. Release the mouse button to drop the feature on a planar face of the model. Example:
To move more than one feature at a time, hold down the Ctrl key as you select the features, then hold down the Shift key while you drag the features. To create a copy of the feature on a model:
Point at a planar face on the feature and hold down the Ctrl key while you drag the feature. Drop the copy on a planar face of the model.
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Chapter 2 SolidWorks Fundamentals
To copy a feature from one part to another part:
Tile the windows, then hold down the Shift key, point at a planar face on the feature, then drag and drop the feature from one window to another. - or You can also use the Copy
and Paste
tools on the Standard toolbar.
Shortcut Menu You have access to a variety of tools and commands on the shortcut menu while you work in the SolidWorks software. When you move the pointer over geometry in the model, over items in the FeatureManager design tree, or over the SolidWorks window borders, right-click to access a shortcut menu of commands that are appropriate for wherever you clicked. Shortcut menus include: • • •
Headings to denote sections of the menu. User-defined names if you apply custom names to features, components, and so on. Groups of related menu items.
To add or delete an item in a SolidWorks menu:
1.
Display the shortcut menu where you want to add or delete a menu item and select Customize Menu. Each item currently visible in the menu is preceded by
.
This menu is for customization purposes only. You cannot run a command from this menu. 2.
To add menu items, select the empty check boxes. To delete menu items, clear the selected check boxes.
3.
Click anywhere outside of the menu to save your changes, or press Enter. To cancel your changes, press Esc.
To restore the shortcut menus to default values or to show all menu items:
1.
Click Tools, Customize, or right-click over the toolbar area (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
2.
On the Options tab, under Shortcut customization: •
Click Show All to display all shortcut menu items.
•
Click Reset to Defaults to reset all shortcut menu items to the default display. Click the same buttons under Menu customization to update SolidWorks menus.
3.
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Click OK.
You can access the "more commands menu" by selecting the double-down arrows the double-down arrows, the shortcut menu expands to offer more menu items.
in the menu. When you click
The double-down arrows appear after you have executed at least one command in the menu. If you have not executed a command in the menu, or if the menu contains fewer than 12 items, the double-down arrows do not appear. The shortcut menu provides an efficient way to work without continually moving the pointer to the main pull-down menus or the toolbar buttons. For instance, with the shortcut menu, you can: •
Select a tool without moving your pointer to the toolbar
•
Open and close sketches
•
Change or view the properties of an item
•
Rename a feature or dimension with the Properties dialog box
•
Hide or show a sketch, plane, axis, or assembly component by right-clicking an item in the FeatureManager design tree or in the graphics area
•
Temporarily roll a model back to an earlier state by right-clicking any feature in the FeatureManager design tree and selecting Rollback
•
Open an assembly component for editing
•
Access the dimension tools and an annotations menu when in a drawing
•
Access the toolbars list when you click a SolidWorks window border
Accepting Features You have several streamlined ways to accept features you create. After creating a preview of a feature, you can: •
Right-click and select OK or Cancel from the shortcut menu.
•
Right-click when the pointer changes to without accepting the values.
to accept the preview, or click to return to the preview
Confirmation Corner Another way to accept features is to use the Confirmation Corner. You can: •
Click the OK or Cancel icons that appear in the Confirmation Corner of the SolidWorks graphics area.
•
Click the Exit Sketch icon in the Confirmation Corner to finish the sketch or click the Delete Sketch icon to discard changes to the sketch.
To turn off the Confirmation Corner, click Tools, Options, General, System Options, and clear Enable Confirmation Corner.
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PropertyManager In an active PropertyManager, you can: •
Click OK
•
Click Cancel
or press Enter. or press Esc.
Pop-up Tooltips Pop-up tooltips guide you when building models. Pop-up tooltips appear with an informational message, then disappear after a few seconds. Here are some examples of pop-up tooltips: Sheet Metal Example. This pop-up tooltip appears when you insert a fold in a sheet metal part. In the Fold PropertyManager, if you select BaseBend1 under Bends to fold, the popup tooltip warns you that the selected bend is already folded. Offset Example. If you try to offset a spline sketch, a pop-up tooltip advises you that you can only sketch offset lines and arcs.
Help If you have questions while you use SolidWorks, you can find answers in several ways: •
SolidWorks User Interface
Use the following tools to get help with items in the SolidWorks window: o
PropertyManagers and dialog boxes. In an active PropertyManager or dialog box, click Help , click the Help button, or press F1.
o
o
o
•
What's This. Click What's This on the Standard toolbar, then click a FeatureManager design tree, ConfigurationManager, PropertyManager, or toolbar item for help on that item. Tooltips. Provides information about tools on toolbars, PropertyManagers, and dialog boxes. When you pause the pointer over a tool for a brief time, a tooltip appears to display the name of the tool. Status Bar. Provides a brief description in the Status Bar at the bottom of the SolidWorks window as you move the pointer over a tool or click a menu item.
SolidWorks Online User's Guide
Provides assistance while you work. To access this resource, click Help on the Standard toolbar, or click Help, SolidWorks Help Topics. The help also contains a glossary of terms.
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•
Quick Tips
Displays a set of pop-up messages that appear while you create SolidWorks documents. Quick Tips give hints and options based on the current SolidWorks mode. Most of the messages have hyperlinks; click a hyperlink to see the associated item in the SolidWorks window. To access this resource, click Help, Quick Tips. Quick Tips are not available when the Online Tutorial is active. •
SolidWorks API and Add-Ins Help Topics
Provides assistance while you work on the SolidWorks Application Programming Interface (API) or other API add-in products. To access this resource, click Help, SolidWorks API and Add-Ins Help Topics. •
Moving from AutoCAD
Helps you transition from 2D AutoCAD to 3D SolidWorks. It compares terms and concepts, explains SolidWorks approaches to design, and provides links into SolidWorks help, tutorials, and other resources. To access this resource, click Help, Moving from AutoCAD. •
Introducing SolidWorks
Introduces concepts and design processes in a high-level approach. It does not give step-by-step procedures on how to create a model; instead, it guides you through the design process by illustrating how to plan models, make parts, build assemblies, then create drawings. This book is shipped to new customers. Introducing SolidWorks is available as an Adobe Acrobat file if you installed the manuals during the installation of the SolidWorks software. To access this resource, click Help, Introducing SolidWorks. •
Online Tutorial
Contains lessons that provide an online alternative to the Introducing SolidWorks book, and helps new users build models faster. To access this resource, click Help, Online Tutorial. o
o
o
•
The Online Tutorial includes several step-by-step lessons that cover SolidWorks topics and several add-in applications. You can execute some SolidWorks commands directly from the Online Tutorial. This is helpful when you need to open a sample part. Click a link, and the SolidWorks software automatically opens the part so you do not have to browse directories to locate the part. When you click a toolbar button in the Online Tutorial window, the corresponding button highlights in the SolidWorks software to help you locate the tool.
Design Portfolio
Contains part examples that help you understand how to combine the various SolidWorks tools to meet your design needs and requirements. To access this resource, click Help, Design Portfolio. •
What's New Manual
Provides information about new functionality in SolidWorks. The What's New Manual is available as an Adobe Acrobat file if you installed the manuals during the installation of the SolidWorks software. To access this resource, click Help, What's New Manual. •
Tip of the Day
Gives helpful hints about the SolidWorks software when you open a new SolidWorks session. To access this resource, click Help, Tip of the Day. To see a tip each time you start a SolidWorks session, select Show tips at startup in the Tip of the Day dialog box. •
Service Packs
Access SolidWorks service packs that are regularly posted on the SolidWorks Web site. These service packs contain software updates and enhancements to the SolidWorks software. Service packs are available for SolidWorks Subscription Service customers only. To check for a new service pack, click Help, Service Packs. •
SolidWorks Release Notes
Provides the latest information about operating systems, graphics cards, new functionality in the latest service pack, and so on. To access this resource, click Help, SolidWorks Release Notes.
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•
About SolidWorks
Displays information about the SolidWorks software. To access this resource, click Help, About SolidWorks. In the dialog box, click Connect to get information from the SolidWorks Web site. For information about add-in applications you installed, click Help, About. •
Partner Solutions
Provides access to the SolidWorks Solution Program Partner Web site. To access this resource, click Help, Partner Solutions.
What's Wrong? Lets you view rebuild errors or warnings in a part or assembly. When there is a rebuild error, the SolidWorks software cannot create the model geometry. When there is a warning, model geometry is still created. Some common rebuild errors include: •
Dangling Dimensions or Relations. Dimensions or relations to an entity that no longer exists
•
Features that cannot be rebuilt, such as a fillet that is too large
You can identify rebuild errors or warnings by icons in the FeatureManager design tree: Icon
Description Indicates an error with the model. This icon appears on the document name at the top of the FeatureManager design tree, and on the feature that contains the error. Indicates an error with a feature. This icon appears on the feature name in the FeatureManager design tree. Indicates a warning underneath the node indicated. This icon appears on the document name at the top of the FeatureManager design tree, and on the parent feature in the FeatureManager design tree whose child feature issued the error. Indicates a warning with a feature. This icon appears on the specific feature in the FeatureManager design tree that issued the warning.
If a document or feature has both an error and a warning, the
icon is displayed.
To review rebuild errors or warnings with the What's Wrong functionality:
Right-click the sketch, feature, part, or assembly name and select What’s Wrong? to display the error. The Rebuild Errors dialog box automatically appears when the error is first generated. The dialog box includes:
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•
Asterisks. If an error message has a prefix of **, click the message to highlight the problem area on the model.
•
Show errors. Displays error messages.
•
Show warnings. Displays warning messages.
•
Display What's Wrong during rebuild. Automatically displays errors each time you rebuild the model. This option affects only the current SolidWorks session.
•
Display full message. Displays the complete message whenever there is an error. Otherwise, an abbreviated message is displayed.
Print Prints the active document. To print the active document:
1.
Click File, Print.
2.
In the dialog box, select from the following options: •
Document Printer o
Name. Specifies the printer.
o
The system provides read-only information about the printer’s status, type, and location.
o
Properties. Sets options that are specific to the selected printer.
o
•
•
System Options o
Line Weights. Specifies the line weights that work best with your printer or plotter.
o
Margins. Specifies values for the top, bottom, left, and right margins for the document.
Document Options o
•
Page Setup. Specifies page setup options and advanced printer options such as scale, orientation, resolution, and so on.
Header/Footer. Specifies headers and footers for the active document.
Print range o
All. Prints all pages of the document.
o
Pages (Drawings only). Prints the sheets you specify.
o
Selection (Drawings only). Prints a selected area of a drawing sheet at a scale you specify.
• Select from the following options. The last set state is remembered on subsequent prints during the current SolidWorks session only. o
Number of copies. Sets the number of copies to print.
o
Print background. Prints the window background, in addition to the model or drawing.
o
o
3.
Print to file. Prints to a file instead of the printer. Type a name for the file in the Print to File dialog box. Convert draft quality drawing views to high quality (Drawings only). Converts the current draft quality view into high quality for printing purposes only.
Click OK.
Page Setup Allows you to change printer settings. You must have a SolidWorks document open to set printer settings. To change printer settings:
1.
Click File, Page Setup.
2.
In the dialog box, select from the following options: •
Printer Settings. Select one of the following: o
o
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Use system settings. Prints the document with Windows print settings, and allows you to change these settings as needed. Use this document's settings. Overrides system print settings with the print settings saved in the current document, and applies any changes to these settings in the current document only. System print settings remain unchanged.
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Chapter 2 SolidWorks Fundamentals
o
Set each drawing sheet individually. Specify the settings for each sheet in the drawing by selecting a drawing sheet in Settings for. In subsequent files that you print, the SolidWorks software remembers the last setting you selected.
•
Resolution and Scale. Set the scale for the printed document. o
Same as window (parts and assemblies only). Prints the current view of the graphics area.
o
Scale to fit (drawings only). Prints the drawing sheet to fit the paper size.
o
Scale. Prints the document at a scaled value (in percent) that you specify.
o
High Quality (drawings only). The SolidWorks software determines the optimum resolution for the printer and paper size combination, generates the raster output and prints it accordingly. When you select High Quality, click File, Print, Properties to set any advanced properties for the selected printer. If there are options for improved raster output, selecte them to get the highest quality printed output.
•
•
Paper. Select: o
Size. Sets the paper size on which you want to print the document.
o
Source. Sets the printer tray where the paper is located.
Drawing Color. Select one of the following: o
o
o
•
3.
Automatic. Sends color information if the printer or plotter driver reports that it is capable of printing color. Otherwise, the SolidWorks software sends black and white information. Color / Gray scale. Sends color data to the printer or plotter regardless of the capabilities that the printer or plotter driver reports. Black and white printers generally print colored entities in gray scale or dithered with this option. Use this option where a color printer or plotter prints in black and white with the Automatic setting. Black and white. Sends all entities to the printer or plotter in black and white regardless of the printer or plotter color capabilities.
Orientation. Select: o
Portrait. Prints the document with a vertical page orientation.
o
Landscape. Prints the document with a horizontal page orientation.
Click OK.
Line Weights You can set the line weights in an active document that work best with your printer or plotter. These settings are saved for all open SolidWorks documents. To set line weights:
1.
Click File, Print.
2.
In the dialog box, under System Options, click Line Weights.
3.
In the Line Weights dialog box, type a value for the line weights (Thin, Normal, Thick, and five additional line thickness settings). If you use specific Line Thickness the settings in the Line Weights dialog box.
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values in a SolidWorks drawing, the lines print according to
4.
Click OK.
5.
Click OK to close the Print dialog box and print the document.
Margins You can set values for the top, bottom, left, and right margins for the printed document. These settings are saved for all SolidWorks documents. To set print margins:
1.
Click File, Print. The Print dialog box appears.
2.
Under System Options, click Margins. The Margins dialog box appears.
3.
Clear the Use printer’s margins check box. NOTE: The Use printer's margins check box prints the document with the printer's default margin values. If you modified the values in the Margins dialog box, select this check box to view the printer's default margin values.
4.
Set the Top, Bottom, Left, and Right margins to the desired values.
5.
Click OK.
6.
Click OK to close the Print dialog box and print the document.
Printing Drawings You can print or plot an entire drawing sheet, or just a selected area of the sheet. You have the option to print in black and white (the default) or in color. You can specify different settings for individual drawing sheet. For basic information about printing and plotting any SolidWorks document, see Print. To specify settings for individual drawing sheets:
1.
Click File, Page Setup. Under Individual Drawing Sheet Control, select Set each sheet individually.
2.
Select a sheet from the Settings for list, and choose settings for the sheet.
3.
Repeat step 2 for each sheet, or leave any sheet at the default settings, and click OK.
To print a drawing in color:
1.
In a drawing, modify the colors of the entities as desired. For information about changing the color, style, and thickness of entities, see Component Line Font, Line Format, and Layers.
2.
Click File, Page Setup. Under Drawing Color, select one of the following, then click OK: •
Automatic. SolidWorks detects the printer or plotter capabilities and sends color information if the printer or plotter driver reports that it is capable of printing color. Otherwise, SolidWorks sends black and white information.
•
Color / Gray scale. SolidWorks sends color data to the printer or plotter regardless of the capabilities that the printer or plotter driver reports. Black and white printers generally print colored entities in gray scale or dithered with this option. Use this option where a color printer or plotter prints in black and white with the Automatic setting.
•
Black and white. SolidWorks sends all entities to the printer or plotter in black and white regardless of the printer or plotter color capabilities.
3.
Click File, Print. In the Print dialog box, under Name, select a printer that supports color.
4.
Click Properties, verify that any options required for color printing are specified appropriately, then click OK. (The options vary for different printers.)
5.
Click OK to print. When the specified printer is set up for color printing, Print Preview displays the drawing in color also.
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To print the whole drawing sheet:
1.
Click File, Print. In the Print dialog box, under Print range, click All or specify the Pages you want to print.
2.
Under Scale, click the Scale To Fit check box to print the entire sheet on the page, or clear the check box and specify a Scale value (by percent).
3.
Click OK.
To print a selected area of a drawing sheet:
1.
Click File, Print. In the Print dialog box, under Print range, click Selection, and click OK. The Print Selection dialog box appears, and a selection frame is displayed on the drawing sheet. The frame reflects the current printer settings (page size, orientation, and so on) as defined under File, Page Setup, Print Setup.
2.
Select a scale factor to apply to the selected area. •
Model scale (1:1). This is the default. This means that the selected area is printed at actual size; a model dimension of 100mm is printed at 100mm. The default sheet scale is used to calculate the correct print size; therefore, for views that use a scale different than the default sheet scale, you may need to use a custom scale to achieve the desired result.
•
Sheet scale (n:n). The selected area is printed as it appears on the full sheet. If the drawing size and the paper size are the same, the entire sheet is printed. Otherwise, only the selected area is printed, as it would appear on the full sheet.
•
Custom scale. The selected area is printed at a scale factor you define. Enter the values you want in the boxes, then click Apply scale. You can use Custom scale to focus on a particular area of a drawing sheet.
When you change the scale factor, the selection frame size changes accordingly. 3.
Drag the selection frame to position it over the area you want to print. You can drag the entire frame, but you cannot drag the individual sides to control the selected area. You can pan or zoom the view, or change the sheet while the selection frame is displayed.
4.
Click OK to print the selected area.
Print Selection Lets you specify an area of the drawing sheet to print. To specify an area of the drawing sheet to print:
1.
In an open drawing, click File, Print.
2.
In the dialog box, under Print range, click Selection, then click OK. The Print Selection dialog box appears, and a selection frame appears on the drawing sheet. The frame reflects the current printer settings (such as page size, and orientation) as defined in the Page Setup dialog box.
3.
Select a scale factor to apply to the selected area: •
Model scale (1:1). The selected area is printed at actual size; a model dimension of 100mm is printed at 100mm. The default sheet scale is used to calculate the correct print size; therefore, for areas that use a scale different than the default sheet scale, you may need to use a custom scale to get the desired result.
•
Sheet scale (1:1). The selected area is printed as it appears on the full sheet. If the drawing size and the paper size are the same, the entire sheet is printed. Otherwise, only the selected area is printed.
•
Custom scale. The selected area is printed at a scale factor you define. Type the values you want in the boxes, then click Apply scale.
Click Example to see Custom scale examples.
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4.
Drag the selection frame to position it over the area you want to print. You can pan or zoom the view while the selection frame is displayed. The pointer changes to
5.
as you position the selection frame.
Click OK to print the selected area.
Custom Scale Examples Drawing Sheet Scale
Custom Scale for Printing
1:1
1:1
Printed Output
A 1 inch x 1 inch box prints at the same scale (1 inch x 1 inch). 1:1
2:1
A 1 inch x 1 inch box prints as a 2 inch x 2 inch box, even though the dimension values remain the same. (Conversely, if you set the custom scale to 1:2, the box prints at 0.5 inches x 0.5 inches.) 1:2
1:1
A 1 inch x 1 inch box prints as a 1 inch x 1 inch box. However, only one-fourth of the drawing sheet prints because the drawing is zoomed in to get the box to the 1:1 scale.
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D-Landscape 1:1
A-Landscape 1:1
A 1 inch x 1 inch box prints as a 1 inch x 1 inch box because the drawing sheet scales are the same. However, only oneeighth of the drawing sheet prints because an A-Landscape sheet is oneeighth the size of a D-Landscape sheet.
Print Preview Previews the image of the active document before you send it to the printer. To preview a print job:
Click Print Preview
on the Standard toolbar, or click File, Print Preview.
Keyboard Shortcuts Keyboard shortcut keys are available for every menu item. Look for the underlined letters on the main menu bar. If you do not see the underlined letters on the main toolbar, press Alt. Press Alt and the underlined letter to display the menu. For example, press Alt+F to display the File menu. Also, look for the underlined letter for each of the menu items. When the menu is displayed, pressing an underlined letter activates the related command. For example, press Alt+F to display the File menu, then press C to close your files. Some commands also have shortcut keys that are displayed on the menu beside the command. For example, the combination Ctrl+N opens a new file.
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This table lists commonly used default keyboard shortcuts: Action Model Views Rotate the model: • horizontally or vertically • horizontally or vertically 90 degrees • clockwise or counterclockwise Pan the model Zoom in Zoom out Zoom to Fit Previous View View Orientation View Orientation menu Front Back Left Right Top Bottom Isometric Selection filters Filter Edges Filter Vertices Filter Faces Toggle Selection Filter toolbar Toggle selection filters (on/off) File menu items New SolidWorks document Open document Open From Web Folder Make Drawing from Part Make Assembly from Part Save Print Additional keyboard shortcuts Access online help when in a PropertyManager or dialog box Rename an item in the FeatureManager design tree (this works for most items) Rebuild the model Force rebuild the model and rebuild all of its features Redraw the screen Cycle between open SolidWorks documents Line to arc/arc to line (sketch mode) Undo Cut Copy Paste Delete Next window Close window
Key Combination
Arrow keys Shift+Arrow keys Alt+ left or right Arrow keys Ctrl+Arrow keys Z z f Ctrl+Shift+Z Spacebar Ctrl+1 Ctrl+2 Ctrl+3 Ctrl+4 Ctrl+5 Ctrl+6 Ctrl+7 e v x F5 F6 Ctrl+N Ctrl+O Ctrl+W Ctrl+D Ctrl+A Ctrl+S Ctrl+P F1 F2 Ctrl+B Ctrl+Q Ctrl+R Ctrl+Tab a Ctrl+z Ctrl+ x Ctrl+ c Ctrl+ v Delete Ctrl+F6 Ctrl+F4
Additionally, you can customize the keyboard shortcut keys to suit your style of working.
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Send Mail Sends the current SolidWorks document to another system using your electronic mail application. To mail a part or sketch to another computer:
1.
Click File, Send To. Your electronic mail application responds with its usual dialog box.
2.
Type your mail password, the mailing address, and any other information required by your mail application.
To mail an assembly or drawing to another computer:
1.
Click File, Send To.
2.
In the dialog box, select one of the following: •
only.
•
and other documents it references.
A list of the referenced documents and their locations, the number of documents, and the combined size of the documents is displayed. If the size of the mail is large, it can cause transmission problems. If you choose to send the assembly or drawing and referenced documents, you do not have to send all of the referenced files. You can click: •
Attach. Attaches the selected reference document to the mail message. (The paper clip icon is added.)
•
Remove. Removes the selected reference document from the mail message. (The paper clip icon is replaced.)
•
Attach All. Attaches all of the reference documents to the mail message. (The paper clip icon is added.) If an assembly document has lightweight components, this dialog box does not appear.
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3.
Click OK.
4.
Type your mail password, the mailing address, and any other information required by your mail application.
Toolbars Toolbars Displays or hides toolbars. See the following: 2D to 3D
Font
Sketch
Align
Layer
SolidWorks Office
Annotation
Line Format
Spline Tools
Assembly
Macro
Standard
Curves
Mold Tools
Standard Views
Dimensions/Relations
Reference Geometry
Surfaces
Drawing
Selection Filter
Tools
Explode Sketch
Sheet Metal
View
Features
Simulation
Web Weldment
Toolbars for installed add-in products are available. These are available only if you select the toolbar from the View, Toolbars menu. You can use flyout toolbars to save space in the graphics area. When you click a flyout button associated with the flyout button appears.
, the toolbar
You can add flyout buttons to any toolbar, including the CommandManager. To make toolbars visible:
1.
Click Tools, Customize.
2.
On the Toolbars tab, under Toolbars, select the toolbars that you want to display; clear the toolbars that you want to hide.
3.
Click OK.
To add a toolbar button to a toolbar:
1.
Click Tools, Customize, Commands.
2.
In the dialog box, select a toolbar in Categories. To add a flyout button, select Flyout Toolbars.
3.
Under Buttons, drag a toolbar button to a toolbar in the SolidWorks window.
4.
Click OK.
To access hidden toolbar buttons:
Occasionally a toolbar is longer than the length of your screen. If this occurs, click the arrows toolbar to access the hidden toolbar buttons.
at the end of the
To move a toolbar:
Click the start or edge of the toolbar and drag. If you drag a toolbar to an edge of the SolidWorks window, the toolbar docks to the edge automatically. - or If you drag a toolbar away from the window edge, it becomes a floating palette. If you accidentally move a toolbar and you want to move it back to its original position, double-click the toolbar title.
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2D to 3D Toolbar The 2D to 3D tools help you convert a 2D drawing to a 3D part. Some of the tools can be used in any sketches. Front. The selected sketch entities become the front view in converting to a 3D part. Top. The selected sketch entities become the top view in converting to a 3D part. Right. The selected sketch entities become the right view in converting to a 3D part. Left. The selected sketch entities become the left view in converting to a 3D part. Bottom. The selected sketch entities become the bottom view in converting to a 3D part. Back. The selected sketch entities become the back view in converting to a 3D part. Auxiliary. The selected sketch entities become an auxiliary view in converting to a 3D part. You must select a line in another view to specify the angle of the auxiliary view. Create Sketch from Selections. The selected sketch entities become a new sketch. You can extract a sketch, for example, and then modify it before creating a feature. Repair Sketch. You can fix errors in a sketch so that the sketch can be used to extrude or cut a feature. Typical errors can be overlapping geometry, small gaps, or many small segments that are collected into a single entity. Align Sketch. Select an edge in one view to align to the edge selected in a second view. The order of selection is important. Extrude. Extrude a feature from the selected sketch entities. You do not have to select a complete sketch. Cut. Cut a feature from the selected sketch entities. You do not have to select a complete sketch.
Align Toolbar The Align toolbar provides tools for aligning annotations such as Notes, Geometric Tolerance Symbols, and so on. See Aligning Annotations. Leftmost Rightmost Uppermost Lowermost Space evenly across Space evenly down Center Horizontal Center Vertical Compact Horizontal Compact Vertical
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Annotations Toolbar The Annotations toolbar provides tools for adding notes and symbols to a drawing, part, or assembly document. Only those annotations that are appropriate for the active document are available; the other tools are displayed in gray. Note Surface Finish Geometric Tolerance Balloon AutoBalloon Stacked Balloon Datum Feature Symbol Weld Symbol Datum Target Insert Block Model Items Center Mark Centerline Hole Callout Cosmetic Thread Multi-jog Leader Dowel Pin Symbol Hole Table Bill of Materials Revision Table Design Table Weldment Cut List
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Assembly Toolbar The Assembly toolbar controls the management, movement, and mating of components. Insert Components New Part New Assembly Large Assembly Mode Hide/Show Components Change Transparency Change Suppression State Edit Component Smart Fasteners Mate Move Component Rotate Component Replace Components Replace Mate Entities Exploded View Explode Line Sketch Interference Detection Change Assembly Transparency Simulation Toolbar
CommandManager The CommandManager is a context-sensitive toolbar that dynamically updates based on the toolbar you want to access. By default, it has toolbars embedded in it based on the document type. When you click a button in the control area, the CommandManager updates to show that toolbar. For example, if you click Sketches in the control area, the Sketch toolbar appears in the CommandManager.
Use the Command Manager to access toolbar buttons in a central location and to save space for the graphics area.
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To access the CommandManager:
1.
Click Tools, Customize.
2.
In the dialog box, on the Toolbars tab, select Enable CommandManager.
3.
Click OK.
To use the CommandManager:
Click a button in the control area. The CommandManager updates to show the toolbar associated with the button you clicked. - or Click
next to a button in the control area.
The flyout toolbar associated with the button you clicked appears. To add buttons to the control area of the CommandManager:
When you add a button to the control area of the CommandManager, the button appears in the current document type only. For example, if you add the Reference Geometry button to the control area of the CommandManager while in a part document, it does not appear in the CommandManager for an assembly document. 1.
Right-click anywhere in the CommandManager and select Customize CommandManager.
2.
In the menu, select the toobars to add.
3.
Click anywhere outside the menu to save your changes, or press Enter. - or -
1.
Click Tools, Customize.
2.
On the Commands tab:
3.
a.
Select Flyout Toolbars in Categories.
b.
Under Buttons, drag the button to the control area of the CommandManager.
Click OK.
The Layer toolbar is not available in the CommandManager. To turn off the toolbar button descriptions:
Right-click anywhere in the CommandManager and select Show Description to clear the check mark.
Curves Toolbar The Curves toolbar provides tools for creating and using curves. Project Curve Split Line Composite Curve Curve Through XYZ Points Curve Through Reference Points Helix and Spiral
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Dimensions/Relations Toolbar and Menus The Dimensions/Relations toolbar and the Tools, Dimensions and Tools, Relations menus provide tools to dimension and to add and delete geometric relations. Not all toolbar buttons have corresponding menu items; conversely, not all menu items have corresponding toolbar buttons. Smart Dimension Horizontal Dimension Vertical Dimension Baseline Dimension Oridinate Dimension Horizontal Ordinate Dimension Vertical Ordinate Dimension Chamfer Dimension Autodimension Add Relation Display/Delete Relations Scan Equal Align Ordinate Constrain All
Drawing Toolbar The Drawing toolbar provides tools for aligning dimensions and creating drawing views. Align Collinear/Radial Align Parallel/Concentric Hide/Show Annotations Detail View Section View Aligned Section View Projected View Standard 3 View Auxiliary View Named View
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Relative View Predefined View Empty View Update View Crop View Broken-out Section Alternate Position View Area Hatch/Fill
Explode Sketch Toolbar With the Explode Sketch tools, you can add route lines to assembly explode line sketches and 3D sketches, and add jogs to sketch lines. Route Line Jog Line
Features Toolbar The Features toolbar provides tools for creating model features. The set of features icons is very extensive so not all of them are included on the default Features toolbar. You can customize this toolbar by adding and removing icons to suit your working style and frequent tasks. See Customize Toolbars for more information. Extruded Boss/Base Revolved Boss/Base Sweep Loft Thicken Extruded Cut Revolved Cut Swept Cut Lofted Cut Thickened Cut Cut with Surface Fillet Chamfer
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Rib Scale Shell Draft Simple Hole Hole Wizard Dome Shape Deform Wrap Move/Size Features Suppress Unsuppress Unsuppress with Dependents Linear Pattern Circular Pattern Mirror Feature Curve Driven Pattern Sketch Driven Pattern Table Driven Pattern Split Combine Join Delete Solid/Surface Imported Geometry Insert Part Move/Copy Bodies Library Feature
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Font Toolbar You can specify the font, font size, font style, and justification for selected notes, dimensions, and geometric tolerances. You can also reset the font properties to the document defaults. The Font toolbar is active only when notes, dimensions, or geometric tolerances are selected. Balloon text and view labels (Section View, Detail View, and so on) are notes and can be formatted with the Font tools. To specify a font:
1.
Select notes, dimensions, or symbols to format. Hold down Ctrl to make multiple selections.
2.
Select from the following font properites: •
Font. Select a font type from the list of font sets available on your system.
•
Font Size. Select the point size to use. The corresponding font size in the document’s default unit of measure is displayed in the next box. (The measurement corresponds to the actual height of the tallest character in the font set.)
•
Font Style. Click the icons for Bold, Italic, or Underline, or a combination of these.
•
Justification. Click the icons for Left Justify, Center Justify, or Right Justify to justify Note text.
To reset text to the document default font:
1.
Select a formatted item.
2.
Click Document Font
.
The text returns to the document font, size, style, and justification.
Layer Toolbar The Layer toolbar contains a list of layers in the active drawing and a tool for specifying the properties of layers. Layer Properties
Line Format Toolbar The Line Format toolbar provides tools for changing the appearance of individual lines, edges, and sketch entities in a drawing. Layer Properties Line Color Line Thickness Line Style Hide Edge Show Edge Color Display Mode
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Macro Toolbar The Macro toolbar controls macro recording, playback, and editing. Run Macro Stop Macro Record\Pause Macro New Macro Edit Macro
Mold Tools Toolbar The Mold Tools toolbar provides tools for creating molded parts and assemblies. Scale Parting Lines Ruled Surface Parting Surfaces Tooling Split Cavity Draft Split Line Offset Surface Ruled Surface Radiate Surface Planar Surface Knit Surface Draft Analysis Undercut Detection
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Reference Geometry Toolbar The Reference Geometry toolbar provides tools for creating and using reference geometry. Plane Axis Coordinate System Point Mate Reference
Sheet Metal Toolbar The Sheet Metal toolbar provides tools for creating and using sheet metal parts. Insert Bends Flatten No Bends Rip Base-Flange/Tab Miter Flange Fold Unfold Sketched Bend Edge Flange Closed Corner Hem Break-Corner/Corner-Trim Jog Lofted-Bend
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Simulation Toolbar The Simulation toolbar contains the tools for using Physical Simulation. Stop Record or Playback Calculate Simulation Reset Components Replay Simulation Linear Motor Rotary Motor Linear Spring Gravity
Sketch Toolbar The tools on the Sketch toolbar affect the entire sketch, rather than individual sketch entities. The Sketch toolbar controls selection, sketch creation, sketch modification, and the sketch grid.
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Select
Circle
Face Curves
Grid/Snap
Ellipse
Mirror Entities
Sketch or Exit Sketch
Partial Ellipse
Sketch Fillet
3D Sketch
Parabola
Sketch Chamfer
Modify Sketch
Spline
Offset Entities
Move or Copy Entities
Polygon
Fit Spline
Rotate or Copy Entities
Rectangle
Trim Entities
Scale or Copy Entities
Parallelogram
Extend Entities
No Solve Move
Point
Split Entities
Line
Centerline
Construction Geometry
Centerpoint Arc
Text
Tangent Arc
Convert Entities
3 Point Arc
Intersection Curve
Linear Sketch Step and Repeat Circular Sketch Step and Repeat Sketch Picture
SolidWorks Office Toolbar The SolidWorks Office toolbar allows you to activate any add-in application included in the SolidWorks Office package. The SolidWorks Office toolbar is unavailable if you did not install SolidWorks 2004 with a SolidWorks Office registration code. PhotoWorks release 2 SolidWorks Animator eDrawings 3D Instant Website SolidWorks Toolbox SolidWorks Utilities FeatureWorks
Spline Tools Toolbar Use tools on the Spline Tools toolbar to control properties of a sketched spline. The Spline tool is on the Sketch toolbar. Spline Point Show Inflection Points Show Minimum Radius Show Curvature Combs Simplify Spline
Standard Toolbar The Standard toolbar controls file management and model regeneration. New Open Save Make Drawing from Part/Assembly Make Assembly from Part/Assembly Print Print Preview Cut
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Copy Paste Delete Undo Redo Rebuild Redraw Edit Color Edit Material Edit Texture Toggle Selection Filter Toolbar Web Toolbar Help What's This? Save Saves the active document to disk. To save a document:
Click Save
or File, Save, or press Ctrl+S.
NOTE: When you save a new document, the Save As dialog box opens so that you can enter a filename or accept a default filename. Save As Saves the active document to disk with a new name or saves it in a different format for export to another application. To save a document with a new filename or format:
1.
Click File, Save As.
2.
In the dialog box, click the Save in box to browse to the location where you want to save the document. Use the locations sidebar to help navigate to the location where you want to save your document. The locations sidebar is available in certain operating systems only.
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3.
Type a name for File name.
4.
Select from the following options, if necessary: •
Save as type. Saves the file in another file format. You can also export files.
•
Description. Provides a description of the model.
•
Save as copy. Saves the document to a new filename without replacing the active document.
•
Save eDrawing data. Saves the document with eDrawings data so you can open the document in the eDrawings Viewer. If you selected Save eDrawings data in SolidWorks document in Tools, Options, System Options, General, you can override this option when you save your document. To override this option, clear Save eDrawing data.
5.
•
References. Displays a list of the documents referenced by the currently selected assembly or drawing. You can edit the locations of the listed files.
•
Down arrow (next to the Save button). Accesses Add to Favorites to create a shortcut to the selected document in your Favorites folder.
Click Save. The document is saved in the location you specified.
Cut Removes the selected items and places them on the Microsoft Windows Clipboard. To cut:
1.
Select the item(s) to cut.
2.
Click Cut
, or Edit, Cut, or press Ctrl+X.
Copy Copies one or more selected items to the Microsoft Windows Clipboard. To copy:
1.
Select one or more items to copy.
2.
Click Copy
, or Edit, Copy, or press Ctrl+C.
Paste Copies the contents of the Clipboard to the current sketch, part, assembly, or drawing document. To paste the contents of the Clipboard:
1.
2.
If necessary, select an appropriate destination for the item being pasted. For example: •
If the Clipboard contains a sketch, select a face or a plane to paste the sketch on.
•
If the Clipboard contains an extruded or revolved feature or a hole, select a face to paste the feature on.
Click Paste
or Edit, Paste, or press Ctrl+V.
Delete Removes one or more selected items. To delete an item:
1.
Select one or more items to delete.
2.
Click Delete
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on the Standard toolbar, click Edit, Delete or press Delete.
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3.
4.
In the dialog box, select: •
Also delete absorbed features. Deletes features that were used to create the item to be deleted listed in And All Dependent Items.
•
Also delete all child features. Deletes features dependent on a previously built feature listed in And All Dependent Items.
Click Yes. If you selected more than one item in step 1, click Yes to All to delete all of the items.
Undo Reverses recent changes you have made, when possible. To undo your last action:
Click Undo
or Edit, Undo, or press Ctrl+Z.
To undo multiple operations:
1.
Click Undo List (to the right of the Undo button) to see the list of actions that are available to undo. The most recent actions are at the top of the list.
2.
Select any action on the list. The action you selected and all actions above it on the list are reversed.
Redo Reverses recent Undo commands you have made, when possible. Redo is available only for sketches in part and assembly documents. To redo your last Undo action:
Click Redo
or Edit, Redo, or press Ctrl+Y.
To redo multiple Undo operations:
1.
Click Redo List (to the right of the Redo button) to see the list of Undo actions that are available to redo. The most recent actions are at the top of the list.
2.
Select any action on the list. The action you selected and all actions above it on the list are redone.
Rebuild Rebuilds the model with any changes that you made. To rebuild the model:
Click Rebuild
or Edit, Rebuild, or press Ctrl+B.
NOTE: When you reorder an imported feature or any other feature with no parent or child, the part does not rebuild - only the FeatureManager design tree rebuilds. Redraw Refreshes the screen, but does not rebuild the part. To refresh the screen:
Click Redraw
or View, Redraw, or press Ctrl+R.
NOTE: Use Redraw to refresh the screen if the graphics do not appear to be complete.
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Color And Optics PropertyManager Use the Color And Optics PropertyManager to apply color and optical properties to selected entities in a model. Selection •
•
Selection filters. Helps you select geometric entities in the model. o
Select Faces
o
Select Features
o
Select Surfaces
o
Select Components
o
Select Bodies
o
Select Parts
(assemblies only)
(assemblies only)
Remove Color. Deletes the color and optical properties from the selected geometry.
Favorite • •
Current Color. Displays the currently selected color in the swatch. Select or Create a Swatch. Displays pre-defined swatches included with the SolidWorks software.
•
Click Create New Swatch to define a custom swatch. Select Existing Color or Add Color. Displays the colors contained in the selected swatch.
•
Add Current Color to Swatch
•
Remove Current Color from Swatch
. Adds the selected color to a custom swatch. . Removes the selected color from a custom swatch.
Color Properties • •
Current Color. Displays the current color of the selected entity. Pick a Color. Displays all colors in the color palette.
• • •
RGB. Defines a color with red, green, and blue values. HSV. Defines a color with hue, saturation, and value entries. Numeric. Allows you to enter numeric values for RGB or HSV: o
Red Component of Color
o
Hue Component of Color
o
Green Component of Color
o
Saturation Component of Color
o
Blue Component of Color
o
Value Component of Color
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Optical Properties •
Transparency. Controls the degree to which light passes through the model.
•
•
Ambience. Approximates the intensity of a light source illuminating a surface from all directions without attenuation or shadowing.
•
•
Diffusion. Controls the intensity of the light on the surface. Diffusion is dependent on its angle to a light source but independent of the position of the viewer.
•
Specularity. Controls the intensity of the light on the surface. Specularity is dependent on the position of the light source and the position of the viewer. Shininess. Controls the reflectivity of the light.
Emissivity. Controls the intensity of radiated light.
Configurations • • •
This configuration All configurations Specify configuration
Materials Editor PropertyManager You can create parts from a specific material with the Materials Editor PropertyManager. The material and its properties propagate to COSMOSWorks, COSMOSXpress, PhotoWorks release 2, mass properties and material properties. The Material icon to a part.
appears in the FeatureManager design tree regardless of whether you applied a material
The Materials Editor PropertyManager controls: Materials •
Select a Material Database. Displays pre-defined material libraries included with the SolidWorks software, or displays custom material libraries.
•
Remove Material. Deletes the material from the model.
•
Create/Edit Material. Creates a new material or edits an existing material.
Visual Properties •
Advanced graphics. Allows you to display the model in RealView or Standard graphics.
•
RealView. Applies a 3D material to the model that dynamically changes when you rotate the model. RealView display applies only if you have a supported graphics card.
•
Standard. Applies a 2D texture to the model. You can control the: o
Scale
. Adjusts the grain of the texture.
o
Angle
o
Blend color. Blends the part color with the texture color.
. Adjusts the rotation of the texture.
•
Use material color. Applies the color shown to the model. This option is not available with all materials.
•
Use material crosshatch. Applies the crosshatch pattern assigned to the material when used as a section view in a drawing.
Physical Properties Displays the physical properties associated with the selected material.
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Texture PropertyManager Apply textures to geometric entities in a model. The Texture PropertyManager controls: Selection •
•
Selection filters. Helps you select geometric entities in the model. The available selection filters are: o
Select Faces
o
Select Features
o
Select Surfaces
o
Select Components
o
Select Bodies
o
Select Parts
(assemblies only)
(assemblies only)
Remove Textures. Deletes the texture from the selected entity.
Texture Selection •
Texture File Locations. Displays pre-defined texture libraries included with the SolidWorks software, or displays custom texture libraries.
•
Texture Tree. Displays 2D texture files.
•
Last 10 Used Textures. Displays the last 10 textures you used.
Texture Properties •
Texture Preview. Displays a preview image of the selected texture.
•
Scale
•
Angle
•
Blend color. Blends the part color with the texture color.
. Adjusts the grain of the texture. . Adjusts the rotation of the texture.
Configurations •
This configuration
•
All configurations
•
Specify configuration
Show Web Toolbar Displays or hides the Web toolbar. To access the Web toolbar when it is hidden:
•
Click Web Toolbar
on the Standard toolbar to display the Web icons.
•
Click Web Toolbar
again to hide the Web toolbar when it is not needed.
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Standard Views Toolbar The Standard Views toolbar provides tools to rotate the model, assembly, or sketch to one of the preset standard views. Front Back Left Right Top Bottom Isometric Trimetric Dimetric Normal To -- a view that is perpendicular to the selected plane or planar face
Surfaces Toolbar The Surfaces toolbar provides tools for creating and modifying surfaces. Extruded Surface Revolved Surface Swept Surface Lofted Surface Offset Surface Radiate Surface Knit Surface Planar Surface Extended Surface Trimmed Surface Filled Surface Mid-Surface Replace Face Delete Face Untrim Surface
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Tools Toolbar The Tools toolbar provides tools for measuring and defining the mass properties of models and for creating equations. Measure Equations Mass Properties Design Table Feature Statistics Deviation Analysis COSMOSXpress. Click Tools, COSMOSXpress.
View Toolbar The View toolbar controls: View Orientation
Hidden Lines Removed
Previous View
Shaded With Edges
Zoom to Fit
Shaded
Zoom to Area
Draft Quality HLR/HLV
Zoom In/Out
Perspective
Zoom to Selection
Shadows In Shaded Mode
Rotate View
Section View
Pan
Curvature
Wireframe
Zebra Stripes
Hidden Lines Visible
RealView Graphics
Web Toolbar The Web toolbar provides support for working over the Internet. Stop Current Jump Reload\Replace Insert Hyperlink Open Internet Address Stop Current Jump Stops the jump that you are attempting. To stop the current local or Internet jump:
Click Stop Current Jump
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Reload Documents Allows you to Reload documents. This is useful if you have read-only access to a document and you want to reload the latest version with any changes made by a colleague. To reload a document:
1.
Click File, Reload in a part or assembly document, or right-click a component in an assembly and select Reload.
2.
Select Open as read-only if you do not want to save any changes to the file. NOTE: If you have write-access to a sub-assembly then you reload it as read-only, you still have writeaccess to the individual components of the sub-assembly. You must reload each of the sub-assembly components as read-only to relinquish write-access privileges.
3.
Click OK. See also Replace Components.
Insert Hyperlink Creates a hyperlink to a document on the Internet, your local network, or on your own hard drive. When you select a hyperlink, the associated document or Web site opens. To create an embedded hyperlink:
1.
Click Insert Hyperlink
on the Web toolbar, or click Insert, Hyperlink.
The Insert Hyperlink dialog box appears. 2.
Type the path in the Link to file or URL box, or click Browse and browse to the document to which you want to link. The path appears in the Path box.
3.
Select the Use relative path for hyperlink check box if you want to specify a directory path relative to the current location instead of the full path.
4.
Click OK to accept the path. The path appears in the graphics area.
To delete an embedded hyperlink:
Click the hyperlink path, then press Delete. Open Internet Address Allows you to specify a Web site or document to view. If the specified path is to a local SolidWorks document, it opens in the SolidWorks application. Other documents and Web sites open in your Internet browser. To open an Internet link:
1.
Click Open Internet Address
on the Web toolbar.
The Open Internet Address dialog box appears.
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2.
Type the address of the document, folder, or computer on the Internet, or click the Browse button and browse to the document or location that you want.
3.
Click OK to continue to open the Internet address; click Cancel to end the operation and close the dialog box.
Weldments Toolbar The Weldments toolbar provides tools for creating weldment parts. Weldment Structural Member Gusset End Cap Fillet Bead Trim/Extend
FeatureManager Design Tree FeatureManager Design Tree The FeatureManager design tree on the left side of the SolidWorks window provides an outline view of the active part, assembly, or drawing. This makes it easy to see how the model or assembly was constructed or to examine the various sheets and views in a drawing. The FeatureManager design tree and the graphics area are dynamically linked. You can select features, sketches, drawing views, and construction geometry in either pane. You can split the FeatureManager design tree and either display two FeatureManager instances, or combine the FeatureManager design tree with the ConfigurationManager or PropertyManager. The FeatureManager design tree makes it easy to: •
Select items in the model by name.
•
Identify and change the order in which features are created. You can drag and drop items in the FeatureManager design tree list to reorder them. This changes the order in which features are regenerated when the model is rebuilt.
•
Display the dimensions of a feature by double-clicking the feature’s name.
•
Rename items by slowly clicking two times on a name to select it and then entering a new name.
•
Suppress and Unsuppress part features and assembly components.
•
View parent/child relations by right-clicking a feature in the list, then selecting Parent/Child.
•
Display the following items: o
Feature descriptions
o
Component descriptions
o
Component configuration names
o
Component configuration descriptions
The FeatureManager design tree provides the following folders and tools: •
Use the rollback bar to temporarily roll the model back to an earlier state.
•
, and selecting Add a new equation, edit, or delete an equation by right-clicking the Equations folder the action you want. (The Equations folder appears when you add the first equation to a part or assembly.)
•
Control the display of dimensions and annotations by right-clicking the Annotations folder
•
Add or modify a material applied to a part by right-clicking the Material icon
•
Add or modify light sources in the Lighting folder
•
View all solid bodies that the document contains in the Solid Bodies folder
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.
. .
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•
View all surface bodies that the document contains in the Surface Bodies folder
.
•
Add your own custom folders, and drag features into the folders to reduce the length of the FeatureManager design tree.
•
Move between the FeatureManager design tree, the PropertyManager, the ConfigurationManager, and Add-In tabs by selecting the tabs at the top of the left pane.
Show Feature's Description In part, assembly, and drawing documents, you can display feature descriptions in the FeatureManager design tree. To show feature descriptions:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Feature’s Description. The FeatureManager design tree displays the feature descriptions. By default, feature names and feature descriptions are the same. You must specify a new feature description in order for it to appear in the FeatureManager design tree. •
•
To change a feature description in a part or assembly, rightclick the feature, select Properties, and type a new Description. To change a feature description in a drawing, you must change the feature description in the part or assembly file.
Feature descriptions
Show Component's Description In part, assembly, and drawing documents, you can display component descriptions in the FeatureManager design tree. Component descriptions can also be displayed in the ConfigurationManager of parts and assemblies. To show component descriptions:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Components’s Description. The FeatureManager design tree displays the component descriptions. NOTES: •
•
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By default, component names and component descriptions are the same. You must specify a new component description in the component part file so it appears in the FeatureManager design tree. Component descriptions appear only if you selected Description in Custom property used as custom description in the General system options. You can select a different item for Custom property used as custom description, but you must set a value for that custom property on the Custom tab of the Summary Information dialog box.
Component description
Show Component's Configuration Name In part, assembly, and drawing documents, you can display component configuration names in the FeatureManager design tree. To show component configuration names:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Components’s Configuration Name. The FeatureManager design tree displays the component configuration names.
Component configuration name Show Component's Configuration Description In part, assembly, and drawing documents, you can display component configuration descriptions in the FeatureManager design tree. Component configuration descriptions can also be displayed in the ConfigurationManager of parts and assemblies. To show component configuration descriptions:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Components’s Configuration Description. The FeatureManager design tree displays the component configuration descriptions. By default, component configuration names and component configuration descriptions are the same. You must specify new component configuration descriptions so they appear in the FeatureManager design tree. You change a component configuration description in the part file.
Component configuration description
Show Configuration's Description In part or assembly documents, you can display configuration descriptions in the ConfigurationManager. By default, configuration names and descriptions are the same. You must specify new configuration descriptions so they appear in the ConfigurationManager. To change a configuration’s description, right-click the configuration in the ConfigurationManager, select Properties, and type a new Description. To show configuration descriptions:
In the ConfigurationManager, right-click the part or assembly name at the top of the tree, and select Tree Display, Show Configuration’s Description. The ConfigurationManager displays the configuration descriptions.
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FeatureManager Design Tree Conventions The FeatureManager design tree uses the following conventions: •
A
symbol to the left of an item’s icon indicates that it contains associated items, such as sketches. Click to expand the item and display its contents.
To collapse all expanded items at once, right-click the document name at the top of the tree, and select Collapse Items. •
Sketches in the FeatureManager design tree are preceded by (+) if they are over defined; they are preceded by (–) if they are under defined; they are preceded by (?) if the sketch could not be solved. (There is no prefix if the sketch is fully defined.)
•
Features are preceded by the rebuild symbol part.
•
Assembly components in the FeatureManager design tree are preceded by (+) if their position is over defined; they are preceded by (–) if their position is under defined; they are preceded by (?) if their position could not be solved; they are preceded by (f) if their position is fixed (locked in place).
•
Assembly mates are preceded by (+) if they are involved in over defining the position of components in the assembly; they are preceded by (?) if they could not be solved.
•
In an assembly, each instance of the component is followed by a number in angle brackets that increments with each occurrence.
•
The state of external references is displayed in the FeatureManager design tree, as follows: o
o
if a change has been made that requires the rebuild of the
If a part or feature has an external reference, its name is followed by –>. The name of any feature with external references is also followed by –>. If an external reference is currently out of context, the feature name and the part name are followed by ->?
o
The suffix ->* means that the reference is locked.
o
The suffix ->x means that the reference is broken.
Parent/Child Relationships Displays the parents and children of a selected feature, sketch, axis, plane, curve, or surface. A parent feature is an existing feature upon which others depend. For example, an extrude is the parent feature to a fillet that rounds its edges. When new features are built upon other features, their existence depends upon the previously-built feature. The new feature is called a child feature. For example, a hole is the child of the solid in which it is cut. To display parent/child relationships:
1.
In the model or in the FeatureManager design tree, right-click the item whose parent/child relationship you want to display.
2.
Select Parent/Child from the menu. The dialog box shows the Parents and Children of the selected feature.
3.
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In this dialog box, you can: •
Right-click an item in the Parents or Children list, and select an option from the shortcut menu, such as Edit Sketch or Edit Feature.
•
Expand features to see additional parent/child relationships.
•
Resize the dialog box to see all of the items listed.
Rollback Bar Temporarily reverts the model to an earlier state, suppressing recently added features. You can add new features or edit existing features while the model is in the rolled-back state. You can use the rollback bar to roll back to absorbed features, roll forward, roll to previous, or roll to the end of models. You can roll back a part with the Rollback Bar in the FeatureManager design tree. The rollback bar is a yellow and black line which turns blue when selected. Drag the bar up or down the FeatureManager design tree to step forward or backward through the regeneration sequence.
You can also use the shortcut menu to roll a model back to an earlier state. Right-click any feature in the FeatureManager design tree and select Rollback. To revert a part to an earlier state:
1.
Place the pointer over the rollback bar in the FeatureManager design tree. The pointer changes to
2.
.
Click the rollback bar. The bar changes color from yellow and black to blue.
3.
Drag the rollback bar up the FeatureManager design tree until it is above the feature(s) you want rolled back. - or Click the rollback bar and use the up and down arrow keys on the keyboard to move the rollback bar up or down. To enable this use of the arrow keys, click Tools, Options, System Options, FeatureManager, and select Arrow key navigation.
4.
To roll forward again, drag the rollback bar to the bottom of the FeatureManager design tree. Icons in the FeatureManager design tree are gray and unavailable when they are rolled back.
To roll back to absorbed features:
1.
In the FeatureManager design tree, click the
to expand the absorbed features within the parent feature.
2.
Right-click an absorbed feature, and select Rollback. A message appears that tells you the absorbed feature will be temporarily unabsorbed for editing purposes.
3.
Click OK.
4.
Drag the rollback bar below the feature you selected in step 2. The feature is unabsorbed and ready for editing.
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To roll a model forward:
1.
Roll the model back to an earlier state in the FeatureManager design tree.
2.
Right-click a rolled back feature in the FeatureManager design tree, and select Roll Forward. The model rolls forward to the selected feature.
To roll a model to its previous state:
1.
Roll the model back to an earlier state in the FeatureManager design tree.
2.
Right-click any feature in the FeatureManager design tree, and select Roll to Previous. The model rolls back to its previous state.
To roll to the end of a model:
1.
Roll the model back to an earlier state in the FeatureManager design tree.
2.
Right-click a rolled back feature in the FeatureManager design tree, and select Roll to End. The model rolls to its original state.
Split Panel Display You can display a split instance of the panel adjacent to the graphics area, usually the FeatureManager design tree. A split display is not limited to duplicate FeatureManager design trees. You can select any combination of the following: •
FeatureManager design tree
•
PropertyManager
•
ConfigurationManager
•
Third party applications that use the panel
This option is available either alone or in conjunction with Window, New Window. Without opening a new window, you can display the same part, assembly or drawing, along with any combination of the panels. With complex designs, for example, you can: •
Display different sections of the part, drawing, or assembly, expanded or collapsed
•
View different details for configurations
•
Pick different selections from each panel
To split the FeatureManager design tree:
1.
Place the pointer at the top of the FeatureManager design tree until it changes to
.
2.
Drag the bar down below the last item in the FeatureManager design tree.
3.
Release the mouse to display a duplicate FeatureManager design tree, below the first. Each instance of the FeatureManager design tree panel displays a set of tabs.
4.
Select the tabs that are appropriate for the panels that you want to display: PropertyManager, ConfigurationManager, FeatureManager design tree, or the panel of a third party application.
To close the split FeatureManager design tree:
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1.
Place the pointer at the top of the duplicate FeatureManager design tree until it changes to
2.
Drag the bar up until it meets the top of the original FeatureManager design tree.
3.
Release the mouse to close the display of the duplicate FeatureManager design tree.
.
Flyout FeatureManager Design Tree The flyout FeatureManager design tree allows you to view both the FeatureManager design tree and the PropertyManager at the same time. The flyout FeatureManager design tree automatically appears when a PropertyManager is active. To expand the flyout FeatureManager design tree, you can: •
Click
next to the document name in the flyout FeatureManager design tree
•
Click the PropertyManager title
The flyout FeatureManager design tree is transparent so you can see the model underneath it.
PropertyManager (left) and flyout FeatureManager design tree (right)
FeatureManager Options Lets you set the default system options related to the FeatureManager design tree. To set the default FeatureManager design tree options:
1.
Click Tools, Options.
2.
On the System Options tab, click FeatureManager.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
FeatureManager Options •
Scroll selected item into view. Specifies that the FeatureManager design tree should automatically scroll to display the feature icon that is related to the selected items in the graphics area. If you have a very complex part or assembly, you may want to turn this option off. Then, when you want the FeatureManager design tree to scroll to a feature you can right-click the feature and select Go To Feature (in Tree).
•
Name feature on creation. When you create a new feature, the feature name in the FeatureManager design tree is automatically selected and ready for you to enter a name of your choice.
•
Arrow key navigation. Lets you use the arrow keys to traverse the FeatureManager design tree, and expand or collapse the design tree and its contents, as follows o
Up arrow - Scrolls up the design tree
o
Down arrow - Scrolls down the design tree
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•
o
Left arrow at top of design tree - Collapses the design tree
o
Right arrow at top of design tree - Expands the design tree
o
Left arrow on an item in the tree - Collapses the item to hide its contents
o
Right arrow on an item in the tree - Expands the item to display its contents, if any
Dynamic highlight. Specifies that the geometry in the graphics area (edges, faces, planes, axes, and so on) is highlighted when the pointer passes over the item in the FeatureManager design tree.
Selecting from the FeatureManager Design Tree There are several ways to select items directly from the FeatureManager design tree. •
Select features, sketches, planes, and axes in the model by clicking their names in the FeatureManager design tree.
•
Select multiple consecutive items in the FeatureManager design tree by holding the Shift key while you select. Click the first item, hold down Shift, and click the last item.
•
Select multiple items in the graphics area, or select non-consecutive items in the FeatureManager design tree by holding the Ctrl key while you select.
•
Perform a text search of the FeatureManager design tree by right-clicking an item in the FeatureManager design tree (except Material or Lighting) and selecting Go To.
Find in FeatureManager Design Tree Lets you do a text search of the FeatureManager design tree for an item. To search the FeatureManager design tree:
1.
Right-click the name of the part, assembly, or drawing at the top of the FeatureManager design tree, and select Go To. - or Right-click the name of a part, feature, sketch, plane, or assembly in the FeatureManager design tree, and select Go To. The Find In FeatureManager Design Tree dialog box appears.
2.
Enter the name of the item (or a part of the name) in the Find what box.
3.
Click Find Next.
4.
Continue to click Find Next until the name of item you are searching for scrolls into view. By default, the tree is searched from the top to the bottom. If you want to reverse the search direction, clear the Start from the top check box.
Add Folders In part or assembly documents, you can add folders to the FeatureManager design tree. You can rename new folders and drag additional features into the new folders. This reduces the length of the FeatureManager design tree. When you select a folder that you added in the FeatureManager design tree, the features in the folder are highlighted in the graphics area. Similarly, when you select a feature in the graphics area that is in a folder you created, the folder is highlighted and expands to show the highlighted feature in the FeatureManager design tree. You can insert features into folders by one of two ways: automatically or manually. You can place any set of continuous features or components into an individual folder. You cannot use Ctrl to select non-continuous features. This maintains parent-child relationships. You cannot add new folders to existing folders.
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To create a new folder and insert features automatically:
In the FeatureManager design tree, right-click a feature and select Add to New Folder. A new folder appears in the FeatureManager design tree. The feature you right-clicked is now in the new folder. You can rename the folder and drag additional features into the folder. To create a new folder and insert features manually:
In the FeatureManager design tree, right-click a feature and select Create New Folder. A new folder appears in the FeatureManager design tree. You can rename the folder and drag additional features into the folder. When you manually drag a feature onto a folder name, the pointer changes to
.
To remove features from a folder:
1.
In the FeatureManager design tree, drag the feature from the folder onto the folder icon The pointer changes to
2.
.
.
Release the mouse button. The feature is removed from the folder, and appears just below the folder.
Opening New and Existing Documents in SolidWorks New SolidWorks Document Creates a new document. New documents use templates as the basis for their format and properties. Templates include user-defined parameters, such as units of measure or other detailing standards. Templates allow you to maintain as many different styles of documents for parts, drawings, or assemblies as you need. A document template can be a part, drawing, or assembly that you saved as a template. To create a new SolidWorks document:
1.
Click New on the Standard toolbar, click File, New, or click New Document in the Welcome to SolidWorks 2004 dialog box.
2.
The New SolidWorks Document dialog box has two versions. Click the appropriate button for the version you want to access: •
Novice. Uses a simpler version of the dialog box, which provides explanations of part, assembly, and drawing documents. If you have the Online Tutorial active, then open a new document, a tutorial template opens. The tutorial template uses the appropriate units, view orientations, and so on, for the tutorial lessons.
•
Advanced. Uses a modified version of the dialog box that shows template icons on various tabs. When you select a document type, a preview of the template appears in the Preview box. In the Advanced version, you can: o
Add your own tabs for storing templates.
o
Click the tutorial tab to access the tutorial template.
o
Click Large Icons
o
Click List
o
to display items with large icons.
to display items with small icons.
Click List Details to display information about each item in the window, including columns for file size and date modified.
3.
Click the type of document you want to open.
4.
Click OK.
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Default Templates You can specify the folder and template file for automatically created parts, assemblies, and drawings. For example, when you import a file from another application or create a derived part, the default template is used for the new document. To specify a folder for document templates:
1.
Click Tools, Options.
2.
On the System Options tab, click Default Templates. The current path and folder for part, assembly, and drawing templates appears.
3.
To change the folder for one of the template types, click the browse button window.
next to the path display
In the New SolidWorks Document dialog box, select the new default template, then click OK. If you need to add a template that does not appear in this dialog box, add the template location with the File Locations option. 4.
5.
Select one of the following options: •
Always use these default document templates
•
Prompt user to select document template
Click OK.
Creating Additional Template Tabs When you open a new SolidWorks document, you select a template for that document from a tab in the advanced version of the New SolidWorks Document dialog box. Initially, all the documents are listed on the same tab, but you can create additional custom tabs on which you can organize your templates. Custom tabs help manage your templates in the following ways: •
Placement - Create folders on any drive, including hard drives, floppy drives, or network drives.
•
Access - Share the contents of network folders, or restrict access to folders if required.
•
Organization - Arrange folder contents to reflect your work environment.
To create a new tab on the advanced version of the New SolidWorks Document dialog box:
1.
In Windows Explorer, create a new folder in the location that you want. For example, you could put a set of templates that you designed in a special folder called:\data\templates\My Special Templates
2.
In the SolidWorks software, click Tools, Options, System Options, File Locations.
3.
Select Document Templates in Show folders for.
4.
Click Add and browse in the Browse For Folder dialog box to find the location of the folder you created in step 1.
5.
Click OK.
6.
Click OK again to close the System Options - File Locations dialog box.
7.
Create a new template and, using Save As, browse to the folder you created in step 1 and name the new template. After you save a template to the new folder, a new tab appears in the advanced version of the New SolidWorks Document dialog box that is named after the folder you specified.
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Setting Default Material Properties You can set the following default material properties for your part or assembly document templates: •
Ambient. How light is reflected and scattered by other objects
•
Diffuse. How light is scattered equally in all directions on the surface
•
Specularity. How surfaces exhibit highlights
•
Shininess. How solid objects alternate between a glossy, reflective surface and a dull, matte surface
•
Transparency. How much light passes through the surface
•
Emission. How light projects from the surface
To set the default material properties for a document template:
1.
Click File, New. The New SolidWorks Document dialog box appears with an available set of templates.
2.
Double-click the part or assembly icon for the type of template that you want to create.
3.
Click Tools, Options, and on the Document Properties tab, click Colors. NOTE: Only options on the Document Properties tab are saved in a document template.
4.
In the Model\Feature colors list, select Shading, then click Advanced. The Advanced Properties dialog box appears.
5.
Set the material properties as desired, then click OK.
6.
Click OK to close the Document Properties - Colors box.
7.
Click File, Save As. The Save As dialog box appears.
8.
9.
In the Save as type list, select a template type: •
Part Templates (*.prtdot)
•
Assembly Templates (*.asmdot)
Type a name in the File name box. The extension is added automatically.
10. Browse to the folder where you want to save your template, then click Save.
Open Opens an existing part, drawing, or assembly document. Also used to import files from other applications. To open an existing part, assembly, or drawing document:
1.
Click Open
on the Standard toolbar, click File, Open, or press Ctrl+O.
2.
In the dialog box, select a file type in Files of type.
3.
Browse to select the part, drawing, or assembly document, or the file from another application that you want to open. NOTES: •
The Description label displays a description if you added one to the model.
•
Use the locations sidebar to help navigate to the location where you want to open your document. The locations sidebar is available in certain operating systems only.
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4.
Select from the following options, if necessary: •
Down arrow o
o
•
(Next to the Open button):
Open as Read-Only. Allows another user to have write access to the document while you have the document open. You cannot save or change the part in Read-Only mode. Add to Favorites. Creates a shortcut to the selected document in your Favorites folder.
Preview. Displays a preview of the SolidWorks part, assembly, or drawing document in the dialog box without opening it. Select a configuration name in Configurations to see a preview of the specified model configuration. If the Preview box does not display the configuration preview, open the document, then open each configuration, and save the document. The next time you open the document, the Preview box shows the selected preview.
5.
•
Advanced. Opens the Configure Document dialog box (assemblies only).
•
View-Only. Opens the part document only for viewing. (Only documents saved in SolidWorks 98 or later may be opened in View-Only mode.) If you are in a part or assembly document, you can change to edit mode by right-clicking in the graphics area and selecting Edit.
•
Lightweight. Opens the assembly or drawing document with lightweight parts.
•
References. Displays a list of the documents referenced by the currently selected assembly or drawing. You can edit the locations of the listed files.
Click Open to open the document, or double-click the configuration name under Configurations to open a specified configuration of the document. If you are opening files from a previous release of SolidWorks, the file may open more slowly than you would like. The Conversion Wizard converts the files so they open more rapidly.
Opening Documents from Part or Assembly Windows While you are editing an assembly, you can open its associated component documents (parts or sub-assemblies) in their own windows. Any changes that you make to the components automatically update the assembly. While you are editing a part with in-context features, you can open the assembly document where the features were created. To open a component from an assembly document:
1.
In the assembly window, right-click a component.
2.
Select Open part or Open Assembly. The component document opens in a separate window.
To open an assembly from a part document:
1.
In the part window, right-click a feature or sketch in the FeatureManager design tree or graphics area that has an external reference.
2.
Select Edit In Context. The assembly that contains the update path for the selected feature opens in a separate window.
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Multi-Threaded Retrieval Documents saved in recent SolidWorks releases are retrieved in multi-threaded mode. (Documents saved in releases prior to SolidWorks 98 cannot be retrieved in multi-threaded mode.) When you retrieve a large part, drawing, or assembly document, the document immediately displays in a view-only state while the actual document and all its components are retrieved in the background. During the view-only state, you can use all functions supported in the SolidWorks Viewer (Zoom, Rotate, and so on), but you cannot switch to another document or start to open another document. After the retrieval is complete, SolidWorks changes to the normal edit state.
SolidWorks Documents in Windows Explorer Use Windows Explorer to see thumbnail images and to access custom property information for SolidWorks documents. To see thumbnail images of SolidWorks documents in Windows Explorer:
Thumbnail images are available only if you use Windows XP, Windows 2000, or Windows Server 2003. 1.
In Windows Explorer, open a folder that contains SolidWorks documents.
2.
Click View, Thumbnails. A thumbnail image of each SolidWorks document in the folder is displayed. If you set up Windows Explorer to show preview images, a preview of the SolidWorks document also appears when the document is selected. You can also view thumbnail icons of SolidWorks parts and assemblies in Windows Explorer. The icon is based on the view orientation of the model when the document was last saved. To enable this functionality, click Tools, Options, System Options, General, and select Show thumbnail graphics in Windows Explorer. You may need to restart SolidWorks and Windows Explorer to see the thumbnail icons in these applications.
To preview a part, drawing, or assembly from Windows Explorer (Windows NT only):
Right-click the name of the part, drawing, or assembly in Windows Explorer, and select Quick View. To access custom property information for SolidWorks documents in Windows Explorer:
If you save custom property information in the Summary Information dialog box, the following properties appear in Windows Explorer: • Description •
Revision
•
Status
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Additionally, Type, Size, Last Saved By and Number of sheets are shown automatically. You cannot save this information in the Summary Information dialog box. 1.
In Windows Explorer, open a folder that contains SolidWorks documents.
2.
Move the pointer over a SolidWorks document. The custom property information is displayed.
To open a SolidWorks document from Windows Explorer:
In Windows Explorer, do one of the following: •
Double-click the name of the SolidWorks document.
•
Right-click the name of the SolidWorks document and select Open.
•
Drag and drop the SolidWorks document (or any document supported by the SolidWorks software) into an empty area of the SolidWorks window, not occupied by another document window.
Drag and Drop Files to a SolidWorks Document •
Drag and drop a part or assembly from Windows Explorer to an open SolidWorks assembly window to add an instance of the part or sub-assembly to the assembly.
•
Drag and drop a part or assembly from Windows Explorer to an open and empty SolidWorks drawing document to create a Standard 3 View drawing of the part or assembly.
•
Drag and drop a zipped (.zip) file into an empty SolidWorks window, or an empty area of an open SolidWorks document. The SolidWorks software opens the zipped files based on where you drop the zipped file. For example, if you drag and drop a .zip file that contains several models into an empty SolidWorks window, each model opens in its own window. The .zip file can contain any file type supported by the SolidWorks software. If the .zip file contains several SolidWorks files and an imported file, such as a .igs file, the .igs file opens in a separate window. NOTES: o
•
If the .zip file contains models that are not on your local computer (if you dragged the .zip file from the Internet), the Browse For Folder dialog box appears for you to download the .zip file to a location on your local computer.
Drag and drop hyperlinked SolidWorks part files from Internet Explorer, version 4.0 or later, to: o
the Feature Palette window
o
a new, empty part document
o
an empty area of a SolidWorks window
o
a drawing or assembly document
If you drop the file into a drawing or an assembly, you are prompted to name the new file on your local disk.
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•
Drag and drop between open documents. Drag a part name from the FeatureManager design tree of an open part file to insert it into an open assembly document.
•
Drag a part or assembly name from the FeatureManager design tree to a drawing document.
Web Folders Overview Web Folders Overview Web Folders is a SolidWorks tool that allows multiple users to share and work on SolidWorks part, assembly, or drawing documents, as well as other file formats, across the Internet. A Web Folder is a shortcut to a web server. Creating a Web Folder You need to create a Web Folder on a web server. Contact your system administrator for assistance. Using Web Folders Requirements: •
The web server must support Web Folders. Check with your system administrator or Internet service provider to see whether your web server supports Web Folders.
•
You must have Microsoft Internet Explorer version 5.0 or greater installed on your computer. If you are installing Internet Explorer, choose the Customize option and then select Web Folders under Web Authoring Components. If Internet Explorer is already installed, contact your system administration for assistance in adding Web Folders.
Accessing Web Folders For users to access a Web Folder you create on a web server, they must have an account on the web server. There are two options for allowing others to access your Web Folder: •
Users have an account on the server.
•
The user's account has the permission to access your Web Folder. Contact your system administrator for information on sharing a Web Folder with other users.
For users to be able to open and edit a SolidWorks document you place on a Web Folder: •
They must have access to the Web Folder.
•
They must have the SolidWorks software installed. If they do not have the SolidWorks software, they can view the SolidWorks document with SolidWorks Explorer.
Web Folder Security Your system administrator determines the Web Folder security policy when they set up access for other users. Contact your system administrator for security information.
Web Folders - Saving and Opening Files You can save a file to a web folder, or open a file from a web folder. To save a file to a web folder:
1.
Create a web folder on a computer with a web server. See your systems administrator to help you set up a web folder on a server.
2.
In SolidWorks, open the file that you want to save to the web folder.
3.
Click File, Save To Web Folder. The Save To Web Folder dialog box appears. The file name of the open file appears in the File name box.
4.
Click the arrow
in the URL box, and select the URL of the web folder on the server.
NOTE: If the web server requires a password, the Enter Network Password dialog box appears. Enter the User Name and Password, then click OK. The web folder opens, and the default folders are displayed. 5.
Double-click the web folder where you want to save the file.
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6.
Click Save. •
If you are saving a part or drawing document, it is saved to the web folder.
•
If you are saving an assembly document, the Copy Referenced Files To Server dialog box appears. Set the desired options, then click OK to save the referenced files to the web folder.
NOTE: When working with part and assembly documents, certain SolidWorks operations generate a Save As dialog box. You cannot save a document to a web folder from the Save As dialog box. To open a file from a web folder:
1.
Click File, Open From Web Folder. The Open From Web Folder dialog box appears.
2.
Click the arrow
in the URL box, and select the URL of the web folder on the server.
If the web server requires a password, the Enter Network Password dialog box appears. Enter the User Name and Password, then click OK. The web folder opens, and the default folders are displayed. 3.
Double-click the web folder that contains the file. All files in that folder appear in the dialog box window.
4.
Select the desired file and click Open. The file opens in SolidWorks.
Change URL With the Change URL dialog box, you can change where on the web server you save referenced files. To change where on the web server you save referenced files:
1.
In the Copy Referenced Files To Server dialog box, select one or more of the files in the Current Reference list.
2.
Click Change URL. The Change URL dialog box appears.
3.
Under New Location, type the new URL location where you want to save the referenced files.
4.
Click OK in the Change URL dialog box.
5.
Click OK in the Copy Referenced Files To Server dialog box. The referenced files are copied to the new URL location.
Copy Referenced Files to Server An assembly document references files called components. Use this dialog box to copy these referenced files to a web folder on a server. To copy referenced files to a web folder:
1.
Open a SolidWorks assembly document.
2.
Click File, Save To Web Folder. The Save To Web Folder dialog box appears. The file name of the open file appears in the File name box.
3.
Click the arrow
in the URL box, and select the web folder where you want to save the files.
If the web server requires a password, the Enter Network Password dialog box appears. If it does not require a password, go to step 5. 4.
Type the User Name and Password, then click OK. The web folder opens, and the default folders are displayed.
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5.
Double-click the web folder where you want to save the file.
6.
Click Save. The Copy Referenced Files To Server dialog box appears with the following information:
7.
•
Current Reference. The current path to the assembly components.
•
Copy the referenced files to. The new path to the web folder where you want to copy the assembly component.
•
Retain Folder Structure check box. Select to retain the same folder structure in the web folder as shown under the Current Reference list.
The following buttons are available: •
Select All. Click to select all files listed under Current Reference. Selected files show a check mark next to them. Only selected files are copied to the web folder.
•
Deselect All. Click to clear all selected files listed under Current Reference.
•
Change URL. Click to display the Change URL dialog box, which is used to change the location of referenced files that you are saving to a web folder. NOTE: At least one file under Current Reference must be selected to use the Change URL dialog box.
8.
Click OK. The referenced files are saved to the web folder.
Selection Highlighting Selected Items Items that you select are highlighted in a solid style font.
Edges that you select highlight as thick solid lines.
Edges of faces that you select highlight as thin solid lines.
To set the selected items highlighting color:
1.
Click Tools, Options, System Options Colors.
2.
Click Selected Item 1 in System colors, then click Edit.
3.
Select a color from the Color palette or click Define Custom Colors and define a new color, then click OK.
4.
Click OK again to close the System Options - Colors dialog box.
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To set the highlight color for faces that you select while in Shaded With Edges or Shaded view mode:
In Shaded With Edges select.
or Shaded
view modes, you can control the color used to highlight faces that you
1.
Click Tools, Options, System Options, Colors.
2.
Click Selected Item 1 in System colors, then click Edit.
3.
Select a color from the Color palette or click Define Custom Colors and define a new color, then click OK.
4.
Click OK again to close the System Options - Colors dialog box. To turn this option off, click Tools, Options, System Options, General, and clear Use shaded face highlighting. Selected faces in Shaded With Edges and Shaded view modes are then highlighted as thin lines.
Dynamic Highlighting When you move the pointer over an edge or a face, edges highlight as thick solid lines; edges of faces highlight as thin solid lines. This is the same highlighting functionality as for selected items. In drawings, edges dynamically highlight as thin phantom lines and edges of faces dynamically highlight as thin dashed lines. Dynamic highlighting is turned on as the default. To turn off dynamic highlighting, click Tools, Options, System Options, Display/Selection and clear Dynamic highlight from graphics view. To set the dynamic highlighting color:
1.
Click Tools, Options, System Options, Colors.
2.
Click Selected Item 1 in System colors, then click Edit.
3.
Select a color from the Color palette or click Define Custom Colors and define a new color, then click OK.
4.
Click OK again to close the System Options - Colors dialog box.
Select Select Select to:
lets you select sketch entities when you are working in a sketch. In a sketch or drawing document, use
•
select sketch entities
•
drag sketch entities or endpoints to reshape the sketch
•
select a model edge or face
•
drag a selection box around multiple sketch entities
•
select a dimension to drag to a new location
•
double-click a dimension that you want to modify
To select items:
1.
Click Select
or Tools, Select.
2.
Click the item that you want to select. Notice that items change color as the pointer passes over them. This dynamic highlighting helps you locate the item to select.
To select multiple items:
Hold down the Ctrl key while you click the items that you want to select.
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To box-select:
Depending on the type of document you are in, you can drag a selection rectangle around the items you want to select. All items that are completely inside the selection rectangle are selected. The following table shows which items are selected when you box-select in a specified document: Document
Item selected
Parts
edges
Assemblies
components
Drawings
annotations
Select Partial Loop Imported models can contain many small edges. To repair or edit imported models, you often need to select a series of connecting edges. When surfaces or solids contain small edges, use Select Partial Loop to choose a chain of connecting edges. The chain direction is based on the relative position of the second open edge that you select: •
Left of midpoint. Chain moves left.
•
Right of midpoint. Chain moves right.
The chain always includes the first edge you first selected. To use Select Partial Loop with solid bodies, the selected edges must be on the same face. To select a partial loop:
Loop direction, with edge 1 and edge 2
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1.
Select the first edge in the chain.
2.
Press Ctrl select the second edge, and do either of the following: •
Position the pointer left of the midpoint to create a chain that moves left.
•
Position the pointer right of the midpoint to create a chain that moves right.
Right of midpoint selected 3.
Right-click and choose Select Partial Loop.
Select Chain You can select a chain of entities attached to the selected entity in both directions until a branch is encountered. To select a chain of sketch entities:
Right-click a sketch entity and choose Select Chain. The entities of sketch geometry such as rectangles and polygons are selected. If the geometry includes branches, the chain stops at the branch. You can continue the selection manually. You can hold Ctrl and select multiple chains.
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Select Other Selects items that are hidden by other items. To select hidden items:
1.
Point at the item you want to select and right-click.
2.
Click Select Other. The pointer changes to
3.
.
Click the right mouse button to step through the items that lie under the point where you clicked. Click the left mouse button when the desired item is highlighted.
Midpoint Selection You can select the midpoint of an entity to create other entities such as planes or axes. To select a midpoint:
Right-click an edge, then click Select Midpoint. The midpoint appears as a circle on the edge.
Selection Filter Use a Selection Filter to help you select specific items in the graphics area or the drawing sheet area. For example, you can set a Selection Filter to filter only model faces. When you select items in the model, only faces can be selected. Selection Filters make it easy to identify the specified items when the pointer passes over them. To toggle the display of the Selection Filter toolbar, click Toggle Selection Filter Toolbar toolbar, or press F5. •
on the Standard
The first three buttons on the Selection Filter toolbar allow you to specify the behavior of the Selection Filter: Toggle Selection Filters. Turns selected filters on or off. You can also press F6. Clear All Filters. Clears all of the selected filters. Select All Filters. Selects all of the filters.
•
The rest of the buttons on the Selection Filter toolbar are filters. Select the filters that match the items you want to select in the graphics area. When a Selection Filter is active, the pointer changes to
.
Selection Filter Hot Keys •
To hide or show the Selection Filter toolbar, press F5.
•
To turn all the selected filters on or off, press F6.
•
To activate or deactivate specific filters, use the following hot keys.
Filter for edges
Press e
Filter for faces
Press x
Filter for vertices
Press v
NOTE: When a Selection Filter is active, the pointer changes to
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Box Selection You can select all entity types in parts, assemblies, and drawings by dragging a selection box. You can select multiple groups of entities by pressing the Ctrl key while dragging multiple box selections. The default geometry type selected is as follows: •
Part documents - edges
•
Assembly documents - components
•
Drawing documents - sketch entities, dimensions, and annotations
You can set up different selection types with the selection filters. In drawings, hidden edges and faces are not selected. To use box selection to select multiple edges in a part:
1.
Drag a selection box around the left face.
2.
Press Ctrl and drag to select the right side of the part.
The edges of the left face are highlighted.
The left side edges remain selected. The right side edges are highlighted and added to the selection.
NOTE: To enable selection of hidden edges, click Tools, Options, System Options, Display/Selection. Under Selection of hidden edges, select the Allow selection in wireframe and HLV modes and Allow selection in HLR and shaded modes check boxes, as desired.
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Loop Selection You can select a loop of connecting edges using the right mouse button, and then apply a feature such as fillet or chamfer to the selection. Hidden edges are selected in all view modes. To do a loop selection:
1.
Right-click the edge as shown.
2.
The edge becomes highlighted and the shortcut menu appears.
Click Select Loop. The edges of the entire outer loop of the front face become highlighted. The handle indicates the face whose edge is loop selected.
3.
Click the handle to change the loop selection to the edges of the other connecting face. The edges of the top face become highlighted. The handle changes to indicate the new face whose edge is loop selected.
Tangent Selection You can select a group of tangent curves, edges, or faces, with the right mouse button. You can then apply a feature, such as fillet or a chamfer, to the selection. Hidden edges are selected in all view modes. To do a tangent selection:
1.
Right-click the face as shown. The face becomes highlighted and the shortcut menu appears.
2.
Click Select Tangency. All five of the tangent faces become highlighted.
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Select through Transparency You can select opaque objects through transparent objects. This includes opaque components through transparent components in an assembly as well as interior faces, edges, and vertices through transparent faces in a part. As you move the pointer over opaque geometry that is behind transparent geometry, the opaque faces, edges, and vertices highlight. Click to select the highlighted geometry in the graphics area.
NOTES: •
For purposes of selection, transparent means more than 10 percent transparent. Entities less than 10 percent transparent are considered opaque.
•
If the entire model is transparent, (or opaque), use Select Other to select an object.
Keyboard Shortcuts You can use keyboard shortcuts to change which entities the pointer selects first:
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•
To select geometry on a transparent entity with an opaque object behind it, press Shift when selecting.
•
To select the part you are editing through an opaque component, press Tab when selecting.
Viewing Models Applying Color and Optic Properties Use the Color and Optics PropertyManager to apply colors and optical properties such as transparency and ambience to a model.
To apply color or optical properties to a selected entity:
1.
Click Edit Color
on the Standard toolbar, or click Edit, Appearance, Color.
2.
Set the properties in the Color And Optics PropertyManager as necessary.
3.
Click OK
.
To add a custom color swatch to the PropertyManager:
1.
Click Edit Color
on the Standard toolbar, or click Edit, Appearance, Color.
2.
In the PropertyManager, under Favorite: a.
Click Create New Swatch
.
b.
In the Save As dialog box, type a swatch name for File name, then click Save. The file extension is .sldclr. The swatch name appears in Select or Create a Swatch.
c.
To add a color to the swatch: i.
Under Color Properties, define the color you want to add.
ii.
Under Favorite, click Add Current Color to Swatch
.
The color is added to the swatch.
d.
To remove a color from the swatch: i.
Click a color in the custom swatch that you do not want to keep.
ii. Click Remove Selected Swatch Color The color is removed from the swatch.
3.
Click OK
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Draft Quality HLR/HLV Draft Quality HLR/HLV displays complex parts, assemblies, and drawings faster when your model is in Hidden Lines Removed or Hidden Lines Visible mode. Use Draft Quality HLR/HLV with any model for the following benefits: •
Real-time rotation. You can control the rotation speed, and display the entire model in real time.
•
Dynamic HLR/HLV recalculation. HLR/HLV displays during model rotation.
•
Resolution and performance. Image resolution and performance are dependent on the settings in the Document Properties- Image Quality dialog box. You can balance image quality (resolution) with performance. In drawing documents, the following functionality is not available with Draft Quality HLR/HLV:
•
Detail, Crop, Broken, or Alternate Position Views
•
Hide/Show Edge
•
Layers
Line Fonts and Component Line Fonts remain thin solid lines. To change the display of Hidden Lines Removed and Hidden Lines Visible to faster mode:
Click Draft Quality HLR/HLV
on the View toolbar, or click View, Display, Draft Quality HLR/HLV.
Shaded and Dynamic Previews Shaded Previews Shaded previews help you visualize features that you create. For example, when you create an extrude feature, as soon as the Extrude PropertyManager appears, the feature is shown as a shaded preview. You can rotate, pan, zoom, and set standard views while maintaining the shaded preview. NOTE: To improve performance, you can turn shaded previews off in the System Options - Performance dialog box.
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Dynamic Previews When you create or edit a feature that supports dynamic previews, you see a dynamic preview in the graphics area of how the model changes when you move the pointer. At first, a shaded preview appears. Click a handle of the shaded preview, then drag the pointer to see the dynamic preview.
Click the handle, as shown
Drag the pointer to see the dynamic preview
Hidden Lines Removed Displays the model with all edges that are not visible from the current view angle removed. To display the model with hidden lines removed:
Click Hidden Lines Removed
or View, Display, Hidden Lines Removed.
Hidden Lines Visible Displays the model with all edges that are not visible from the current view angle in gray. To display the model with hidden lines visible:
Click Hidden Lines Visible
on the View toolbar, or click View, Display, Hidden Lines Visible.
You can display hidden edges as either solid or dashed lines. To change the display style, click Tools, Options, System Options, Display/Selection.
Applying, Creating, and Editing Materials You can apply a material to a part, and create or edit a material with the Materials Editor PropertyManager. The material and its properties propagate to COSMOSWorks, COSMOSXpress, PhotoWorks release 2, mass properties and material properties. The Material icon appears in the FeatureManager design tree regardless of whether you applied a material to a part.
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To apply a material to a part:
1.
In an open part, click RealView Graphics Graphics.
on the Standard toolbar, or click View, Display, RealView
If you do not have a supported graphics card, RealView Graphics is unavailable. You do not need to use RealView Graphics to apply a material to a part. 2.
Click Edit Material
on the Standard toolbar, or click Edit, Appearance, Material.
3.
Set the properties in the Materials Editor PropertyManager as necessary.
4.
Click OK
.
The material is applied to the part, and the material name appears in the FeatureManager design tree next to the Material icon
.
To create a custom material:
When you create a material, you derive the properties from a SolidWorks default material, then change the properties as necessary to create a different material. 1.
In an open part, click Edit Material
on the Standard toolbar, or click Edit, Appearance, Material.
2.
In the PropertyManager, under Materials: a.
Click an item in Select a Material Database to specify the material library where you want to create a material.
b.
Expand a material classification, then select a material.
c.
Click Create/Edit Material.
3.
Set the properties as necessary on the General Information, Visual Properties, Physical Properties, and Crosshatch tabs.
4.
Click OK.
5.
Click OK
to close the PropertyManager.
To edit a custom material:
You cannot edit SolidWorks default materials. You can, however, edit materials that you created.
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1.
In an open part, click Edit Material
on the Standard toolbar, or click Edit, Appearance, Material.
2.
In the PropertyManager, under Materials: a.
Click a database you created in Select a Material Database to specify the material library that contains the material you want to edit.
b.
Select a material that you created.
c.
Click Create/Edit Material.
3.
Set the properties as necessary on the General Information, Visual Properties, Physical Properties, and Crosshatch tabs.
4.
Click OK.
5.
Click OK
to close the PropertyManager.
To delete a material from a part:
1.
In a part with a material applied to it, click Edit Material Appearance, Material.
on the Standard toolbar, or click Edit,
2.
In the PropertyManager, under Materials, click Remove Material.
3.
Click OK
.
The material is removed from the part and the material name is removed from the Material icon FeatureManager design tree.
in the
Materials - Supported Graphics Cards The following Nvidia® Quadro® graphics cards support RealView Graphics
display:
•
Quadro FX 2000
•
Quadro4 750 XGL
•
Quadro FX 1000
•
Quadro4 700 XGL
•
Quadro4 980 XGL
•
Quadro4 700 Go GL
•
Quadro4 900 XGL
•
Quadro FX Go700 (for Dell™ Precision™ M60 Mobile Workstation only)
•
Quadro4 780 XGL
•
Quadro FX 500
Materials - General Information The General Information tab controls the following properties when you create or edit a material: Database Selection Displays the material libraries: •
Solidworks Materials. A pre-defined library that contains SolidWorks materials. You cannot create or edit materials in this library.
•
. Creates a new material database.You must create a new material database to create or edit a material. If you select , the Save As dialog box appears where you set the location of the new database.
Material Classification Displays the material classes in your custom material databases. Material Name Displays the material names in your custom material databases. Materials - Visual Properties The Visual Properties tab controls the following properties when you create or edit a material: RealView Graphics Lists all of the 3D materials used to display models using RealView Graphics. Although you can select a material from this list, it does not appear if you do not have a supported graphics card. Texture Lists all of the 2D textures available in the Texture PropertyManager.
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PhotoWorks Material Lists all of the materials available in PhotoWorks release 2, if you have the add-in product. When you render a model, this material is propagated to PhotoWorks release 2. Color Lists all of the colors used in the Color And Optics PropertyManager. Materials - Physical Properties The Physical Properties tab controls the following properties when you create or edit a material: Material Properties Displays the physical properties for the material. You can change the Value only. If you enter a unit for Value, the units update according to the units you set in the Document Properties - Units dialog box. Materials - Crosshatch The Crosshatch tab controls the following properties when you create or edit a material: Crosshatch •
None. No crosshatch is associated with the material.
•
Solid. A solid black crosshatch is associated with the material.
•
Hatch. A crosshatch with Scale and Angle is associated with the material. The Pattern list displays available crosshatches.
RealView Graphics When you apply a material to a part, use RealView Graphics to display the model with realistic-looking materials. RealView Graphics is available with supported graphics cards only. To turn on RealView Graphics:
Click RealView Graphics on the View toolbar, or click View, Display, RealView Graphics. You can turn off RealView Graphics when your assembly is in large assembly mode.
Perspective Displays a perspective view of the model. A perspective view is the view normally seen by the eye. Parallel lines recede into the distance to a vanishing point. You can create a Named View in a drawing of a perspective view of a model. To display the model in Perspective view:
Click Perspective
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on the View toolbar, or click View, Display, Perspective.
Modify Perspective Perspective is related to the size of the object being observed and the distance of that object from the observer. You can modify the perspective by specifying the Object Sizes Away value in the Perspective PropertyManager. The smaller the value, the greater the amount of perspective distortion. To change the perspective:
1.
With Perspective
selected, click View, Modify, Perspective.
The Perspective View PropertyManager appears. 2.
Under Observer Position, type a value in the Object Sizes Away
3.
Click OK
box.
.
Creating a Section View A section view displays a view of the model cut through the part or assembly. When you create a section view, then toggle the view off and on, the section view state is retained. Zebra stripes are not available with an active section view.
To create a section view:
1.
In a part or assembly document, click Section View Section View.
on the View toolbar, or click View, Display,
2.
In the PropertyManager, under Section 1, set the properties in the Section View PropertyManager as necessary.
3.
To create additional section views, select Section 2 and Section 3, then repeat step 2. You can use the same planes to create additional section views. Section 3 is unavailable until Section 2 is selected.
4.
Click OK
.
To save a section view:
1.
In the Section View PropertyManager, under Options, click Save View.
2.
In the Named View dialog box, type a name for View name.
3.
Click OK. The Orientation dialog box appears with the new section view.
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Section View PropertyManager Displays a view of the model cut through the part or assembly. When you create a section view, you use planes or faces as references to make the model cut. The Section View PropertyManager controls: Section 1 and Section 2 •
Planes. Selects the Front Plane section view.
•
Reference Section Plane/Face. Displays the plane or face to create the section view. Reverse Section Direction
, Top Plane
, and Right Plane
that you can use to create the
changes the direction of the cut to the opposite side.
•
Offset Distance
.
•
X Rotation
. Rotates the reference section along the X-axis.
•
Y Rotation
. Rotates the reference section along the Y-axis.
•
Edit Color. Changes the color of the section view while the PropertyManager is active. The colors are used only while the PropertyManager is active. The colors are not displayed after the section view is created.
Section 3 This section appears after you select Section 2. Use Section 2 and Section 3 to create additional section views in the model. Options •
Save View. Saves the section view as a named view in the Orientation dialog box. If you insert a saved section view in a drawing, only the view orientation and perspective view data are shown. The actual section view is not visible.
•
Reset. Resets the selections to the default values.
•
Show section cap. Displays the section view with the color specified in the Edit Color box. Clear this option to see inside the model.
Shaded Displays a shaded view of the model. When you select a face on a model that is in shaded view, the entire face is highlighted. To display a model in shaded view:
Click Shaded on the View toolbar, or click View, Display, Shaded. You can control: • • •
The color of shaded parts. The color of individual part faces. The light intensity and direction on the shaded parts.
When in shaded view, the sketch plane is displayed as a translucent plane. This behavior is controlled by the Display plane when shaded option. Click Tools, Options, System Options, Sketch.
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Shaded With Edges Displays a shaded view of the model with edges visible. To display a model in Shaded With Edges view:
Click Shaded With Edges on the View toolbar, or click View, Display, Shaded With Edges. You can also control the color of the shaded edges.
Shadows Displays a shadow under the model. When shadows are displayed, the light appears from the top-most part of the model in the current view. The shadow does not dynamically change positions when you rotate the model. NOTE: When you have shadows enabled, system performance is slower during dynamic view operations (zoom, pan, rotate, and so on). To turn on shadows:
Click Shadows In Shaded Mode
on the View toolbar, or click View, Display, Shadows In Shaded Mode.
NOTE: To change the placement of the shadow, turn Shadows In Shaded Mode off, rotate the model, then turn the shadows on again.
Orientation Rotates and zooms the model or drawing to a preset view. You can select from the standard views (Normal To, Front, Back, Isometric, and so on for a model, Full Sheet for a drawing) or add your own named views to the list. You can return your model or drawing to a previous view by clicking Previous View can undo the last 10 view changes.
, on the View toolbar. You
To select a view:
Click Standard Views
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Viewing Models Normal To To display a model in Normal To view:
1.
2.
In the model, select one of the following: •
Plane or planar face
•
Cylindrical or conical face
•
Any feature created with a single sketch
Click Standard Views
, and select Normal To
If you click Normal To
.
again, the model flips 180°.
To select a view orientation with Normal To:
With this method, the first face you choose is parallel to the screen and the second face you choose is at the top of the view. 1.
Hold down Ctrl and select two planar faces. The second planar face cannot be parallel to the first.
2.
Click Standard Views
, and select Normal To
.
Orientation Dialog Box To display the Orientation dialog box:
Do one of the following: •
Click View Orientation
•
Click View, Modify, Orientation.
on the View toolbar.
•
Press the Space Bar.
•
Right-click in a drawing sheet and select Zoom/Pan/Rotate, View Orientation. To keep the Orientation list open, click
in the dialog box.
To add a new named view to the Orientation dialog box:
1.
Use the Rotate, Zoom, and Pan commands to create the desired view.
2.
With the Orientation dialog box open, click New View
3.
In the Named View dialog box, type a name for View name, and click OK.
.
The name appears at the top of the list of views. You can display the view by double-clicking its name. To delete a named view from the Orientation dialog box:
You can delete a named view from the Orientation dialog box only if you created the named view with the above procedure. In the Orientation dialog box, select the named view you want to delete and press Delete.
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To change the orientation of the standard model views in the Orientation dialog box:
1.
In the Orientation dialog box, double-click one of the named views to select the new orientation. For example, if you want what is currently the Left view to become the front view, double-click Left.
2.
Click (do not double-click) the name of the standard view you want to assign to the current orientation of the model. For example, click Front if you want the current view to become the front.
3.
Click Update Standard Views selected view.
4.
Click Yes to confirm the update.
. This updates all of the standard views so they are relative to the
To return all standard model views to their default settings in the Orientation dialog box:
1.
In the Orientation dialog box, click Reset Standard Views
2.
Click Yes to confirm the update.
.
Add a Named View The Named View dialog box appears when you select New View in the Orientation dialog box. 1.
Use the Rotate, Zoom, and Pan commands to create the desired view.
2.
Enter a descriptive name for the view, and click OK. Display the named view by double-clicking on its name in the Orientation list.
Textures Use the Texture PropertyManager to apply 2D textures to part and assembly documents for a more realistic finish.
To apply a texture to a part or assembly document:
1.
In a part or assembly document, click Edit Texture Appearance, Texture.
on the Standard toolbar, or click Edit,
2.
Set the properties in the Texture PropertyManager as necessary. You cannot apply textures to weld beads or cosmetic threads.
3.
Click OK
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To create custom textures:
1.
Create a folder in your installation directory where you want to store texture files.
2.
Place any files to use as textures in the folder you created in step 1. The images must be in .jpg, .bmp, or .png format.
3.
In the SolidWorks software, click Tools, Options, System Options, File Locations.
4.
Select Textures in Show folders for, then click Add.
5.
In the Browse For Folder dialog box, browse to the folder you created in step 1.
6.
Click OK. The next time you apply a texture, the folder path appears in the Texture PropertyManager in the Texture File Locations list, and you can select your custom textures. When you create a custom texture, you can also apply the texture to a material when you create or edit a material.
Wireframe Displays all the edges of the model. To display the model in wireframe:
Click Wireframe
on the View toolbar, or click View, Display, Wireframe.
Manipulating Models Middle Mouse Button Functions Three-button Mouse If you use a three-button mouse, you can dynamically use the following view commands: •
Pan all document types - Hold down Ctrl and drag with the middle mouse button. (In an active drawing, you do not need to hold down Ctrl.)
•
Rotate part or assembly - Drag with the middle mouse button.
•
Zoom all document types - Hold down Shift and drag with the middle mouse button.
•
The middle mouse button acts the same as the left mouse button if one of the dynamic view commands (Zoom In/Out
, Pan
, or Rotate View
on the View toolbar) is active.
If you open the part or assembly in View-Only mode or in the or in SolidWorks Viewer, you can only rotate the part or assembly with the middle mouse button if it was saved with Fast HLR/HLV , Shaded With Edges , or Shaded
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mode.
Wheel-type Mouse If you use a wheel-type mouse, you can zoom in to the position of the pointer instead of the center of the graphics area by spinning the wheel backwards. This is the default behavior. If the pointer is outside of the graphics area, the center of the model zooms into view. While rolling the mouse wheel, you must keep the pointer on the area where you want to zoom. To turn this function off, click View, Modify, Zoom About Screen Center. Zoom the view in or out by spinning the wheel forward or back. The model zooms to the center of the screen. This can also be combined with the middle mouse button rotate command by holding down the wheel while you spin it. To use the wheel to pan the view, hold down Shift while you spin the wheel. If you select an entity by pressing down and releasing the mouse wheel, you can then rotate the model around the selected entity by holding down the mouse wheel while moving the mouse. Often the settings for the wheel override the SolidWorks software settings. To change this, SolidWorks recommends that you turn off the wheel when using the SolidWorks software. This is done in the Windows Control Panel for the mouse. If this fails, check with the manufacturer for a new driver or for issues concerning the current mouse drivers.
Pan Scrolls the part, assembly, or drawing in the document window. To pan with the mouse:
1.
Click Pan
or View, Modify, Pan.
The pointer changes to 2.
.
Hold the mouse button down and drag in the direction you want to scroll.
To pan with the arrow keys:
Hold down the Ctrl key and use the Arrow keys. To pan with the middle mouse button:
Hold down the Ctrl key and the middle mouse button, then drag in the direction you want to pan.
Rotate View Rotates the model view. When you rotate a part or assembly with high-quality transparency, the application dynamically switches to a lowquality transparency, enabling you to rotate the model faster. Once you complete the rotation, the model switches back to high-quality transparency. This is especially important if your part or assembly is complex. Optionally, you can choose to retain high-quality transparency while rotating or moving the model with the rotate or pan tools. Depending on your graphics card, this option may result in slower performance. TIP: To set the type of transparency, click Tools, Options, and on the System Options tab, select Performance. Select the appropriate transparency options.
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To rotate the model view:
1.
Click Rotate View
or View, Modify, Rotate.
2.
Press the mouse button and drag to rotate the view. NOTE: Click View, Modify, Rotate About Screen Center to rotate the view around the center of the screen or the origin of the model. TIP: Use the arrow keys to rotate the view vertically or horizontally. (Hold down Shift to rotate in 90-degree increments). Hold down Alt and use the left-right arrow keys to rotate clockwise or counterclockwise.
To rotate the view about a selected vertex, edge, or face:
1.
Click Rotate View
or View, Modify, Rotate.
2.
Click the vertex, edge, or face to rotate about.
3.
Press the mouse button and drag to rotate the view.
NOTE: To change the speed of the view rotation, click Tools, Options, and on the System Options tab select View Rotation. Use the Mouse speed slider to change the speed of rotation; in the Arrow keys box, you can change the angle increment used when rotating with the arrow keys.
Previous View After moving your model to one or more views, you can return your model or drawing to a previous view. You can undo the last 10 view changes. To see previous views:
Click Previous View
on the View toolbar.
Zoom to Fit Zooms in or out so you can see the entire model, assembly, or drawing sheet. To see the entire model:
Click Zoom to Fit
on the View toolbar, or click View, Modify, Zoom to Fit.
Zoom to Area Zooms in to an area that you select by dragging a bounding box. To zoom in to a selected area:
1.
Click Zoom to Area
2.
Point at one corner of the area you want to enlarge. The pointer changes to
on the View toolbar, or click View, Modify, Zoom to Area.
.
3.
Press the mouse button and drag the bounding box diagonally to enclose the area.
4.
Release the mouse button. The view is zoomed in to the selected area.
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Zoom In/Out Zooms in and out. To zoom in or out:
1.
Click Zoom In/Out
on the View toolbar, or click View, Modify, Zoom In/Out.
2.
Press the mouse button and drag up (toward the top of the screen) to zoom in, or drag down to zoom out.
TIP: Press z to zoom out or Shift+Z to zoom in. NOTE: If you have a wheel-type mouse, you can zoom in to the position of the pointer instead of the center of the graphics area by spinning the wheel backwards. This is the default. If the pointer is outside of the graphics area, the center of the model zooms in to view. You do not need Zoom In/Out enabled when you use the wheel to zoom. To turn this function off, click View, Modify, Zoom About Screen Center. The model zooms to the center of the screen. While rolling the mouse wheel, you must keep the pointer on the area where you want to zoom.
Zoom to Selection Zooms in on a portion of the model, assembly, or drawing that you select. To zoom to selection:
1.
Click an entity to which you want to zoom, or hold Ctrl and click several entities.
2.
Click Zoom to Selection
on the View toolbar, or click View, Modify, Zoom to Selection.
The view is zoomed in to the selected entity.
Customizing SolidWorks Overview of SolidWorks Options Customize functionality to suit your needs. Click Tools, Options to display system options and document property settings. Options Dialog Box Structure The SolidWorks Options dialog box structure emphasizes the difference between system options and document properties. The Options dialog box has two tabs: •
System Options. The system options are stored in the registry and are not part of the documents. Therefore, these changes affect all documents, current and future.
•
Document Properties. The document properties apply only to the current document, and the Document Properties tab is available only when a document is open. New documents get their document settings (such as Units, Image Quality, and so on) from the document properties of the template used to create the document. Use the Document Properties tab when you set up document templates.
The options listed on each tab are displayed in tree format on the left side of the dialog box. As you click an item in the tree, the options for the item appear on the right side of the dialog box. The title bar displays the title of the tab and the title of the options page.
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To access the Options dialog box:
You can access the Options dialog box in any of the following ways: •
Click Tools, Options. The Options dialog box appears with the System Options tab active.
•
Right-click in the FeatureManager design tree area and select Document Properties. (There must be no items selected in the FeatureManager design tree or graphics area in order to select Document Properties.) The Options dialog box appears with the Document Properties tab active.
•
Click Grid/Snap on the Sketch toolbar. The Options dialog box appears with the Grid/Snap page of the Document Properties tab active.
Document Templates Templates are documents (part, drawing, and assembly documents) that include user-defined parameters. When you open a new part, drawing, or assembly, you select a template to use for your new document. Templates allow you to maintain as many different documents for parts, drawings, or assemblies as you need. A template can be a part, drawing, or assembly document that you saved as a template. For example, you can create: •
A document template using millimeters and another template using inches
•
A document template using ANSI and another template using ISO dimensioning standard
You can organize your document templates by placing them on different tabs in the New SolidWorks Document dialog box. TIP: If you use small units of measure such as angstroms, nanometers, microns, mils, or microinches, you might want to create specific templates as the basis for documents that use the units. The templates could include settings for such Document Properties as: •
grid spacing
•
extension line and break line gap
•
dimension offset distance and break dimension gap
•
note bent leader length
•
balloon bent leader length
•
arrow size and section view arrow size
•
text scale and text display size
•
material density
To create a template:
1.
Click New
on the Standard toolbar, or click File, New.
The New SolidWorks Document dialog box appears with an available set of templates. 2.
Double-click the appropriate icon for the type of template that you want to create: Part, Assembly, or Drawing.
3.
Click Tools, Options. On the Document Properties tab, select options to customize your new document template, then click OK. NOTE: Only options on the Document Properties tab are saved in a document template.
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4.
Click File, Save As.
5.
In the Save as type list, select a template type: •
Part Templates (*.prtdot)
•
Assembly Templates (*.asmdot)
•
Drawing Templates (*.drwdot)
6.
Type a name in the File name box. The extension is added automatically.
7.
Browse to the folder where you want to save your template, then click Save.
Customize Commands Adds, removes, and rearranges command buttons to customize your toolbars. You can: •
add command buttons and place them on more than one toolbar
•
remove command buttons that you never use
•
rearrange command buttons on toolbars, or move command buttons from one toolbar to another
To customize command buttons on your toolbars:
1.
With a document open, click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
2.
On the Commands tab, under Categories, select the toolbar that you want to change.
3.
Under Buttons, point at the toolbar button to see the tooltip that describes the button. If you click the button, a definition appears under Description.
4.
Do any of the following to customize the command buttons: To... Add a command button or place it on more than one toolbar Remove a command button from a toolbar Rearrange a command button on a toolbar Move a command button from one toolbar to another
5.
Then... In the Customize dialog box, click and drag a button to any toolbar. In the SolidWorks window, click and drag the button from the toolbar to the graphics area. In the SolidWorks window, click and drag the button from the toolbar to another area of the toolbar. In the SolidWorks window, click and drag a button from one toolbar to a different toolbar.
Click OK.
Customize Headers and Footers You can specify headers and footers for the active document before printing. To create a header or footer:
1.
Click File, Print. The Print dialog box appears.
2.
Under Document Options, click Header/Footer. The Header/Footer dialog box appears.
3.
Select a predefined header or footer from the Header and Footer lists. - or Click Custom Header or Custom Footer to create a unique header or footer and do the following: a.
Select an area of the document where you want the header or footer to appear: Left section, Center section, or Right section.
b.
Select the items you want to appear on the page (Page Numbers Date
c.
, Time
, or Filename
, Number of Pages
,
).
Click OK.
The Header preview and Footer preview boxes update according to the items you selected. 4.
Click OK to close the Header/Footer dialog box.
5.
Click OK to close the Print dialog box and print the document.
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Customize Keyboard Customizes your keyboard to suit your style of working with SolidWorks. To customize your keyboard:
1.
With a document open, click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
2.
Click the Keyboard tab.
3.
Click the appropriate buttons to Assign a new shortcut key, Remove a shortcut key, or Reset All shortcut keys to their original state. Customization options:
4.
•
Categories. Select the menu that contains the command you want.
•
Commands. Select the command for which you want to assign or remove a shortcut key.
•
Press new shortcut key. Type a single key or a combination of keys.
•
Current keys. Displays the current shortcut key for the selected command.
•
Description. Displays the description for the selected command.
Click OK.
Customize Macro Button When you create a macro, you can assign a bitmap to the macro button on the toolbar. The SolidWorks software includes sample bitmaps, or you can create your own bitmap. You can also specify which method (a procedure that operates on an object) within a macro you want to run. For more information, see the SolidWorks API Help Topics. If you create a bitmap for a macro button, the bitmap must meet these requirements: •
Dimension = 16 x 16 pixels
•
Color = 16 colors
•
Background color = white
To run a specific macro method and create a custom macro button:
1.
With a document open, click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
2.
In the dialog box, on the Commands tab:
3.
a.
Select Macro in Categories.
b.
Under Buttons, drag the Macro
button to any toolbar in the SolidWorks window.
In the Customize Macro Button dialog box: a.
Under Appearance: i.
Click Choose Image.
ii.
In the Icon path dialog box, select a bitmap image (*.bmp), then click Open. The SolidWorks software provides bitmap images to use as custom buttons. These are located in/data/user macro icons. Select Preview to see the image in the Icon path dialog box.
iii. If necessary, type a Tooltip and Prompt message, which provides a brief description of the function of the tool on the status bar.
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b.
Under Action: i.
Click
and open the macro you want to use.
ii.
If necessary, select a Method. When you select a method, only that method runs in the macro. The method is in the form: <module_name>.<method_name>.
iii. Click OK.
4.
c.
Type a key in Shortcut to assign a shortcut key to the macro.
d.
Click OK.
Click OK again to close the Customize dialog box.
To edit a customized macro button:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when creating custom macro buttons.
2.
Right-click the customized macro button in the toolbar that you want to edit.
3.
In the Customize Macro Button dialog box, edit the macro as necessary, then click OK.
4.
Click OK again to close the Customize dialog box.
Customize Menus Customizes a SolidWorks menu to suit your style of working. To add or delete an item in a SolidWorks menu:
1.
Click the menu you want to add or delete a menu item and select Customize Menu. Each item currently visible in the menu is preceded by
.
This menu is for customization purposes only. You cannot run a command from this menu. 2.
To add menu items, select the empty check boxes
. To delete menu items, clear the selected check boxes
. 3.
Click anywhere outside of the menu to save your changes, or press Enter. To cancel your changes, press Esc.
To set SolidWorks menus or shortcut menus to default values or to show all menu items:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
2.
3.
On the Options tab, under Shortcut customization or Menu customization, click: •
Show All. Displays all menu items.
•
Reset to Defaults. Resets all menu items to the default display.
Click OK.
To customize a SolidWorks menu:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
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2.
On the Menus tab, click the appropriate buttons to Rename a menu item, Remove or Add a menu item, or Reset All menus to their original state. Customization options: Categories. Select the menu to change. Commands. Select the command to add, rename, relocate, or remove. Change what menu. Displays the code name of the selected menu. Position on menu. Lets you select a menu position, including Auto, At Top, or At Bottom. Name of command. Displays the code name of the selected command. Description. Displays the description of the selected command.
3.
Click OK.
Customize Options If you customized SolidWorks menus or shortcut menus, you can set them back to default values or show all menu items. To set SolidWorks menus or shortcut menus to default values or to show all menu items:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
2.
3.
On the Options tab, under Shortcut customization or Menu customization, click: •
Show All. Displays all menu items.
•
Reset to Defaults. Resets all menu items to the default display.
Click OK.
Customize Toolbars Customizes, displays, or hides toolbars. You can position toolbars and set their visibility based on the document type (part, assembly, or drawing). You can also set which toolbars are visible for when there are no documents open. The SolidWorks software remembers which toolbars to display and where to display them for each document type. For example, with a part document open, you can choose to display only the Standard and Features toolbars. Whenever you create or open any part document, only these toolbars are displayed. Meanwhile, for an assembly document, you can choose to display only the Assembly and Selection Filter toolbars. Whenever you create or open an assembly document, only these toolbars are displayed. To customize which toolbars appear for part, assembly, or drawing documents:
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1.
Open a part, assembly, or drawing document.
2.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
3.
On the Toolbars tab, select the toolbars you want to display and clear the toolbars you want to hide. Your selections apply to the type of SolidWorks document that is currently open.
4.
Select from the following options: •
Large icons. Displays large toolbar buttons.
•
Show tooltips. Displays a note to identify each toolbar button when you pause the pointer over a button.
•
Use large tooltips. Displays expanded tooltips that show both the name of a toolbar button and a brief description of its functionality. This is available only when Show tooltips is selected.
5.
Click: •
OK to accept the changes.
•
Reset to undo the changes and return to previous settings
•
Cancel to discard the changes and close the dialog box.
You can move toolbars as desired. Toolbars can be either docked in one of the toolbar areas or floating. To move a toolbar:
Click the start or edge of the toolbar and drag. If you drag a toolbar to an edge of the SolidWorks window, the toolbar docks to the edge automatically. - or If you drag a toolbar away from the window edge, it becomes a floating palette.
Skins You can apply skins as background images to the PropertyManager. Skins are images that appear behind the PropertyManager data, similar to this wood sample skin. You can also create your own PropertyManager buttons. Only bitmap (.bmp) files are supported as skins. SolidWorks offers sample skins for your use. The sample skins are located in\data\skins. You can also create customized skins with editing software, then add your customized skins to the skins folder. To enable and view skins:
1.
Click Tools, Options, System Options, Colors.
2.
Under System colors, select an item in PropertyManager Skin. To disable skins, select None.
3.
Click OK. When you activate the PropertyManager, the skin appears.
To create a customized skin bitmap file:
1.
Open your graphics editing software and create a bitmap file. You can use any color (including true colors), resolution, or size setting.
2.
Save the skin as\data\skins\<skin_bitmap_file_name>.bmp. For example, background.bmp. The image is tiled, so it is best to use tilable images when applying textures as the background.
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To customize the PropertyManager buttons:
After you create your background skin bitmap file, you can customize any of the OK, Cancel, Help, Keep Visible, Back, Next, Preview, and Undo buttons. You are encouraged to customize all buttons so they match. If you do not customize a button with a skin, the default SolidWorks button is applied. The button colors are blended to the background color. If you have dark background colors, the default buttons may be difficult to read. 1.
Create the skin bitmap file as described in the procedure above.
2.
Create the button skin bitmap file with your graphics editing software, using the following guidelines: •
File Name. The button skin bitmap file name must be <skin_bitmap_file_name>__.bmp, for example, background__ok.bmp. The “__” is a double underscore. Also, the button name must be ok, cancel, help, pin, back, next, preview, or undo. The pin button name refers to the Keep Visible button.
3.
•
Display States. You must display the button in four states: off, on, mouse over, and unavailable. Here is an example using the Cancel button:
•
Pixel Size. Each individual button state must be 32 by 32 pixels. Therefore, each group of four buttons must be 32 pixels high and 128 pixels wide. Here is an example of the pixel size using the Cancel button.
•
Colors. The buttons can have a color palette of 2, 8, 16, or 256 colors. True colors are not supported.
•
Transparency. To set any part of the button skin bitmap file to transparent, set the RGB color for that area to 255, 0, 255. Transparent areas display the color and design used in the background skin bitmap file. Here is an example using the OK button:
Add the button skin bitmap files to\data\skins\. The button skin bitmap files automatically integrate into the background skin when you enable the skin.
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SolidWorks Tools Add-Ins Lets you integrate other compatible software applications with your installed SolidWorks software. The add-in software applications must be installed on your computer. To use another software application along with SolidWorks:
1.
Click Tools, Add-Ins. The list of installed, compatible software appears in the dialog box.
2. 3.
Select one or more applications that you want to use. Click OK. Some add-in applications provide a tab at the top of the FeatureManager design tree panel. The tab contains information related to the specific add-in.
These tabs include the SolidWorks Animator tab at the far right.
You can also add an add-in application's toolbar to the SolidWorks window.
Conversion Wizard When you open a SolidWorks document from an earlier version, it may take more time than you are used to experiencing. After the document has been opened and saved, subsequent opening time returns to normal. The SolidWorks Conversion Wizard automatically converts all of your SolidWorks documents from an earlier version to the current SolidWorks format. Depending on how many files you have, the conversion process may take a while, but once it is done, the documents open more rapidly. Once a document is converted, you can no longer open the file in the older SolidWorks version. To access the Conversion Wizard, click the Microsoft Start button, then click Programs, SolidWorks 2004, SolidWorks Tools, Conversion Wizard. The Conversion Wizard has the following options: •
Create a backup for files to convert. Backs up all of your files before the conversion. If you choose to back up your SolidWorks files, the Conversion Wizard copies the files to a sub-folder named Solidworks Conversion Backup. The wizard asks you for the location of the files to be converted, and leads you through the process.
•
Include subfolders. Converts all SolidWorks documents in the main folder and its subfolders.
•
Visibility: o
o
Run SolidWorks in background. The SolidWorks software runs while the files are being converted, but it is invisible to the user. Show SolidWorks window. The SolidWorks software runs while the files are being converted, and is visible to the user.
•
Save pre-2003 drawings with "Automatic update of BOM". Sets the option, Automatic update of BOM, which automatically updates a drawing's Bill of Materials when changes are made to the model for all drawings created prior to SolidWorks 2003.
•
Convert drawings to Detached Drawings format automatically. Converts all converted drawing documents to Detached format.
•
Ignore files with missing references. Documents dependent on missing reference files are not converted.
•
Backup Folder: o
Path. Displays the location where the backup files are saved. Click Browse to change the location.
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At the end of the conversion process, two report files exist in the folder to which you directed the conversion: •
Conversion Wizard Log.txt. Contains a list of files that converted.
•
Conversion Wizard Failed.txt. Contains a list of files that did not convert.
Copy Options Wizard When you select options for the SolidWorks application, those options settings are saved in a registry file. To maintain uniformity among the SolidWorks users at your location, you or your network administrator can use the Copy Options Wizard to apply the same options to other SolidWorks installations on your network. To use the Copy Options Wizard:
1.
Click the Microsoft Windows Start button, then click Programs, SolidWorks 2004, SolidWorks Tools, Copy Option Wizard.
2.
In the dialog box: •
To capture your SolidWorks options information from the registry file, select An existing user and select your name. - or -
•
To capture SolidWorks options from a registry file you created, select A previously created registry file, then click Browse to locate the file.
3.
Click Next.
4.
Under SolidWorks option settings destination, select: •
Users and computers on the network. Copy the SolidWorks options directly to Both users and computers, Only users, or Only computers on the network. Depending on the option you choose, the next dialog box allows you to select the users or computers to which the settings will apply. - or -
•
Create a registry file. The SolidWorks registry options of the current system are copied to a swOptions.reg file that you can use with SolidWorks supported operating systems. Copy this swOptions.reg file to another computer and double-click the file. The registry options are automatically copied to the registry of the new computer.
5.
Click Next.
6.
Click Finish.
Manufacturing Network The Manufacturing Network is an online directory of SolidWorks-enabled service vendors. This directory lists contract design and manufacturing companies who can help reduce your product's time to market. Each company in the directory is a SolidWorks user; there is no need to translate SolidWorks documents to an intermediate file format. The Manufacturing Network is free of charge. NOTE: You need an Internet connection to access the Manufacturing Network. To access the Manufacturing Network:
Click Tools, Manufacturing Network. - or In your Internet browser, go to http://www.solidworks.com/swmn.
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Moving from AutoCAD Moving from AutoCAD supports users in the transition from 2D AutoCAD to 3D SolidWorks. It compares terms and concepts, explains SolidWorks approaches to design, and provides links into SolidWorks Help, tutorials, and other resources. To access Moving from AutoCAD:
Click Help, Moving from AutoCAD.
Quick Tips Quick Tips are a set of pop-up messages that appear while you create SolidWorks documents. These messages give hints and options based on the current SolidWorks mode. Most of the messages have hyperlinks; click the hyperlink to see the associated item in the SolidWorks window. Quick Tips are not available when the Online Tutorial is active. There are four icons associated with the Quick Tips status. These appear in the lower-right corner of the SolidWorks window: Icon
Status Available, but not currently displayed Currently displayed Not available Temporarily disabled
To turn on Quick Tips:
Click Help, Quick Tips or click
.
To turn off Quick Tips:
Click Help, Quick Tips, or click
.
Quick Tips are mode-specific. For example, if you have Quick Tips displayed when you have a part document open, then you click , Quick Tips are no longer displayed in part modes. However, if you open an assembly document, Quick Tips reappear.
SolidWorks API The SolidWorks Application Programming Interface (API) is a COM programming interface to the SolidWorks software. The API contains hundreds of functions that you can call from Visual Basic (VB), Visual Basic for Applications (VBA), VB.NET, C++, C#, or SolidWorks macro files. These functions provide the programmer with direct access to SolidWorks functionality. To access the API help, click Help, SolidWorks API and Add-Ins Help Topics. There are tips, code fragments, and examples of API functions on the SolidWorks Web page: www.solidworks.com/api.
SolidWorks Service Packs If you are a SolidWorks subscription customer, you can take advantage of SolidWorks service packs that are regularly posted on the SolidWorks Web site. These service packs contain software updates and enhancements to the SolidWorks software. To check for a new service pack, click Help, Service Packs, and click the Check button. Select the Check for a new service pack once a week check box if you want the software to automatically check the SolidWorks Web site once a week.
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SolidWorks Web Site If your computer is connected to the Internet, you can visit the SolidWorks Web site to learn more about SolidWorks Corporation and its products. To access the SolidWorks Web site:
1.
Click Help, About SolidWorks.
2.
In the dialog box, click Connect.
Recording and Playing Macros New Macro You can create a new macro from the Macro toolbar or from a menu item. Creating a new macro is different from recording a macro. When you create a new macro, you program the macro directly from your macro editing application. When you record a macro, you create the macro from within the SolidWorks software. To create a new macro:
1.
Click New Macro
on the Macro toolbar, or click Tools, Macro, New.
The New Macro dialog box appears. 2.
Type a File name.
3.
Click Save. Your macro editing application opens where you can create a new macro.
Record/Pause Macro You can record operations performed with the SolidWorks user interface and replay them with SolidWorks macros. A macro contains the equivalent calls to the API functions that were made when the operations were performed with the user interface. A macro can record your mouse clicks, menu choices, and keystrokes to play back later. You can create a new macro without recording one first. To record a macro:
1.
Click Record\Pause Macro
on the Macro toolbar, or click Tools, Macro, Record.
2.
Perform the steps you want to record.
3.
When you are done, click Stop Macro
4.
In the dialog box, type a name for File name and click Save. (The .swp extension is automatically added to the filename.)
on the Macro toolbar, or click Tools, Macro, Stop.
To pause while recording a macro:
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Click Record\Pause Macro
or Tools, Macro, Pause.
Click Record\Pause Macro
again to continue recording.
Edit Macro Edits or debugs a macro that you recorded previously. To edit a macro:
1.
Click Edit Macro
on the Macro toolbar, or click Tools, Macro, Edit.
If you have previously edited macros, you can select the macro directly from the menu when you click Tools, Macro. This menu lists the last nine edited macros. 2.
In the dialog box, select a macro file (.swp) and click Open. You can also edit .swb files. When you run or edit an .swb file, it is automatically converted to a .swp file.
3.
Edit the macro. (For details, use the help in the macro editor.)
Run Macro Opens a dialog box that lets you select the macro you want to run. To run a macro:
1.
Click Run Macro
on the Macro toolbar, or click Tools, Macro, Run.
The Run Macro dialog box appears. 2.
Locate the macro (.swp) file you want to run and click Open. NOTE: You can also open .swb files.
Stop Macro Stops recording the macro and opens a dialog box so you can save the macro. To stop recording a macro:
1.
While you are recording a macro, click Stop Macro
or Tools, Macro, Stop.
The Save As dialog box appears. 2.
Type a name for the macro and click Save to save it. (The .swp extension is automatically added to the filename.) - or Press Cancel to cancel the macro.
Assign a Macro to a Shortcut Key or Menu You can assign your own macros to shortcut keys or create new menu items for them. When you assign a macro to a shortcut key or to a menu, you can specify which method (a procedure that operates on an object) within the macro you want to run. NOTE: Before you assign a macro to a shortcut key or to a menu item, you must create a macro folder and record a macro in your SolidWorks installation directory.
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To create a macro folder and record a macro:
1.
Create a folder named \Macros in your SolidWorks installation directory (in the same folder as SOLIDWORKS.exe). This \Macros folder is where you must keep the all the macros that you access from a key or a menu.
2.
Record a macro and make sure it has a .swp extension.
3.
Save the macro in the \Macros folder.
To assign a macro to a shortcut key:
1.
With a document open, click Tools, Customize, Keyboard.
2.
Select Macros in Categories. If Macros is not listed, you must create a macro folder and record a macro in your SolidWorks installation directory, as described in the first procedure.
3.
Select the name of the macro in Commands. The macro is in the form: <macro_name>:<module_name>.<method_name>. The macro description appears in Description.
4.
Type a value for Press new shortcut key to assign a shortcut key to the macro, and click Assign. The shortcut key name appears in Current keys.
5.
Click OK.
To assign a macro to a new menu item:
1.
With a document open, click Tools, Customize, Menus.
2.
Select Macros in Categories. If Macros is not listed, you must create a macro folder and record a macro in your SolidWorks installation directory, as described in the first procedure.
3.
Select the name of the macro in Commands. The macro is in the form: <macro_name>:<module_name>.<method_name>. The macro description appears in Description.
4.
Select the menu and sub-menu, if necessary, where you want to add the new menu item for your macro in Change what menu.
5.
Select a position for the new menu item in Position on menu.
6.
Type a command name for Name of command.
7.
Click Add, then click OK.
VBA Visual Basic for Applications (VBA) is the engine that records, runs, or edits macros in SolidWorks. Recorded macros are saved as .swp VBA project files. You can read and edit .swb and .swp (VBA) files with the VBA editor. When you edit an existing .swb file, the file automatically converts into a .swp file. You can export a module to a file that you can use in other VB projects. You can use VBA to create forms and to provide more user interaction with your recorded macros. For more information on VBA, look to the Help menu in the VBA editor.
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Object Linking and Embedding - OLE Object Linking vs. Embedding When using OLE, you can link or embed files. •
Linking files. When you link a file: o
The file remains in its original location.
o
Anything you change in the original file affects all the files to which it is linked.
o
If you double-click a SolidWorks image in a Microsoft Word document, the SolidWorks software launches for you to edit the original file (if you have SolidWorks installed on your PC).
For example, if you edit a SolidWorks assembly document that is linked to several Word documents, the changes you make are reflected in both the original SolidWorks file and all of the Word documents. •
Embedding files. When you embed one file in another: o
The original file becomes part of the file in which you embedded it.
o
Any changes you make to the embedded SolidWorks document affect only that document.
o
o
Any changes you make to the original SolidWorks file do not affect the document embedded in the Word file. If you double-click a SolidWorks image in a Word document, the SolidWorks software launches for you to edit the file (if you have SolidWorks installed on your PC).
Embedding is useful if you want discrete control over the data.
Object You can embed an OLE object from another program into the active SolidWorks document. You can either open another program from within SolidWorks and create a new object, or you can insert an existing file. To create a new OLE Object:
1.
Click Insert, Object. The Insert Object dialog box appears.
2.
Click Create New.
3.
In the Object Type box, click the type of document you want to create (for example, Microsoft Excel Worksheet.) Only documents from OLE-compliant applications that are installed on your computer appear in the list.
4.
Select the Display As Icon check box if you want the new object to appear as an icon in your document.
5.
Click OK. A new document appears inside your active document. The toolbars and menus for this new document appear in place of the SolidWorks toolbars and menus. If you chose Display As Icon, an icon appears in your SolidWorks document, and the parent application opens in another window.
6.
Edit the object as though you were working in the parent application.
7.
When you finish editing, click in the SolidWorks document window anywhere outside the embedded object. The SolidWorks toolbars and menus become available again. If you chose Display As Icon, click File, Exit or File, Close & Return to <part name> in the parent application.
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To insert an existing file as an OLE object:
1.
Click Insert, Object. The Insert Object dialog box appears.
2.
Click Create from File.
3.
Click Browse, locate the file you want to insert, and click Open.
4.
Select from the following check boxes: •
Link. Displays a picture of the file contents in the SolidWorks document. The picture is linked to the original document, and changes made to the original document are reflected in the SolidWorks document.
•
Display As Icon. Displays the new object as an icon in the SolidWorks document.
NOTE: If you select both of these check boxes, the new object is displayed as an icon, and the SolidWorks software creates a shortcut to the original document. If you select neither of these check boxes, the new object is displayed in the SolidWorks document, but it is not linked. 5.
Click OK to insert the file. NOTE: To change the display of the OLE object, click Edit, Object, Display Content, Display as Icon, or Reset Size.
To edit an OLE object with its application:
1.
Right-click the OLE object and select Edit with. The OLE object opens in its parent application, such as Visio, Microsoft Word, or Microsoft Excel.
2.
Edit the OLE object as desired, then close it and return to the SolidWorks document. The OLE object displays your edits.
To delete an OLE object:
Select the object and click Delete
, click Edit, Delete, or press the Delete key.
TIP: You can undo the deletion of any OLE object that is inserted into a SolidWorks drawing, assembly, or part document. Click Undo
or Edit, Undo Delete.
Display Content Displays the contents of an OLE object embedded in your SolidWorks document. To display the contents an OLE object:
1.
Select the OLE object.
2.
Click Edit, Object, Display Content. If the Object menu item is not displayed in the Edit menu, you may need to add it to the menu.
Display as Icon Displays an embedded OLE object as an icon. To display an OLE object as an icon:
1.
Select the OLE object.
2.
Click Edit, Object, Display as Icon. If the Object menu item is not displayed in the Edit menu, you may need to add it to the menu.
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Reset Size Restores an embedded OLE object to its original height and width. To reset an OLE object to its original size:
1.
Select the OLE object.
2.
Click Edit, Object, Reset Size. - or Right-click the OLE object and select Reset Size.
Inserting SolidWorks Data in Other Applications Using OLE, you can link or embed the SolidWorks document with any other OLE-compliant application. For example, you can place a part in a product data sheet you created with Microsoft Word. To use a SolidWorks document in another application:
1.
In the desired application, click Insert, Object. A dialog box appears that allows you to insert an existing object or to dynamically create and insert a new object. The dialog box that appears depends on the application you are using.
2.
Select the desired options, including whether you want to link the SolidWorks document to this document and whether you want the SolidWorks document to appear as an icon in this document. The SolidWorks document or its icon appears.
OLE Object Property Lets you specify the size and scale of the OLE object inserted in a SolidWorks document. To set the size or scale of an OLE object:
1.
Right-click the OLE object in the document and select Properties. The OLE Object Property dialog box appears.
2.
Type a decimal value for the Width, Height, or Scale into the corresponding boxes.
3.
Click OK.
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3 Sketching
Sketching in SolidWorks Most SolidWorks features begin with a 2D sketch. For information about using sketches to create solid model geometry, see Features Overview. You can also create 3D sketches with SolidWorks. In a 3D sketch, the entities exist in 3D space; they are not related to specific sketch planes. The sketch topics include: •
Starting a new 2D sketch
•
Accessing and using the sketching tools
•
Taking advantage of inferencing
•
Deriving a new sketch from another
•
Dimensioning the sketch and adding and deleting geometric relations
•
Fully defining sketches
•
Sketching on the face of a part
•
Selecting a starting plane for a sketch
•
Deciding how complex the sketch should be
•
Creating a 3D sketch
You can toggle the display of sketches. The sketch entities in the graphics area are hidden or shown when you click View, Sketches. (All sketches must be closed.)
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Sketch Create a 2D sketch to build a 3D model. To create a 2D sketch in a new part:
1.
In a new part document, click a sketch tool on the Sketch toolbar, such as Rectangle
.
- or Click Sketch 2.
on the Sketch toolbar, or click Insert, Sketch.
Click a plane on which to create the sketch: Front Plane, Top Plane, or Right Plane. When you move the pointer to the edge of a plane, the edges are highlighted in red, and you can select the plane. You can also select a plane from the flyout FeatureManager design tree. The message Editing Sketch appears in the status bar at the bottom of the SolidWorks window. If you turned on the sketch grid, the grid appears in the graphics area.
3.
If you clicked Sketch
in step 1, click a tool on the Sketch toolbar to create the sketch.
4.
Create the sketch, and dimension the sketch entities.
5.
Click Exit Sketch
on the Sketch toolbar, click Insert, Exit Sketch, or click a sketch-based feature on
the Features toolbar (Extruded Boss/Base
, for example) to create a feature from the sketch.
To edit an existing sketch:
•
Click Sketch
on the Sketch toolbar, or click Insert, Sketch. Select an existing sketch to edit.
- or •
Right-click a sketch in the FeatureManager design tree, or right-click a sketch entity in the graphics area, and select Edit Sketch.
To create a new 2D sketch in a part with existing sketches:
1.
Click a sketch tool on the Sketch toolbar, such as Rectangle - or Click Sketch
on the Sketch toolbar, or click Insert, Sketch.
2.
Click a plane, face, or edge to add a new sketch.
3.
If you clicked Sketch
4.
Create the sketch, and dimension the sketch entities.
5.
Click Exit Sketch
in step 1, click a tool on the Sketch toolbar to create the sketch.
on the Sketch toolbar, click Insert, Exit Sketch, or click a sketch-based feature on
the Features toolbar (Extruded Boss/Base
3-2
.
, for example) to create a feature from the sketch.
Sketch on the Face of a Part To create new features on a part, you sketch on the face of the part where you want to locate the feature. To sketch on model faces:
1.
Select the planar model face on which you want to sketch.
2.
Click a sketch tool on the Sketch toolbar, click Sketch
, or click Insert, Sketch.
The following happens: •
•
A grid appears on the face that you selected (if you selected Display grid in Tools, Options, Document Properties, Grid/Snap). The message Editing Sketch appears in the status bar at the bottom of the SolidWorks window.
To sketch on a different face, exit the current sketch, select the new face, and open a new sketch.
Starting a New 2D Sketch When you open a new part document, first you create a sketch. You can start by selecting: •
A sketch entity tool (line, circle, and so on) or the Sketch tool
•
A plane
To start a sketch with a sketch entity tool or with the Sketch tool:
1.
Click a sketch entity tool (line, circle, and so on) on the Sketch toolbar. - or Click Sketch
on the Sketch toolbar, or click Insert, Sketch.
You are prompted to select a plane, and the three planes (Front Plane, Top Plane, and Right Plane) are displayed.
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Chapter 3 Sketching
2.
Select a plane. The plane rotates to the Normal to orientation.
3.
Create a sketch with the sketch entity tool, or select a tool on the Sketch toolbar and create a sketch.
To start a sketch with a plane:
Select a plane in the FeatureManager design tree and click a sketch entity tool on the Sketch toolbar. - or Select a plane in the FeatureManager design tree and click Sketch
on the Sketch toolbar.
The plane is displayed in Normal to orientation.
Starting the Sketch Does it matter where I start sketching? When you create a new part or assembly, the three default planes are aligned with specific views. The plane you select for your first sketch determines the orientation of your part. For example, if you choose *Front in the Orientation dialog box (or add a front view to a drawing), the view is normal to the Front Plane. If you open a new part and select a sketch tool, you are prompted to select a plane. If your first sketch is a top view, select the Top Plane.
3-4
•
If your first sketch is a left or right view, select the Right Plane.
•
You do not have to use one of the default planes for your first sketch; you can create a new plane at any angle. The orientation of views is still determined by the default planes, however.
•
You can reorient the part (to change Front to Top for example) with Update Standard Views Orientation dialog box.
in the
Starting the Sketch How complex should sketches be? In many cases, you can produce the same result by creating an extruded feature with a complex profile, or an extruded feature with a simpler profile and some additional features. (You often face this choice when planning the base feature for a part.) For example, if the edges of an extrusion need to be rounded, you can draw a complex sketch that contains sketch fillets (A), or draw a simple sketch and add the fillets as separate features later (B)
A Complex sketch
B Simple sketch Add fillet features Here are some things to consider: •
Complex sketches rebuild faster. Sketch fillets can be recalculated much faster than fillet features, but complex sketches can be harder to create and edit.
•
Simple sketches are more flexible and easier to manage. Individual features can be reordered and suppressed, if necessary.
Working in a Sketch In an open sketch, the SolidWorks window displays: •
The CommandManager with the Sketch toolbar active
•
Information about the sketch in the status bar
•
A sketch origin
•
A sketch grid
Status Bar The following information is in the status bar at the bottom of the sketch window: •
The coordinates of the pointer’s location when sketching an entity.
•
The state of the sketch: Over Defined, Under Defined, or Fully Defined. See Sketch Geometry Status.
•
The text, "Editing Sketch." This makes it obvious that you are in sketch mode if the sketch grid is off while you are working.
•
A description of a menu item or button when the pointer is over an item. This description is on the left side of the status bar.
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Chapter 3 Sketching
To display or hide the status bar:
Click View, Status Bar. Sketch Origin The sketch origin is displayed in red in an open sketch. Use the sketch origin to help you understand the coordinates of the sketch. Every sketch in the part has its own origin, so there usually are multiple sketch origins in a part. When a sketch is open, you cannot turn off the display of its origin.
Opening a New Sketch You must select a plane on which to create a new sketch. You can create a sketch on any of the default planes (Front Plane, Top Plane, or Right Plane), a created plane, a flat surface, or a face of a solid object. To open a new sketch on the Front Plane:
1.
Click Front Plane in the FeatureManager design tree.
2.
Click Sketch
to open a 2D sketch.
- or Click 3D Sketch
to open a 3D sketch.
To insert an alternate plane on which to sketch, see Creating a Construction Plane. You can also create a new sketch by extracting entities from an existing sketch.
Inferencing Pointers and Lines While sketching, notice that the appearance of the pointer changes to provide feedback about the pointer’s current task, position, and the geometric relations that are automatically applied. •
When you move the pointer along the length of any sketched curve, it first appears as an endpoint pointer, changes to the on-curve pointer, and then to a midpoint pointer, and so on.
•
When two lines intersect, the pointer changes to indicate the intersection.
•
When you sketch an arc, the pointer changes as it moves around the arc. The pointer provides information about dimensions as you sketch lines or arcs, such as the length, angle, or radius of the sketch entity.
•
3-6
•
When you select the various sketch or dimension tools, the pointer carries an appropriate symbol with it. Shown are the Rectangle, Circle, Spline, Point, Trim, Extend, and Dimension pointers, but there are many others.
As you sketch, the SolidWorks software monitors your activity and provides inferencing lines to help you work more efficiently. While sketching, notice that dashed inferencing lines align the pointer with lines or points that you have already sketched and with existing model geometry. •
When the endpoint of any line you are creating aligns with another point that you have already sketched, a dashed inferencing line indicates this alignment. This helps you align endpoints with each other so you can sketch without using a grid.
•
When you sketch arcs, inferencing lines and dimensions guide you to create the size and shape arc that you want.
TIP: Brown inference lines indicate that a relation is added automatically; blue inference lines indicate that no relation is added. However, if the inference line is blue and the pointer for a sketch entity (such as a line) includes the H (horizontal) or V (vertical) symbol, a relation is created.
Sketch Modes There are two modes for sketching in 2D: click-drag or click-click. SolidWorks responds to your cues to determine the mode as follows: •
If you click the first point and drag, you are in click-drag mode.
•
If you click the first point and release the pointer, you are in click-click mode. When you sketch entities in click-click mode and end a line or arc on the endpoint of an existing sketch entity, the tool stays active but does not show a preview from the last location.
Only click-drag mode is available for 3D sketching. When the Line and Arc tools are in click-click mode, they create a chain of segments as you click. To terminate a sketch chain, do one of the following: •
Double-click to terminate the chain of entities and leave the tool active.
•
Right-click and select End chain, which is the same as double-clicking.
•
Press Esc to terminate the chain and release the tool.
•
Move the pointer outside the view window to stop dragging. You can then choose another tool, which also terminates the chain.
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Chapter 3 Sketching
Autotransitioning You can transition from sketching a line to sketching a tangent arc, and vice versa, without selecting the arc tool. You can also toggle between line and arc with the A key. To autotransition between line and arc:
1.
Click Line
on the Sketch toolbar, or click Tools, Sketch Entities, Line and sketch a line.
2.
Click the endpoint of the line, then move the pointer away. The preview shows another line.
3.
Move the pointer back to the endpoint, then away again. The preview shows a tangent arc.
4.
Click to place the arc.
5.
Move the pointer away from the arc endpoint. The preview shows a line. You can draw a line or change to an arc as in Step 3. To toggle between line and arc without returning to the endpoint, press A.
Silhouettes You can select the silhouette edge of a rounded surface, such as a cylinder. Use the silhouette edge with the Convert Entities, Offset Entities, Smart Dimensions, or Add Relations tools. You can also select and reference silhouette vertices to add dimensions or relations. Silhouette edges are included in box-select operations. To select a silhouette edge:
1.
In an open sketch on a model face or plane (or in an active drawing view), move the pointer over a cylindrical face until the pointer changes to
.
To set silhouette edge visibility, click Tools, Options, System Options, Display/Selection, and select Dynamic highlight from graphics view. 2.
Select the highlighted edge.
Cutting, Copying, and Pasting in Sketches Cutting, Copying, and Pasting Sketch Entities You can cut and paste, or copy and paste, one or more sketch entities from one sketch to another or within the same sketch. In an open sketch, you can: •
Copy the sketch within the same document or to different documents. Hold down Ctrl while dragging the sketch. To copy one or more sketch entities, select the entities, then click Edit, Copy, or press Ctrl+C. Click in the graphics area, then click Edit, Paste or press Ctrl+V. The center of the sketch entities is placed where you clicked.
3-8
•
Move a sketch within the same sketch. Hold down Shift while dragging the sketch.
•
Move a sketch between different documents (the second document must have an open sketch). Hold down Ctrl and drag the sketch into the second document. Release Ctrl, hold down Shift, and drop the sketch.
Copying and Pasting Entire Sketches You can copy an entire sketch and paste it on a face in the current part, or you can paste it into a different sketch, or into a part, assembly, or drawing document. The target document must be open. When you copy a sketch, the relations are not copied. To copy and paste a sketch:
1.
Select the closed sketch in the FeatureManager design tree.
2.
Click Edit, Copy, or press Ctrl+C.
3.
Click in the sketch or document where you want to paste the center of the sketch.
4.
Click Edit, Paste, or press Ctrl+V.
Modify Sketch Use the Modify Sketch tool to move, rotate, or scale an entire sketch. To move, rotate, scale, or copy individual sketch entities, use the Move or Copy Entities, Rotate or Copy Entities, or Scale or Copy Entities tools. To move a sketch:
1.
Open a sketch or select a sketch in the FeatureManager design tree, and click Modify Sketch Sketch toolbar, or click Tools, Sketch Tools, Modify.
2.
In the dialog box:
on the
•
To move the sketch geometry incrementally, under Translate, type a value for X value and Y value and press Enter.
•
To move a specified point of the sketch to a specific location, under Translate, select Position selected point and click a point in the sketch. Type a value for X value and Y value and press Enter. The Modify Sketch tool translates the entire sketch geometry in relation to the model (including the sketch origin). The sketch geometry does not move relative to the origin of the sketch. - or -
•
To move a sketch in the graphics area, use the pointer: o o
3.
Press the left-mouse button
to move the sketch.
Point at the end points or center of the black origin to display one of three flip symbols. Right-click to flip the sketch on the X axis, the Y axis, or both.
Click Close.
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Chapter 3 Sketching
To rotate a sketch:
1.
Open a sketch or select a sketch in the FeatureManager design tree, and click Modify Sketch Sketch toolbar, or click Tools, Sketch Tools, Modify.
2.
In the dialog box: •
on the
Type a value for Rotate to set the rotation value and press Enter. - or -
•
Rotate a sketch in the graphics area with the pointer: o o
Press the right-mouse button
to rotate the s ketch around the black origin.
Point at the center point of the black origin to display a point symbol . Click and drag the center of rotation independently of the sketch, then rotate the sketch around the black origin.
You cannot move a sketch that has multiple external references. When a sketch has multiple external references, the pointer has a ? on the left button. 3.
Click Close.
To scale a sketch:
1.
Open a sketch or select a sketch in the FeatureManager design tree, and click Modify Sketch Sketch toolbar, or click Tools, Sketch Tools, Modify.
2.
In the dialog box, under Scale About, select: •
on the
Sketch origin. Applies a uniform scale about the origin of the sketch. - or -
• 3.
Moveable origin. Scales the sketch about the moveable origin.
Type a value for Factor, and press Enter. You cannot scale a sketch that has external references.
4.
Click Close.
Edit Sketch Edit Sketch opens an existing sketch so you can edit it. To edit a sketch:
1.
Right-click one of the following: •
the sketch in the FeatureManager design tree
•
a feature built from the sketch, either in the graphics area or in the FeatureManager design tree
•
a sketch entity in the graphics area For features built from multiple sketches (such as lofts and sweeps), right-click the sketch in the FeatureManager design tree.
2.
Select Edit Sketch.
3.
To close the sketch when you are finished editing, right-click in the sketch and select Exit Sketch. You can also edit an existing sketch by clicking Sketch
3-10
, then selecting the sketch to edit.
Exit Sketch You exit a sketch when you: •
Create a feature from a sketched profile. For example, when you extrude a base, boss, or a cut from a sketch.
•
Click Rebuild
•
Click Exit Sketch
•
Click Insert, Exit Sketch.
•
Select Exit Sketch from the shortcut menu.
•
Click Exit Sketch
•
Click Edit, Exit Sketch without Saving Changes.
on the Standard toolbar, or click Edit, Rebuild. on the Sketch toolbar.
or Cancel
in the Confirmation Corner.
Derived Sketch Derives a sketch from another sketch that belongs to the same part, or derives a sketch from another sketch in the same assembly. When you derive a sketch from an existing sketch, you are assured that the two sketches will retain the characteristics that they share in common. Changes that you make to the original sketch are reflected in the derived sketch. To derive a sketch from a sketch in the same part:
1.
Select the sketch from which you want to derive a new sketch.
2.
Hold the Ctrl key and click the face on which you want to place the new sketch.
3.
Click Insert, Derived Sketch. The sketch appears on the plane of the selected face, and the status line indicates that you are editing the sketch.
4.
Position the derived sketch by dragging and dimensioning it to the selected face. (The derived sketch is rigid and drags as a whole entity.)
To derive a sketch from a sketch in the same assembly:
1.
Right-click the part on which you want to place a derived sketch.
2.
Select Edit Part.
3.
Select the sketch (in the same assembly) from which you want to derive a new sketch.
4.
Hold the Ctrl key and click the face on which you want to place the new sketch.
5.
Click Insert, Derived Sketch. The sketch appears on the plane of the selected face, and you are editing the sketch.
6.
Position the derived sketch by dragging and dimensioning it to the selected face. (The derived sketch is rigid and drags as a whole entity.)
Note the following: •
If you delete a sketch from which a new sketch was derived, you are prompted that all derived sketches will automatically be underived. Click Yes or No.
•
You cannot add or delete sketch entities in a derived sketch. However, you can re-orient it with dimensions and geometric relations.
•
When you make changes to the original sketch, the derived sketch updates automatically.
•
To break the link between the derived sketch and its parent sketch, right-click the derived sketch in the FeatureManager design tree and select Underive. (After the link is broken, the derived sketch no longer updates when you change the original sketch.)
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Chapter 3 Sketching
Sketch Plane References When you delete a parent feature that has child features built from sketches, you have the option to keep the child features and have the sketch plane references dangle. You can dangle a sketch plane reference by editing the sketch plane definition and removing the plane definition. To create dangling sketch plane references:
1.
Select a parent feature that has a child feature. The child must be a sketch-based child, and the sketch must be dependent on the parent.
2.
Press the Delete key.
3.
In the dialog box, clear Also delete all child features, then click Yes. The dialog box warns that the plane is missing for the sketch used to create the child feature.
4.
Click Close. In the FeatureManager design tree, the part icon, the child feature, and the sketch used to create the child feature display warning icons that indicate the sketch plane is dangling. You can use the Edit Sketch Plane command to replace the reference plane.
Edit Sketch Plane Changes the sketch plane. To change the plane of a sketch:
1.
Select the sketch in the FeatureManager design tree, and click Edit, Sketch Plane. - or Right-click the sketch in the FeatureManager design tree, and select Edit Sketch Plane.
2.
Select a new plane in the FeatureManager design tree or select a new planar face in the model for Sketch Plane/Face
3.
Click OK
. .
Shaded Sketch Plane When you are editing a sketch in Shaded With Edges or Shaded mode, you can display the sketch plane as a shaded plane. To turn the shaded sketch plane on or off:
Click Tools, Options, System Options, Sketch. Select Display plane when shaded. If the display is slow due to the shaded plane, it may be because of the Transparency options. With some graphics cards, the display speed improves if you use low transparency. To set a low transparency, click Tools, Options, System Options, Performance and clear High quality for normal view mode and High quality for dynamic view mode.
3-12
Reference Plane Normal to Edge You can sketch on a reference plane, created automatically, normal to an edge. To sketch on a reference plane normal to an edge:
1.
In a part, select an edge and click Sketch
.
A reference plane normal to the selected edge is created at the end point of the edge closest to the selected area. The origin for the new plane appears at the edge's end point. 2.
Sketch an entity such as a rectangle or circle on the plane.
3.
Create a feature such as a boss or a cut.
Example using a reference plane normal to an edge: Select edge
Plane with origin at endpoint of edge
Sketch on plane
Extruded cut normal to plane
Sketch Tools Align Grid Aligns the sketch grid with the model edge that you select. To align the grid to a model edge:
1.
Open a sketch on a model face.
2.
Click Tools, Sketch Tools, Align, Grid.
3.
Click the model edge to which you want to align the grid.
4.
In the dialog box, click Apply to apply the change. The grid shifts to align with the edge you selected and the origin is placed at the end of the edge closest to where you clicked.
5.
Click OK to accept the change. - or Click Close to close the dialog box. If you previously clicked Apply, the change is saved; if you did not click Apply, the dialog box closes without change.
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Chapter 3 Sketching
Automatic Inferencing Lines You can turn off automatic inferencing lines while editing a sketch or while sketching in a drawing document. If automatic inferencing lines are turned off, you no longer automatically infer to all model edges, active sketch entities, or non-active sketch entities. Turning off inferencing lines in a complex sketch or drawing may improve sketching performance and reduce the chance of unwanted relations. NOTE: To inference to temporary axes, make the temporary axes visible. Click View, Temporary Axes. To turn off the automatic inferencing lines:
Click Tools, Sketch Settings, Automatic Inferencing Lines to turn on or off the automatic inferencing lines. In drawings, you must activate the inferencing lines for current sketch entities. You have to activate the inferencing lines for each new entity that you sketch. To activate the inferencing lines for an entity in a drawing:
1.
Click a sketch entity tool, such as Line
.
2.
Move the pointer over the entity you want to infer to. The color of the pointer changes to orange
once the inferencing lines are active for the entity.
To wake up the edges of a model to use inferencing:
1.
Open a sketch on the planar face of the model.
2.
Click a sketch entity tool, such as Line
3.
Move the pointer over the model edge to activate it.
.
If the model is cylindrical, the center point appears as a black cross. Example: To infer to the center of a cylinder, select a sketch entity tool and wake up the edges of the cylinder. Then you can infer to the center point.
Automatic Solve Specifies whether SolidWorks should automatically do the computation to solve the sketch geometry of your part as you create it. To turn automatic computation on or off:
Click Tools, Sketch Settings, Automatic Solve. A check mark next to the menu item means that computations are solved automatically. NOTE: When you are in the process of changing many dimensions in an active sketch, you may want to turn off the Automatic Solve option temporarily.
3-14
No Solve Move No Solve Move
lets you move sketch entities without solving the dimensions or relations in the sketch.
If dimensions or relations exist between the selected entities and other sketch entities or model geometry, a warning message appears. The message asks if you want to delete the constraints caused by the dimensions or relations: •
If you click Yes, the constraints are deleted, and the entities are moved.
•
If you click No, the constraints are not deleted, and the selected entities are copied to the location to which you moved them.
To use No Solve Move:
•
Click No Solve Move
on the Sketch toolbar.
•
Click Tools, Sketch Settings, No Solve Move.
Move or Copy PropertyManager Move, rotate, and scale items (or copies of items) in sketches and drawings. These operations do not create relations. Operation Move, Rotate, or Scale. Determines the operation you want to perform. This is pre-selected depending on which tool you clicked. For example, if you clicked Move or Copy Entities , then Move is selected. Sketch items or annotations
. Select from the following:
•
In sketches: sketch entities and some annotations (those that can be cut, copied, and pasted)
•
In drawings: sketch entities and all annotations
Copy. Copies the entities in Sketch items or annotations. Number of Copies (available when Copy is selected). Specifies the number of times to copy the entities in Sketch items or annotations. Click in the graphics area to create the number of instances specified. Keep relations (available when Move or Rotate is selected). Maintains relations between sketch entities. When cleared, relations are broken only between selected entities and those that are not selected; relations among the selected entities are maintained. Scale Factor (available when Scale is selected). Specifies the scale factor for the selected entities. The scale factor increases arithmetically (not geometrically). Base Point Base point . Defines the point from which the items are moved, scaled, or rotated. Click in the graphics area or specify coordinates to define the base point. Start X coordinate
. Displays the base point X coordinate.
Start Y coordinate
. Displays the base point Y coordinate.
Destination (available when Move is selected) Relative offset. Sets all geometry to move by the same relative amount. Delta X
(available when Relative offset is selected). Determines the X destination coordinate.
Delta Y
(available when Relative offset is selected). Determines the Y destination coordinate.
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Chapter 3 Sketching
Destination . Defines the point to which the items are moved. Click in the graphics area or specify coordinates to define the destination point. End X coordinate
. Determines the X destination coordinate.
End Y coordinate
. Determines the Y destination coordinate.
Rotate (available when Rotate is selected) Angle
. Specifies the angle of rotation.
Check Sketch for Feature Usage Check a sketch for errors that might prevent it from creating a feature. For each Feature usage type, its required sketch Contour type is displayed. If you select a new Feature usage type from the list, the corresponding Contour type changes. Each Contour type forces a different set of checks on the sketch in addition to the general checks that are common to all contour types. To check a sketch for feature usage:
1.
In an open sketch, click Tools, Sketch Tools, Check Sketch For Feature. In the dialog box, Feature usage lists all of the ways to use the sketch in a feature:
2.
•
If the sketch was used to create a feature, the feature type is displayed in Feature usage.
•
If the sketch was not used to create a feature, <none> is displayed in Feature usage and the contour is checked for errors that are common to all contour types.
Click Check. The sketch is checked according to the contour type required by the feature type listed in the Feature usage box. If the sketch passes the checks, a No problems found message appears. If there is an error, a message describes the error and, if appropriate, the error is highlighted. It finds one error for each check.
3.
To check your sketch for possible use in other feature types, select another type in Feature usage and click Check.
4.
Click Reset to return to the original Feature usage type.
5.
Click Close. Alternatively, the dialog box closes automatically when you exit the sketch, rebuild, change to a new document, and so on.
Allowed Contour Types Contour type:
Features that use the contour type:
Single Open
Base Extrude Thin, Base Revolve Thin, Boss Extrude Thin, Boss Revolve Thin, Cut Extrude, Cut Extrude Thin, Cut Revolve Thin, Loft Guide, SheetMetal Base Flange, Surface Loft Section, Sweep Path Or Guide, Sweep Section
Single Closed
Cut Extrude Thin, Loft Guide, Loft Section, Surface Loft Section, Sweep Path Or Guide
Multiple Disjoint Closed
Base Extrude, Base Extrude Thin, Base Revolve, Base Revolve Thin, Boss Extrude, Boss Extrude Thin, Boss Revolve, Boss Revolve Thin, Cut Extrude, Cut Revolve, Cut Revolve Thin, SheetMetal Base Flange, Sweep Section
General
Mold Parting Surface, Rib, SheetMetal 3D Bend, Surface Extrude, Surface Revolve, Surface Sweep Section, <none> (The contour is checked for errors that are common to all contour types.)
3-16
Sketch Contour Single Open Single open contours can be used for extrudes, revolves, sections, paths, guides, and sheet metal. Typical open contours are sketched with lines or splines.
Sketch Contour Single Closed Single closed contours can be used for extrudes, revolves, sections, paths, guides, and sheet metal. Typical closed contours are sketched with circles, squares, closed splines, and other closed geometric shapes.
Sketch Contour Multiple Contained Closed Multiple contained closed contours can be used for extrudes, revolves, and sheet metal. If there is more than one contour, one contour must contain the rest. Typical multiple contained closed contours are sketched with circles, rectangles, and other closed geometric shapes.
Sketch Contour Multiple Disjoint Closed Multiple disjoint closed contours can be used for extrudes, revolves, and sheet metal; for example, to cut several holes on the face of a part. Typical multiple disjoint closed contours are sketched with circles, rectangles, and other closed geometric shapes.
Circular Sketch Step and Repeat Use the Circular Sketch Step and Repeat tool to create a circular pattern of sketch entities. To create a circular pattern of sketch entities:
1.
Open a sketch on a model face and sketch an item to repeat.
2.
With the sketch entities selected, click Circular Sketch Step and Repeat click Tools, Sketch Tools, Circular Step and Repeat.
on the Sketch toolbar, or
You can also select the entities after you click Circular Sketch Step and Repeat. The names of the selected sketch entities appear under Items to repeat. 3.
Under Arc, set: •
Radius. Measures the distance from the center of the pattern to a center point or vertex on the selected entities. If you select Fixed, the Radius is displayed as an explicit value when the pattern is complete.
•
Angle. Measures the angle from the center of the selected entities to the center point or vertex of the pattern.
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Chapter 3 Sketching
4.
Under Center, either: •
Set values for the X and Y coordinates to position the center point or vertex of the pattern. - or -
• 5.
6.
Drag the center point or vertex of the pattern in the graphics area. The X and Y coordinates update accordingly.
Under Step, set: •
Number. Specifies the number of pattern instances, including the original sketch entity.
•
Total angle (available when Equal is selected). Specifies the angle between the first and last instance in the pattern.
•
Spacing (available when Equal is cleared). Specifies the angle between the pattern instances.
•
Reverse Rotation
•
Equal. Sets an equal distance between each pattern instance.
•
Constrain spacing (available when Equal is cleared). Constrains the Total angle between pattern instances in the pattern.
. Reverses the pattern rotation.
If you type values for Radius, Angle, X or Y, Number, Spacing, or Total Angle, (instead of clicking the buttons) you must click Preview to see a preview of the pattern. You can then adjust any of the values and click Preview again. You can drag one of the selection points to set the radius and angle and the spacing between instances.
7.
Select a number in Instances and press Delete to delete that instance in the pattern. The number then appears in Instances deleted. To return the instance to the pattern, select the number in Instances deleted and press Delete.
8.
Click OK.
To edit a circular sketch step and repeat pattern feature:
1.
Right-click the pattern sketch and select Edit Sketch.
2.
Select an instance and click Tools, Sketch Tools, Edit Circular Step and Repeat. - or Right-click an instance and select Edit Circular Step and Repeat.
3.
Set the Number of pattern instances, then click OK. Additionally, you can modify the pattern in the following ways:
4.
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•
Double-click the angle dimension and change the angle in the Modify dialog box (available only if you cleared Equal and selected Constrain spacing when you created the pattern).
•
Drag the center point of the pattern to a new location (available only if you cleared Equal when you created the pattern).
•
Change the rotation of the pattern by dragging the center point of the pattern or by selecting a pattern instance and dragging it.
•
Change the radius of the pattern arc by dragging the first instance of the pattern by its center point or vertex (available only if you cleared Equal when you created the pattern).
•
Select and delete individual pattern instances.
Exit the sketch.
Constrain Spacing and Fixed Options Circular Sketch Step and Repeat Pattern •
Select the Constrain spacing check box to constrain the Total Angle between pattern instances in the circular pattern. After the pattern is created, you can change the angle (or spacing) by double-clicking the dimension and using the Modify dialog box. (This option is only available if the Equal check box is not selected.)
•
The Fixed option is related to the Radius value. If you select the Fixed check box, the result is as follows: o
The radius is displayed as an explicit dimension.
o
You can control the radius by double-clicking the dimension and using the Modify dialog box.
Return to Circular Sketch Step and Repeat.
Constrain All Sets constraints on the sketch entities of an unconstrained imported .DXF or .DWG drawing. To solve relations in an imported drawing:
1.
Import a sketch from a .DXF or .DWG drawing.
2.
Click Tools, Relations, Constrain All. The command tries to solve all the apparent relations in the sketch and reports the number of constraints that were added to the sketch.
Contour Selection Select sketch contours and model edges, and apply features to them. This allows you to use a partial sketch to create features. To select and extrude contours:
1.
In an active sketch, right-click in the graphics area and select Contour Select Tool. The pointer changes to
2.
.
Select a contour. The contour can include model edges. To select multiple contours, hold down Ctrl.
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Chapter 3 Sketching
3.
Click a feature to apply to the selected contours; Extruded Boss/Base, for example.
A tooltip appears when a contour cannot be selected for one of the following reasons: •
The part has too many edges.
•
Edges are created on offset planes.
•
Edges are chamfered.
•
Edges are filleted.
Contour selection is also restricted as follows: •
•
When reusing a sketch, you can select only on the original face. If, for example, part of the face has been extruded, the tool does not recognize the new face. You can select contours only on the face with the sketch. If, for example, the face with the sketch is cut by a solid object (as shown at right), the tool can select the part of the face still visible but does not recognize the solid object.
Example of Sketch Reuse
3-20
Sketch used for revolve surface
Same sketch reused for surface extrude
Sketch used for sweep thin feature
Same sketch used for boss extrude thin feature
Close Sketch to Model Closes a sketch with an open profile, using existing model edges. To use an open profile sketch to extrude using existing model edges:
1.
Open a sketch on a model face.
2.
Sketch an open profile with endpoints that are coincident with model edges on the same face boundary.
3.
Click Tools, Sketch Tools, Close Sketch to Model. An arrow points in the direction in which the sketch will close. (The extruded boss will either be within the sketch lines or outside of the sketch lines.)
4.
In the dialog box, select Reverse direction to close the sketch, if necessary.
5.
Click Yes when the arrow points in the correct direction.
6.
Click Extruded Boss/Base
or Insert, Boss, Extrude,
or Extruded Cut or Insert, Cut, Extrude, and specify the End Condition in the PropertyManager. 7.
Click OK
.
Construction Geometry You can convert sketch entities in a sketch or drawing to construction geometry. Construction geometry is used only to assist in creating the sketch entities and geometry that are ultimately incorporated into the part. Construction geometry is ignored when the sketch is used to create a feature. Construction geometry uses the same line style as centerlines. To convert sketch entities to construction geometry:
In an open sketch, select one or more sketch entities and do one of the following: •
Select For construction in the PropertyManager.
•
Click Construction Geometry
•
Click Tools, Sketch Tools, Construction Geometry.
•
Right-click a sketch entity and select Construction Geometry (drawings only).
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on the Sketch toolbar.
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Chapter 3 Sketching
Convert Entities You can create one or more curves in a sketch by projecting an edge, loop, face, curve, or external sketch contour, set of edges, or set of sketch curves onto the sketch plane. To convert an entity:
1.
In an open sketch, click a model edge, loop, face, curve, external sketch contour, set of edges, or set of curves.
2.
Click Convert Entities
on the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities.
The following relations are created: o
o
On Edge. Created between the new sketch curve and the entity, which causes the curve to update if the entity changes. Fixed. Created internally on the endpoints of the sketch entity so the sketch remains in a "fully defined" state. This internal relation is not displayed when you use Display/Delete Relations. Remove the Fixed relation by dragging the endpoints.
Detach Segment on Drag You can detach a segment (line, arc, ellipse, or spline) from the other entities it is attached to in a sketch, if dimensions or relations do not prevent dragging. Detach Segment on Drag is not available in 3D sketches. To detach a sketch segment:
1.
In an open part, click Tools, Sketch Settings, Detach Segment on Drag.
2.
Select the entity that you want to detach from another sketch entity and drag it to a new location. Detach Segment On Drag does not delete relations. Delete relations before you drag an entity to detach. See Sketch Relations PropertyManager.
Extend Entities You can add to the length of a sketch entity (line, centerline, or arc). Typically, you use Extend Entities to extend a sketch entity to meet another sketch entity. To extend a sketch entity:
1.
In an open sketch, click Extend Entities The pointer changes to
2.
on the Sketch toolbar, or click Tools, Sketch Tools, Extend.
.
Move the pointer over the sketch entity to extend. The selected entity appears in aqua, and a preview appears in pink in the direction to extend the entity.
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3.
If the preview extends in the wrong direction, move the pointer to the other half of the line or arc.
4.
Click the sketch entity to accept the preview.
Face Curves You can extract iso-parametric (UV) curves from a face or surface. Applications of this functionality include extracting the curves for imported surfaces and then performing localized cleanup using the face curves. You can specify a mesh of evenly spaced curves or a position that creates two orthogonal curves.
Mesh
Position
Each curve created by this process becomes a separate 3D sketch. However, if you are editing a 3D sketch when you invoke the Face Curves tool, all extracted curves are added to the active 3D sketch. To extract iso-parametric curves:
1.
Click Face Curves
or Tools, Sketch Tools, Face Curves, then select a face or surface.
- or Select a face or surface, then click Face Curves
or Tools, Sketch Tools, Face Curves.
A preview of the curves appears on the face. The curves are one color in one direction and another color in the other direction. The colors correspond to the colors in the Face Curves PropertyManager. The name of the face appears in the Face 2.
Under Selections, choose either: o o
3.
Mesh - evenly spaced curves. Specify an integer number of curves for Direction 1 and Direction 2. Position - the intersection of two orthogonal curves. Drag the position in the graphics area or specify the percentage distance from the bottom for Direction 1 and from the right for Direction 2. •
Direction 1 On/Off or Direction 2 On/Off check box - clear if the curve is not required.
•
Position Vertex - select a vertex or point to specify the intersection of the two curves. This vertex cannot be dragged.
Under Options, select or clear: o o
4.
box.
Constrain to model - when selected, the curves are updated if the model changes. Ignore holes - useful for imported surfaces with internal gaps or loops. When selected, the curves are generated across holes as though the surface were intact. When cleared, the curves stop at the edges of holes.
Click OK
.
The curves appear as 3D sketches in the FeatureManager design tree. NOTE: If surface edge information cannot be matched, edge curves cannot be generated. The error message states: "Failed to create X out of X face curves. Please consider using convert entities." You can generate the missing curves by opening a 3D sketch and using the Convert Entities
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sketch tool.
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Chapter 3 Sketching
Intersection Curve Intersection Curve
opens a sketch and creates a sketched curve at the following kinds of intersections:
•
A plane and a surface or a model face
•
Two surfaces
•
A surface and a model face
•
A plane and the entire part
•
A surface and the entire part
You can use the resulting sketched intersection curve in the same way that you use any sketched curve, including the following tasks: •
Measure thickness at various cross sections of a part. (See steps below.)
•
Create sweep paths that represent the intersection of a plane and the part.
•
Make sections out of imported solids to create parametric parts.
To use the sketched curve to extrude a feature, the sketch that opens must be a 2D sketch. Other tasks can be performed using a 3D sketch. •
To open a 2D sketch, select the plane first then click Intersection Curve.
•
To open a 3D sketch, click Intersection Curve first then select the plane.
To measure the thickness of a cross section of a part:
1.
With a part open, click Intersection Curve Curve. A 3D sketch opens (because you clicked
2.
on the Sketch toolbar, or Tools, Sketch Tools, Intersection
before selecting a plane).
Select the intersecting items: •
Select a plane that intersects a face of the part.
•
Click the face of the part. A sketched spline appears at the intersection of the plane and the top face.
3.
Rotate the part, then click the opposite (inside) face of the part. Another sketched spline appears on the inside face.
You can also select the part in the FeatureManager design tree. A sketched spline appears on every face where the plane intersects.
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4.
Click Tools, Measure and measure the distance between the two sketched splines.
Linear Sketch Step and Repeat Use the Linear Sketch Step and Repeat tool to create a linear pattern of sketch entities. To create a linear pattern of sketch entities:
1.
Open a sketch on a model face and sketch one or more items to repeat.
2.
With the sketch entities selected, click Linear Sketch Step and Repeat Tools, Sketch Tools, Linear Step and Repeat.
on the Sketch toolbar, or click
You can also select the sketch entities after you click Linear Sketch Step and Repeat. The names of the selected sketch entities appear in Items to repeat. 3.
4.
Under Direction 1, set: •
Number. Total number of pattern instances, including the original sketch.
•
Spacing. Distance between pattern instances. If you select Fixed, the Spacing value is displayed as an explicit value when the pattern is complete.
•
Angle. Angle of rotation for the pattern.
•
Reverse Direction 1
. Reverses the direction of the pattern.
If you type values for Number, Spacing, or Angle, (instead of clicking the buttons) you must click Preview to see a preview of the pattern. You can then adjust any of the values and click Preview again. You can also change the Spacing and Angle by dragging the selection point in the pattern preview.
5.
To create a pattern in two directions, repeat step 3 and set values for Direction 2. In two-directional patterns, you can select Constrain angle between axes.
6.
Select a position (column, row) in Instances and press Delete to delete that instance in the pattern. The position appears in Instances deleted. To return the instance to the pattern, select the position in Instances deleted and press Delete.
7.
Click OK.
To edit the linear sketch step and repeat pattern feature:
1.
Right-click the pattern sketch and select Edit Sketch.
2.
Select an instance and click Tools, Sketch Tools, Edit Linear Step and Repeat. - or Right-click an instance and select Edit Linear Step and Repeat.
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Chapter 3 Sketching
3.
Change the Number of instances in one or both directions, and click OK. Additionally, you can modify the pattern in the following ways:
4.
•
Drag a point or vertex on one of the pattern instances.
•
Change the angle of the pattern by double-clicking the angle and changing its value in the Modify dialog box.
•
Add dimensions and change their values using the Modify dialog box.
•
Add relations to the pattern instances.
•
Select and delete individual pattern instances.
Exit the sketch to complete the new pattern feature.
Fixed Spacing in Linear Sketch Step and Repeat The Fixed check box in the Linear Sketch Step and Repeat dialog box applies to the Spacing value for each linear direction. If you select the Fixed check box before creating the linear array, the result is as follows: •
Corresponding points on the first and second instance are joined with a construction line, and this line is dimensioned.
•
The resulting dimension is displayed as an explicit sketch dimension.
•
You can control the spacing by double-clicking the dimension and using the Modify dialog box.
Constrain Angle in Linear Sketch Step and Repeat The Constrain angle between axes check box is available if you define two pattern directions. If you select Constrain angle between axes, the result is as follows: •
The angle between the two directions is defined by a construction line through corresponding points on the first and second instance, in each direction.
•
After the pattern is created, by clicking OK, you can change this angle by double-clicking the dimension and using the Modify dialog box.
Return to Linear Sketch Step and Repeat.
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Mirror Entities You can mirror sketch entities around a centerline. When you create mirrored entities, the SolidWorks software applies a symmetric relation between each corresponding pair of sketch points (the ends of mirrored lines, the centers of arcs, and so on). If you change a mirrored entity, its mirror image also changes. Mirror Entities is not available in 3D sketches. To mirror existing sketch entities:
1.
In an open sketch, click Centerline
on the Sketch toolbar and sketch a centerline.
2.
Select the centerline and the items you want to mirror.
3.
Click Mirror Entities
on the Sketch toolbar, or click Tools, Sketch Tools, Mirror.
To mirror sketch entities as you sketch them:
1.
Click Centerline
2.
Click Mirror Entities
on the Sketch toolbar and sketch a centerline. on the Sketch toolbar, or click Tools, Sketch Tools, Mirror. Symmetry symbols
appear at both ends of the centerline. 3.
Create the sketch entities that you want to mirror. The entities are mirrored as you sketch them.
4.
To turn mirroring off, click Mirror Entities
again.
Move, Rotate, Scale, or Copy Move, rotate, scale, or copy items in sketches and drawings with the Move or Copy PropertyManager. The Move or Copy operations do not create relations. To create relations, you must add relations. To move or copy sketch entities:
1.
In an open sketch, click Move or Copy Entities Move or Copy.
2.
To copy the sketch entities, in the PropertyManager, under Operation, select Copy, and set the Number of Copies
3.
on the Sketch toolbar, or click Tools, Sketch Tools,
to create.
Select the sketch entities or annotations to move. In parts and assemblies, you can select any annotations that can be cut, copied, and pasted. In drawings, you can select all annotations. The pointer changes to , which indicates that the entities are ready to move. If you selected the entities before you clicked Move or Copy Entities, this pointer does not appear; go to step 5.
4.
In the graphics area, right-click. The pointer changes to
5.
.
Click to set the base point.
The pointer changes to
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.
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Chapter 3 Sketching
6.
Click to set the destination point.
7.
The sketch entities are set and the PropertyManager closes. If Keep Visible
is selected, the pointer changes to
(if Copy is selected) or
(if Copy is
cleared). With the •
pointer, you can: Right-click to accept the move and close the PropertyManager. - or -
•
With the
Move the pointer away from the destination point. The pointer changes to additional sketch entities.
, and you can move
pointer, you can:
•
Click to place additional copies of the sketch entities.
•
Click OK
to close the PropertyManager.
To rotate or copy sketch entities:
1.
In an open sketch, click Rotate or Copy Entities Rotate or Copy.
on the Sketch toolbar, or click Tools, Sketch Tools,
2.
To copy the sketch entities, in the PropertyManager, under Operation, select Copy, and set the Number of
3.
Copies to create. Select the sketch entities or annotations to rotate. In parts and assemblies, you can select any annotations that can be cut, copied, and pasted. In drawings, you can select all annotations. The pointer changes to , which indicates that the entities are ready to rotate. If you selected the entities before you clicked Rotate or Copy Entities, this pointer does not appear; go to step 4.
4.
In the graphics area, right-click. The pointer changes to
5.
Click to set the base point. This is the point about which to rotate the entities. The pointer changes to
6.
.
.
Move the pointer to set the rotation angle, then click and drag the pointer to rotate the sketch entities. When you drag the pointer, angle snap increments vary depending on the distance of the pointer from the base point. Exact angle values are displayed when you inference to model geometry.
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7.
Right-click to accept the rotation and to close the PropertyManager. - or If Keep Visible
is selected, click and drag the pointer to rotate the same sketch entities or to rotate
additional copies of the sketch entities. When you right-click to accept the rotation, Angle Click OK
is set to 0.
, or right-click again to close the PropertyManager.
To scale or copy sketch entities:
1.
In an open sketch, click Scale or Copy Entities Scale or Copy.
2.
To copy the sketch entities, in the PropertyManager, under Operation, select Copy, and set the Number of Copies
on the Sketch toolbar, or click Tools, Sketch Tools,
to create.
If you select Copy, and:
3.
•
the scale of the copied sketch entity is too large or too small, the number of copies is reduced.
•
set the Scale Factor , then change the Number of Copies accommodate the copies specified.
, the Scale Factor updates to
Select the sketch entities or annotations to scale. In parts and assemblies, you can select any annotations that can be cut, copied, and pasted. In drawings, you can select all annotations. The pointer changes to , which indicates that the entities are ready to scale. If you selected the entities before you clicked Scale or Copy Entities, this pointer does not appear; go to step 5.
4.
In the graphics area, right-click. The pointer changes to
5.
.
Click to set the base point. This is the point about which to scale the entities. The pointer changes to
6.
Set the Scale Factor
. .
The Scale Factor increases arithmetically (not geometrically). The example shows a sketch entity with copies at scale factors of 2, 3, and 4.
7.
Right-click to accept the scaled entity and close the PropertyManager. If Keep Visible
is selected, Scale Factor
is set to 1.0, and you can continue to scale sketch
entities. Click OK to close the PropertyManager. (If Scale Factor is not set to 1.0, click OK to close the PropertyManager.)
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Chapter 3 Sketching
Offset Entities Use the Offset Entities tool to create sketch curves offset from one or more selected sketch entities, edges, loops, faces, curves, set of edges, or set of curves by a specified distance. The selected sketch entity can be construction geometry. The offset entities can be bidirectional. The SolidWorks software creates an on-edge relation between each original entity and the corresponding sketch curve. If the original entity changes, then the offset curve also changes when you rebuild the model. To create a sketch curve offset from a model edge:
1.
In an open sketch, select one or more sketch entities, a model face, a model edge, or external sketch curves.
2.
Click Offset Entities
3.
In the PropertyManager, under Parameters, set:
on the Sketch toolbar, or click Tools, Sketch Tools, Offset Entities.
When you click in the graphics area, the Offset Entity is complete. Set the Parameters before you click in the graphics area.
4.
•
Offset Distance . Set a value to offset the sketch curve by a specified distance. You can also hold down the mouse button and drag the pointer in the graphics area to see a dynamic preview. When you release the mouse button, the Offset Entity is complete.
•
Reverse. Changes the direction of a one-directional offset.
•
Select chain. Creates an offset of all contiguous sketch entities.
•
Bi-directional. Creates offset entities in two directions.
Click OK
or click in the graphics area.
To change the size of a sketch curve offset:
Double-click the offset’s dimension and change the value. In a bi-directional offset, change the dimensions of the two offsets individually.
Override Dims on Drag/Move You can override dimensions by dragging sketch entities. The sketch dimensions update at the end of the drag. They remain driving dimensions and update in the part, assembly, and drawing. You can set an option to enable this functionality in all documents, or you can enable it for the active document only. To set the option for all documents:
1.
Click Tools, Options, System Options, Sketch.
2.
Select Override Dims on Drag/Move and click OK.
To enable the functionality in the active document:
Click Tools, Sketch Settings, Override Dims on Drag/Move. To move a dimensioned sketch entity:
1.
Select Override Dims on Drag/Move by one of the above methods.
2.
In an open sketch, select a sketch entity.
3.
Drag the sketch entity. - or Click Tools, Sketch Tools, Move or Copy, and set the values in the Move or Copy PropertyManager.
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Sketch Chamfer The Sketch Chamfer tool applies a chamfer to adjacent sketch entities in 2D and 3D sketches. This tool is available for both 2D and 3D sketches. The Chamfer tool on the Features toolbar chamfers entities such as edges in parts. To create a sketch chamfer:
1.
In an open sketch, click Sketch Chamfer Chamfer.
on the Sketch toolbar, or click Tools, Sketch Tools,
2.
In the PropertyManager, set the Chamfer Parameters as necessary.
3.
In the graphics area, select the two sketch entities to chamfer. To select the sketch entities, you can: •
Hold Ctrl and select two sketch entities.
•
Select a vertex.
The chamfer is applied immediately. 4.
Click OK to accept the chamfer, or click Undo to remove the chamfer. You can undo a sequence of chamfers in reverse order.
Sketch Chamfer Parameters •
•
Angle-distance o
Distance 1
is applied to the first sketch entity selected.
o
Direction 1 Angle
is applied from the first sketch entity toward the second.
Distance-distance o
Equal distance check box selected. Distance 1
o
Equal distance check box cleared. Distance 1 Distance 2
Angle-distance
is applied to both sketch entities. is applied to the first sketch entity selected.
is applied to the second sketch entity selected. Distance-distance
Equal distance
Sketch Fillet The Sketch Fillet tool trims away the corner at the intersection of two sketch entities to create a tangent arc. This tool is available for both 2D and 3D sketches. The Fillet tool on the Features toolbar fillets entities such as edges in parts. Example of Sketch Fillets The four corners of the rectangle are filleted with the same radius and with Keep constrained corners selected.
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Chapter 3 Sketching
To create a fillet in a sketch:
1.
In an open sketch, click Sketch Fillet
2.
Set the properties in the Sketch Fillet PropertyManager.
3.
Select the sketch entities to fillet. (You can select non-intersecting entities. The entities are extended, and the corner is filleted.) To select the sketch entities, you can:
4.
on the Sketch toolbar, or Tools, Sketch Tools, Fillet.
•
Hold Ctrl and select two sketch entities.
•
Select a corner.
Click OK to accept the fillet, or click Undo to remove the fillet. You can undo a sequence of fillets in reverse order.
Sketch Fillet PropertyManager The Sketch Fillet PropertyManager controls the following properties during creation of a sketch fillet. The Fillet tool on the Features toolbar fillets entities such as edges in parts. Fillet Parameters •
Radius
. Controls the fillet radius.
Consecutive fillets with the same radius are not dimensioned individually; they have an automatic Equal relation with the first fillet in the series. •
Keep constrained corners. Maintains the virtual intersection point if the vertex has dimensions or relations. When cleared, and if the vertex has dimensions or relations, you are asked if you want to delete those geometric relations when the fillet is created.
•
Undo. Undoes the last fillet. You can undo a sequence of fillets in reverse order.
Split Entities You can split a sketch entity to create two sketch entities. Conversely, you can delete a split point to combine two sketch entities into a single sketch entity. Use two split points to split a circle, full ellipse, or a closed spline. You can dimension to a split point. Also, you can insert parts at split points in a routing assembly. To split a sketch entity:
1.
In an open sketch, click Split Entities Entities. The pointer changes to
2.
on the Sketch toolbar, or click Tools, Sketch Tools, Split
.
Click the sketch entity at the location where you want the split to occur. The sketch entity splits into two entities, and a split point is added between the two sketch entities.
To combine two split sketch entities into one:
In an open sketch, click the split point and press Delete.
Trim Entities Use Trim Entities to:
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•
Trim a line, arc, circle, ellipse, spline, or centerline to its intersection with a line, arc, circle, ellipse, spline, or centerline.
•
Delete a line, arc, circle, ellipse, spline, or centerline.
•
Extend a sketch segment until it is coincident with another entity.
To delete a sketch entity:
1.
In an open sketch, click Trim Entities
2.
Move the pointer red, then click.
on the Sketch toolbar, or click Tools, Sketch Tools, Trim.
over a sketch until the sketch segment that you want to trim (delete) is highlighted in
The segment is deleted up to its intersection with another sketch segment (line, arc, circle, ellipse, spline, or centerline) or model edge. The entire sketch segment is deleted if it does not intersect with any another sketch segment. To extend a sketch entity:
Drag the endpoint of a sketch entity until it is coincident with another entity. You cannot use Trim Entities to extend a sketch segment unless there is another entity to which you can extend the segment.
Dimensions and Relations Dimensions You dimension sketch entities and other objects with the Smart Dimension tool. The type of dimension is determined by the items you click. For some types of dimensions (point-to-point, angular, circular), where you place the dimension also affects the type of dimension that is added. You can drag or delete a dimension while the Smart Dimension tool is active. To add a dimension to a sketch or drawing:
1.
Click Smart Dimension on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart. The default dimension type is Parallel. Optionally, you can choose a different dimension type from the shortcut menu. Right-click the sketch, and select More Dimensions. Choose from Horizontal, Vertical, Ordinate, Horizontal Ordinate, or Vertical Ordinate. If you are editing a drawing view, you have additional choices of Baseline and Chamfer.
2.
Select the items to dimension, as shown in the table below. As you move the pointer, the dimension snaps to the closest orientation.
3.
Click to place the dimension.
To dimension the...
Click...
•
Length of a line or edge
The line.
•
Angle between two lines
Two lines, or a line and a model edge.
Note: Placement of the dimension affects the way the angle is measured. Example
•
Distance between two lines
Two parallel lines or a line and a parallel model edge.
•
Perpendicular distance from a point to a line
The point and the line or model edge.
•
Distance between two points
Two points.
•
Radius of an arc
The arc.
•
True length of an arc
The arc, then the two end points
SolidWorks 2004 Reference Guide
One of the points can be a model vertex. Example Example
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Chapter 3 Sketching
•
Diameter of a circle
The circumference.
Displayed as linear or diameter, depending on placement. Example
•
Distance when one or both entities is an arc or a circle
The centerpoint or the circumference of the arc or circle, and the other entity (line, edge, point, and so on).
By default, distance is measured to the centerpoint of the arc or circle, even when you select the circumference. Example
The dimension shortcut menu provides Display Options. The choices available depend on the type of dimension and other factors and may include the following: •
Center between witness lines
•
Offset Text
•
Show Parentheses
•
Show as Inspection
Horizontal Dimension You can specify a horizontal dimension between two entities. The horizontal direction is defined by the orientation of the current sketch. To specify a horizontal dimension:
1.
In an open sketch, click Horizontal Dimension Dimensions, Horizontal. The pointer changes to
on the Dimensions/Relations toolbar, or click Tools,
.
2.
Select the two entities to dimension.
3.
Click a location to place the dimension.
Vertical Dimension You can create a vertical dimension between two points. The vertical direction is defined by the orientation of the current sketch. To create a vertical dimension:
1.
Click Vertical Dimension
on the Dimensions/Relations toolbar, or click Tools, Dimensions, Vertical.
2.
Click the two points to dimension.
3.
Click a location to place the dimension.
Lock Dimensions When you create a dimension, the dimension snaps to the closest orientation as you move the pointer. When the preview indicates the dimension type you want, right-click to accept the dimension. You can then move the pointer to place the dimension in another location without changing the dimension type. To lock a dimension:
3-34
1.
In an open sketch, click Smart Dimension Dimension, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Click the items to dimension.
3.
Move the pointer around until the preview indicates the dimension type you want.
4.
Right-click to lock the dimension type.
5.
Move the pointer around until the dimension is in the location you want.
6.
Click to place the dimension.
Point-to-Point Dimensions You can place a horizontal, vertical, or linear dimension between two sketch points, sketch segment endpoints, or model vertices. The model origin can also be one of the two points. Select the two points, then move the pointer around to observe the dimension preview. To create a dimension between two points:
1.
Click Smart Dimension
on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart.
2.
Click one point.
3.
Click the other point.
4.
Move the pointer to show the dimension preview.
5.
Click to place the desired dimension.
Point-to-Point Dimensions These distance dimensions were all created by selecting the same two points, then selecting a different location for each dimension.
Arc Dimensions The default dimension type for an arc is radius. You only need to select the arc for this dimension type. You can dimension the true length of the arc. To dimension the true length of an arc:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Click the arc.
3.
Click the two endpoints of the arc.
4.
Move the pointer to show the dimension preview.
5.
Click to place the dimension.
Arc Dimensions When you dimension an arc, the default dimension type is radius.
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To dimension the true length of an arc, select the arc and the two endpoints of the arc.
Circular Dimensions You can create a circular dimension as a diametrical dimension or as a linear dimension. By placing the dimension at an angle, the dimension is displayed as a diameter. By placing the dimension vertically or horizontally, it is displayed as a linear dimension. To create a circular dimension and then rotate the dimension around the circle:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Select the circle.
3.
Drag the dimension and click to place it.
4.
In the Modify box, set a value if necessary and click
.
If the Modify box does not appear, either double-click the dimension or select Input dimension value in Tools, Options, System Options, General. 5.
If the dmension is a diametrical dimension, select the dimension drag handle and drag to rotate the dimension to reposition it.
Circular Dimensions By placing the dimension at an angle, the dimension is displayed as a diameter.
By placing the dimension vertically or horizontally, it is displayed as a linear dimension. To modify the angle of a linear dimension, click the dimension, then drag the handle on the text. The dimension snaps to 15 degree increments.
To change the display of a circular dimension from linear to radial, right-click the dimension, select Properties, then clear the Display as linear dimension check box.
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Angular Dimensions Between Two Lines You can place an angular dimension between two lines or a line and a model edge. Select the two entities, then move the pointer to observe the dimension preview. The angle to be dimensioned changes based on the pointer position. To create an angular dimension between two lines:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Click one line.
3.
Click the second line.
4.
Move the pointer to show the angular dimension preview.
5.
Click to place the dimension.
Angular Dimensions These angular dimensions were all created by selecting the two sketch lines, then selecting a different location for each dimension.
Angular Dimensions Between Three Points You can place an angular dimension between three sketch points, sketch segment endpoints, or model vertices. The model origin can also be used as one of the three points. Select the point for the vertex of the angle, then select the other two points. To create an angular dimension between three points:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
2.
Click a point to be the vertex of the angle.
3.
Click the other two points.
4.
Move the pointer to show the angular dimension preview.
5.
Click to place the angular dimension.
SolidWorks 2004 Reference Guide
on the Dimensions/Relations toolbar, or click Tools,
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Chapter 3 Sketching
Dimensions Between Arcs or Circles By default, distances are measured to the center of an arc or circle. You can also dimension between concentric circles and use extension lines. To change the way the distance is measured:
1.
Right-click the dimension, and select Properties.
2.
Set First arc condition and Second arc condition, then click OK. In these examples, First arc condition is set to Center, and Second arc condition is set as shown.
Center
Min
Max
You can drag the extension lines to new attachment points in circles and arcs. The dimensions update automatically. In the following example, the extension line of the right circle is dragged from the Min attachment point to the Center. Attachment at Min
Attachment dragged to Center
You can drag an arc radial dimension, and the dimension moves automatically between outside and inside. Arc dimension inside
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Arc dimension outside
To dimension between concentric circles and display extension lines:
1.
In an open sketch, click Smart Dimension on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart.
2.
Click one concentric circle, then click the second concentric circle.
3.
To display extension lines, right-click. Extension lines
4.
Click to place the dimension. To display extension lines after placing the dimension, click the Select right-click the dimension and select Display Options, Show extension lines.
tool, then
Autodimension Use the Autodimension tool to automatically insert dimensions in a sketch. You can also autodimension a sketch to model entities. The Autodimension PropertyManager controls: Entities to Dimension •
All entities in sketch. Dimensions all entites in the sketch.
•
Selected entities. Dimensions only the selected entities.
Horizontal Dimensions •
Scheme. Sets the horizontal dimension scheme and sets the entity as the vertical point of origination for the dimensions.
•
Dimension placement o
Above sketch. Places dimensions above the sketch.
o
Below sketch. Places dimensions below the sketch.
Vertical Dimensions •
Scheme. Sets the vertical dimension scheme and sets the entity as the horizontal point of origination for the dimensions.
•
Dimension placement o
Left of sketch. Places dimensions to the left of the sketch.
o
Right of sketch. Places dimensions to the right of the sketch.
To autodimension a sketch:
1.
In an open sketch, click Autodimension Dimensions, Autodimension.
2.
Set the properties in the Autodimension PropertyManager.
3.
Click OK
SolidWorks 2004 Reference Guide
on the Dimensions/Relations toolbar, or click Tools,
.
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Chapter 3 Sketching
To autodimension a sketch to model entities:
1.
Create a sketch on a model face.
2.
In the open sketch, click Autodimension Dimensions, Autodimension.
on the Dimensions/Relations toolbar, or click Tools,
The color of the entities autodimensioned in the graphics area correspond to the colors shown in the PropertyManager. 3.
Click OK
.
Geometric Relations Click Add Relations on the Dimensions/Relations toolbar, or click Tools, Relations, Add to create geometric relations (such as tangent or perpendicular) between sketch entities, or between sketch entities and planes, axes, edges, or vertices. You can also add relations while you create individual sketch entities, or when you select two exisitng entities. Existing Relations and Add Relations sections appear in all sketch entity PropertyManagers. When you create relations, at least one of the items must be a sketch entity. The other item (or items) can be either a sketch entity or an edge, face, vertex, origin, plane, axis, or curve from another sketch that forms a line or arc when projected on the sketch plane. Geometric relations can also be created automatically. See Automatic Relations.
Automatic Relations You can choose whether geometric relations are automatically created as you create sketch entities. To turn automatic relations on or off:
Click Tools, Sketch Settings, Automatic Relations, or click Tools, Options, System Options, Sketch, and select Automatic Relations. As you sketch, the pointer changes shape to show you which relations can be created. When Automatic Relations is turned on, the relations are added.
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Horizontal
Vertical
Coincident
Midpoint
Intersection
Tangent
Perpendicular
Brown inference lines indicate that a relation is added automatically; blue inference lines indicate that no relation is added.
Add Relations/Properties PropertyManager The Add Relations PropertyManager appears when you click Add Relation on the Dimensions/Relations toolbar. The Properties PropertyManager appears when you select multiple sketch entities in the graphics area. You can create geometric relations between sketch entities, or between sketch entities and planes, axes, edges, or vertices. Selected Entities Displays the names of selected sketch entities. Add entities to the list by selecting them in the graphics area. Existing Relations •
Relations
•
Information on).
. Displays relations that exist for the selected sketch entity. . Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations •
You can add relations to the selected entities from the list. The list includes only relations that are possible for the selected entities. Equal
and Midpoint
relations are not available in 3D sketches.
When you add relations to entities, at least one item must be a sketch entity. Other items can include additional sketch entities, edges, faces, vertices, origins, planes, or axes. You can also include sketch curves from other sketches that form lines or arcs when projected onto the sketch plane. Options For construction. Converts the entities to construction geometry (not available in Add Relations PropertyManager).
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Chapter 3 Sketching
Sketch Relations The following table describes the entities that you can select for a relation and the characteristics of the resulting relation. Relation
Entities to select
Resulting relations
Horizontal or Vertical
One or more lines or two or more points.
The lines become horizontal or vertical (as defined by the current sketch space). Points are aligned horizontally or vertically.
Collinear
Two or more lines.
The items lie on the same infinite line.
Coradial
Two or more arcs.
The items share the same centerpoint and radius.
Perpendicular
Two lines.
The two items are perpendicular to each other.
Parallel
Two or more lines.
The items are parallel to each other.
A line and a plane (or a planar face) in a 3D sketch.
The line is parallel to the selected plane.
ParallelYZ
A line and a plane (or a planar face) in a 3D sketch.
The line is parallel to the YZ plane with respect to the selected plane.
ParallelZX
A line and a plane (or a planar face) in a 3D sketch.
The line is parallel to the ZX plane with respect to the selected plane.
AlongZ
A line and a plane (or a planar face) in a 3D sketch.
The line is normal to the face of the selected plane.
Tangent
An arc, ellipse, or spline, and The two items remain tangent. a line or arc.
Concentric
Two or more arcs, or a point The arcs share the same centerpoint. and an arc.
Midpoint
A point and a line.
The point remains at the midpoint of the line.
Intersection
Two lines and one point.
The point remains at the intersection of the lines.
Coincident
A point and a line, arc, or ellipse.
The point lies on the line, arc, or ellipse.
Equal
Two or more lines or two or more arcs.
The line lengths or radii remain equal.
Symmetric
A centerline and two points, lines, arcs, or ellipses.
The items remain equidistant from the centerline, on a line perpendicular to the centerline.
Fix
Any entity.
The entity’s size and location are fixed. However, the end points of a fixed line are free to move along the infinite line that underlies it. Also, the endpoints of an arc or elliptical segment are free to move along the underlying full circle or ellipse.
Pierce
A sketch point and an axis, edge, line, or spline.
The sketch point is coincident to where the axis, edge, or curve pierces the sketch plane. The pierce relation is used in Sweeps with Guide Curves.
Merge Points
Two sketch points or endpoints.
The two points are merged into a single point.
NOTES:
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•
When you create a relation to a line, the relation is to the infinite line, not just the sketched line segment or the physical edge. As a result, some items may not touch when you expect them to.
•
When you create a relation to an arc segment or elliptical segment, the relation is actually to the full circle or ellipse.
•
If you create a relation to an item that does not lie on the sketch plane, the resulting relation applies to the projection of that item as it appears on the sketch plane.
•
Additional relations are created automatically when you use Offset Entities and Convert Entities.
Sketch Relations Callouts In an open sketch, when you double-click a sketch entity in the graphics area, the PropertyManager opens and callouts appear for all the relations of the selected entity. Alternatively, when you select a relation under Relations graphics area.
in the PropertyManager, a callout appears in the
The callouts display the relations applied to the selected sketch entity and the names of the related sketch entities. The color of the callout specifies the status of the entity (under defined, over defined, dangling, and so on). The default system color for fully defined status is black. In the callouts, fully defined status is blue, the same as for under defined. The other colors in the callouts follow the system defaults. The status also appears next to Information
in the PropertyManager.
To delete a relation, select the relation under Relations, or select the callout in the graphics area, and press Delete. To open the Display/Delete Relations PropertyManager, double-click the callout .
Sketch Geometry Status Sketch geometry can be in any of the following states. The color in parenthesis indicates the color of the sketch state. •
Dangling (brown). The sketch geometry can no longer be resolved (for example, a dimension to a deleted entity).
•
Over Defined (red). The sketch geometry is either in conflict or is redundant.
•
Fully Defined (black). The sketch geometry fully describes all of the sketch entities.
•
Under Defined (blue). The sketch geometry is not defined and is free to change.
•
Not Solved (pink). The sketch geometry cannot determine the position of one or more sketch entities.
•
Driven (gray). The dimension’s value is driven by solving the sketch.
•
Invalid (yellow). This sketch geometry would be geometrically invalid if the sketch were solved.
Sketch Status Conventions Sketches can be in any of five states described below. The state of the sketch is displayed in the status bar at the bottom of the SolidWorks window. •
Fully Defined. All the lines and curves in the sketch, and their positions, are described by dimensions or relations, or both.
•
Over Defined. Some dimensions or relations, or both, are either in conflict or are redundant. To view and remove conflicting relations, see Display/Delete Relations PropertyManager.
•
Under Defined. Some of the dimensions or relations in the sketch are not defined and are free to change. You can drag endpoints, lines, or curves until the sketch entity changes shape.
•
No Solution Found. The sketch is not solved. The geometry, relations, and dimensions that prevent the solution of the sketch are displayed.
•
Invalid Solution Found. The sketch is solved but results in invalid geometry, such as a zero length line, zero radius arc, or self-intersecting spline.
With the SolidWorks software, it is not necessary to fully dimension or define sketches before you use them to create features. However, you should fully define sketches before you consider the part complete. To always use fully defined sketches to create features, click Tools, Options, System Options, Sketch, and select Use fully defined sketches.
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Chapter 3 Sketching
Display/Delete Relations PropertyManager The Display/Delete Relations PropertyManager appears when you click Display/Delete Relations Dimensions/Relations toolbar.
on the
Relations •
Filter. Specifies which relations to display, such as All in this sketch, Selected Entities, or any of the following: o
Dangling
o
Over Defined/Not Solved
o
External
o
Defined In Context
o
Locked
o
Broken
•
Selected Entities (available when Filter is set to Seleted Entities). Displays the names of entities you select in the sketch.
•
Relations . Displays existing relations based on the selected Filter. When you select a relation from the list, the names of the related entities are displayed under Entities and the sketch entity is highlighted in the graphics area. The status of external references is displayed the same as in the FeatureManager design tree.
•
Information . Displays the status of the selected sketch entity. If the relation was created within the context of an assembly, the status can be Broken or Locked.
•
Suppressed. Suppresses the relation for the current configuration. The name of the relation turns gray and the Information status changes (from Satisfied to Driven, for example).
• •
Undo last relation change . Deletes or replaces the last action. Delete and Delete All. Deletes the selected relations or deletes all the relations.
Entities •
Entities used in the selected relation: o o
o
Entity. Lists each selected sketch entity in Relations. Status. Displays the status of the selected sketch entity, such as Fully Defined, Under Defined, and so on. Defined In. Displays the location where the entity is defined, such as Current Sketch, Same Model, or External Model.
Information for external entities in assemblies: o
Entity. Displays the entity name for sketch entities in the Same Model or External Model.
o
Owner. Displays the part to which the sketch entity belongs
o
•
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Owner and Assembly. Displays the name of the top-level assembly where the relation was created for sketch entities in an External Model.
Replace. Replaces the selected entity with another entity. In the graphics area, select an entity for Entity to replace the one selected above, and click Replace. If the replacement is not appropriate, the status is Invalid. o
Undo last relation change
. Undoes the last Replace action.
o
Replace in all relations. Replaces the sketch entity in all relations.
Configurations For models with multiple configurations, you can apply the selected relations to This configuration, All configurations, or Specify configurations. If you select Specify configurations, select configurations in the Configurations list. Click All to select all the configurations in the list. Click Reset to reset the selections to the original settings.
Scan Equal Use the Scan Equal tool to scan a sketch for entities with equal lengths or radii, and set an Equal relation between sketch entities that are the same length or radius. To locate sketch entities with equal radii or line lengths:
1.
In an open sketch, click Scan Equal Scan Equal.
on the Dimensions/Relations toolbar, or click Tools, Relations,
If equal sketch entities exist, the appropriate selections are available: • Length. Two or more lines are equal.
2.
3.
4.
•
Radii. Two or more arcs have equal radii.
•
Both. An arc has a radii equal to a line length.
To see the equal sketch entities, select one of the available selections. The following occurs: •
The entities are highlighted in the sketch.
•
Value. Displays the length or radii.
•
Line Count and Arc Count. Displays the number of equal entities.
Click for additional options: •
Find Next. Available if additional sets of equal entities exist.
•
Set Equal. Creates an Equal relation between the highlighted entities.
Click Close.
External vs. Defined in Context External - A relation that is "External" is a relation between a sketch entity and something outside of that sketch. This thing can be an edge or vertex within the same model or it can be an edge or vertex within a different model within an assembly. Defined in Context - A relation that is "Defined in Context" is a relation between a sketch entity in one part and some entity in another part. This relation occurs within the context of the assembly. Entities that are "Defined in Context" are listed as "External" because they have relations outside of the sketch. However, not all "External" relations are "Defined in Context" because they may be relations within the same part file.
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Chapter 3 Sketching
Splines Splines You can create spline curves. Splines can have as few as two points, and you can specify tangency at the end points. You can create spline curves in 3D sketches. To create a spline:
1.
Click Spline
on the Sketch toolbar, or Tools, Sketch Entities, Spline.
The pointer changes to
.
2.
Click to place the first point and drag out the first segment.
3.
Click the endpoint and drag out the second segment.
4.
Repeat until the spline is complete. Alternatively, you can click on each through point to create the spline, then double-click when the spline is complete.
To add relations to the spline points:
Select points and use Add Relations in the active PropertyManager to specify relations between spline points or endpoints. To reshape a spline:
1.
In an open sketch, select the spline. Handles appear on the through points and the segment end points.
2.
You can modify the spline using the following techniques: •
Drag the handles.
•
Remove through spline points.
•
Right-click and select Spline Point, Moving Frame, or Simplify Spline.
To change the properties of a spline:
In an open sketch, select a spline and edit its properties in the Spline PropertyManager. You can specify the spline to be Proportional. To create a two-point spline with tangency:
1.
In an open sketch, click Spline points.
on the Sketch toolbar and sketch a spline with three or more spline
2.
Right-click the spline and select Simplify Spline.
3.
In the dialog box, click Smooth until the spline contains only two points, then click OK. The endpoints of the spline retain their slope. You can also add tangency to a two-point spline by adding a relation as described above.
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Add tangent relation between spline and line
Simplify spline to two points with slope retained
Proportional Splines A newly created spline is non-proportional by default. You can change its shape by dragging a spline point or endpoint. A proportional spline retains its shape when you drag the endpoints; the entire spline resizes proportionally. You can add dimensions and relations to internal points of proportional splines.
Spline PropertyManager The Spline PropertyManager controls the following properties of a sketched Spline: Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You cannot add relations to splines. You can add relations to the spline points. Click a point on the spline to add a relation. Options For construction. Converts the entity to construction geometry. Parameters Specify any appropriate combination of the following parameters to define the spline if the spline is not constrained by relations. Spline Point Number. Highlights the selected spline point in the graphics area. X Coordinate. Specifies the x coordinate of the spline point. Y Coordinate. Specifies the y coordinate of the spline point. Proportional.Retains the spline shape when you drag an endpoint; the entire spline resizes proportionally.
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Chapter 3 Sketching
Fit Spline Use the Fit Spline tool to fit sketch segments to a spline. Fit splines are parametrically linked to underlying geometry so that changes to the geometry update the spline. Fit spline chooses the most logical fit to the geometry you select, but you can modify the fit. If you select an entity that has been fit, the entity is no longer part of the spline. If you select an entity that is not part of the spline, the spline adjusts to include the selected entity. You can also include model edges in a fit spline. However, you cannot constrain other geometry to the splines.
Sketch has four entities
Fit Spline tool converts the geometry to a single spline
The Fit Spline PropertyManager controls: Parameters •
Delete geometry. Deletes the original sketch segments from the sketch. Otherwise, the segments remain as construction geometry separate from the spline. When cleared, you can select the Constrained, Unconstrained, or Fixed options.
•
Closed spline. Creates a closed contour spline.
•
Constrained. Parametrically links the fitted spline to the defining geometry.
•
Unconstrained. Creates the fitted spline as the same shape as the original defining geometry but with no constraints. You can dimension, constrain, and drag the spline.
•
Fixed. Creates the fitted spline as the same shape as defining geometry but it is fixed in space.
•
Edit Chaining. Allows you to edit the chain of splines created. Editing applies only to the order of the noncontiguous spline elements, not the sketch entities. Click
or
to undo or redo the edits.
Tolerance •
Tolerance
. Specifies the maximum deviation allowed from the original sketch segments.
•
Actual Deviation. Updates based on the Tolerance value and the geometry selected. This is automatically calculated.
To fit sketch segments to a spline:
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1.
In an open sketch, click Tools, Spline Tools, Fit Spline.
2.
In the graphics area, click the sketch entities to fit to the spline.
3.
Set the properties in the Fit Spline PropertyManager.
4.
Click OK
.
Simplify Spline Use the Simplify Spline tool to reduce the number of points in a spline and to increase system performance in models with complex spline curves. You can also simplify splines that were created from imported models or from tools such as Convert Entities, Offset Entities, Intersection Curve, and Face Curves. To simplify a spline:
1.
In an open sketch, select the spline in the graphics area, then click Simplify Spline toolbar, or click Tools, Spline Tools, Simplify Spline.
on the Spline Tools
2.
In the dialog box, set a value for Tolerance and press Enter, or click Smooth. (You can continue to click Smooth until only two spline points remain). The SolidWorks software: •
Adjusts the tolerance and calculates a new curve with fewer spline points. The original spline is displayed in the graphics area along with a preview of the smoothed curve.
•
Displays the Number of spline points in In original curve and In simplified curve.
•
Displays the simplified Tolerance, which measures the intended deviation of the simplified curve from the original curve. Click Previous to return through the sequence as far as the original curve.
3.
Click OK.
Insert Spline Point The Insert Spline Point command adds one or more points to the spline. With spline points, you can: •
Use spline points as handles to pull the spline into the shape you want
•
Add dimensions between spline points or between spline points and other entities
•
Add relations to spline points
To insert spline points:
1.
In an open sketch, right-click the spline and select Insert Spline Point, or click Tools, Spline Tools, Insert Spline Point. The pointer changes to
2.
. If the pointer is not on the spline, the pointer changes to
.
Click one or more places on the spline where you want to insert a point.
To delete spline points:
In an open sketch, select a point and press Delete.
Moving Frame The moving frame is a way to manipulate a spline without adding points. You can use the moving frame in a part or drawing document. The moving frame is available for both 2D or 3D splines. NOTE: The moving frame can be used with splines created in SolidWorks that you are able to modify. It cannot be used with imported or converted splines.
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Chapter 3 Sketching
To add a moving frame to a spline:
Right-click the sketched spline and select Moving Frame. You can use the moving frame in the following ways:
•
Drag the moving frame by the frame point to move it along the spline to wherever you want to place it.
•
Pull the frame handles to change the shape of the spline curve. Select the frame and modify the X and Y coordinates of the frame point by entering new values in the Frame Point Properties PropertyManager.
•
•
Add multiple moving frames to a spline, making it possible to control the curve of the spline where there are no spline points. Only the active frame is fully displayed. Other frames are displayed as small triangles on the outside of the curve.
•
When used in conjunction with Curvature Comb, the center handle of each moving frame joins with the curvature comb.
Frame Point PropertyManager The Frame Point Properties PropertyManager controls the following properties of a spline Moving Frame: Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity.
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Parameters You can specify any appropriate combination of the following parameters to define the frame point if the frame point is not constrained by relations. When you change one or more parameters, the other parameters update automatically. X Coordinate Y Coordinate Curvature - of the spline at the frame point Tangency - of the moving frame at the frame point
3D Frame Point PropertyManager The 3D Frame Point PropertyManager controls the following properties of a spline Moving Frame: Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined and so on) is
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Parameters You can specify any appropriate combination of the following parameters to define the frame point if the frame point is not constrained by relations. When you change one or more parameters, the other parameters update automatically. X Coordinate Y Coordinate Z Coordinate Curvature - of the spline at the frame point Tangency - in the XY plane Tangency - in the XZ plane Tangency - in the YZ plane
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Chapter 3 Sketching
Curvature Combs Curvature combs provide visual enhancement of the slope and curvature of most sketch entities in part, assembly, and drawing documents.
To show the curvature combs of a sketch entity:
1.
In an open sketch, right-click a sketch entity and select Show Curvature Combs. A comb appears that displays the curvature of the entity. For splines, the comb crosses the spline at inflection points. The comb changes shape dynamically as you drag the sketch entity and its curvature changes.
2.
In the PropertyManager, move the Scale slider to adjust the size of the curvature comb.
3.
Click OK
.
The comb remains visible when you close the sketch (unless the sketch is made into a feature). To change the scale of all curvature combs in a sketch:
1.
In an open sketch, right-click a sketch entity with curvature combs displayed and select Modify Curvature Scale.
2.
In the PropertyManager, move the Scale slider to adjust the size of the curvature comb.
3.
Click OK
.
To hide the curvature comb of a sketch entity:
In an open sketch, right-click the sketch entity and select Show Curvature Combs.
Curvature Scale The Scale slider adjusts the size of all the curvature combs in the active sketch.
Inflection Points The Show Inflection Points tool displays all points where the concavity of a spline changes. The inflection point symbol appears at the point where the spline changes from concave to convex. To display inflection points of a spline:
In an active spline sketch, select a spline, right-click, and select Show Inflection Points. The inflection points appear.
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Minimum Radius The Show Minimum Radius tool displays the radial measurement of the curve with the smallest radius of a spline. To display the minimum radius of a spline:
In an active spline sketch, select a spline, right-click, and select Show Minimum Radius. The minimum radius curve appears with the radial measurement.
2D Sketching Line Creates a sketched line. To sketch a line:
1.
Click Line
on the Sketch toolbar, or click Tools, Sketch Entities, Line.
The pointer changes to
.
2.
Click in the graphics area to start the line.
3.
Complete the line in one of the following ways: •
Drag the pointer to the end of the line and release.
•
Release the pointer, move the pointer to the end of the line, and click again. A horizontal or vertical line automatically snaps to the grid points if grid snap is on.
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Chapter 3 Sketching
To modify the line by dragging:
In an open sketch, do one of the following: •
To change the length of the line, select one of the endpoints and drag to lengthen or shorten the line.
•
To move the line, select the line and drag the line to another position.
•
To change the angle of a line, select an endpoint and drag to a different angle. If the line has a vertical or horizontal relation, delete the vertical or horizontal relation in the Line PropertyManager before dragging to a new angle.
To change the line properties:
In an open sketch, select a line and edit its properties in the Line PropertyManager.
Line PropertyManager The Line PropertyManager controls the following properties of a sketched Line. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the line if the line is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Start X Coordinate Start Y Coordinate End X Coordinate End Y Coordinate Length Angle. Relative to the grid, with horizontal 180°, vertical 90°, and the positive direction counterclockwise. Delta X. Difference between the start and end X coordinates. Delta Y. Difference between the start and end Y coordinates.
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Points You can insert points into sketches and drawings. To create sketch points:
1.
Click Point
on the Sketch toolbar, or Tools, Sketch Entities, Point.
The pointer changes to 2.
.
Click in the graphics area to place the point. The Point tool remains active so you can continue to insert points.
To change the properties of a point:
In an open sketch, select a point and edit its properties in the Point PropertyManager.
Point PropertyManager The Point PropertyManager controls the following properties of a sketched Point. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Parameters You can specify the following parameters to define the point if the point is not constrained by relations. X Coordinate Y Coordinate
Circle You can create a sketched circle. To create a circle:
1.
Click Circle on the Sketch toolbar, or click Tools, Sketch Entities, Circle. The pointer changes to
.
2.
Click in the graphics area to place the center of the circle.
3.
Move the pointer and click to set the radius.
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To modify a circle by dragging:
In an open sketch: • • •
Enlarge the circle by dragging its edge away from its center point. Make the circle smaller by dragging its edge toward its center point. Move the circle by dragging its center point.
To change the properties of a circle:
In an open sketch, select the circle and edit its properties in the Circle PropertyManager.
Circle PropertyManager The Circle PropertyManager controls the following properties of a sketched Circle. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the circle if the circle is not constrained by relations. Center X Coordinate Center Y Coordinate Radius
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Ellipse Use the Ellipse tool to create a complete ellipse. Use the Partial Ellipse tool to create an elliptical arc. To create an ellipse:
1.
Click Ellipse
on the Sketch toolbar, or Tools, Sketch Entities, Ellipse.
The pointer changes to
.
2.
Click in the graphics area to place the center of the ellipse.
3.
Drag and click to set the major axis of the ellipse.
4.
Drag and click again to set the minor axis of the ellipse.
To change the properties of an ellipse:
In an open sketch, select the ellipse and edit the properties in the Ellipse PropertyManager.
Partial Ellipse You can create a partial ellipse (an elliptical arc) from a centerpoint, a start point, and an end point, similar to creating a Centerpoint Arc. To create a partial ellipse:
1.
In an open sketch, click Partial Ellipse Ellipse. The pointer changes to
on the Sketch toolbar, or click Tools, Sketch Entities, Partial
.
2.
Click in the graphics area to place the center of the ellipse.
3.
Drag and click to define one axis of the ellipse.
4.
Drag and click to define the second axis. The circumference guideline remains.
5.
Drag the pointer around the circumference to define the extent of the ellipse, then click to complete the ellipse.
To change the partial ellipse properties:
In an open sketch, select the ellipse and edit its properties in the Ellipse PropertyManager.
Ellipse PropertyManager The Ellipse PropertyManager controls the following properties of a sketched Ellipse or Partial Ellipse. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity.
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Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the ellipse if the ellipse is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Some parameters are available only for a Partial Ellipse. Center X Coordinate Center Y Coordinate Start X Coordinate (Partial Ellipse only) Start Y Coordinate (Partial Ellipse only) End X Coordinate (Partial Ellipse only) End Y Coordinate (Partial Ellipse only) Radius 1 Radius 2 Angle (Partial Ellipse only)
Centerlines Use centerlines to create symmetrical sketch elements (see Mirror Entities) and revolved features (see Revolve), or as construction geometry. To create a centerline:
1.
Click Centerline
on the Sketch toolbar, or click Tools, Sketch Entities, Centerline.
The pointer changes to
.
2.
Click to start the centerline.
3.
Drag, or move the pointer and click, to set the end of the centerline.
To change the centerline properties:
In an open sketch, select a centerline and edit its properties in the Line PropertyManager.
Virtual Sharp A virtual sharp creates a sketch point at the virtual intersection point of two sketch entities. Dimensions and relations to the virtual intersection point are retained even if the actual intersection no longer exists, such as when a corner is removed by a fillet or chamfer. To create a virtual sharp:
1.
In an open sketch, hold down Ctrl and select two sketch entities.
2.
Click Point
on the Sketch toolbar, or click Tools, Sketch Entities, Point.
A virtual sharp appears at the point where the sketch entities would intersect. Set the virtual sharp display style in Tools, Options, Document Properties, Virtual Sharps.
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Centerpoint Arc Use the Centerpoint Arc tool to create an arc from a centerpoint, a start point, and an end point. To create a centerpoint arc:
1.
In an open sketch, click Centerpoint Arc Centerpoint Arc. The pointer changes to
on the Sketch toolbar, or click Tools, Sketch Entities,
.
2.
Click in the graphics area to place the start point of the arc, then click where you want to place the end point of the arc.
3.
Drag to set the angle and the radius of the arc.
4.
Click to place the arc.
5.
Set the properties in the Arc PropertyManager.
6.
Click OK
.
To change the properties of the arc:
In an open sketch, select the arc and edit the properties in the Arc PropertyManager.
Tangent Arcs Creates an arc, tangent to a sketch entity. You can transition from sketching a line to sketching a tangent arc without selecting the Tangent Arc tool by autotransitioning. To create a tangent arc:
1.
Click Tangent Arc
on the Sketch Tools toolbar, or Tools, Sketch Entity, Tangent Arc.
2.
Click the pointer on the end point of a line, arc, ellipse, or spline. The Arc PropertyManager appears and the pointer changes to
3.
.
Drag the arc to the desired shape. NOTE: SolidWorks infers from the pointer motion whether you want a tangent or normal arc. There are four intent zones, with eight possible results as shown. Moving the pointer in a tangent direction creates a tangent arc. Moving the pointer in a normal direction creates a normal arc. You can toggle between tangent and normal arcs by returning to the end point and moving away in a new direction.
4.
Release the mouse button.
To change the properties of the arc, select the arc to open the Arc PropertyManager.
3 Point Arc You can create an arc by specifying three points (start, end, and midpoint). To create a 3 point arc:
1.
Click 3 Point Arc
on the Sketch toolbar, or click Tools, Sketch Entities, 3 Point Arc.
The Arc PropertyManager appears and the pointer changes to
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2.
Click where you want the arc to start.
3.
Drag to where you want the arc to end.
4.
Release the pointer.
5.
Drag the arc to set the radius and to reverse the arc, if necessary.
6.
Release the pointer.
7.
Make any necessary changes in the PropertyManager and click OK
.
To change the properties of the arc:
Select the arc and edit the properties in the Arc PropertyManager.
Arc PropertyManager The Arc PropertyManager controls the following properties of a sketched Centerpoint Arc, Tangent Arc, or 3 Point Arc. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entities to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the arc if the arc is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Center X Coordinate Center Y Coordinate Start X Coordinate Start Y Coordinate End X Coordinate End Y Coordinate Radius Angle. Subtended by the arc.
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Parabolas You can create a parabolic curve. To create a parabola:
1.
Click Parabola
on the Sketch toolbar, or Tools, Sketch Entities, Parabola.
The pointer changes to 2.
.
Click to place the focus of the parabola and drag to enlarge the parabola. The parabola is outlined.
3.
Click on the parabola and drag to define the extent of the curve.
To modify the parabola:
1.
In an open sketch, select a parabola. (The pointer changes to
2.
Drag the vertex to shape the curve. The pointer changes to • •
when it is over a parabola.) when you select the vertex.
To flatten the curve, drag the vertex away from the focus. To make a sharper curve, drag the vertex closer to the focus. A move icon appears next to the pointer when you move the vertex.
•
To change the length of a side of the parabola without modifying the curve of the parabola, select an endpoint and drag.
•
To move the parabola to a new location, select the curve of the parabola and drag.
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•
To modify the length of both sides of the parabola without changing the arc of the parabola, drag the parabola away from its endpoints.
To change the properties of a parabola:
In an open sketch, select a parabola and edit its properties in the Parabola PropertyManager.
Parabola PropertyManager The Parabola PropertyManager controls the following properties of a sketched Parabola. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the parabola if the parabola is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Start X Coordinate Start Y Coordinate End X Coordinate End Y Coordinate Center X Coordinate Center Y Coordinate Apex X Coordinate Apex Y Coordinate
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Polygons You can create equilateral polygons with any number of sides between 3 and 40. To create a polygon:
1.
Click Polygon
on the Sketch toolbar, or click Tools, Sketch Entities, Polygon.
The pointer changes to
.
2.
Set the properties in the Polygon PropertyManager as necessary.
3.
Click in the graphics area to place the center of the polygon, and drag out the polygon.
4.
To sketch another polygon, click New Polygon and repeat steps 2 through 5.
5.
Click OK
.
The Polygon tool is still active. You can create additional polygons, although the PropertyManager does not open. To release the tool, click the tool on the Sketch toolbar, click another tool, or press Esc. To modify the polygon by dragging:
In an open sketch: •
Resize the polygon by dragging it by one of its sides. - or -
•
Move the polygon by dragging one of its vertices or its center point.
To edit a polygon:
1.
In an open sketch, select one of the sides of the polygon and click Tools, Sketch Tools, Edit Polygon. - or Right-click a side of the polygon and select Edit polygon.
2.
Modify the polygon in the Polygon PropertyManager.
Polygon PropertyManager The Polygon PropertyManager controls the following properties during creation of a sketched Polygon. Existing Relations No relations exist for polygons. Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You cannot add relations to polygons. However, you can add relations to the points and lines of polygons. Options For construction. Converts the entity to construction geometry.
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Parameters You can specify any appropriate combination of the following parameters to define the polygon. When you change one or more parameters, the other parameters update automatically. •
Number of Sides
. Sets the number of sides in the polygon. A polygon can have 3 to 40 sides.
•
Inscribed circle. Displays an inscribed circle inside the polygon to define the size of the polygon. The circle is construction geometry.
•
Circumscribed circle. Displays a circumscribed circle outside of the polygon to define the size of the polygon. The circle is construction geometry.
•
Center X Coordinate
. Displays the X coordinate for the center of the polygon.
•
Center Y Coordinate
. Displays the Y coordinate for the center of the polygon.
•
Circle Diameter
•
Angle
•
New Polygon. Lets you to create another polygon.
. Displays the diameter of the inscribed or circumscribed circle.
. Displays the angle of rotation.
Rectangles You can create rectangles whose sides are horizontal or vertical with respect to the sketch grid. For rectangles whose sides are at a different orientation, create a Parallelogram. To create a rectangle:
1.
Click Rectangle
on the Sketch toolbar, or Tools, Sketch Entities, Rectangle.
The pointer changes to 2.
.
Click to place the first corner of the rectangle, drag, and release when the rectangle is the correct size and shape. Instead of dragging, you can move the pointer and click again (click-click mode).
While dragging, the dimensions of the rectangle are dynamically displayed.
To change the size or shape of a rectangle:
In an open sketch, drag a side or vertex. You can force sketch segments to detach when you drag them. Click Tools, Sketch Settings, Detach Segment on Drag. To change the properties of an individual line in the rectangle:
In an open sketch, select the line and edit the properties in the Line PropertyManager.
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Parallelograms You can create a parallelogram and also create a rectangle whose sides are not horizontal or vertical with respect to the sketch grid. To create a parallelogram:
1.
2.
Click Parallelogram
on the Sketch toolbar, or click Tools, Sketch Entities, Parallelogram.
The pointer changes to
.
Click to place the first corner of the parallelogram, drag, and release when one edge of the parallelogram is the correct length. Instead of dragging, you can move the pointer and click again (click-click mode).
3.
Click again and drag until the parallelogram is the correct size and shape. •
Press Ctrl while dragging to create a parallelogram at any angle. You can reshape and resize the parallelogram by dragging its corners and sides.
•
Drag without pressing Ctrl to create a rectangle at an angle. You can resize the rectangle by dragging its corners and sides. You cannot change the angle of the rectangle by dragging.
Text You can sketch text on the face of a part and extrude or cut the text. The text can be inserted on any set of continuous curves or edges, including circles or profiles made up of lines, arcs, or splines. Example of Sketch Text The text is sketched along the outside edge of the face of the part, formatted, then cut.
A sketched spline creates an offset edge. A second sketch places the text on the offset line. The text is formatted, then extruded.
If the curve is a sketch entity, or a set of sketch entities, and the sketch text is in the same sketch as the curve, convert the sketch entities to construction geometry.
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To sketch text on a part:
1.
Click a face of a part. Click Text
on the Sketch toolbar, or click Tools, Sketch Entities, Text.
To create a profile for placing the text, sketch a circle or a continuous profile from lines, arcs, or splines in a sketch, close the sketch, then open another sketch for the text. 2.
In the graphics area, select an edge, curve, sketch, or sketch segment. The selected item appears under Curves
3.
.
In the PropertyManager, under Text, type the text to display. The text appears in the graphics area as you type.
4.
Set the properties in the Sketch Text PropertyManager as necessary.
5.
Click OK
6.
With the sketch still open, Extrude or Cut the text.
.
To edit sketch text:
1.
In an open sketch, right-click the text (the pointer changes to Properties.
when it is over the sketch text) and select
2.
Edit the text and its properties in the Sketch Text PropertyManager as necessary.
Sketch Text PropertyManager You can sketch text on the face of a part and extrude or cut the text. The text can be inserted on any set of continuous curves or edges, including circles or profiles made up of lines, arcs, or splines. You can specify the following properties in the Sketch Text PropertyManager. Curves Select edges, curves, sketches, or sketch segments. The name of the selected entity appears in the box, and the text appears along the entity. Text •
Text. Type text in the Text box. The text appears along the selected entity in the graphics area. If no entity is selected, the text appears horizonally starting at the origin.
•
Style. You can select individual characters, or groups of characters, to apply Bold Rotate
or Italic
or to
.
Click Rotate to rotate the selected text 30 degrees counterclockwise. For other rotation angles, click Rotate and then edit the code in the Text box. For example, for an angle of 10 degrees clockwise, replace with . To return to zero degrees rotation, delete the code and brackets. For angles of 180 degrees, use the Flip Vertical or Flip Horizontal buttons. •
Alignment. Justify the text Left Align , Center Align , Right Align Alignment is available only for text along a curve, edge, or sketch segment.
•
Flip. Flip the text in the Flip Vertical
•
and back . Flip Vertical is available only for text along a curve, edge, or sketch segment. Width Factor . Widen each character evenly by the specified percentage. Width Factor is not available when Use document's font is selected
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direction and back
, or Full Justify
, or in the Flip Horizontal
.
direction
•
Spacing . Change the spacing between each character by the specified percentage. Spacing is not available when the text is fully justified or when Use document's font is selected.
•
Use document's font. Clear to choose another font.
•
Font. Click to open the Font dialog box and choose a font style and size.
Sketch Picture You can insert a picture (.bmp, .gif, .jpg, .jpeg, .tif, and .wmf) on a sketch plane. Pictures can be used as an underlay for creating 2D sketches. The Sketch Picture PropertyManager controls the picture's position, size, angle, orientation, and aspect ratio setting. •
The picture is inserted with its (0, 0) coordinate at the sketch origin, an initial size of 1 pixel per 1 mm, and locked aspect ratio.
•
The picture is embedded in the document (not linked). If you change the original image, the sketch picture does not update.
•
If you sketch on top of the picture, there is no snap to picture, inferencing, or autotracing capability. If the image is moved, or deleted and replaced, the sketch does not update.
•
If you hide the sketch, the picture is also hidden.
•
Pictures can be inserted into assemblies when editing a part in context, but they cannot be inserted into assembly sketches.
Example of Sketch Picture A sketch picture is inserted with its (0, 0) coordinate at the sketch origin.
To insert a picture on a sketch plane:
1.
In an open sketch, click Sketch Picture Picture.
on the Sketch toolbar, or click Tools, Sketch Tools, Sketch
2.
In the dialog box, browse to the picture file and click Open. The picture is inserted.
3.
Set the properties in the Sketch Picture PropertyManager as necessary. You can resize the picture in the graphics area by dragging its handles. You can drag the picture without changing its size when the pointer changes to
4.
Click OK
.
.
To edit the picture after you have inserted it, double-click the picture.
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Sketch Picture PropertyManager You can insert a sketch picture onto either side of a sketch plane. The Sketch Picture PropertyManager controls the following properties. Origin X Position. Enter an X coordinate value for the origin of the picture. Origin Y Position. Enter a Y coordinate value for the origin of the picture. Angle. Enter a value in degrees. A positive angle rotates the picture counterclockwise. Width. Enter a value for the picture width. If Lock Aspect Ratio is selected, the height adjusts automatically. Height. Enter a value for the picture height. If Lock Aspect Ratio is selected, the width adjusts automatically. Lock Aspect Ratio. Select to keep a fixed width and height aspect ratio. Flip Horizontally. Click to flip the picture horizontally within its borders. Flip Vertically. Click to flip the picture vertically within its borders. NOTE: Values in the Sketch Picture PropertyManager update automatically when you change the size or position of the picture in the graphics area.
3D Sketching 3D Sketching A 3D sketch consists of lines and arcs in series, and splines. You can use a 3D sketch as a sweep path, as a guide curve for a loft or sweep, a centerline for a loft, or as one of the key entities in a routing system. (The routing functionality is an add-in application.) To begin a 3D sketch, click 3D Sketch on the Sketch toolbar, or click Insert, 3D Sketch. A space handle helps you maintain orientation while sketching on several planes. By default, you sketch relative to the default coordinate system in the model. To switch to one of the other two default planes, click the sketch tool and press Tab. The origin of the current sketch plane is displayed. Before you begin a 3D sketch, change the view orientation to Isometric. It is easier to create a 3D sketch in an isometric orientation because the X, Y, and Z directions are visible. The sketch tools available in 3D sketching are: Line creates 3D lines. Spline creates 3D splines. Point creates 3D points. Centerline creates construction geometry. Convert Entities creates one or more entities in a 3D sketch by projecting an edge, loop, face, external curve, external sketch contour, set of edges, or set of external curves onto the sketch plane. Face Curves extracts 3D iso-parametric curves from faces or surfaces.
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Sketch Fillet rounds the intersections of sketched lines. Sketch Chamfer bevels the intersections of sketched lines. Intersection Curve creates a sketched curve at intersections. Trim Entities trims or extends a sketch entity in a 3D sketch. Extend Entities extends a sketch entity in a 3D sketch. Construction Geometry converts sketched curves in a 3D sketch to construction geometry. As you sketch a line, the line snaps to one of the major directions, X, Y, or Z, if applicable, and is constrained as Horizontal, Vertical, or Along Z, respectively. The relations are added with respect to the current coordinate system for the 3D sketch. See Dimensioning a 3D Sketch. You are not restricted to drawing lines along one of the three major directions. You can sketch in the current sketch plane at an angle to one of the major directions, or you can sketch out-of-plane if the endpoint of the line snaps to existing model geometry.
To create an arc in a 3D sketch:
1.
Click Sketch Fillet
on the Sketch toolbar, or click Tools, Sketch Tools, Fillet.
2.
In the PropertyManager, under Fillet Parameters, set the Radius
3.
Select two intersecting line segments, or select their intersection. Selecting an intersection
.
Three intersections filleted
Line Snap While you create a line in a 3D sketch, you can snap the line to geometry that already exists in the part, such as model surfaces or vertices, and sketch points. •
Snap is not enabled if you are sketching in one of the major coordinate directions.
•
If you are sketching on a plane, and the SolidWorks software infers a snap to a non-planar point, a temporary 3D graphics box is displayed to indicate an off-planar snap.
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3D Lines You can create lines in 3D sketches. To create a line in a 3D sketch:
1.
Click 3D Sketch
on the Sketch toolbar, or click Insert, 3D Sketch.
2.
Click Standard Views directions.
3.
Click Line
4.
Click in the graphics area to start the line.
, then select Isometric
on the View toolbar so you can view all three
on the Sketch toolbar, or click Tools, Sketch Entities, Line.
The 3D Line PropertyManager appears and the pointer changes to
.
Each time you click, the space handle appears to help you sketch on the different planes.
5.
If you want to change planes, press Tab.
6.
Drag to where you want the line segment to end.
7.
To continue the line, select the end point and press Tab to change to another plane if necessary.
8.
Drag the second segment and release the pointer.
To modify the line by dragging:
•
To change the length of the line, select one of the endpoints and drag to lengthen or shorten the line.
•
To move the line, select the line and drag the line to another position.
To change the line properties:
In a 3D sketch, select a line and edit its properties in the Line PropertyManager.
3D Line PropertyManager The 3D Line PropertyManager controls the following properties of a sketched 3D Line. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry.
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Parameters You can specify any appropriate combination of the following parameters to define the line if the line is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Start X Coordinate Start Y Coordinate Start Z Coordinate End X Coordinate End Y Coordinate End Z Coordinate Length Angle. Relative to the grid, with horizontal 180°, vertical 90°, and the positive direction counterclockwise. Delta X. Difference between the start and end X coordinates. Delta Y. Difference between the start and end Y coordinates. Delta Z. Difference between the start and end Z coordinates.
3D Splines You can create splines in 3D sketches. To create a spline in a 3D sketch:
1.
Click 3D Sketch
on the Sketch toolbar, or Insert, 3D Sketch to open a 3D sketch.
2.
Click Standard Views directions.
3.
Click Spline
4.
Click in the graphics area to place the first point and drag the first segment.
, then select Isometric
on the View toolbar so you can see all three
on the Sketch toolbar, or Tools, Sketch Entities, Spline.
The Spline PropertyManager appears. Each time you click, the space handle appears to help you sketch on the different planes.
5.
If you want to change planes, press Tab.
6.
Select the endpoint and drag the second segment.
7.
Repeat until the spline is complete. Alternatively, you can click to place each through point, then double-click to place the endpoint and complete the spline.
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To add relations to the spline points:
Select points and add relations between points or endpoints, or between the spline points and other sketch entities in the Point PropertyManager. To reshape a spline:
1.
In a 3D sketch, select the spline. Handles appear on the through points and endpoints.
2.
You can modify the spline using the following techniques. •
Drag the handles to reshape the spline.
•
Add or remove through spline points to aid in shaping the spline. Right-click the spline and select Spline Point, or select a spline point and press Delete.
•
Insert a moving frame along the curve of the spline to manipulate the spline shape. Right-click the spline and select Moving Frame.
•
Smooth the spline. Right-click the spline and select Simplify Spline.
To change the properties of a spline:
In a 3D sketch, select a spline and edit its properties in the Spline PropertyManager.
3D Spline PropertyManager The 3D Spline PropertyManager controls the following properties of a sketched 3D Spline: Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined, and so on) is
Add Relations You cannot add relations to splines. NOTE: You can add relations to the spline points. Click a point on the spline to add a relation. Options Select the For construction check box to convert the entity to construction geometry. Parameters Specify any appropriate combination of the following parameters to define the spline if the spline is not constrained by relations. Spline Point Number. When you scroll through the points, the corresponding coordinates appear below X Coordinate. The x coordinate of the spline point. Y Coordinate. The y coordinate of the spline point. Z Coordinate. The z coordinate of the spline point. Proportional. A proportional spline retains its shape when you drag the endpoints; the entire spline resizes proportionally. You can add dimensions and relations to internal points of proportional splines.
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3D Points You can insert points into 3D sketches. To create sketch points in a 3D sketch:
1.
Click 3D Sketch
on the Sketch toolbar, or Insert, 3D Sketch to open a 3D sketch.
2.
Click Standard Views directions.
3.
Click Point
4.
Click in the graphics area to place the point.
, then select Isometric
on the View toolbar so you can view all three
on the Sketch toolbar, or Tools, Sketch Entities, Point.
The Point PropertyManager appears. The Point tool stays active so you can continue to insert points. To change the properties of a point:
In a 3D sketch, select the point and edit its properties in the Point PropertyManager.
3D Point PropertyManager The 3D Point PropertyManager controls the following properties of a sketched 3D Point. Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area. NOTE: When you sketch a 3D point on a face or surface, the point automatically has a coincident relation with the face or surface.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined and so on) is
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Parameters You can specify the following parameters to define the point if the point is not constrained by relations. X Coordinate Y Coordinate Z Coordinate
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3D Circle PropertyManager The 3D Circle PropertyManager controls the following properties of a 3D Circle. To create a circle in a 3D sketch, open a 3D Sketch on a circular face of a part, click Convert Entities
, and select the circular edge.
Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined and so on) is
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options Select the For construction check box to convert the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the circle if the circle is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Center X Coordinate Center Y Coordinate Center Z Coordinate Radius
Coordinate System - 3D Sketching When creating a 3D sketch, by default, you sketch relative to the default coordinate system in the model. To switch to one of the other two default planes, click the desired sketch tool, and press the Tab key. The origin of the current sketch plane is displayed.
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•
To change the coordinate system for your 3D sketch, click the desired sketch tool, hold down the Ctrl key, and click a plane, a planar face, or a user-defined coordinate system.
•
If you select a plane or a planar face, the 3D sketch planes rotate so that the XY sketch plane is aligned with the selected item.
•
If you select a coordinate system, the 3D sketch planes rotate so that the XY sketch plane is parallel to the XY plane of the coordinate system.
Space Handle When working in a 3D sketch, a graphical assistant is provided to help you maintain your orientation while you sketch on several planes. This assistant is called a space handle. The space handle appears when the first point of a line or spline is defined on a selected plane. Using the space handle, you can select the axis along which you want to sketch. By default, you sketch relative to the default coordinate system in the model. To switch to one of the other two default planes, click the sketch tool and press Tab. The origin of the current sketch plane is displayed.
Dimensioning a 3D Sketch When working in a 3D sketch, you can sketch lines to the approximate length, and then dimension them. •
You can add a length dimension by selecting two points, a line, or two parallel lines.
•
You can add an angular dimension by selecting either three points or two lines.
Virtual Sharps - 3D Sketch A virtual sharp represents a sketch point at the virtual intersection of two sketch entities. Virtual sharps appear automatically in 3D sketches for: •
Fillets
•
Sketch Chamfers
You can delete the automatic virtual sharps. To insert a virtual sharp between two sketch entities:
1.
Select the sketch entities.
2.
Click Point
or Tools, Sketch Entity, Point.
A virtual sharp appears at the point where the entities would intersect. You can add dimensions and relations to virtual sharps in 3D sketches.
3D Arc PropertyManager The Arc PropertyManager controls the following properties of an arc in a 3D sketch. To create an arc in a 3D sketch, use Sketch Fillet
on the Sketch toolbar to fillet two lines.
Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry.
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Parameters You can specify any appropriate combination of the following parameters to define the arc if the arc is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Center X Coordinate Center Y Coordinate Center Z Coordinate Start X Coordinate Start Y Coordinate Start Z Coordinate End X Coordinate End Y Coordinate End Z Coordinate Radius Angle. Subtended by the arc.
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4 2D to 3D Conversion
2D to 3D Conversion Overview You can convert 2D sketches into 3D models. Example of 2D to 3D Conversion: The original drawing is imported into a part document as Sketch1. The sketch entites in the lower left corner become the Front view. The top left becomes the Top view. The lower right becomes the Right view. The upper right is an Auxiliary view.
The Front view is at the lower left. The Top, Right, and Auxiliary views are folded perpendicular to the Front view.
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Chapter 4 2D to 3D Conversion
An isometric view displays the orientation of the sketches.
Align the left edges of the Auxiliary and Top sketches, then the Right and Auxiliary sketches.
Extrude the base feature.
4-2
Cut or extrude other features. In this example, a round hole, a rectangular hole, and a rectangular notch are cut to complete the part.
The 2D sketch can be an imported drawing, or it can be a sketch constructed in SolidWorks. In either case, it must be a single sketch in a part document. NOTE: Even though the sketch can be an imported drawing, it must be imported into a sketch in a part document. You can copy and paste the drawing from a drawing document, or you can import the drawing directly into a 2D sketch in a part document. The conversion procedure is generally as follows: 1.
In a part document, import a drawing into a sketch or construct a new sketch.
2.
Edit the sketch.
3.
Extract sketches for views from the Front, Top, and so on. The sketches fold up into the appropriate orientation.
4.
Align the sketches.
5.
Extrude the base feature.
6.
Cut or extrude other features.
The tools for the conversion process are on the 2D To 3D Toolbar.
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Chapter 4 2D to 3D Conversion
2D to 3D Toolbar The 2D to 3D tools help you convert a 2D drawing to a 3D part. Some of the tools can be used in any sketches. Front. The selected sketch entities become the front view in converting to a 3D part. Top. The selected sketch entities become the top view in converting to a 3D part. Right. The selected sketch entities become the right view in converting to a 3D part. Left. The selected sketch entities become the left view in converting to a 3D part. Bottom. The selected sketch entities become the bottom view in converting to a 3D part. Back. The selected sketch entities become the back view in converting to a 3D part. Auxiliary. The selected sketch entities become an auxiliary view in converting to a 3D part. You must select a line in another view to specify the angle of the auxiliary view. Create Sketch from Selections. The selected sketch entities become a new sketch. You can extract a sketch, for example, and then modify it before creating a feature. Repair Sketch. You can fix errors in a sketch so that the sketch can be used to extrude or cut a feature. Typical errors can be overlapping geometry, small gaps, or many small segments that are collected into a single entity. Align Sketch. Select an edge in one view to align to the edge selected in a second view. The order of selection is important. Extrude. Extrude a feature from the selected sketch entities. You do not have to select a complete sketch. Cut. Cut a feature from the selected sketch entities. You do not have to select a complete sketch.
Importing Drawings into Part Documents You can import a 2D drawing directly into a sketch in a part document for conversion into a 3D model. To import a drawing into a part document:
1.
Open the drawing (.dwg or .dxf file) in SolidWorks. The DXF/DWG Import dialog box appears.
2.
Select Import to a new part and click Next.
3.
Select Import to a 2D sketch. NOTE: It is recommended that you select Skip CrossHatch Import when importing for conversion.
4.
Click Finish. The drawing appears as Sketch1 in the FeatureManager design tree. To continue with the conversion, edit the sketch and extract new sketches.
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Extracting Sketches To create a base feature from a 2D drawing, extract sketches to specify the appropriate views. The sketches fold up automatically into the correct orientation as though the drawing were a piece of paper. Specify which portions of the drawing are the sketches for the front view, the right view, and so on. You can also create auxiliary sketches that are not parallel to the principal view planes. To extract a sketch for the front view:
1.
While editing a sketch, select the sketch entities that make up the front view. NOTE: You must define a Front view before defining any of the other views. You can box select, chain select, or hold Ctrl and select entities individually.
2.
Click Front
on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Front.
A new sketch appears in the FeatureManager design tree. To extract other orthogonal sketches:
1.
While still editing the original sketch, select the sketch entities that make up one of the orthogonal views, such as the top, right, left, bottom, or back.
2.
Click the corresponding icon on the 2D to 3D toolbar or on the Tools, Sketch Tools, 2D to 3D menu. A new sketch appears in the FeatureManager design tree. The sketch folds into the correct orientation to the Front view.
To extract auxiliary sketches:
1.
While editing a sketch, select the sketch entities that make up the auxiliary view.
2.
Hold Ctrl and select a line in another view to specify the angle of the auxiliary view.
3.
Click Auxiliary
on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Auxiliary.
Example of Auxiliary View: Sketch entities for auxiliary view Line defines angle of auxiliary view
Next, align the sketches.
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Chapter 4 2D to 3D Conversion
Aligning Sketches After extracting sketches for conversion to a 3D part, you can align the sketches before creating the base feature. The sketch selected first moves to align with the sketch selected second. To align sketches:
1.
Select a line or a point in a sketch to be aligned with another sketch.
2.
Hold Ctrl and select a line or a point in the second sketch to which the first sketch is to be aligned.
3.
Click Align Sketch
on the 2D to 3D toolbar, or click Tools, Sketch Tools, Align, Sketch.
Example of Aligning Sketches: Two sketchs, Top and Auxiliary, are not aligned. The Top sketch is to remain stationary while the Auxiliary sketch moves into alignment.
Top sketch Select the line indicated in the Auxiliary sketch, then hold Ctrl and select the line indicated in the Top sketch.
Click Align Sketch . The Auxiliary sketch moves into alignment with the Top sketch.
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Auxiliary sketch
Extruding in 2D to 3D You can extrude base features and other features using Extrude
on the 2D to 3D toolbar with partial sketches.
NOTE: Extruded Boss/Base on the Features toolbar accepts only complete sketches. To extrude a feature:
1.
Edit a sketch.
2.
Select the sketch entities required for the feature. NOTE: It is not necessary to select a complete sketch.
3.
Hold Ctrl and select a point (in any sketch) to be the starting point for the extrusion. NOTE: If you do not select a starting point, or if you select a point in the edited sketch, the plane of the sketch is considered to be the starting point.
4.
Click Extrude on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Extrude, and click in the graphics area to establish the direction of the extrusion. The Base-Extrude PropertyManager appears.
5.
Edit the properties in the Base Extrude PropertyManager. NOTE: For 2D to 3D conversion, you can specify the depth of a blind extrusion by selecting a sketch entity. Click Depth
6.
Click OK
and select an entity in a sketch. .
Example of Extruding in 2D to 3D Conversion: Select the sketch entities (in the Front sketch at the lower left) as the basis for the base extrusion. Hold Ctrl and select a starting point (upper left vertex in the Top sketch).
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Click in the graphics area to establish the direction of the extrusion.
In the Base-Extrude PropertyManager, click Depth and select the line shown to specify the depth of the extrusion.
Cutting in 2D to 3D You can cut features using Cut
on the 2D to 3D toolbar with partial sketches.
NOTE: Extruded Cut on the Features toolbar accepts only complete sketches. To cut a feature:
1.
Edit a sketch.
2.
Select the sketch entities required for the feature. NOTE: It is not necessary to select a complete sketch.
3.
Hold Ctrl and select a face to be the starting point for the cut.
4.
Click Cut on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Cut, and click in the graphics area to establish the direction of the cut. The Cut-Extrude PropertyManager appears.
5.
Edit the properties in the Base Extrude PropertyManager. NOTE: For 2D to 3D conversion, you can specify the depth of a blind cut by selecting a sketch entity. Click Depth
6.
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Click OK
and select an entity in a sketch. .
Example of Cutting in 2D to 3D Conversion: Select the sketch entities shown in the auxiliary view to define the cut. Hold Ctrl and select the face shown on the base feature as the starting point.
Click Cut on the 2D to 3D toolbar and click in the graphics area to establish the direction of the cut.
In the Cut-Extrude PropertyManager, click Depth and select the line shown in the front view to specify the depth of the cut. Click OK
.
Click Hidden Lines Visible View toolbar to see the cut.
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Additional Conversion Tools Repair Sketch Repair Sketch can often fix errors in a sketch so that the sketch can be used to create a feature. Some tools (Extrude and Cut, for example) repair sketches automatically when they detect errors they can fix. You can also repair sketches manually. Repair Sketch is particularly useful for sketches created by importing DXF/DWG files. Repair Sketch proceeds automatically as follows: •
Delete zero length line and arc segments (zero length is a segment less than ±1.0e-8 meters)
•
Merge colinear lines that overlap
•
Eliminate gaps of less than ±1.0e-8 meters in colinear lines
•
Collect small segments in colinear lines with no gaps greater than ±1.0e-8 meters
•
Merge coincident lines (separated by less than ±1.0e-8 meters) into one line
To repair a sketch automatically:
1.
Select a sketch in the FeatureManager design tree.
2.
Click Extrude
or Cut
on the 2D to 3D toolbar, or click Extruded Base/Boss
or Extruded
Cut on the Features toolbar. A warning message states the error and offers to repair the sketch. 3.
Click OK to attempt the repair and continue to create the feature.
To repair a sketch manually:
1.
Select a sketch in the FeatureManager design tree.
2.
Click Repair Sketch
on the 2D to 3D toolbar, or click Tools, Sketch Tools, Repair Sketch.
Create Sketch from Selections With Create Sketch from Selections , you can extract only those elements of a sketch (usually in an imported drawing) that you require to create a feature. You can extract a sketch, for example, and then modify it before creating a feature. To create a sketch from selections:
1.
Edit a sketch.
2.
Select the sketch entities you want in the new sketch.
3.
Click Create Sketch from Selections
, or click Tools, Sketch Tools, Create Sketch from Selections.
A new sketch appears in the FeatureManager design tree.
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5 Reference Geometry
Reference Geometry Overview Reference geometry defines the shape or form of a surface or a solid. Reference geometry includes planes, axes, coordinate systems, points, and 3D curves. You can use reference geometry in the creation of several kinds of features: •
planes are used in lofts and sweeps
•
split lines are used in some drafts and chamfers
•
an axis is used in a circular pattern
This chapter includes: •
Creating and using planes
•
Creating and using axes
•
Creating local coordinate systems
•
Converting sketch lines to construction geometry
•
Creating 3D curves
•
Creating reference points
Updating Reference Geometry in Document Templates You control the visibility of reference geometry and the names of the default planes in the document templates. To update the document templates:
1.
Click Open
2.
Select Template Files (*.prtdot, *.asmdot, *.drwdot) from the Files of type list.
3.
Browse to the desired file, and click Open.
4.
Make the necessary changes to the document template including the following:
5.
or File, Open.
•
Rename the planes
•
Toggle the visibility of the reference geometry (for example, click View, Origins.)
Click Save or File, Save to update the existing document template. Click File, Save As to update the name of the document template as well.
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Chapter 5 Reference Geometry
Planes Creating Planes You can create planes in part or assembly documents. You can use planes to sketch, to create a section view of a model, for a neutral plane in a draft feature, and so on. You can preselect items before you click Plane . If you preselect items, SolidWorks attempts to select the appropriate type of plane. You can always select a different type of plane. You can right-click in the graphics area and select a plane type from the shortcut menu. When you have selected enough entities to create a plane, the OK
pointer appears. Right-click to create the plane.
NOTE: The created plane is 5% larger than the geometry on which the plane is created, or 5% larger than the bounding box. This helps reduce selection problems when planes are created directly on faces or from orthogonal geometry. To create a construction plane:
1.
Click Plane
on the Reference Geometry toolbar, or click Insert, Reference Geometry, Plane.
The Plane PropertyManager appears. 2.
Under Selections, select the type of plane you want to create and the items to create the plane: •
Through Lines/Points. Create a plane through an edge, axis, or sketch line, and a point, or through three points.
Select three points. Parallel Plane at Point. Create a plane through a point parallel to a plane or face. •
Select a face or planar face.
5-2
Then select a midpoint.
The new plane is parallel to the selected face through the chosen midpoint.
At Angle. Create a plane through an edge, axis, or sketch line at an angle to a face or plane.
• a.
Select a plane or planar face, and then select an edge, axis, or sketch line.
b.
Enter the angle between the planes in the Angle box.
c.
Select the Reverse direction check box, if necessary. The behavior of the plane is as follows:
If the selected line is in the same plane as the selected plane, the new plane rotates around the selected line.
If the selected line is parallel to the selected plane, the new plane moves to the parallel line and rotates around the line.
If the selected line is skewed with respect to the selected plane, the selected line is projected onto the selected plane and then the plane rotates around the projected line. In this sample, use Plane 1 and Axis 1 to create a new plane at an angle. Sketch the extrusion profile on Plane 4. Create the Y-shaped pipe. Offset. Create a plane parallel to a plane or face, offset by a specified distance. This is the default plane created.
• a.
Select a plane or planar face.
b.
Enter the offset distance in the Distance box.
c.
Select the Reverse direction check box, if necessary.
d.
To create multiple planes offset the same Distance from the selected plane, enter the number of planes in the Number of Planes to Create
Single offset plane
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Multiple offset planes
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Chapter 5 Reference Geometry
Normal to Curve. Create a plane through a point and perpendicular to an edge or curve.
• a.
Select an edge or curve, and a vertex or point.
b.
Select the Set origin on curve check box to place the origin on the curve; the default is to place the origin on the vertex or point.
In this example, you select just the helix to create the new plane. Plane 4 is perpendicular to the end of the tapered helix.
A circle is swept along the helix to create a spring.
The helical spring is used in a battery contact terminal.
On Surface. Create a plane on a non-planar face or angular surface. See Plane On Surface Examples.
• a.
Select a surface.
b.
Select a sketch point on the surface.
• a.
Drag and Drop. You can also drag and drop to create a plane. Select an existing plane border.
b.
Hold down the Ctrl key and drag the plane. The Plane PropertyManager appears with Offset Distance new plane appears in the graphics area.
c.
Drop the new plane in the new location.
d.
Adjust the values in the PropertyManager.
The selected items appear in the Reference Entities appears in the graphics area. 3.
Click OK
selected. A preview of the
box. A preview of the new plane
to create the plane.
The new plane appears in the graphics area and is listed in the FeatureManager design tree. NOTES:
5-4
•
To cancel the transaction, click Cancel
.
•
To display the Planes online help topic, click Help
•
To create multiple planes, click Keep Visible
. to keep the Plane PropertyManager displayed.
Plane On Surface Examples You can create the following types of planes using the On Surface •
tool in the Plane PropertyManager:
Any surface and a point that is not on that surface, using a projected sketch or the closest point 1.
Select the sketch point and the model surface.
Two options appear in the Plane PropertyManager: Project to nearest location on surface and Project onto surface along normal. 2.
Select one of these options. A preview of the new plane appears.
Project to nearest location on surface is selected. The new plane is created at the point on the surface closest to the selected sketch point.
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Project onto surface along sketch normal is selected. The new plane is created at the point on the surface obtained by projecting the sketch point normal to the plane on which the sketch point is located. Select the Reverse check box if the plane preview does not appear.
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Chapter 5 Reference Geometry
•
A cylindrical face and a plane 1.
Select the cylindrical face.
2.
Select a plane that intersects the axis of the cylinder.
The preview of the new plane is created tangent to the selected face, along the line where the plane intersects the surface. 3.
Select the Normal plane check box (optional).
A preview of the new plane appears with an Offset angle of 45 degrees. You can adjust the offset angle, as needed. The new plane intersects the axis of the cylinder.
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•
A conical face and a plane 1.
Select the conical face.
2.
Select a plane that intersects the selected face.
The preview of the new plane is created tangent to the selected surface, along the line where the plane intersects the surface. 3.
Select the Normal plane check box (optional).
The plane preview changes. The axis of the selected face is used for an at-angle plane relative to the selected plane, creating a new plane normal to the selected surface. 4.
Adjust the angle of the new plane in the Offset
box.
The new plane
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Chapter 5 Reference Geometry
•
A surface, a plane, and an edge 1.
Select a surface.
2.
Select a plane that cuts through the surface.
3.
Select an edge on the surface. A preview of the new plane appears.
The plane is created tangent to the selected surface at the point where the selected plane intersects the selected edge.
Plane tangency
The new plane
Changing Plane Names To change the names for construction planes in the current document:
1.
Click-pause-click the plane’s name in the FeatureManager design tree.
2.
Type a new name. TIP: As you create additional construction planes, it is a good idea to change their names to indicate their purpose.
To change the default names used for planes:
You can create new default plane names to replace the existing plane names. You save this information in a document template.
Plane Display You can set the following plane display options for part and assembly documents: •
Face color
•
Transparency
•
Intersection display and color
NOTE: You must enable the Display shaded planes option to display shaded planes. To set the plane display:
5-8
1.
Open a part or assembly document.
2.
Click Tools, Options. On the Document Properties tab, click Plane Display.
3.
Under Faces, set the following options:
•
Front Face Color. Displays the Color dialog box that you use to set the front face color of planes.
Front face color
Back face color
•
Back Face Color. Displays the Color dialog box that you use to set the back face color of planes.
•
Transparency. Controls the plane transparency (0% displays a solid face color; 100% displays no face color).
0% transparency
75% transparency
100% transparency
NOTE: Edges take the same color as the front and back faces, are not transparent, and are always displayed. 4.
Under Intersections, set the following options: •
Show intersections. Select or clear the Show intersections check box to display or hide the intersection of planes.
Plane intersection lines displayed • 5.
Plane intersection lines hidden
Line Color. Displays the Color dialog box that you use to set the plane intersection line color.
Click OK to accept the changes, or Cancel to discard the changes and exit the dialog box.
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Chapter 5 Reference Geometry
Hiding or Showing Planes You can turn the display of planes on or off. To toggle the display of planes:
Click View, Planes. A check mark next to the menu item means planes are visible (except for planes you have hidden individually). To hide or show individual planes:
1.
Right-click the plane in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show. NOTE: Individual planes always are highlighted when you select them, even when hidden.
Moving, Resizing, and Copying Planes You can move, resize, and copy planes using the plane handles and edges. To display the plane’s handles:
•
Click the plane’s name in the FeatureManager design tree or in the graphics area, - or -
•
Click the edge of the plane.
Using the plane’s handles and edges, you can do the following: •
Resize the plane by dragging a corner or edge handle.
•
Move the plane by dragging the edge of the plane.
•
Copy the plane by selecting a plane in the graphics area. Then hold down the Ctrl key and, using the edge, drag to a new location. An offset plane is created.
To modify the offset distance, angle, or distance between planes:
1.
Double-click the plane to display the offset distance or angle.
2.
Double-click the dimension or angle and type a new value in the Modify dialog box. - or -
1.
Right-click the name of the plane in the FeatureManager design tree.
2.
Select Edit Feature.
3.
In the PropertyManager, enter new values to define the plane, then click OK
.
Automatic Sizing of Planes and Axes Planes and axes that you create are automatically sized to either the geometry on which they are created, or to the bounding box of the model geometry. As the geometry changes size, the planes and axes update accordingly. You can override the automatic sizing by manually changing the plane or axis size, which disables future autosizing for that entity. You can re-enable autosizing by selecting Autosize from the shortcut menu. NOTE: The created plane is 5% larger than the geometry on which the plane is created, or 5% larger than the bounding box. This helps reduce selection problems when planes are created directly on faces or from orthogonal geometry.
5-10
To see an example of automatic sizing of planes:
1.
Select a planar face and create an offset plane. Offset plane 1 appears and is automatically sized to the geometry of the face from which it was created.
2.
Click View, Planes.
3.
Edit the sketch to double the dimension of the bottom edge of the model, then exit the sketch. The plane 1 size updates automatically when you change the geometry of the face on which it was created.
4.
Drag upwards to manually resize the top edge of plane 1. Autosizing becomes disabled.
5.
Edit the sketch again to change the bottom edge dimension back to the original size, then exit the sketch. Plane 1 does not resize automatically because autosizing is disabled.
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Chapter 5 Reference Geometry
6.
Right-click plane 1 in the graphics area and select Autosize. Autosizing is re-enabled. Plane 1 automatically resizes to the updated model geometry.
Axis Overview You can use an axis in creating sketch geometry or in a circular pattern. Every cylindrical and conical face has an axis. Temporary axes are those created implicitly by cones and cylinders in the model. You can set the default to either hide or show all temporary axes. To display temporary axes:
Click View, Temporary Axes. A check mark next to the menu item means temporary axes are visible.
To turn the display of axes on or off:
Click View, Axes. A check mark next to the menu item means axes are visible (except for axes you have hidden individually). To hide or show an individual axis:
1.
Right-click the axis in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show.
Reference Axis You can create a reference axis, also called a construction axis. To create a reference axis:
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1.
Click Axis
on the Reference Geometry toolbar, or click Insert, Reference Geometry, Axis.
2.
Select the axis type in the Axis PropertyManager, then select the required entities for that type.
3.
Verify that the items listed in Reference Entities
4.
Click OK
5.
Click View, Axes to see the new axis.
.
correspond to your selections.
Reference Axis The Axis PropertyManager appears when you create a new axis or edit an existing axis. The PropertyManager controls the following properties: Reference Entities. Displays the selected entities. One Line/Edge/Axis. Select a sketch line, an edge, or select View, Temporary Axes and then select the axis that is displayed. Two Planes. Select two planar faces, or select View, Planes, and then select two planes. Two Points/Vertices. Select two vertices, points, or midpoints. Cylindrical/Conical Surface. Select a cylindrical or conical face. Point and Surface. Select a surface or plane and a vertex point, or midpoint. The resultant axis is normal to the selected surface or plane through the selected vertex, point, or midpoint. If the surface is non-planar, the point must be on the surface.
Coordinate System You can define a coordinate system for a part or assembly. Use this coordinate system with the Measure and Mass Properties tools, and for exporting SolidWorks documents to IGES, STL, ACIS, STEP, Parasolid, VRML, and VDA. To create a coordinate system:
1.
Click Coordinate System Coordinate System.
on the Reference Geometry toolbar, or click Insert, Reference Geometry,
2.
Use the Coordinate System PropertyManager to create the coordinate system. You can amend your selections:
3.
•
To change your selections, right-click in the graphics area and select Clear Selections.
•
To reverse the direction of an axis, click its Reverse Axis Direction PropertyManager.
Click OK
button in the
.
You may need to locate a coordinate system where there are insufficient entities available to define the coordinate system. In this case, you can define a coordinate system someplace on the part that does provide the entities you need. Then you can move the new origin to the desired location. The new location must contain at least one point or vertex. To translate a coordinate system to a new location:
1.
Click Coordinate System
or Insert, Reference Geometry, Coordinate System.
2.
Define the coordinate system at a location on the part that provides the entities you need to control the angle and direction of each axis.
3.
Click in Origin, then select the point or vertex to which you want to translate the origin.
4.
Click OK. The origin moves to the location that you selected. When you create a coordinate system, it is a good idea to give it a meaningful name to explain its purpose. Click-pause-click the coordinate system’s name in the FeatureManager design tree and enter a new name.
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Chapter 5 Reference Geometry
To toggle the display of coordinate systems:
Click View, Coordinate Systems. A check mark next to the menu item means coordinate systems are visible. To hide or show individual coordinate systems:
1.
Right-click the coordinate system in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show. Individual coordinate systems always are highlighted when you select them, even when hidden.
Coordinate System PropertyManager The Coordinate System PropertyManager appears when you add a new coordinate system to a part or assembly or edit an existing coordinate system. The PropertyManager controls the following properties: Origin. Select a vertex, point, midpoint, or the default point of origin on a part or assembly for the coordinate system origin. X axis, Y axis, and Z axis. Select one of the following for the Axis Direction Reference: •
Vertex, point, or midpoint. Aligns the axis toward the selected point.
•
Linear edge or sketch line. Aligns the axis parallel to the selected edge or line.
•
Non-linear edge or sketch entity. Aligns the axis toward the selected location on the selected entity.
•
Planar face. Aligns the axis in the normal direction of the selected face. Reverse Axis Direction. Reverses the direction of an axis.
Origin The model origin appears in blue and represents the (0,0,0) coordinate of the model. When a sketch is active, a sketch origin appears in red and represents the (0,0,0) coordinate of the sketch. Dimensions and relations can be added to the model origin, but not to a sketch origin. To toggle the origin display:
Click View, Origins. A check mark next to the menu item means origins are visible (except for origins you have hidden individually).
Centroid If you select centroid as the reference point for a table-driven or sketch-driven pattern, the system determines the centroid based on the type of seed feature.
5-14
•
For cylindrical, conical, or revolved features, the centroid is the intersection of the axis of revolution with the X-Y plane of the pattern.
•
If the sketch consists of lines and arcs, such as rectangles or oval shapes, and if the sketch plane is parallel to the X-Y plane, the centroid is defined as the centroid of the sketch.
•
For any other condition, the centroid is the centroid of the face of the seed feature.
•
If there is more than one seed feature, the centroid of the first seed feature is used.
•
If the seed feature is generated from a sketch that includes multiple contours, the centroid of the largest closed contour is used.
Converting Sketch Lines to Construction Geometry You can convert sketched entities into construction geometry to use in creating model geometry. To convert one or more sketch entities to construction geometry:
1.
In an open sketch, select the sketch entities to convert.
2.
Do one of the following: •
Click Construction Geometry
on the Sketch toolbar.
•
Select the For construction check box in the PropertyManager.
To convert sketch entities in a drawing to construction geometry:
Select the sketch entities that you want to convert and use one of the following methods: •
Click Construction Geometry
on the Sketch toolbar.
•
Click Tools, Sketch Tools, Construction Geometry.
•
Select the For construction check box in the PropertyManager.
•
Right-click any selected sketch entity and select Construction Geometry.
Curve Overview You can create several types of 3D curves by using these methods: •
Projected Curve - from a sketch projected to a model face or surface, or from sketched lines on intersecting planes
•
Composite Curve - from a combination of curves, sketch geometry, and model edges
•
Helix and Spiral - by specifying a circular sketch, pitch, number of revolutions, and height
•
Split Line - from a sketch projected to planar or curved (silhouette) faces
•
Curve Through Reference Points - from user-defined points or existing vertices
•
Curve Through XYZ Points - from a list of X,Y, Z coordinates for points
You can then use the curves to create solid model features. For example, you can use a curve as the path or guide curve for a sweep feature, as the guide curve for a loft feature, as a parting line for a draft feature, and so on. You can turn the display of curves on or off. To toggle the display of curves:
Click View, Curves. A check mark next to the menu item means curves are visible (except for curves you have hidden individually). To hide or show individual curves:
1.
Right-click the curve in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show. Individual curves always are highlighted when you select them, even when hidden.
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Chapter 5 Reference Geometry
Curve Through XYZ Points 1.
Click Curve Through XYZ Points XYZ Points.
on the Curves toolbar, or click Insert, Curve, Curve Through
2.
Create new sets of coordinates by double-clicking cells in the X, Y, and Z columns and entering a point coordinate in each one. (Created outside of a sketch, the X, Y, and Z coordinates are interpreted with respect to the Front plane coordinate system.) The numbers in the Point column define the order in which the points are connected.
3.
Click OK to display the curve. The Curve Through XYZ Points tree.
icon appears next to the curve name in the FeatureManager design
Tips for working with this tool:
•
Open an existing curve file. Click Browse and navigate to a curve file to open. You can open .sldcrv files or .txt files that use the same format as .sldcrv files. You can also create 3D curves in Excel for example, save them as .txt files, then open them in SolidWorks. To be able to open text files, they must contain only coordinate data (not the X, Y, or Z labels , or other extraneous data).
•
Change coordinates. Double-click in a cell and enter a new value. (As you enter values, notice the preview of the curve is displayed in the graphics area.)
•
Add a row. Double-click in a cell in the row below the last numbered row.
•
Insert a row. Drag the cursor across a row to select it, then click Insert. A new row is inserted above the selected row.
•
Delete a row. Drag the cursor across a row to select it, then press the Delete key.
•
Save the curve file. Click Save or Save As, navigate to the desired location, and specify the filename. If you do not specify an extension, the SolidWorks application adds the extension .sldcrv.
Curve Through Reference Points Creates a curve through points located on one or more planes. 1.
Click Curve Through Reference Points Through Reference Points.
on the Curves toolbar, or click Insert, Curve, Curve
The Curve Through Reference Points PropertyManager appears. 2.
Select the sketch points or vertices, or both, in the order in which you want to create the curve. As you select, the entities are listed in the Through Points box.
3.
If you want to close the curve, select the Closed Curve check box.
4.
Click OK
.
The Curve Through Reference Points design tree.
Create curves to connect sketch points between two loft profiles.
5-16
icon appears next to the curve name in the FeatureManager
Create the propellers for the fan using a loft feature and a circular pattern.
Here is the completed fan assembly.
Curve from File To create a curve from an existing file containing coordinate values:
1.
Create a file containing coordinate values for curve points using a text editor or worksheet application. The file format must be a three-column, tab or space-delimited list of only X, Y, and Z coordinates. Do not include any column headings, such as X, Y, and Z.
2.
Save the file as a text file.
3.
Click Curve Through XYZ Points XYZ Points.
4.
Click Browse to locate the file, then click Open.
on the Curves toolbar, or click Insert, Curve, Curve Through
The coordinates from the file are displayed in the Curve File dialog box. Notice the numbers in the Point column, indicating the order in which the points will be connected. 5.
Examine the preview of the curve, and edit the coordinates if necessary, until you are satisfied with the result. (Double-click in any cell, then edit the value.)
6.
Click OK.
Helix and Spiral You can create a helix or spiral curve in a part. The helix can be used as a path or guide curve for a swept feature, or a guide curve for a lofted feature. To create a helix or spiral:
1.
Open a sketch and sketch a circle. The diameter of this circle controls the diameter of the helix.
2.
Click Helix and Spiral
3.
Set values in the Helix/Spiral PropertyManager.
on the Curves toolbar, or click Insert, Curve, Helix/Spiral.
To define a helix, you specify two values, and the third value is automatically calculated. 4.
Click OK
.
The helix and the sweep profile are on the neck of the bottle.
A boss-sweep feature (shown in blue) creates the threads on the neck of the bottle.
Spiral spring
Spiral spring in the internal mechanism of a clock
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Chapter 5 Reference Geometry
Helix/Spiral PropertyManager The Helix/Spiral PropertyManager appears when you create a new helix or spiral in a sketch or edit an existing helix or spiral. The PropertyManager controls the following properties: Defined By •
Pitch and Revolution. Creates a helix defined by Pitch and Revolutions.
•
Height and Revolution. Creates a helix defined by Height and Revolutions.
•
Height and Pitch. Creates a helix defined by Height and Pitch.
•
Spiral. Creates a spiral defined by Pitch and Revolutions.
Parameters •
Height (Helix only). Sets the height.
•
Pitch. Sets the rate of change of radius for each revolution. The Pitch value must be at least 0.001 and not greater than 200000.
•
Revolutions. Sets the number of turns.
•
Reverse direction. Extends the helix backwards from the point of origin, or creates an inward spiral.
•
Start angle. Sets where to start the first turn on the sketched circle.
•
Clockwise. Sets the direction of the turns to clockwise.
•
Counterclockwise. Sets the direction of the turns to counterclockwise.
Taper Helix •
Taper Helix. Creates a tapered helix.
•
Taper Angle. Sets the angle of the taper.
•
Taper outward. Tapers the helix outward.
Projecting Sketched Curves You can project a sketched curve onto a model face to create a 3D curve. You can also create a 3D curve that represents the intersection of two extruded surfaces generated by creating sketches on two intersecting planes. You can preselect items before you click Projection appropriate type of projection. •
. If you preselect items, SolidWorks attempts to select the
If you preselect two sketches, the Sketch onto Sketch option is activated with the two sketches shown under Sketches to Project
.
•
If you preselect a sketch and one or more faces, the Sketch onto Face(s) option is activated with the selected items shown in the correct boxes.
•
If you preselect one or more faces, the Sketch onto Face(s) option is activated.
You can right-click in the graphics area and select a projection type from the shortcut menu. When you have selected enough entities to create a projected curve, the OK
pointer appears. Right-click to create the projected curve.
To project a curve:
1.
Click Projection
on the Curves toolbar, or Insert, Curve, Projected.
The Projected Curve PropertyManager appears. 2.
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Under Selections, set Projection Type to one of the following:
Sketch onto Face(s)
Use this selection to project a sketched curve onto a model face. •
Under Sketch to Project design tree.
, select the curve in the graphics area or from the flyout FeatureManager
•
Under Projection Faces
•
Select the Reverse Projection check box, or click the handle in the graphics area, if necessary.
, select the cylindrical face on the model where you want to project the sketch.
Original sketch to project onto a face
Projected curve
Projected curve used as a sweep path
Sketch onto Sketch
Use this selection to create a curve that represents the intersection of sketches from two intersecting planes. •
Create a sketch on each of two intersecting planes, closing each sketch when you are done.
•
Align the sketch profiles such that when they are projected normal to their sketch plane; the implied surfaces will intersect, creating the desired result.
•
Under Sketches to Project graphics area.
, select both sketches in the flyout FeatureManager design tree or the
The two sketches (gray) project onto each other to form the 3D curve (green).
The curve is used as a path for a sweep.
The swept geometry is used to create this power adapter.
A preview of the projected curve appears. 3.
Click OK
to create the projected curve, or Cancel
to cancel the transaction.
Replacing a Sketch of a Projected Curve You can replace one or more of the sketches that make up a projected curve of two sketches projected onto one another. To replace a sketch in a projected curve:
1.
Right-click the Curve feature in the FeatureManager design tree, or right-click the curve in the graphics area, and select Edit Feature. The Curve PropertyManager appears.
2.
3.
Choose one of the following methods to clear the unwanted sketch from the Sketch to Project box: •
Click the sketch in the flyout FeatureManager design tree.
•
Click the sketch in the graphics area.
• Select the sketch in the Sketches to Project box under Selections, and press Delete. Select the replacement sketch in either the flyout FeatureManager design tree or in the graphics area, then click OK
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Chapter 5 Reference Geometry
Split Lines The Split Line tool on the Curves toolbar projects a sketch to curved or planar faces. It divides a selected face into multiple separate faces, enabling you to select each face. You can also project a sketch onto a surface body. You can use this tool to create two types of split lines: •
Projection. Projects a sketch line on a surface.
•
Silhouette. Creates a split line on a cylindrical part.
To create a projection split line:
1.
Sketch a line to project as a split line.
2.
Click Split Line
on the Curves toolbar, or click Insert, Curve, Split Line.
The Split Line PropertyManager appears. 3.
Under Type of Split, select Projection.
4.
Under Selections, do the following:
5.
•
If necessary, click the Sketch to Project box and select the sketched line in the flyout FeatureManager design tree or in the graphics area.
•
Click the Faces to Split box and select the faces around the perimeter of the part that you want the split line to pass through.
•
Select the Single Direction check box to project the split line in only one direction.
•
Select the Reverse Direction check box, if necessary, to project the split line in the opposite direction.
Click OK
.
The sketch line is projected onto the faces you selected. In this example, the four sides were selected. The split line appears on each face, dividing each face into two sections. Example of a projected split line on a surface:
Before
5-20
After
To create a silhouette split line:
1.
Click Split Line
on the Curves toolbar, or click Insert, Curve, Split Line.
The Split Line PropertyManager appears. 2.
Under Type of Split, click Silhouette.
3.
Under Selections, do the following:
4.
•
Under Direction of Pull , in the flyout FeatureManager design tree or graphics area, select a plane to project through the model's silhouette (outer edges).
•
Under Faces to Split
Click OK
, select one or more faces to split. The faces cannot be planar.
.
The plane is projected through the model, creating silhouette split lines where the plane intersects the outer edges of the selected faces.
The selected plane is projected through the model in the direction of pull.
A silhouette split line is created on the model where the selected plane projected through the outer model edges.
Composite Curve You can create composite curves by combining curves, sketch geometry, and model edges into a single curve. Use a composite curve as a guide curve when creating a loft or a sweep. To create a composite curve:
1.
Click Composite Curve
on the Curves toolbar, or click Insert, Curve, Composite.
2.
Click the items (sketch entities, edges, and so on) that you want to join. The selected items appear in the Composite Curve Property Manager, under Entities to Join in the Sketches, Edges, and Curves to Join
3.
Click OK
to create the composite curve.
Select the edges on the model for the curve.
SolidWorks 2004 Reference Guide
box.
Create the sweep profile sketch, then use the composite curve as the sweep path.
Here is the completed sweep cut.
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Chapter 5 Reference Geometry
Reference Points You can create several types of reference points to use as construction objects. You can also create multiple reference points that are a specified distance apart on curves. Click View, Points to toggle the display of reference points. When you select items, the SolidWorks software attempts to select the appropriate point construction method. For example, if you select a face, SolidWorks selects the Center of Face construction method in the PropertyManager. You can always select a different type of point construction method. To create a single reference point:
1.
Click Point
on the Reference Geometry toolbar, or click Insert, Reference Geometry, Point.
2.
In the PropertyManager, select the type of reference point to create.
3.
In the graphics area, select the entities to use to create the reference point.
4.
Click OK
.
To create multiple reference points along a curve:
1.
In a model with a curve, click Point Geometry, Point.
2.
In the PropertyManager:
3.
on the Reference Geometry toolbar, or click Insert, Reference
•
Select Along curve distance or multiple reference point
•
Select a curve along which you want to create the reference points.
•
Select a distribution type: Distance, Percentage, or Evenly Distribute.
•
Set values for Number of specified points according to distance.
Click OK
.
and for Enter the distance/percentage value
.
Point PropertyManager The Point PropertyManager appears when you create a new reference point or edit an existing reference point. When you select items, the SolidWorks software attempts to select the appropriate point construction method. For example, if you select a face, SolidWorks selects the Center of Face construction method in the PropertyManager. You can always select a different type of point construction method. The PropertyManager controls the following properties: Reference Entities. Displays the selected entities used to create a reference point. Arc Center. Creates a reference point at the center of the selected arc or circle. Center Of Face. Creates a reference point at the center of gravity of the selected face. You can select planar or non-planar faces. Intersection. Creates a reference point at the intersection of the two selected entities. You can select edges, curves, sketch segments, and reference axes. Projection. Creates a reference point from one entity projected onto another. Select two entities: the entity to project and the entity onto which to project. You can project points, endpoints of curves and sketch segments, and vertices of solids and surfaces onto planes and faces (planar or non-planar). The point is projected normal to the plane or face.
5-22
Along curve distance or multiple reference point. Creates a set of reference points along edges, curves, or sketch segments. Select the entity and create the reference points using these options: •
Enter the distance/percentage value according to distance. Set a distance or percentage value to create the reference points. If the value is too large to create the specified number of reference points, a message warns you to set a smaller value.
•
Distance. Creates the number of reference points spaced at the distance you set, starting from the closest endpoint. The first reference point is created at this distance from the endpoint, not on the endpoint.
•
Percentage. Creates the number of reference points spaced at the percentage you set, starting from the closest endpoint. Percentage means percentage of the length of the selected entity. For example, select a 100mm-long entity. If you set the number of reference points to 5 and the percentage to 10, the 5 reference points are spaced 10 percent of the total entity length (or 10mm) apart from each other.
•
Evenly Distribute. Evenly distributes the number of reference points on the entity. If you edit the number of reference points, the reference points update their position relative to the starting endpoint.
•
Number of reference points. Set the number of reference points to create along the selected entity. The reference points are created using the selected Distance, Percentage, or Evenly Distribute option.
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Chapter 5 Reference Geometry
5-24
6 Features
Features Overview Features are the individual shapes that, when combined, make up the part. You can also add some types of features to assemblies. Features include multibody part capability. You can include separate extrude, revolve, loft, or sweep features, within the same part document. Features include: •
Base/Boss, and Cut
•
Extrude, Revolve, Sweep, and Loft
•
Fillet/Round, Chamfer, and Draft
•
Hole - Simple and Hole Wizard
•
Scale
•
Shell
•
Rib
•
Dome
•
Shape
•
Pattern and Mirror
Some features originate as sketches; other features, such as shells or fillets, are created when you select the appropriate tool or menu command and define the dimensions or characteristics that you want. Surfaces Surfaces are another type of feature. You can use surfaces to create or modify solid features. Other ways you can use surfaces include the following: •
Import from other applications
•
Thicken to create solid geometry
•
Extrude, revolve, sweep, loft, knit, or offset from a model face or surface
•
Extend, fillet, or trim a surface
•
Create a mid surface
•
Fill surface
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Chapter 6 Features
Features Toolbar The Features toolbar provides tools for creating model features. The set of features icons is very extensive so not all of them are included on the default Features toolbar. You can customize this toolbar by adding and removing icons to suit your working style and frequent tasks. See Customize Toolbars for more information. Extruded Boss/Base Revolved Boss/Base Sweep Loft Thicken Extruded Cut Revolved Cut Swept Cut Lofted Cut Thickened Cut Cut with Surface Fillet Chamfer Rib Scale Shell Draft Simple Hole Hole Wizard Dome Shape Deform
6-2
Wrap Move/Size Features Suppress Unsuppress Unsuppress with Dependents Linear Pattern Circular Pattern Mirror Feature Curve Driven Pattern Sketch Driven Pattern Table Driven Pattern Split Combine Join Delete Solid/Surface Imported Geometry Insert Part Move/Copy Bodies Library Feature
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Chapter 6 Features
Feature Previews You can display detailed previews and control what displays with the Detailed Preview PropertyManager. You can access the Detailed Preview PropertyManager from the PropertyManager in the following features: •
Extrudes
•
Ribs
•
Drafts
In the Detailed Preview PropertyManager you can select: •
Highlight new or modified faces. Display new extrude, rib, or draft features, or the faces that were affected by the previous edit. If you check this option, new or modified faces are highlighted in a different color, as opposed to appearing shaded as they do in the standard PropertyManager. All separate bodies appear in the preview.
•
Show only new or modified bodies. Display only new or modified bodies. All separate bodies are hidden in the preview. Only separate bodies are affected.
Detailed Preview - Extrudes
6-4
Extruded Cut. Standard preview from PropertyManager
Detailed View PropertyManager. Neither Highlight new or modified faces nor Show only new or modified faces are checked.
Detailed View PropertyManager. Highlight new or modified faces is checked.
Detailed View PropertyManager. Both Highlight new or modified faces and Show only new or modified faces are checked. All separate bodies are hidden in the preview.
Detailed Preview - Ribs
Ribs. Normal PropertyManager preview
Detailed View. Neither Highlight new or modified faces nor Show only new or modified faces are checked.
Detailed View. Highlight new or modified faces is checked.
Ribs applied to feature.
Detailed Preview - Draft
Draft. Normal PropertyManager preview.
Detailed View PropertyManager. Neither Highlight new or modified faces nor Show only new or modified faces are checked.
Detailed View PropertyManager. Highlight new or modified faces is checked.
Detailed View PropertyManager. Both Highlight new or modified faces and Show only new or modified faces are checked. All separate bodies are hidden in the preview.
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Chapter 6 Features
To use detailed preview:
1.
Create a model with an extrude, a rib, or a draft. You can also use an existing model, and add an extrude, a rib, or a draft, or click Edit Feature and review the most recent extrude, rib, or draft.
2.
Click Detailed Preview in the PropertyManager for the extrude, the rib, or the draft.
3.
In the Detailed Preview PropertyManager, select one of the following: • •
Highlight new or modified faces Show only new or modified faces
Highlight new or modified faces 4.
Click Detailed Preview to return to the normal PropertyManager. - or Click OK
6-6
to apply the new feature.
If you leave both check boxes clear, the preview is identical to the preview in the normal PropertyManager.
Show only new or modified faces
Chamfers Creates a beveled feature on selected edges or a vertex. To create a chamfer:
1.
Click Chamfer
on the Features toolbar, or click Insert, Features, Chamfer.
2.
Under Chamfer Parameters, do the following: •
Click Edges and Faces or Vertex
•
Select one of the following from the PropertyManager (or right-click to use the shortcut menu): o
Distance-distance
o
Angle-distance
o
Vertex
•
Select the Equal Distance check box to specify a single value for distance or vertex.
•
Select the Keep features check box if you want to retain features such as cuts or extrudes that would otherwise be removed when you apply the chamfer.
Original part
3.
, then select an entity in the graphics area.
Click OK
Keep features cleared
Keep features checked
.
Chamfer Distance-distance
Enter values for both distances on either side of the selected chamfer edges, or click Equal Distance and specify a single value.
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Chapter 6 Features
Chamfer Angle-distance Enter values for distance and angle in the Chamfer PropertyManager or in the graphics area. An arrow appears that points in the direction in which the distance is measured. If necessary, click Flip direction.
Chamfer Vertex
Chamfer-vertex Enter values for the distances on each side of the selected vertex, or click Equal Distance and specify a single value.
Deform Deform The deform feature allows you to alter the shape of a model locally or globally. You can apply the deform feature to both SolidWorks and imported models. There are two deform types: Curve to curve and Point. With each type, dynamic options control which faces or bodies are deformed, and the resulting geometry of the model. The curve to curve and point descriptions are an overview. For complete options: •
Curve to curve options
•
Point options
For examples on how to apply the deform feature: •
To deform a model using Curve to curve
•
To deform a model using Point
Curve to Curve Overview With Curve to curve deform, you select connected Initial curves , and connected Target curves under Deform curves. The curves you select can be part of the model, or separate sketches. The curves can be curved or linear entities.
6-8
Under Deform Region, you can specify the Bodies to be deformed: •
With Fixed edges selected, you can specify Fixed curves/edges/faces deform
•
, and Additional faces to
.
With Fixed edges cleared, you can control the area to deform by specifying a Deform radius
.
You can create different shapes when you select or clear the Uniform option. With Shape Options, you can also control the shape of the deformation by specifying a level of stiffness. Point Overview With Point deform, you select a point on a body or a point in space. A point on a body can be: •
point on an edge
•
point on a face
•
vertex
The point you select is the center of the deformation. You can control the deformation by specifying: •
Deform distance
. The length of the pull of the center of the deformation.
•
Deform radius
•
Bodies to be deformed not belong to a body.
. . Specify in a multibody part environment, or when the point you select does
You can also control the area of the deformation with the Deform region. When the Deform region check box is selected, additional controls appear: •
Fixed curves/edges/faces
•
Additional faces to deform
. Entities not affected by the deformation. .
If items selected as fixed entities contradict with deform entities, the latest item overrides any previous, contradictory item. For example, if you first specified a face to deform, and then specified the same face as fixed, the face would be fixed. •
Deform region check box. Clear the Deform region check box to control the shape of the deformation by selecting an edge or a sketch line, and then specifying a Deform radius creates a bending-type deformation, though not an exact bending.
. The Deform axis
option
With Shape Options, you can also control the shape of the deformation by specifying a level of stiffness.
Deform Curve to Curve Deform Feature Using Curve to Curve You can use Curve to curve deformations to: •
Modify the shape of complex models. deformation on a complex model
•
Change dimensions in an imported model. deformation on an imported model
•
Fill the gaps between surfaces. deformation to fill surfaces
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Chapter 6 Features
There are many options in Curve to curve deformations. Some options are only available with specific selections. However, you can combine options. The procedure below only uses some of these options. See curve to curve options for details and models that display how these options interact. To deform a model using curve to curve:
This procedure uses a multibody part. You select the curves on one body as the Initial curves, and the curves along the second body as the Target curves. 1.
Click Deform
2.
Under Deform Type, select Curve to curve.
3.
Under Deform curves:
a.
on the Features toolbar, or click Insert, Features, Deform.
Select each of the top edges of the block as Initial curves
.
The selected edges, as shown in this example, are outlined in green.
b.
Click in Target curves , and select the bottom circular edge of the round extrude feature, as shown. The selected edge, as shown in this example, are outlined in purple.
6-10
c.
Align the connector along the profiles. A connector is made up of a point along each curve, and the connecting entity between the two points. You can drag the points along each of the curves to synchronize the alignment.
d.
Click either of the connector handles.
e.
Click the arrow on the connector handle - the pointer changes to - to align the direction vectors so that they point in the same direction.
f.
Right-click and select Add Connector.
g.
Repeat Add Connector, and add a connector for each corner of the bottom rectangular profile.
h.
Right-click and select Show Connection Lines.
Align connector
The connection lines should be evenly distributed along the entire perimeter. If they are not, align the connectors. Uneven distribution of the connection lines can cause twisted geometry. i.
Align direction vectors
Align the connectors by dragging the handles on each curve. The connectors should be evenly distributed along the perimeter of the circle, and at the center of each rounded corner. Aligning the Connectors
Add connectors and Show Connection Lines
Note how the perimeter of the rectangular model (green), and the perimeter of the deform preview are parallel along the four sides. 4.
Under Deform Region, click Fixed edges. Fixed curves/edges/faces
and Additional faces to be deformed
appear.
These options are only available when you click Fixed edges. Both of these options are optional. The geometry of your model, and the intended deformation dictate their usage.
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Chapter 6 Features
5.
Click in Fixed curves/edges/faces
, then select the bottom of the base.
6.
Under Shape Options, click Stiffness - medium
7.
Click OK
.
.
If you encounter problems, such as the error message Could not replace geometries, under Shape Options, move the Shape accuracy slider. Other solutions include adding additional connectors, and re-aligning existing connectors. You can also select Ignore warning when a warning message appears. The system attempts to complete the process and provides additional information on what options to modify to maximize success. Deform Feature Curve to Curve Options This type of deformation is based on initial curves and target curves. Deform Curves Under Deform curves, select one or more connected curves as the Initial curves curves as the Target curves
. The curves can be curved or linear, and be part of the model or separate sketches.
Initial curves
6-12
, and one or more connected
Target curves
curve to curve deformation with fixed curve
Fixed curve Deform Region Under Deform Region, you can specify the following options: •
Fixed Edges
•
Uniform
•
Fixed curves/edges/faces
•
Additional faces to deform
•
Bodies to be deformed
Fixed Edges Select Fixed edges to display additional deformation options: •
Fixed curves/edges/faces
•
Additional faces to deform
. Select entities that are unaffected by the deformation. . Select multiple faces to deform.
Clear Fixed edges and specify a Deform radius to create a bending-type deformation, though not an exact bending, with a specified radius. Uniform Select Uniform to create different shape options. Example of deform with Uniform selected and cleared: Uniform is independent of other options under Deform Region. Fixed Curves, Edges and Faces When you specify Fixed curves/edges/faces
, the selected entities are not deformed.
With closed contours of fixed edges, the deformation depends on the position of the Initial curves
:
•
If the Initial curves
are within the closed contour, the deformation is confined to the contour.
•
If the Initial curves
are outside of the closed contour, no point inside the contour is deformed.
Example of the fixed edges option
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Chapter 6 Features
Additional Faces to be Deformed You can select Additional faces to deform
to include additional faces in the deformation.
Example of the additional faces option Bodies to be Deformed Specifying Bodies to be deformed
is geometry-dependent:
•
Required. If the Initial curves
are sketch curves, you must select Bodies to be deformed
.
•
Optional. If you have a multibody part, you can select Bodies to be deformed , after you specify the initial body to deform by selecting the initial and target curves under Deform Curves. Example of the bodies to be deformed option You can use the options Fixed curves/edges/faces , Bodies to be deformed , and Additional faces to deform in any combination, dependent on the geometry of the model and the desired results. If the selected options are conflicting, the latest item overrides any previous, contradictory item. For example, if you first specified a face to deform, and then specified the same face as fixed, the face would be fixed.
Shape Options You can also control the shape of curve to curve deformations by modifying the degree of stiffness, the Shape accuracy
, and the Weight
.
Stiffness There are three levels of stiffness: •
Stiffness - minimum
•
Stiffness - medium
•
Stiffness - maximum
You can combine any stiffness level with the options under Deform Region. Example of shape stiffness levels Shape Accuracy Shape accuracy . The shape accuracy slider controls the surface quality. The default quality can be inadequate in high curvature areas. When you increase the accuracy by moving the slider to the right, you can increase the success rate of the deform feature. Move the slider only as needed; increasing surface accuracy decreases performance.
Minimum Example of shape accuracy
6-14
Maximum
Weight Weight . If you clear Uniform and select Fixed edges, the weight slider appears. The weight slider controls the degree of influence between two options: •
Fixed edges. The entities you specify under Fixed curves/edges/faces
•
Moving curves. The edges and curves you specify under Deform Curves as Initial curves Target curves
. , and
.
Fixed
Moving
Example of weight value Ignore Warning If an error message appears: • Verify your input. In curve to curve deformations, add new connectors or realign existing connectors. •
Verify the preview.
•
Improve the surface quality using Shape accuracy
•
Clear the Uniform check box under Deform Region.
•
Select Ignore warning under Shape Options. The system attempts to complete the deformation process by ignoring small errors. For example, short edges may be merged or the body check may be skipped.
•
If you select Ignore warning, inspect whether the results are topologically and geometrically correct.
•
Read the warning
•
Click Check on the Tools toolbar, or click Tools, Check to check the part. If you get additional, system-generated warnings from HOOPS routines, such as
under Shape Options.
following the build.
Normal vector is of zero or nearly zero length the problematic area is highlighted. Example of Deform with Uniform Selected
Uniform cleared
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Uniform selected
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Chapter 6 Features
Example of Deform Curve to Curve with Fixed Edges
Model with no deformation
Deformation with no fixed edges selected
Fixed curves/edges/faces selected, as shown
Example of Deform Curve to Curve with Additional Faces
(1) Initial curve
, (2) Target curve
Top face selected for Additional faces to be deformed
6-16
.
and Fixed edges/curves/faces
selected
No face selected. The bottom face is affected by the deformation of the body.
Example of Deform Curve to Curve Bodies to be Deformed
Select one body to deform
Select multiple bodies to deform
Example of Deform Curve to Curve Stiffness
No deformation applied Stiffness - minimum
Stiffness - medium
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Stiffness - maximum
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Chapter 6 Features
Example of Deform Shape Accuracy
Accuracy slider - Minimum
Accuracy slider - Maximum
Example of Deform Curve to Curve Weight
Fixed curves/edges/faces
Fixed
6-18
Moving
Fixed
Moving
Fixed
Moving
Deform Point Deform Feature Using Point There are many options in Point deformations. Some options are only available with specific selections. However, you can combine options. The procedure below only includes some only of these options. See point options for details and models that display how these options interact. Point deformation that affects a small area may not display using default image quality settings. Click Tools, Options, Document Properties, Image Quality. To increase the quality, move the Shaded and draft quality HLR/ HLV resolution slider to the right, or select Optimize edge length. To deform a model using point:
1.
Click Deform
2.
Under Deform Type, select Point.
3.
Under Deform point, select these items: •
on the Features toolbar, or click Insert, Features, Deform.
Face. When you select a point on a face, the default Deform direction is perpendicular to the face (Normal to picked is selected). If you clear Normal to picked, select a Deform direction using a linear edge, a sketch line, a planar face, or a plane. If necessary, click to reverse the direction.
a.
•
Edge. When you select a point on an edge, the default Deform direction is an average between the normals to the two adjacent faces (Normal to picked is selected). The location of the edge on the model determines the center of the deformation.
•
Vertex. When you select a vertex, the default Deform direction is an average between the normals to all adjacent faces (Normal to picked is selected).
•
Point. When you select a point in space, there is no default deform direction (Normal to picked is cleared). You must specify the Deform direction, and under Deform Region, you must select one or more bodies to deform.
Select a point on an edge, a point on a face, a vertex, or a point in space as the Deform point
Select a point on an edge
SolidWorks 2004 Reference Guide
Select a point on a face
.
Select a point in space and a Deform direction
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Chapter 6 Features
4.
b.
Click Reverse deform direction
to reverse the direction.
c.
With a point in space as the Deform point , select a linear edge, a face, or a plane as the Deform direction. With a point on an edge, a point on a face, or a vertex, you can keep Normal to picked selected.
d.
Type a value for Deform distance
.
Under Deform Region, select these items: a.
Set a value for Deform radius
.
b.
Select Deform region to confine the deformation to the area enclosed by the perimeter of the face selected. With Deform region you can also select Fixed curves/edges/faces to be deformed
and Additional faces
.
When you select a point on a face, and select Deform region, you can confine the deformation to the area enclosed by the perimeter of the face selected. When you select a point on an edge, a vertex, or a point in space, the deformation is not directly affected by this option. c. 5.
Select Bodies to be deformed
when the model includes multiple bodies.
Under Shape Options: •
Select a level of stiffness. Deform region selected
Deform region cleared
Stiffness - minimum
Stiffness - medium
Stiffness - maximum
6-20
•
Deform axis . When the Deform region check box is clear, you can control the shape of the deformation by selecting a linear edge, a sketch line, a planar face or a plane as a deform axis.
Shape accuracy . Move the slider to control surface quality. Increasing the quality also increases the success rate of the deform feature. For example, if you get an error message Could not replace geometries, move the slider towards the right. Move the slider only as needed; increasing surface accuracy decreases performance. 6.
Click OK
.
Deform Feature Point Options This type of deformation is based on a point and its pull direction vector. Deform Point Point to deform. Under Deform point, you can select a point to deform on a face, an edge,a vertex, or a point in model space. •
Face. Select a point on a face, and the default Deform direction is perpendicular to the face (Normal to picked is selected). If you clear Normal to picked, select a Deform direction by specifying an edge, a sketch line, or a planar face, or a plane. If necessary, click
to reverse the deform direction.
o
Linear edge or sketch line. Deform direction is parallel to the specified entity.
o
Planar face or plane. Deform direction is perpendicular to the planar face or plane.
The location of the point on the face determines the center of the deformation. Example of a point on a face •
Edge. Select a point on an edge, and the default Deform direction is an average between the normals to the two adjacent faces (Normal to picked is selected). If you clear Normal to picked, select a Deform direction in the manner described in the section above. The location of the point on the edge determines the center of the deformation. Example of a point on an edge
•
Vertex. Select a vertex, and the default Deform direction is an average between the normals to the three adjacent faces (Normal to picked is selected). If you clear Normal to picked, select a Deform direction in the manner described in the section above.
•
Point. When you select a point in space, there is no default deform direction (Normal to picked is cleared). You must specify the deform direction. Under Deform Region, you must also select one or several bodies to deform. Example of a point in space
Deform Region The interaction between the options under Deform Point and selecting the Deform region check box independently are as follows: Under Deform Point:
Under Deform Region:
Point on an edge
Deform region check box
Results •
Vertex Point in space Point on a face
• Deform region check box
•
•
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The area of the deformation is not affected by selecting the Deform region check box independently. Other options are enabled The area of the deformation is affected by selecting the Deform region check box independently. Other options are enabled
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Chapter 6 Features
The Deform region check box enables the following options: •
Fixed/curves/edges/faces
•
Additional faces to deform
. Select entities that are unaffected by the deformation. . Select multiple faces to deform.
When the Deform region check box is cleared, it enables an additional option under Shape Options: Deform axis
.
Example of a point on a face and Deform region Deform distance and deform radius. Two of the parameters that control the deformation are distance and radius. •
Under Deform point, specify a Deform distance
.
•
Under Deform Region, specify a Deform radius checkbox to change the Deform radius.
. You do not need to select the Deform region
Example of Deform distance and Deform radius Fixed/curves/edges/faces . Besides Deform distance and Deform radius , you can control the shape of the deformation by selecting one of several curves, an edges, or faces. The selected entities are not deformed. With closed contours, deformation behavior depends on the following: •
If the center of the deformation is within the closed contour, the deformation is confined to the contour.
•
If the center of the deformation does not belong to the closed contour, no point inside the contour is deformed. Example of a fixed curve, edge, or face
If items selected as fixed entities contradict, the latest item overrides any previous, contradictory item. For example, if you first specified a face to deform, and then specified the same face as fixed, the face would be fixed. Additional faces to deform
. You can also select more than one face on the model to deform.
Example of multiple faces Bodies to be deformed
. You can deform more than one body in a multibody part environment.
Example of multiple bodies
Under Deform Region: •
Specify Fixed/curves/edges/faces , and Additional faces to deform select the Deform region check box.
, only when you
•
Select Bodies to be deformed
•
Select each option individually, or combine all three options in the same model.
, with Deform region selected or cleared.
Shape Options You can also control the shape of point deformations by modifying the degree of stiffness, specifying a deform axis, and modifying the Shape accuracy
6-22
.
Stiffness There are three levels of stiffness: •
Stiffness - minimum
•
Stiffness - medium
•
Stiffness - maximum
You can combine the stiffness level with other controls. Example of shape stiffness levels Deform Axis With the Deform region check box cleared, you can control the shape of the deformation by selecting a linear edge or a sketch line as a deform axis. •
The Deform axis
•
The Deform radius specified radius.
determines the shape of the deformation using the Deform radius
.
option creates a bending-type deformation, though not an exact bending, with a
Example of the deform radius axis You can combine the deform axis with stiffness levels. Shape Accuracy Shape accuracy . The shape accuracy slider controls the surface quality. When you increase the accuracy by moving the slider to the right, you can increase the success rate of the deform feature. Move the slider only as needed; increasing surface accuracy decreases performance.
Minimum
Maximum
Point deformation that affects a small area may not display using default image quality settings. Click Tools, Options, Document Properties, Image Quality. To increase the quality, move the Shaded and draft quality HLR/ HLV resolution slider to the right, or select Optimize edge length. Ignore Warning If an error message appears: •
Verify your input.
•
Verify the preview.
•
Improve the surface quality using Shape accuracy
•
Clear the Uniform check box under Deform Region.
•
Select Ignore warning under Shape Options. The system attempts to complete the deformation process by ignoring small errors. For example, short edges may be merged or the body check may be skipped.
•
If you select Ignore warning, inspect whether the results are topologically and geometrically correct.
•
Read the warning
•
Click Check on the Tools toolbar, or click Insert, Tools, Check to check the part. If you get additional, system-generated warnings from HOOPS routines, such as
under Shape Options.
following the build.
Normal vector is of zero or nearly zero length, the problematic area is highlighted.
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Chapter 6 Features
Maintain Boundary Maintain boundary appears only when you select the Deform region check box. Clear Maintain Boundary to reduce the deform region, create new edges and move the boundaries. Additional Faces Only Additional faces only appears when: •
You select the Deform region check box
•
Clear Maintain boundary
When you include the Fixed/curves/edges/faces option, all entities are deformed except the fixed edges. To deform only the top face of the model while fixing one of the edges, select Additional faces only. Example of Deform Select Different Points on Face
Point. Different points selected on the same face. Example of Deform Select Point on an Edge
Point. Different points selected on the same edge.
6-24
Example of Deform Select Point Point. With a point in space, you must always select the Deform direction, and under Deform region, specify the Body to be deformed.
Deform direction. Parallel to the edge of the extrude with draft feature, circled in red.
Deform direction. Perpendicular to the face of the main extrude feature,circled in red.
Example of Deform Region - 1 Both examples use the same initial face to deform, with Deform distance - 60, and Deform radius - 100.
Deform region selected
Deform region cleared
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Chapter 6 Features
Example of Deform Distance and Deform Radius
Deform distance: 20 - Deform radius: 80
Deform distance: 50 - Deform radius: 80
Deform distance: 50 - Deform radius: 40
Deform distance: 80 - Deform radius: 40
Example of Deform Select Curve-Edge-Face
6-26
All examples use the same Deform distance
and Deform radius
Before deform
Deform with no fixed entities selected
Preview of fixed edges
Deform with fixed edges selected
Example of Deform Point with Additional Faces All examples use the same initial face to deform, with Deform distance - 60, and Deform radius - 100.
Single face selected to deform under Deform point
One additional face selected under Additional faces to deform
Two additional faces selected under Additional faces to deform Example of Deform with Multiple Bodies Point on edge selected as Deform point , and face selected as the Deform direction. All examples use Deform distance - 60, and Deform radius - 100.
No additional body selected as Bodies to be deformed
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.
6-27
Chapter 6 Features
One additional body selected as Bodies to be deformed
Two additional bodies selected as Bodies to be deformed
.
.
Example of Deform Point Shape Stiffness All examples use the same options except for the stiffness.
Stiffness - minimum
Stiffness - medium
Stiffness - maximum
Example of Deform with Deform Axis
No deformation
6-28
No Deform axis selected
Edge selected as Deform axis
Example of Deform Maintain Boundary
Maintain Boundary checked
Maintain Boundary cleared
Example of Deform Region - 2 Deform region cleared
Deform region selected
With point on a face selected, clearing or selecting the Deform region check box affects the deformation.
With point on an edge selected, clearing or selecting the Deform region check box does not affect the deformation.
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Chapter 6 Features
Example of Deform Axis
No Deform axis
Edge selected as the Deform axis
Domes You can create one or more dome features simultaneously on the same model. The Parameters in the dome PropertyManager include: •
Faces to Dome
. Select one or more planar or non-planar faces.
you can apply domes to faces whose centroid lies outside the face. This allows you to apply domes to irregularly shaped contours. •
Distance. Set a value for the distance by which the dome expands.
•
Reverse Direction
•
Constraint Point or Sketch . Control the dome feature by selecting a sketch to constrain the shape of the sketch. When you use a sketch as a constraint, the Distance is disabled.
•
Direction. Click Direction , and select a direction vector from the graphics area to extrude the dome in a direction other than normal to the face. As a direction vector, you can use a linear edge or the vector created by two sketch points.
•
Elliptical dome. Specify an elliptical dome for cylindrical or conical models. An elliptical dome's shape is a half ellipsoid, with a height equal to one of the ellipsoid radii.
•
Continuous dome. Specify a continuous dome for polygonal models. A continuous dome's shape slopes upwards, evenly on all sides. If you clear Continuous dome, the shape rises normal to the edges of the polygon.
. Click to create a concave dome (default is convex).
Continuous dome is not available when you use a Constraint Point or Sketch
or a Direction
vector. •
Show preview. Check for a preview. On cylindrical and conical models, you can set Distance to 0. The software calculates the distance using the radius of the arc as a basis for the dome. It creates a dome that is tangent to the adjacent cylindrical or conical face.
6-30
To create a dome:
1.
Click Dome
on the Features toolbar, or click Insert, Features, Dome.
2.
In the PropertyManager, under Parameters, follow the guidelines listed above.
3.
Click OK
.
Example of Dome on Irregular non-Planar Faces
Irregular-shaped, non-planar faces
Dome applied to non-planar faces
Example of Dome with Elliptical Option
Elliptical dome checked
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Elliptical dome cleared
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Chapter 6 Features
Example of Continuous Dome Continuous dome option
Checked
Cleared
Example of Dome with Zero Distance
Conical and elliptical dome features with a Distance of zero.
Drafts Draft Overview Draft tapers faces using a specified angle to selected faces in the model. One application is to make a molded part easier to remove from the mold. You can insert a draft in an existing part or draft while extruding a feature. You can apply draft to solid or surface models. When creating a draft using a parting line with step draft, you can select Perpendicular steps to prevent tapering of the slanted faces. Using the draft feature, you can specify the following: •
Neutral plane
•
Parting line
•
Step draft
Draft Feature Creates a feature that tapers selected model faces by a specified angle, using either a Neutral Plane or a Parting Line. You can apply draft to either solid or surface models. You can also apply a draft angle as a part of an extruded base, boss, or cut.
6-32
To draft a model face to a neutral plane: Example
1.
Click Draft
2.
Under Type of Draft, select Neutral Plane.
3.
Under Draft Angle
4.
Under Neutral plane, do the following:
5.
6.
on the Features toolbar, or Insert, Features, Draft.
, enter the number of degrees.
•
Select either a face or a plane to serve as the neutral plane. The draft angle is measured perpendicular to this plane.
•
Select Reverse direction
to slant the draft to slant in the opposite direction.
Under Faces to draft , select the faces to draft in the graphics area, and choose an item from the Face propagation list if you want to propagate across additional faces: •
Along Tangent. Extend the draft to all faces that are tangent to the selected face.
•
All Faces. Draft all faces extruded from the neutral plane.
•
Inner Faces. Draft all faces extruded from the neutral plane.
•
Outer Faces. Draft all faces next to the neutral plane.
Click OK
.
Example of Draft on Surface
No draft to surface model
Neutral Plane draft applied
Draft with Neutral Plane Using Neutral Plane as the Type of Draft, you can draft some of the outer faces, all the outer faces, some of the inner faces, all of the inner faces, faces that are tangent, or a combination of both the inner and outer faces. Face Propagation
Selection in Graphics Area
Draft Results
None. Only the selected face is drafted. The top face is used as the Neutral Plane in all the examples.
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Chapter 6 Features
Along Tangent. Extend the draft to all faces that are tangent to the selected face. (The faces meet with filleted corners). The outer faces include any of the faces you select on the bass-extrude. All Faces. Draft all faces next to the neutral plane and extruded from the neutral plane. The inner faces include any faces on the three boss-extrudes.
Inner Faces. Draft all inner faces extruded from the neutral plane.
Outer Faces. Draft all outer faces next to the neutral plane.
Neutral Plane The Neutral Plane is the plane or face that you choose to determine the pull direction when creating a mold. The Z axis direction of this chosen plane is the direction in which the part ejects from the mold. Reverse direction changes the direction of the draft, not the direction of the pull. In the example below, Plane 1 is the Neutral Plane, with the arrow indicating the pull direction.
6-34
Parting Line Draft The parting line option lets you draft surfaces around a parting line. The parting line can be non-planar. In a draft using a parting line, you can also include a Step draft. To draft on a parting line, you can first divide the faces to be drafted by inserting a split line, or you can use an existing model edge. Then you specify the direction of pull, or the side of the parting line from which material is removed. You can check the draft angles on your model using the draft analysis tool. Draft analysis creates a color-coded rendition of the model faces based on the angle and the direction of pull criteria that you specify. To insert a draft angle parting line:
1.
Sketch the part to be drafted.
2.
Insert a split line curve, if desired.
3.
Click Draft
4.
Under Type of Draft, select Parting Line.
on the Features toolbar or click Insert, Features, Draft.
Under some conditions, select the Allow reduced angle check box. 5.
Under Draft Angle, enter the Draft angle
.
6.
Under Direction of Pull, select an edge or face in the graphics area to indicate the direction of pull. Note the arrow direction, and click Reverse Direction
7.
Under Parting Lines
if desired.
, select the parting lines in the graphics area.
Note the arrow direction. To specify a different draft direction for each segment of the parting line, click the name of the edge in the Parting Lines box, and click Other Face.
First draft direction
Other Face selected
NOTE: In this example, all parting lines were selected, using the same face. 8.
9.
Choose the Face propagation type: •
None. Draft only the selected face.
•
Along Tangent. Extend the draft to all faces that are tangent to the selected face.
Click OK
.
Draft applied with first direction
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Draft applied with Other Face
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Chapter 6 Features
Allow Reduced Angle Option The Allow reduced angle check box is available only with Parting Line draft. NOTE: When you select this option, the draft angle on some portions of the drafted face may be smaller than the specified draft angle.
Use the Allow reduced angle check box under the following condition: The normal of one or more side faces adjacent to the edge and the faces being drafted is nearly perpendicular to the Direction of Pull. With this model type and condition, select the Allow reduced angle check box when the maximum angle between the pull direction and the normal of the steep face, plus the draft angle, is greater than or equal to 90°. The vertical blue arrow represents the Direction of Pull (Top plane). The red arrow represents the surface normal at its maximum angle to the pull direction. When the sum of the angle produced by the maximum angle and the Draft Angle is 90° or greater, select the Allow reduced angle check box to create the draft.
Draft applied (Draft Angle
is 25°).
The image above displays the same 25° draft applied. However, it is enhanced by applying an offset face and displaying curvature on the offset face.
In this example, the draft angle towards the narrow ends of the drafted face is reduced below the specified 25° to create the draft.
6-36
Parting Line with Step Draft A step draft is a variation of a parting line draft. The step draft creates one face rotated about the plane used as the Direction of Pull. This results in small faces, reperesenting the steps (highlighted in blue in the example below).
Model with parting line
Parting line draft
Parting line with step draft
You can check the draft angles on your model using the draft analysis tool. Draft analysis creates a color-coded rendition of the model faces based on the angle and the direction of pull criteria that you specify. To insert a draft angle using parting line with step draft:
1.
Sketch the part to be drafted.
2.
Create a plane.
3.
Create desired parting line. Make sure that: •
4.
At least one parting line segment is coincident to the parting plane on each draft face. • All other parting line segments are in the pull direction of the plane. • None of the parting line segments are perpendicular to the plane. Insert a split line curve.
5.
Click Draft on the Features toolbar or click Insert, Features, Draft.
6.
Under Type of draft, select Step Draft. •
•
Select Tapered steps if you want the surfaces to generate in the same manner as the tapered surfaces. Select Perpendicular steps if you want the surfaces perpendicular to the original main face.
7.
Under Draft Angle
8.
Under Direction of Pull, do the following: • •
, enter the number of degrees.
Select a plane to indicate the direction of the pull. Select Reverse direction to slant the draft in the opposite direction.
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Chapter 6 Features
9.
Under Parting Lines • • •
, do the following:
Select the parting line segments in the graphics area. Note the direction of the preview arrow. Click Other Face to specify a different draft direction for each segment of the parting line. Select the Face propagation type: None. Draft only the selected face. Along Tangent. Extend the draft to all faces that are tangent to the selected face (faces that meet with fillets or rounds.)
10. Click OK
.
Tapered and Perpendicular Draft Steps
Model with no draft applied
Tapered steps applied
Perpendicular steps applied
Extrudes Extrude Feature An extrude operation can either add material to a part (in a base or boss) or remove material from a part (in a cut or hole). Extrude extends a sketched profile in one or two directions as either a thin feature or a solid feature.
A circle extruded as a solid feature
6-38
A circle extruded as a thin feature
A rectangle extruded as a solid feature
A rectangle extruded as a thin feature (with draft)
You can also extrude in a direction other than normal to the profile of the sketch by selecting a direction vector.
Extrude Feature Overview When you extrude a feature you specify an extrusion End Condition. Depending on the type of extrusion you select, additional options are available. Extrude Direction •
Observe the preview to verify the direction and depth of the feature.
•
Select the parameters under Direction 1 to extrude the feature in one direction from the sketch plane.
•
Select Direction of Extrusion
•
Select the parameters under Direction 2 to extrude the feature in both directions from the sketch plane.
to extrude in a direction other than normal to the profile of the sketch.
End Condition •
If you choose Blind or Mid Plane, you must specify the Depth
•
If you choose Offset From Surface, you must specify the Offset.
.
When you choose Offset from Surface, you can specify Translate Surface. When you specify the Translate Surface option, the end of the extrusion is a translation of the reference surface, rather than a true offset. •
If necessary, select the Reverse offset check box. If the End Condition you specified relies on the selection of a surface or vertex, click that item in the graphics area. The selection is listed in the Face/Plane
•
box.
Up To Body. Specify the body you want to extrude up to in the graphics area. The selection is listed in the Solid/Surface Body box. TIP: You can use Up To Body when making extrusions in an assembly. Up To Body extends the sketch only up to the selected body. If the sketch that you extrude extends outside of the selected face or surface body, Up To Body can do some automatic extension of one analytic face to terminate the extrusion. The Up To Body option is also useful with mold parts, if the body you extrude to has an uneven surface.
Depth Depth
specifies the depth of the extrusion.
Reverse Direction Click Reverse Direction graphics area.
SolidWorks 2004 Reference Guide
to extend the feature in the opposite direction from that shown in the preview in the
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Chapter 6 Features
Link to Thickness Link to Thickness is used on sheet metal parts. Selecting this option automatically links the depth of an extruded boss to the thickness of the base feature. Flip Side Flip Side to Cut appears only when you are extruding a cut. By default, material is removed from the inside of the profile. Selecting Flip Side to Cut removes all material from the outside of the profile.
Default cut
Flip side cut
Draft Click Draft On/Off outward check box.
to add a draft to the feature. Enter a Draft Angle
No draft
10° draft angle inward
. If necessary, select the Draft
10° draft angle outward
Thin Feature Thin Feature adds (or removes) thin-walled volumes to the model. A Thin Feature base can also be used as a basis for a sheet metal part.
6-40
•
Select One-Direction, Two-Direction, or Mid-Plane
•
Enter a Thickness
•
If you selected Two-Direction, enter a Thickness
•
If necessary, select the Cap ends check box and enter a Cap Thickness
for the thin feature. for the second direction. .
Extrude Direction Along Vector You can extrude 2D and 3D sketches normal to the face, or you can select a Direction of Extrusion
.
You can also select a Direction with the Dome feature.
Use any of the following for Direction of Extrusion Cylindrical faces
Linear edges
Conical faces
Linear sketch entities
Planar faces
Reference axes
Sketch points
References planes
Vertices
Points in reference geometry
Example of Translate Surface
Translate Surface cleared
Translate Surface selected
Offset from Surface 7mm
Offset from Surface 27mm
Select the Translate Surface check box when a larger offset is required.
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Chapter 6 Features
End Condition Extrude When you extrude a profile, you need to select a Type from the Extrude Feature dialog box. Isometric View
Top View
Function Blind. Extends the feature from the sketch plane for a specified distance.
Through All. Extends the feature from the sketch plane through all existing geometry.
Up To Next. Extends the feature from the sketch plane to the next surface that intercepts the entire profile. (The intercepting surface must be on the same part.)
Up To Vertex. Extends the feature from the sketch plane to a plane that is parallel to the sketch plane and passing through the specified vertex. Sketch vertices are now valid selections for Up To Vertex extrusions.
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Up To Surface. Extends the feature from the sketch plane to the selected surface.
Offset From Surface. Extends the feature from the sketch plane to a specified distance from the selected surface.
Up To Body. Extends the feature from the sketch plane to a specified body. You can use Up To Body with assemblies, mold parts, or multibody parts.
Mid Plane. Extends the feature from the sketch plane equally in both directions.
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Chapter 6 Features
Extruded Boss/Base Listed below are the steps you follow to create an extruded boss/base feature. For related information about the extrude feature, see the following: •
Extrude feature overview
•
Extrude thin feature
•
Examples of thin features
To create an extruded base or boss:
1.
With a sketch active, click Extruded Boss/Base Extrude.
2.
Under Direction 1, do the following:
on the Features toolbar or Insert, Boss/Base,
•
Select an End Condition.
•
Examine the preview and if necessary, click Reverse Direction direction.
•
To extrude in a direction other than normal to the profile of the sketch, select Direction of Extrusion
to extrude in the opposite
.
•
Enter a Depth
.
•
If necessary, click Draft On/Off
•
Enter a Draft Angle.
•
If necessary, select the Draft outward check box.
to add a draft to the feature.
3.
If necessary, select the Direction 2 check box to apply the extrusion in a second direction. Follow the procedure listed under step 2.
4.
To create a thin-walled feature, select the Thin Feature check box and do the following: •
Select a Type: One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and if necessary, click Reverse Direction the opposite side.
•
Enter a Direction 1 Thickness
• •
If you selected Two-Direction as the Type, enter a Direction 2 Thickness . Click the Cap ends check box to cap the ends of a closed profile base feature and create a hollow part. Enter a Cap Thickness
•
.
.
Click the Auto fillet corners check box to round-off the corners. This applies only to open profile thin based features. Enter a Fillet Radius
5.
to create the thin feature on
Click OK
.
.
For bosses on sheet metal parts, click Link to Thickness tab to link the depth of the boss to the thickness of the base feature.
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Boss/Base-Extrude The Extrude PropertyManager defines the characteristics of extruded features. You can create either solid features or thin features. To create a solid feature:
1.
In the PropertyManager under Direction 1, set the End ConditionType to determine how the feature extends. •
If you choose Blind or Mid-Plane, specify the Depth
.
•
If you choose Up To Vertex, select a Vertex
•
If you choose Up To Surface, specify the the Face/Plane
•
If you choose Offset From Surface, specify the Face/Plane
in the graphics area. in the graphics area. , and enter the Offset Distance
. Click the Reverse Direction check box, if appropriate. TIP: To select a plane, use the flyout FeatureManager design tree. •
If you choose Up To Body, specify the body you want to extrude up to in the graphics area. TIP: You can use Up To Body when making extrusions in an assembly. Up To Body extends the sketch only up to the selected body. If the sketch that you extrude extends outside of the selected face or surface body, Up To Body can do some automatic extension of one analytic face to terminate the extrusion. The Up To Body option is also useful with mold parts, if the body you extrude to has an uneven surface.
2.
If you extrude a cut, you can select Flip side to cut. By default, material is removed from the inside of the profile. Flip Side to Cut lets you sketch the portion that you want to remain, and remove the material surrounding the profile. NOTE: When you extrude a cut, you can create multibody parts, as well as select which bodies are affected by the cut.
3.
If necessary, click Reverse Direction the preview.
to extend the feature in the opposite direction from that shown in
4.
If necessary, click Draft On/Off to add a draft to a feature while you extrude it. Set the Draft Angle, and check the Draft outward check box, if necessary.
5.
To create an extrusion in the other direction, click Direction 2, and follow the same steps.
6.
Click OK
.
To create a thin feature:
1.
In the Extrude PropertyManager, under Direction 1, set the End Condition Type to determine how the feature extends.
2. 3.
Click Thin Feature. For Type, select One-Direction, Mid Plane, or Two-Direction. •
If you choose One-Direction or Mid Plane, set the Thickness
•
If you choose Two-Direction, set the Direction 1 Thickness
. and the Direction 2 Thickness
. 4.
If necessary, select the Cap ends check box and enter the Cap Thickness
SolidWorks 2004 Reference Guide
.
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Chapter 6 Features
5.
6.
If you created an open profile you can select the following options: •
Click the Auto fillet corners check box to automatically create a round at each edge where lines meet at an angle.
•
Enter a Fillet Radius
Click OK
to specify the inside radius of the round.
.
Extrude Thin Feature Whenever you sketch an open profile, you can select Thin Feature in the PropertyManager. Type The Type specifies whether to extrude the thin feature in One-Direction, Mid-Plane, or Two-Direction. •
One-Direction extrudes the sketch in one direction using the specified wall thickness.
•
Mid-Plane extrudes the sketch in both directions, dividing the specified wall thickness equally on both sides of the sketch geometry.
•
Two-Direction extrudes the sketch in both directions, using a different wall thickness on each side of the sketch geometry (as specified for Direction 1 Thickness
and Direction 2 Thickness
).
Wall Thickness The wall thickness specifies the thickness of the thin feature wall. Reverse Reverse Direction allows you to add the wall thickness to the inside of the sketched profile. The default is to add the wall thickness to the outside of the sketched profile. Additional Options For thin feature base extrusions only, you can specify the following additional options: •
Cap Ends - If you create a closed profile sketch, you can use the Cap Ends option. This option covers (caps) the ends of the feature, creating a hollow part. If you select this option, you must also specify the Cap Thickness
•
.
Auto Fillet corners - If you create an open profile sketch, you can use the Auto Fillet corners option. This option creates a round at each edge where lines meet at an angle. If you select this option, you must also specify the Fillet Radius
(the inside radius of the round).
Examples of Thin Feature Extrude
Direction 1 and Direction 2 extude
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Direction 1 and Direction 2 thickness
Cap ends applied to thin feature
Auto fillet corners applied to thin feature
Cut Feature A cut is a feature that removes material from a part or an assembly. With multibody parts, you can use cuts to create disjoint parts. You can control which parts to keep and which parts are affected by the cut. You can create a cut by using any of the following: •
Extrude
•
Revolve
•
Sweep
•
Loft (from one or more sketches)
•
Thicken feature (from a surface)
Cutting Tools You can use features to cut a solid model. The model can be a single part or a multibody part. To cut a solid model with any of these tools:
1.
Display the base model you want to cut.
2.
Create the sketches, based on the feature to use as the cutting tool. The feature you select depends on your base model and the shape you want the cut to produce. Cutting tools include: •
Extruded Cut
•
Revolved Cut
•
Swept Cut
•
Lofted Cut
•
Thickened Cut
•
Cut with Surface
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Chapter 6 Features
3.
Use the feature to cut the base model.
Extruded Cut
Revolved Cut
Swept Cut
Lofted Cut
Thickened Cut
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Cut with Surface
Surface Cut With multibody parts, you can select which bodies to keep when you use a surface to cut multiple parts. You can cut a solid body with a plane, as well as with a surface.
To cut a solid body with a surface or a plane:
1.
Click Insert, Cut, With Surface. The SurfaceCut PropertyManager appears.
2.
Select the surface or the plane to use for the cut.
The surface or the plane appears under Surface Cut Parameters. 3.
Examine the preview, and if necessary, click
Flip cut to reverse the direction of the cut.
The arrow points in the direction of the solid to discard.
4.
With multibody parts, under Feature Scope, select one of the following: •
All bodies. The surface cuts all bodies every time the feature regenerates. If you add new bodies to the model that are intersected by the cutting surface, these new bodies are also regenerated to include the cut.
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Chapter 6 Features
•
Selected bodies. The surface cuts only the bodies you select using the pointer . If you add new bodies to the model that are intersected by the cutting surface, you need to use Edit Definition to select those bodies, and to add them to the list of selected bodies. If you do not add the new bodies to the list of selected bodies, they remain intact.
•
Auto-select. The option is selected by default, and is only available if you click Selected bodies. When you first create a model with multibody parts, the cutting surface automatically processes all the relevant intersecting parts. The Auto-select option is faster than the All bodies option, since it processes only the bodies on the initial list, and does not regenerate the entire model. If you click Selected bodies, and clear Auto-select, you must select the bodies you want to cut from the graphics area. The solid bodies you select are highlighted in the graphics area, and listed in the Feature Scope box. In the example below, only the yellow body (third from the right), was not selected.
5.
Click OK , right-click the surface in the FeatureManager design tree, and select Hide Surface Body to hide the cutting surface.
The bodies are cut and the cutting surface is hidden.
Extruded Cut When you use the Extruded Cut Preview
tool, you can display an additional PropertyManager by selecting Detailed
to enhance details and choose entities to display.
To create an extruded cut:
1.
With a sketch active, click Extruded Cut
2.
Under Direction 1: •
Select an End Condition.
•
Click in Direction of Extrusion, other than normal to the sketch.
on the Features toolbar or click Insert, Cut, Extrude.
then select an entity to extrude the feature in a direction
Example of extrude along direction vector • •
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Examine the preview and if necessary, click Reverse Direction direction. If necessary, select Flip side to cut.
to extrude in the opposite
•
Click Draft On/Off
to add a draft to the feature.
•
Enter a Draft Angle.
•
Select Draft outward to change the draft direction.
3.
If necessary, select Direction 2 to apply the cut extrude in a second direction. Follow the procedure listed under step 2 above.
4.
To create a thin-walled feature, select Thin Feature and do the following:
5.
6.
7.
•
Select a Type: One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and if necessary, click Reverse Direction the opposite side.
•
Enter a Direction 1 Thickness
•
If you selected Two-Direction as the Type, enter a Direction 2 Thickness
to create the thin feature on
.
With multiple sketch entities, click Selected Contours
.
:
•
In the graphics area choose the sketches you want as the cutting tools.
•
In the PropertyManager, the selections appear in Selected Contours
.
With multibody parts, click Feature Scope: a.
In the graphics area, select the bodies you want cut for Solid Bodies to Affect
b.
In the PropertyManager, select the scope of the operation.
c.
Click OK
d.
Click OK to exit the PropertyManager.
Click OK
, and in the Bodies to Keep dialog box, select which bodies to keep after the cut.
.
Cut extrude
Flip side to cut selected
Cut extrude with Draft
Cut extrude with Thin Feature
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.
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Chapter 6 Features
Example of Extrude - Direction of Extrusion You can specify extrude direction with 2D and with 3D sketches by specifying a direction vector as the Direction of Extrusion. Direction vectors include: Cynlindrical faces
Linear edges
Reference axes
Vertices
Points in reference geometry
Conical faces
Sketch points
Linear sketch entities
Reference planes
Planar faces
Preview - normal extrude Sketch entity used for Direction of Extrusion
Extrude applied Using sketch for Direction of Extrusion Example of Cut Extrude Selected Contours
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Example of Cut Extrude Feature Scope
Select body to cut
Keep all bodies after cut
Select bodies to keep after cut
Fillets Fillet You can create different types of fillets. The PropertyManager dynamically displays the appropriate options, based on the type of fillet you create. Fillets include previews for all fillet types. You can select a Partial preview, a Full preview, or No preview in the Fillet PropertyManager. If you choose a face or more than one edge on the model and select Partial preview, you can cycle through all the filleted edge previews. To view each fillet preview in turn, press A (the default toggle key). Example You can select an edge or you can apply a fillet to a feature. Using Select Feature or Select Loop on the shortcut menu applies the same radius fillet to all edges that make up the feature. Example
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Chapter 6 Features
To create a constant radius fillet or round:
1.
Click Fillet
on the Features toolbar, or Insert, Features, Fillet/Round.
2.
Select the edges, loops, and faces you want to fillet in the graphics area - or right-click on the feature and choose Select feature to fillet all the edges on the feature.
3.
Under Fillet Type, select Constant radius.
4.
Under Items to Fillet, do the following: •
Specify the Radius
•
Verify that the edges you want to fillet are displayed in the Edges
•
If necessary, select the Multiple radius fillet check box. Then highlight each Edge, and specify the Radius
5.
box.
for that edge.
•
The default setting is Tangent propagation. It extends the fillet to all faces that are tangent to the selected face. Click to clear the Tangent propagation check box, if necessary.
•
Select Partial preview to see only the first edge preview in a series, Full preview to see a fillet preview of all the edges, or No preview to prevent any preview. No preview improves rebuild time with complex models.
If your model includes cut or boss features, use Keep features under Fillet Options when you apply a fillet radius large enough to absorb the cut or boss feature. Clear the check box if you want the features absorbed by the fillet. Example If the feature you want to fillet is an attachment, you can omit the fillet from the attachment edges. Under Fillet Options, Feature attachment, click the Omit attach edges check box. Example
6.
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Click OK
.
Other fillet topics: Fillet Overview
Full Round Fillet
Constant Radius Fillet
Round Corner Fillet
Variable Radius Fillet
Multiple Radius Fillet
Setback Fillet
Face Blend Fillet
Example of Fillet Selections
Click on face
SolidWorks 2004 Reference Guide
Use Select Feature on the shortcut menu
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Chapter 6 Features
Fillet Keep Features Options
Model with no fillets
Model with Keep features applied to fillets for front boss and right cut features
Model with Keep features applied to all fillets
Example of Fillet Omit Attach Edges
Omit attach edges check box checked: attachment edge without the fillet
Omit attach edges check box cleared: fillet included on the attachment edge
Example of Fillet by Feature
Select one or more features
6-56
Fillet applied to all features
Fillet Overview Fillet/Round creates a rounded internal or external face on the part. You can fillet all edges of a face, selected sets of faces, selected edges, or edge loops. Select a Partial preview, a Full preview, or No preview in the Fillet PropertyManager. Fillets now include previews with all fillet types except face fillets and full round fillets. If you choose a face or more than one edge on the model and select Partial preview in the Fillet PropertyManger, you can cycle through all the filleted edges. To view each fillet preview in turn, press A (the default toggle key). Example Fillets include the following types: Full round fillet. With full round fillets, you can select three adjacent face sets (two or more tangent faces), and apply a fillet that is tangent to the three face sets.
Full Round Fillet
Constant Radius Fillet
Multiple Radius Fillet
Round Corner Fillet
Setback Fillet
Variable Radius Fillet
Face Fillet
Recommendations for Fillets In general, it is best to follow these rules when making fillets: •
Add larger fillets before smaller ones. When several fillets converge at a vertex, create the larger fillets first.
•
Add drafts before fillets. If you are creating a molded or cast part with many filleted edges and drafted surfaces, in most cases you should add the draft features before the fillets.
•
Save cosmetic fillets for last. Try to add cosmetic fillets after most other geometry is in place. If you add them earlier, it takes longer to rebuild the part.
•
To enable a part to rebuild more rapidly, use a single Fillet operation to treat several edges that require equal radius fillets. Be aware, however, that when you change the radius of that fillet, all the fillets created in the same operation change.
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Chapter 6 Features
Example of Fillet Previews
Constant radius fillet using Partial preview
Constant radius fillet using Full preview
Variable radius fillet
Constant Radius Fillet To fillet multiple model edges or faces:
6-58
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, click Constant radius.
3.
Under Items to Fillet, do the following: •
Enter a Radius
.
•
In the graphics area, select Edges, Faces, Features and Loops
•
Clear the Tangent propagation check box if you do not want the fillet to extend to all faces that are tangent to the selected face or edge.
•
Select Full preview, Partial preview, or No preview.
to fillet.
Tangent Propagation Tangent edges
Starting with a block, apply a fillet to the edge, as shown.
Edge selected to fillet
Result: Example of fillet with Tangent propagation check box checked
Result: Example of fillet with Tangent propagation check box cleared
4.
5.
Under Fillet Options, do the following: •
If necessary, clear the Keep features check box. Example
•
If necessary, click the Round corners check box.
•
Select the Overflow Type.
Click OK
.
Overflow Type •
Default. The system chooses one of the following options, depending on the geometry conditions (convexity of edges being filleted and the adjacent edges, and so on).
•
Keep edge. Maintains the integrity of adjacent linear edges. However, the fillet surface is broken into separate surfaces, and in many cases the top edge of the fillet may have a dip in it.
•
Keep surface. Uses the adjacent surface to trim the fillet. As a result, the fillet edge is continuous and smooth, but the adjacent edge is disturbed.
Keep edge
SolidWorks 2004 Reference Guide
Keep surface
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Chapter 6 Features
Multiple Radius Fillet Using multiple radius fillets, you can create fillets with the following features: •
Select a different radius value for each selected edge.
•
Create corners using three edges with different radii that meet at a common vertex.
•
Select surfaces as well as edges. However, you cannot assign multiple radii to faces with common edges.
•
Select a Full preview, a Partial preview, or No preview in the Fillet PropertyManager.
To create multiple radius fillets:
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, select Constant radius.
3.
Under Items to Fillet, do the following: •
Select the Multiple radius fillet check box.
•
Enter the Radius
•
In the graphics area, highlight the Edges, Faces, Features and Loops
for the first edge or loop. to fillet.
The edge or loop and the radius is listed in the Edges, Faces and Loops box. •
Enter the Radius
for the next edge or loop to fillet, and in the graphics area, select the next
Edges, Faces and Loops
.
Repeat until you have selected all the edges to fillet.
4.
•
The default setting is Tangent propagation. It extends the fillet to all faces that are tangent to the selected face. Clear the Tangent propagation check box, if necessary.
•
Select Full preview, Partial preview, or No preview.
If necessary, under Fillet Options, clear the default Keep features check box. Example
5.
Click OK
.
Dimensions for multi radius fillet
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Multi radius fillets applied
Round Corner Fillet Fillets with round corners allow you to control the transition between edges at the corners. A rounded fillet blends the adjoining edges, eliminating or smoothing the sharp juncture where the two edges meet. To create round corner fillets:
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, keep the default Constant radius.
3.
Under Items to fillet, do the following: •
Clear the Tangent propagation check box.
•
Enter a Radius
•
In the graphics area, select two or more adjacent Edges, Faces, Features and Loops
. to fillet.
- or right-click on the feature and choose Select feature to fillet all the edges on the feature. • 4.
Select Full preview, Partial preview, or No preview.
Under Fillet Options, click Round corners. If necessary clear the Keep features check box.
5.
Click OK
.
Fillets applied without Round corners
Fillets applied with Round corners
Example of Full Round Fillet
Two instances of a full round fillet applied to tangent face sets
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Chapter 6 Features
Single instance of a full round fillet applied to tangent face set
Setback Fillet With setback fillets, you can create a smooth transition between the blended surface, along the edge of the part, into the fillet corner. You select a vertex and a radius, and then assign the same or different setback distances for each edge. The setback distance is the point along each edge at which the fillet starts to blend into the three faces that meet at the common vertex. Example of Setback Fillet Preview
Setback fillet shown with Full preview, and
Setback fillet shown with Full preview, and
with the same setback Distance applied to all three edges.
with a different setback Distance to all three edges.
Setback Distance (12mm)
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of 12mm
uniform for all edges
applied
Setback Distance different for all edges (4mm, 8mm, and 12mm)
To create setback fillets:
1.
Create a part that includes edges, meeting at a vertex, that you want to blend together.
2.
Click Fillet
3.
Under Fillet Type, keep the default Constant radius.
4.
Under Items to Fillet, do the following:
on the Features toolbar or click Insert, Features, Fillet/Round.
•
Select the Multiple radius fillet check box.
•
Clear the Tangent propagation check box.
•
In the graphics area, select three or more edges with a common vertex. You must select all the edges that meet at the common vertex.
The edges are listed in the Edge, Faces, Features and Loops • 5.
Select Full preview, Partial preview, or No preview.
If you want to apply the same setback distance to all edges, do the following: •
Under Setback Parameters, enter a Distance
•
Select one or more vertices for the Setback Vertices
•
Click Set All to apply equal setback distances to all edges on each vertex.
The values are displayed in the Setback Distances box 6.
box.
. box.
and on the callouts in the graphics area.
If you want to apply a different setback distance to each edge, do the following: •
Select one or more vertices for the Setback Vertices
•
Select Vertex <1> in the Setback Vertices box
•
Select the first edge (E1) in the Setback Distances box
•
Enter a Distance
•
Select the next edge (E2) belonging to Vertex <1>, and enter a Distance
•
Repeat the process for all edges belonging to Vertex <1>.
•
To apply the same Setback Distances Set Unassigned. The current Distance
•
box. . .
for the first edge (E1).
to all unspecified edges in the remaining vertices, click
is applied to all remaining vertices.
To apply different Setback Distances
to the remaining vertices, repeat the process for each
vertex (Vertex <2>, Vertex <3>, and so on) in the Setback Vertices box 7.
Click OK
SolidWorks 2004 Reference Guide
for that edge.
.
.
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Chapter 6 Features
Example of Setback Fillets
Model with no setback fillets applied
Model with preview of selected edges
Model with preview of setback callouts
Model with setback fillets applied
Variable Radius Fillet You can create variable radius fillets by specifying a different radius for each vertex of the edges you want to fillet. Variable radius fillets work on both solid and surface models. Between the two vertices in a sketch entity, there are variable radius control points that operate as follows: •
You can assign a radius value to each control point, or just assign values to one or both enclosing vertices.
•
The system defaults to three control points located at equidistant increments of 25%, 50%, and 75% along the edge.
•
You can change the relative position of each control point.
•
You can add or subtract control points along the edge you select to fillet. Adding or subtracting control points along the edge positions the control points in equidistant increments along the edge you select. Example of variable radius control points and tips on how to use them with a part.
To insert variable radius fillets:
1.
Click Fillet
2.
Under Fillet Type, select Variable Radius.
3.
Under Items to Fillet, do the following: o
on the Features toolbar or click Insert, Features, Fillet/Round.
Select the edges to fillet in the graphics area. NOTE: If you want to position and assign radii to the control points between the vertices, select a single edge, assign a value to the vertices first, and then manipulate the control points for that sketch segment. Once the first sketch segment is complete, select the second sketch segment, and repeat the process. The edges are listed in the Edges, Faces, Features, and Loops
box.
Under Variable Radius Parameters, the vertices are listed in the Attached Radii
6-64
o
Clear Tangent propagation if necessary.
o
Select Full preview, Partial preview, or No preview.
box.
4.
5.
If you want to apply the same radius to all unassigned vertices in the Attached Radii following: a.
Under Variable Radius Parameters, enter a Radius
b.
Click Set All to apply equal radii to all vertices.
box, do the
.
To apply a different radius to all unassigned radii, do as follows: o
Under Variable Radius Parameters, select V1 in the Attached Radii radius to V1.
o
Enter a Radius
o
Select V2 in the Attached Radii
o
o
box to assign the
for the first vertex. box, and enter a Radius
for the second vertex.
To apply the same radius to all remaining vertices (and still retain the value assigned to V1), click Set unassigned. To keep applying different radii to the remaining vertices, select the remaining unassigned vertices in the Attached Radii
box, and enter a Radius
for each.
NOTE: You do not have to assign radius values to all the vertices in the Vertex list. However, you must assign a radius value to at least one vertex for each chain of edges. The software calculates the radii of the unassigned vertices, based on the following:
6.
o
the values of the adjacent vertices to which you have assigned radius values
o
the length of edges that connect the vertices
To apply radius values and manipulate control points, do the following: o
Select the first unassigned control point in the graphics area, located by default at 25%. NOTE: You can leave one or all control points unassigned.
o
Changing control point position: If necessary, drag the control point to a new position. The pointer changes to
o
.
Enter a radius value in the callout, or select P1 in the Attached Radii
box, and enter a Radius
. o
o o
To apply the same radius to all remaining control points (and still retain the value assigned to P1), select the remaining control points (P2 and P3), and click Set unassigned. If necessary, repeat the process for the remaining control points, P2 and P3. Add control points: If necessary, you can add additional control points by selecting the control point, pressing Ctrl and dragging the new control point into position. Or, from the PropertyManager, you can increment the value in the control points box . Adding new control points through the PropertyManager places the points at default positions. If necessary, you can then drag the control points to a new position.
o
Subtract control points: You can remove specific control points by right-clicking, and selecting Delete from the shortcut menu. Or, from the PropertyManager, you can decrement the value in the control points box . Deleting new control points through the PropertyManager removes the points from the default positions. NOTE: You can edit radius values for vertices or control points, but you cannot add new control points after you first build the part.
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Chapter 6 Features
7.
8.
Select a transition type. •
Smooth transition creates a fillet that changes smoothly from one radius to another when matching a fillet edge to the adjacent face.
•
Straight transition creates a fillet that changes from one radius to another linearly without matching edge tangency with an adjacent fillet.
Click OK
.
NOTE: You can remove an assigned radius value by selecting the vertex in the Attached Radii
box,
and pressing Delete. Radius values calculated by the software are not shown in the Attached Radii box or in the Radius
box.
Example of Variable Radius Fillet
Model with tangent faces
Edges to fillet
Variable radius fillets applied
To change radius values after they are inserted:
1.
Double-click the VarFillet feature in the FeatureManager design tree.
2.
Double-click and modify the dimensions displayed on the vertices in the graphics area. Radius values calculated by the software are not shown in the graphics area.
3.
4.
You can modify the value and position of control points: •
Select the control point in the Attached Radii in the graphics area.
box, or double-click and modify the dimension
•
Select the control point, the pointer changes to
, and drag the control point to the new position.
Click OK
.
Example of Variable Radius Fillet on Surface
No fillet applied to revolved surface
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Variable radius fillets applied to revolved surface
Example of Variable Radius Control Points
No control points
Variable radius control points
With control points
Using Variable Radius Control Points You can manipulate and assign radius values to the control points between the vertices of a variable radius fillet. Variable radius fillets now include previews. You can select a Full preview, a Partial preview, or No preview in the Fillet PropertyManager. TIPS: Here are some some tips on how to use variable radius fillet control points: •
You can assign a radius value to each control point, or just assign values to one or both enclosing vertices.
•
The system defaults to three control points located at equidistant increments of 25%, 50%, and 75% along the edge between the two variable radii.
•
You can change the relative position of each control point using the following methods:
•
o
Change the percentage of the control point in the callout
o
Select the control point and drag it to a new location
You can add or subtract control points along the edge you select to fillet, either as you create the fillet, or after you create the fillet by using Edit Definition. Adding or subtracting control points along the edge positions the control points in equidistant increments along the edge you select. o
Add control points: You can select a control point and Ctrl-drag to create an additional control point at a new location. Or, from the PropertyManager, you can increment the value in the control points box positions.
o
. Adding new control points through the PropertyManager adds points in the default
Subtract control points: You can remove specific control points by right-clicking, and selecting Delete from the shortcut menu. Or, from the PropertyManager, you can decrement the value in the control points box . Deleting new control points through the PropertyManager removes the points from the default positions.
•
You can select more than one sketch entity to fillet. Complete each entity before selecting any additional entities under Items to Fillet
, in the following manner:
o
Apply a radius to each vertex first
o
Apply radius values to one or all control points
o
Change the position of a control point before or after you apply a radius value
o
Add new control points, if necessary
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Chapter 6 Features
Model with single sketch entity selected and three default, unassigned control points.
Model with radii assigned to control points in default locations. NOTE: If you want to select two sketch segments, assign radii to the vertices and to the control points of the first sketch entity, before selecting any additional sketch entities.
Model with two sketch segments selected, and radius assigned to vertex from the second entity. NOTE: Before assigning radii to the control points, you should assign a radius to the vertex.
Model with two sketch segments selected, and all control points with assigned radii. NOTE: Both the old and new control point position are displayed, but only the new position includes the callout.
You can assign radius values to any number of control points, or leave them as unassigned.
Variable radius fillet applied
Return to Variable Radius Fillet
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Full Round Fillet With full round fillets, you can select three adjacent face sets (one or more tangent faces), and apply a fillet that is tangent to the three face sets. To create a full round fillet:
1.
Open the part to which you want to apply the fillet. Detail on the model
2.
Click Fillet on the Features toolbar, or Insert, Features, Fillet/ Round.
3.
Under Fillet Type, select Full round fillet.
4.
Under Items to Fillet, do the following:
5.
•
For Side Face Set 1 , select the top face, as shown on the right.
•
For Center Face Set , select the side face of the model, as shown on the right.
•
For Side Face Set 2 , select the face opposite Side Face Set 1, as shown. Note: Make sure that the Tangent Propagation check box is selected.
Click OK
.
The full round fillet is applied to one side of the model. Note: You can apply a full round fillet to the other side of the model. However, you need to create the second full round fillet as a separate feature.
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Chapter 6 Features
Full Round Fillet Details Note the following about the sketch used for the sample part on the right:
•
The three sketch entities indicated by the arrows are tangent to each other, as shown above.
•
Vertical relations are applied to the endpoints of the tangent sketch entities, as shown above.
Face Fillet You can blend non-adjacent faces with a face fillet. To insert a face fillet:
1.
Create a part with two or more adjacent, non continuous faces.
2.
Click Fillet
3.
Under Fillet Type, click Face fillet.
4.
Under Item to Fillet, do the following:
on the Features toolbar or Insert, Features, Fillet/Round.
•
Enter a Radius
•
In the graphics area, select first face or set of faces to blend. The selections are listed in the Face Set 1
•
.
box.
Click the Face Set 2
box and select the faces in the graphics area to blend with Face Set 1.
NOTE: If you select more than one face for either Face Set 1 or Face Set 2, each set of faces must be smoothly connected for the face fillet to properly propagate to all faces. • 5.
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces.
Under Fillet Options, you can do either of the following: •
Click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross section as opposed to a circular cross section. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary.
•
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Click the Help point check box to resolve an ambiguous selection. Then click a vertex close to the location where you want to insert the fillet.
6.
Click OK
.
Face Set 1 and Face Set 2 selected
Face fillet applied
Example of Curvature Continuous Fillet
No face fillet
Curvature continuous cleared
Curvature continuous checked
Using Help Point with Face Fillets When creating a face fillet between two faces, it may not be clear where the face blend should occur. Use Help point to define the desired location. Create a Help point by clicking a vertex on the side where you want the face fillet. The fillet is created at the location closer to the Help point.
Face Fillet with Hold Line You can determine the radius and shape of a face fillet by setting a boundary, or hold line, for the fillet. The hold line can be an edge on the part or a split line projected on a face to be filleted. In a face fillet with hold line, the radius of the fillet is driven by the distance between the hold line and the edge to be filleted. To insert a face fillet using an edge:
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, click Face fillet.
3.
Under Item to Fillet, do the following: •
Do not enter a Radius determines the radius.
•
In the graphics area, select first face or set of faces to blend. The selections are listed in the Face Set 1
•
box.
Click the Face Set 2
SolidWorks 2004 Reference Guide
. The distance between the hold line and the edge that is filleted
box, and select the faces in the graphics area to blend with Face Set 1.
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Chapter 6 Features
•
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces. For Face Set 1, select a model face to fillet. For Face Set 2, select an adjacent face from the model to fillet. In this instance, include the additional model face for Face Set 2, to fillet along the entire edge of the model
The Hold line determines where the fillet ends. In this model, the lower edge of the faces selected for Face Set 2. 4.
Under Fillet Options, click the model edge or edges that mark the end of the fillet. The names are listed in the Hold lines box. If necessary, click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross section as opposed to a circular cross section. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary. When you use Hold lines and the Curvature continuous options together, you can select a hold line for each face.
5.
Click OK
.
The faces that share an edge with the hold lines are removed by the fillet. Example of Face Fillet Hold Lines
Faces to fillet
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Hold lines
Face fillet applied
Face Fillet with Split Line A split line is another way of creating a face fillet with a hold line. Instead of selecting an edge as the hold line, you use a split line. To create a face fillet with split line:
1.
Create a split line on a model face.
2.
Click Fillet
3.
Under Item to Fillet, do the following:
on the Features toolbar or Insert, Features, Fillet/Round.
•
Do not enter a Radius the model face).
•
In the graphics area, select first face or set of faces to blend. The selections are listed in the Face Set 1
4.
. The radius is determined by the hold line (the split line you created on
box.
•
Click the Face Set 2
box, and select the faces in the graphics area to blend with Face Set 1.
•
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces.
Under Fillet Options, click the model edge or edges that mark the end of the fillet. The names are listed in the Hold lines box. If necessary, click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross section as opposed to a circular cross section. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary.
5.
Click OK
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.
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Chapter 6 Features
Holes Simple Hole Hole creates various types of hole features in the model. You place a hole and set a depth on a planar face. You can specify its location by dimensioning it afterwards. Recommendations In general, it is best to create holes near the end of the design process. This helps you avoid inadvertently adding material inside an existing hole. Also, if you are creating a simple hole which does not require additional parameters, use Simple Hole. The second option, using Hole Wizard introduces additional parameters that are not required with simple holes. Simple Hole provides better performance than Hole Wizard for simple holes. Hole Wizard
creates holes with complex profiles, such as Counterbore or Countersunk.
To insert a simple hole:
1.
Select a planar face on which to create the hole.
2.
Click Simple Hole
3.
Under Direction 1, do the following to select an End Condition:
or click Insert, Features, Hole, Simple.
•
If you choose Blind, specify the Depth
.
•
If you choose Up to Vertex, select a Vertex
•
If you choose Up to Surface, specify the the Face/Plane
•
If you choose Offset from Surface, specify the Face/Plane
in the graphics area. in the graphics area. , and enter the Offset distance
. Select the Reverse offset check box, if appropriate. To select a plane, use the flyout FeatureManager design tree. 4.
To extrude in a direction other than normal to the profile of the sketch, select Direction of Extrusion
5.
Type in a Hole Diameter
6.
If necessary, click Draft On/Off outward check box, if necessary.
7.
Click OK
to add a draft to the hole. Set the Draft Angle, and select the Draft
.
Normal to sketch extrusion
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.
Direction vector extrusion
.
To position the hole:
1.
Right-click the hole feature in the model or the FeatureManager design tree, and select Edit Sketch.
2.
Add dimensions to position the hole. You can also modify the hole diameter in the sketch.
3.
Exit the sketch or click Rebuild
.
To change the diameter, depth, or type of the hole, right-click the hole feature in the model or the FeatureManager design tree, and select Edit Definition. Make the necessary changes, and click OK. Example of Hole Offset
True offset - Translate surface check box cleared
SolidWorks 2004 Reference Guide
Translated surface - Translate surface check box selected
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Chapter 6 Features
Creating a Simple Hole To create a simple hole:
1.
Select an End Condition to determine how far the feature extends. •
If you choose Blind, specify the Depth
.
•
If you choose Up to Vertex, select a Vertex
•
If you choose Up to Surface, specify the the Face/Plane
•
If you choose Offset from Surface, specify the Face/Plane
in the graphics area. in the graphics area. , and enter the Offset distance
. Select the Reverse offset check box, if appropriate. Select the Translate surface check box if you want to use an offset relative to the surface or the plane selected. If you want to use a true offset, clear the Translate surface check box. TIP: To select a plane, use the flyout FeatureManager design tree. 2.
Type in a Hole Diameter
.
3.
If necessary, click Draft On/Off outward check box, if necessary.
4.
Click OK
to add a draft to the hole. Set the Draft Angle, and select the Draft
.
End Condition Types The Type determines how far the hole extends.
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Blind
Extends the feature from the sketch plane for a specified distance.
Through All
Extends the feature from the sketch plane through all existing geometry.
Up to Next
Extends the feature from the sketch plane to the next surface that intercepts the entire profile. (The intercepting surface must be on the same part.)
Up to Surface
Extends the feature from the sketch plane to the selected surface. Click on a face to specify the surface.
Offset from Surface
Extends the feature from the sketch plane to a specified distance from the selected surface. Click on a face to specify the surface. Specify an Offset.
Up to Vertex
Extends the feature from the sketch plane to a plane that is parallel to the sketch plane and passing through the specified vertex. Click on a Vertex.
Hole Wizard Hole Wizard Overview The Hole Wizard user interface includes the following capabilities: Dynamic Updating The hole type you select determines the capabilities, available selections, and graphic previews. After you select a hole type, you determine the appropriate fastener. The fastener dynamically updates the appropriate parameters. The interface uses a three column format (Property, Parameter 1, Parameter 2), along with an overall graphic preview based on end condition and depth. Parameters may include one or two values. You can adjust the width of each parameters column. In addition to the dynamic graphic preview based on end condition and depth, graphics in the parameter columns show specific details, as they apply to the type of hole you select. Capabilities Functionality includes tabs for the following hole types: •
Counterbore
•
Countersink
•
Hole
•
Tap
•
PipeTap
•
Legacy
When you create a hole using the Hole Wizard, the type and size of the hole, based on the Description, appears in the FeatureManager design tree. You can create holes on a plane with the Hole Wizard, as well as holes on planar faces. Holes on a plane allows you to create holes at an angle to the feature. You can edit the plane you create to use with the Hole Wizard. Pre-Selection and Post-Selection Note the following regarding pre-selection and post-selection of a face when using the Hole Wizard hole: •
When you pre-select a planar face, and click Hole Wizard is a 2D sketch.
on the Features toolbar, the resulting sketch
•
If you first click Hole Wizard 3D sketch.
•
Unlike a 2D sketch, you cannot constrain a 3D sketch to a line. However, you can constrain a 3D sketch to a face.
, and select either a planar or a non-planar face, the resulting sketch is a
Favorite Name For each hole type (except Legacy), you can create, save, update, or delete hole types to include your favorite properties parameters. This allows you to apply any saved hole types to a SolidWorks document.
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Chapter 6 Features
Hole Wizard Holes as Assembly Features You can add any hole wizard hole as an assembly feature that extends through more than one component. Functionality includes display of cosemetic threads on assembly feature holes. Using the Hole Series tab, you can create hole features in the components of the assembly. Unlike other assembly features, the holes are contained in individual parts as externally referenced features. To access hole wizard:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the appropriate tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
Hole Wizard on a Plane
Example of Non-Planar Hole Wizard Hole
NOTE: On models with multiple features, you can add hole wizard holes to any of the features in the model.
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Hole Wizard Hole Placement You can position a single hole created with Hole Wizard. You can also create and position multiple holes, using the initial instance as the seed. To position a single Hole Wizard hole:
1.
Click Hole Wizard to create the Hole Wizard hole, and enter the information in the Parameters column for each Property that you want to customize.
2.
Click Next to display the Hole Placement dialog box.
3.
Drag the hole to its approximate position by clearing the Point
The pointer changes from 4.
Use Dimension hole.
5.
Click Finish.
to
or Add Relations
tool on the Sketch Tools toolbar.
. on the Sketch Relations toolbar to position and fully define the
To create and position multiple Hole Wizard holes:
1.
Create the Hole Wizard hole, selecting the hole type and the parameters.
2.
Click Next to display the Hole Placement dialog box.
3.
Using the Point
4.
Click Dimension
5.
Click Finish.
SolidWorks 2004 Reference Guide
tool, click where you want to create each hole. and add the appropriate dimensions for each hole to fully define.
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Chapter 6 Features
Favorite Hole Types When you select either the Countersink, Counterbore, Hole, Tap, or Pipe Tap tabs, you can create favorite hole types. Favorite hole types can include any of the characteristics that are relevant to that hole type. Once you create a favorite hole type using the appropriate information from the Property and Parameters columns, you add the hole to the files. You can later select the favorite hole type by scrolling down the list, and apply it to the part. You can update (change values, but retain the same favorite name), or delete a favorite hole type. Property Each tab in the Hole Definition dialog box represents a hole type. Select a hole type, and the appropriate changes display in the Property column. For example, the Property column includes a listing for Standard as well as Screw type. For each item listed in the Property column, the appropriate items are displayed in the Parameters column. Return to overview Parameters Each tab in the Hole Definition dialog box represents a hole type. Select a hole type, and the appropriate changes display in the Parameters column, where you enter information to customize each hole type. The listings and previews in the Parameters column vary, depending on which hole type you select. For example, all hole types include, as a Property, a Standard recognized by the industry. The Standard includes definitions such as ISO and JIS. Other descriptions and values, however, depend on which tab (hole type) you select. The different and appropriate parameters are displayed in the Property and Parameters columns. The system also updates dynamically, reacting to the information that you enter in the Parameters column. For example, with a countersink type, you can adjust the Hole Fit & Diameter to be either: Close, Normal, or Loose. As you select each of these values, the diameter changes, based on dimensions you have set in other areas. Close Normal Loose NOTE: Some values do not use the document’s units. Instead, they adopt units based on the selected fastener type. Return to overview
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Delete Favorite Hole To delete a favorite hole type:
1.
Select the appropriate tab from the Hole Definition dialog box.
2.
Scroll down the list of Favorites to select.
3.
Click Delete.
Retrieve Favorite Hole To retrieve a favorite hole type:
1.
Select the appropriate tab from the Hole Definition dialog box.
2.
Scroll down the list of Favorites to select.
Update Favorite Hole To update a favorite hole type:
1.
Select the appropriate tab from the Hole Definition dialog box.
2.
Scroll down the list of Favorites to select.
3.
Enter the information in the Parameters column for each Property that you want to update.
4.
Click Update and click Yes to the prompt to apply the new values to the same favorite hole type.
New Favorite Name Use the New Favorite Name dialog box to add a specific hole wizard configuration to your list. The favorite hole type is available for future holes you create. To add a new favorite name:
1.
Click Hole Wizard want to customize.
, and enter the information in the Parameters column for each Property that you
2.
Under Favorites, click Add to display the New Favorite Name dialog box.
3.
Accept the default name retrieved from the Description, or type in the name of your choice.
4.
Click OK.
Hole Series You can use Hole Series to create a series of holes through the individual parts of an assembly.
The Hole Series is an assembly feature which creates hole features in the components of the assembly. A Hole Series extends through each unsuppressed component in the assembly that intersects the axis of the hole (the components do not have to touch). Unlike other assembly features, the holes are contained in the individual parts as externally referenced features. If you edit a Hole Series within an assembly, the individual parts are modified.
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Chapter 6 Features
To create a Hole Series:
1.
Suppress the components in your assembly that you do not want to be cut by the hole.
2.
Select a plane or planar face in your assembly, and click Hole Wizard Hole, Wizard.
, or Insert, Assembly Feature,
The Hole Definition dialog box appears. 3.
Click the Hole Series tab. The Hole Series is divided into First Part, Middle Parts, and Last Part.
4.
•
The First Part is the part whose face you selected. The counterbored or countersunk hole, if any, is in the First Part.
•
The Last Part is the last part through which the hole passes. The Last Part contains the tap, or the bottom of the hole if it is a blind hole.
•
The Middle Parts are all the other parts through which the hole passes.
If you want all parts of the hole series to be the same diameter if you change the Size property, select the Automatically select middle and end hole sizes based on first hole size check box. This sets the diameters for the middle and last parts by choosing the closest available hole size to the diameter of the first part. The available hole sizes depend on the selected screw type. Select this check box before you set a diameter for the hole in the first part.
5.
Enter parameters for the hole series: a.
b.
c.
On the First Part tab: •
Choose a Standard, Style, Screw type, and Size.
•
If you select a Screw type of C'Bore or C'Sink, choose a Hole Fit.
•
The parameters of the hole appear in the box. You can change the parameters.
On the Middle Parts tab: •
Select a size, or accept the default.
•
Choose a Screw type.
On the Last Part tab: •
Select a Style (Hole or Tap). If you select Tap, choose Bottoming Tapped hole, or Tapped hole. Select from the cosmetic thread display options. If you select Hole, choose a Screw type.
•
For a tapped hole, select a Tap Drill Type. If you select Blind, choose a depth. This is the depth from the front face of the Last Part in the hole series. If you select Up To Next, choose a Thread Type.
• 6.
The parameters of the hole appear in the box. You can change these parameters.
Click Next. The Hole Placement dialog box appears.
7.
Add dimensions to locate the center of the hole, or add sketch points to create multiple holes.
8.
Click Finish to add the holes to your assembly and close the dialog box.
NOTES: •
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You cannot use Hole Series on assembly components which are multiple instances of the same part, unless each instance is a separate configuration of the part.
•
You cannot edit the parameters of a Hole Series hole in an individual part (unless you underive the feature), although you can delete or suppress the hole. To edit the parameters of the hole in context of the assembly, go to the assembly and edit the Hole Series. If you underive the Hole Series hole in an individual part it becomes a Hole Wizard hole with no reference to the assembly.
Hole Wizard Holes Hole Wizard Custom Standards Click Tools, Options, System Options, Data Options, Edit Standards Data to display the Configure Data dialog box. Create Standards To create new hole wizard standards:
1.
On the Standards tab, type a name for Create new standard name.
2.
Select an industrial or national standard in Create from to specify the type of standard.
3.
Click Create. The new standard name appears in the Derived Standards list. The new standard includes data from the selected industrial or national standard.
4.
Click Apply to save your changes and continue editing, or click OK to save your changes and close the Configure Data dialog box.
Delete Standards You can delete derived hole wizard standards. To delete one of your standards:
1.
Select any standard you created from the Derived Standards list.
2.
Click Delete.
3.
Click Apply to save your changes and continue editing, or click OK to save your changes and close the Configure Data dialog box.
Edit Hole Wizard Standards You can edit derived hole wizard standards. To edit the data:
1.
Click Tools, Options, System Options, Data Options.
2.
Click Edit Standards Data.
3.
On the Edit Data tab, select a catalog from the tree.
4.
Expand the catalog, then the chapters and the pages beneath the catalog to select the Hole Wizard hole to edit. Each row in the table refers to a Hole Wizard configuration.
5.
Editing values: •
Change: To change a value, click in the table and edit the value.
For example, under Bolts and Screws , Machine Screws change the Size name, the Pitch, the Diameter, and so on.
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, Hex Screw - Ansi
, you can
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Chapter 6 Features
6.
•
Add. To add a new row of data, scroll to the bottom of the table and type values in the row with the asterisk.
•
Delete. To delete a row of data, click the button at the beginning of the row and press Delete.
Click Apply to save your changes and continue editing, or click OK to save your changes and close the Configure Data dialog box.
Hole Wizard - Edit Standards Data You can create your own standards for Hole Wizard holes by deriving new standards from an existing standard. To customize existing standards, Hole Wizard uses the same database used by the SolidWorks Toolbox add-in. You do not need to have SolidWorks Toolbox installed on your system to create new standards for Hole Wizard holes. To create your own Hole Wizard standards:
1.
Click Tools, Options, System Options, Data Options.
2.
Click Edit Standards Data. The Configure Data dialog box appears.
Counterbore When you select the Counterbore tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The preview also updates, depending on your selections. To access hole wizard and use counterbore type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Counterbore tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a counterbore hole:
1.
Determine what type of fastener you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Metric or JIS. Screw type, select for example Button or Hex Screw. Size, select a size for your fastener. The Description updates.
Preview with the Counterbore tab
NOTE: Once you have selected a type of fastener, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameters for the hole you want to create on your part. •
•
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End Condition & Depth, select an end condition from the list and enter a depth. Note how the preview for the end condition updates and items in the Parameters column change appropriately. Hole Fit & Diameter, select a fit and enter a diameter. Note that when you change the hole fit, the value updates, increasing or decreasing as appropriate.
Preview of Up to Vertex Example of dynamic counterbore values
3.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Note: Setting a Head Clearance value other than 0.00 adds that value to the Counterbore value above it.
Dynamic Changes with Counterbore Holes For example, if you select Up To Vertex: •
The preview updates to show a vertex.
•
In the End Condition & Depth box, the depth becomes unavailable.
•
In the Selected Item & Offset box, the vertex becomes available so you can select a vertex from the graphics area. The offset box becomes unavailable.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Countersink When you select the Countersink tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The preview also updates, depending on your selections. To access hole wizard and use countersink type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Countersink tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a countersink hole:
1.
Determine what type of fastener you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Metric or BSI. Screw type, select for example Flat Head or Oval Head. Size, select a size for your fastener. The Description updates.
Preview with the Countersink tab
NOTE: Once you have selected a type of fastener, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameters for the hole you want to create on your part. •
•
3.
End Condition & Depth, select an end condition from the list and enter a depth. Note how the preview for the end condition updates and items in the Parameters column, change appropriately. Hole Fit & Diameter, select a fit and enter a diameter. Note that when you change the hole fit, the value updates, increasing or decreasing as appropriate.
Preview of Offset From Surface Example of dynamic countersink values
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
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4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Dynamic Changes with Countersink Holes For example, if you select Offset From Surface: •
The preview updates to show an offset.
•
In the End Condition & Depth box, depth becomes unavailable.
•
The Selected Item & Offset box becomes available so you can select an item in the graphics area from which to offset, and enter an offset value.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Hole When you select the Hole tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The graphic preview also displays only information that applies to holes that do not fall into the other identified categories. To access hole wizard and use hole type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Hole tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a hole:
1.
Determine what type of fastener you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Inch or DIN. Screw type, select for example Screw Clearances or Fractional Drill Sizes. Size, select a size for your fastener. The Description updates properly.
Preview with the Hole tab
NOTE: Once you have selected a type of fastener, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameters for the hole you want to create on your part. •
•
3.
Hole Type & Depth, select an end condition from the list and enter a depth. Note how the preview for the end condition updates and items in the Parameters column update appropriately. Hole Diameter & Fit, select a fit and enter a diameter. Note that when you change the hole fit, the value updates, increasing or decreasing as appropriate.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
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4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Preview of Up to Surface Example of dynamic hole values
Dynamic Changes with Regular Holes For example, if you select Up To Surface: •
The preview updates to show a reference surface at which the hole stops. Note that the reference surface does not need to be flat.
•
The Hole Type & Depth box becomes unavailable.
•
The Selected Item & Offset box becomes available so you can select a reference surface in the graphics area at which the hole stops.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Tap When you select the Tap tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The graphic preview also displays only information that applies to tap holes. To access hole wizard and use tap type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Tap tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a tap hole:
1.
Determine what type of tap you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ISO or DIN. Screw type, select a Bottoming Tapped Hole or a Tapped hole. Size, select a size for your tap. The Description updates.
Preview with the Tap tab
NOTE: Once you have selected a tap type, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameter for the hole you want to create on your part. •
3.
Tap Drill Type & Depth, select an end condition from the list and enter a depth if appropriate. Note how the preview for the end condition updates and opens the appropriate items in the Parameters column.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
SolidWorks 2004 Reference Guide
Preview of Through All Example of dynamic tap values NOTE: You can click the Add Cosmetic Thread arrow to display the options. For tapped holes with cosmetic threads created in the Hole Wizard, the hole diameter is the diameter of the tap drill. For tapped holes without cosmetic threads, the hole diameter is the basic major diameter of the thread: the cylinder is at nominal thread diameter. NOTE: To create a hole at the tap drill size for the thread: Make a plain hole with the screw type set to Tap Drills, and choose the appropriate thread size.
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4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Dynamic Changes with Tap Holes For example, if you select Through All: •
The preview updates to show a hole that extends through all of the part.
•
The Tap Drill Type & Depth and the Selected Item & Offset boxes become unavailable.
•
The Tap Drill Diameter & Angle box is displayed. The diameter is available, but the angle is not.
•
The Thread Type & Depth box, available with Tap holes, displays the most likely calculated values, along with the option to change both the thread type and the depth.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
NOTE: For tapped holes with cosmetic threads created in the Hole Wizard, the hole diameter is the diameter of the tap drill. For tapped holes without cosmetic threads, the hole diameter is the outer diameter of the thread. Pipe Tap When you select the Pipe Tap tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The graphic preview also displays only information that applies to pipe tap holes. To access hole wizard and use pipe tap type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Pipe Tap tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a pipe tap hole:
1.
Determine what type of pipe tap you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Inch or DIN. Screw type: select Tapered Pipe Tap. Size, select a size for your pipe tap. The Description updates properly.
Preview with the Pipe Tap tab
NOTE: Once you have selected a pipe tap type, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameter for the hole you want to create on your part. •
3.
Tap Drill Type & Depth, select an end condition from the list and enter a depth if appropriate. Note how the preview for the end condition updates and opens the appropriate items in the Parameters column.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
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Preview of Through All Example of dynamic pipe tap values NOTE: You can click the Add Cosmetic Thread arrow to display the options.
4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Dynamic Changes with Pipe Tap Holes For example, if you select Through All: •
The preview updates to show a hole that extends through all of the part.
•
The Tap Drill Type & Depth and the Selected Item & Offset boxes become unavailable.
•
The Tap Drill Diameter & Angle box is displayed. The diameter is available but the angle is not.
•
The Thread Depth box, available with Pipe Tap holes, displays the most likely calculated value, along with the option to change the depth.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Legacy Use the Legacy tab to edit any holes that you created prior to the SolidWorks 2000 release. When you select the Legacy tab in the Hole Definition dialog box, all the information including the graphic preview, displays in the same format as when you originally created the hole, prior to the SolidWorks 2000 release. NOTE: If you scroll through the list, the Hole type list now includes all the new hole types that are part of the Hole Wizard. To access hole wizard legacy type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Legacy tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To edit a hole created prior to SolidWorks 2000:
1.
With the part open, right-click the hole in FeatureManager design tree and select Edit Definition. The hole type you created is displayed, along with existing dimensions and a preview.
2.
To change a dimension in the Section dimensions box, click-pause-click, then enter a new dimension value.
3.
If necessary, select the End condition from the list.
4.
Specify the Face, Vertex, or Offset, if the end condition requires it.
5.
Click Next.
6.
Drag the hole center to the desired location or dimension the center point as required.
7.
Click Finish.
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Lofts Loft Overview Loft creates a feature by making transitions between profiles. A loft can be a base, boss, cut, or surface. You can manipulate a loft in the following ways: •
Create a loft as a thin feature.
•
Synchronize loft profiles.
•
Control the magnitude and direction of a tangency in a loft.
•
Add, position, and edit new loft sections.
•
Add side tangency to lofts that use guide curves.
•
View the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. When you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. You create a loft using two or more profiles. Only the first, last, or first and last profiles can be points. For a solid loft, the first and last profiles must be model faces or faces created by split lines, planar profiles, or surfaces.
Other loft topics:
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Loft: split line
Loft: guide curve and planar profile
Loft: centerline
Loft: guide curve and non-planar profile
Loft: thin feature
Loft: tangency control
Loft: add sections
Loft: side tangency
Loft Features You can create a loft by connecting profiles. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. To create a loft:
1.
Click Loft
, or Insert, Boss, Loft. Select the profile sketches in order in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. TIP: For each profile, select the point from which you want the path of the loft to travel. In the PropertyManager, the sketches are listed under Profiles
.
2.
Examine the path preview. If necessary, click Move Up or Move Down profiles, or re-select the sketches to connect different points on the profiles.
to adjust the order of the
3.
Under Start/End Tangency: If you want to select a different option for Start tangency type or End tangency type, click Start/End Tangency. •
Select the start and end tangency type.
•
To control tangency, enter a start and an end tangent length in the PropertyManager, or drag the arrows in the graphics area. If necessary, click Reverse Tangent Direction
4.
5.
Under Options, select the following check boxes if necessary: •
Maintain tangency causes the surfaces in the resulting loft to be tangent if the corresponding segments are tangent.
•
Advanced smoothing obtains smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs.
•
Close loft creates a closed body along the loft direction. This connects the last sketch and the first sketch automatically.
•
Show preview displays shaded previews by default. Click to clear the Show preview check box to view the path and the guide curves.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
If you are using guide curves, click Guide Curves as guide curves. If necessary, click Move Up
6.
.
, then select the sketches in the graphics area to use or Move Down
to reorder multiple guide curves.
You can add side tangency between adjacent faces that lie along the path of a guide curve. This creates a smoother transition between the adjacent faces. Select All Faces in the Guide tangency type list. NOTE: For best results when using side tangency, the profiles should also be tangent to the tangency faces at the point where each profile meets the guide curve. Ideal tolerance is 2 degrees or less. Avoid profiles with connection points greater than 2 degrees off tangency.
7.
Under Centerline Parameters: If you are using a centerline parameter as opposed to a guide curve, click
8.
Centerline Parameters , then select the sketch in the graphics area to use as the centerline. Click the Thin Feature check box to create a thin feature. •
Set the Type, and click Reverse Direction
•
Click the Direction 1 Thickness
SolidWorks 2004 Reference Guide
if necessary.
, and if necessary the Direction 2 Thickness
.
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9.
Click OK
to create the loft.
NOTE: After you create a loft, you can add and edit additional loft sections. Other loft topics:
Loft: split line
Loft: guide curve and planar profile
Loft: centerline
Loft: guide curve and non-planar profile
Loft: thin feature
Loft: tangency control
Loft: add sections
Loft: side tangency
Example of Shaded Loft Preview
Loft shaded preview
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Loft feature applied
Example of Loft Control Tangency
Loft with no control tangency
Loft with control tangency
Example of Loft Using Maintain Tangency
Sketch profile with preview
Loft without using Maintain tangency option
Loft using Maintain tangency option
Click Maintain tangency to cause the corresponding surfaces in the resulting loft to be tangent if the corresponding lofting segments are tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs may be converted to splines. Example of Using Close Loft
Shaded loft preview with Close loft cleared.
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Loft with Close loft cleared
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Shaded loft preview with Close loft selected.
Loft with Close loft selected
Click Close loft under Options to create a closed body along the loft direction. This connects the last sketch and the first sketch automatically. Example of Loft with Side Tangency
Loft with side tangency not applied
Loft with side tangency applied
Loft with Thin Feature You can create a Thin Feature loft. To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness .
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, if necessary.
and if using Two-Direction as the Type, a Direction 2 Thickness
Loft Thin Feature Samples
Loft
Loft with thin features
Loft with Non-Planar Profile You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles. The guide curves help you control the intermediate profiles that are generated. View the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. After you create a loft, you can add and edit additional loft sections. To create a loft using non-planar profiles:
1.
Create at least one non-planar profile. The non-planar profile can be a model face or a model edge.
2.
Set up the planes needed for the profile sketches. Use existing planes, or create new planes. The planes do not have to be parallel.
3.
Sketch the profiles.
4.
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Lofted Cut Cut, Loft
on the Features toolbar, or Insert,
•
Lofted Surface on the Surfaces toolbar or Insert, Surface, Loft The non-planar profile is represented by the boss-extrude with rounded top. The planar profiles are sketched on planes 4 and 5.
5.
Under Profile: a.
Select the Profiles to loft in the graphics area. Select the face of the non-planar profile and the other profiles in order, by clicking a corresponding point on each profile. You do not have to select the vertices precisely; the vertex closest to the selection point is used. A shaded preview connecting the selected entities appears in the graphics area.
6.
b.
You can change the synchronization between the profiles by manipulating the connectors.
c.
Examine the preview, and click Move Up
or Move Down
to reorder the profiles.
To control tangency at the start and end of the loft, click Start/End Tangency.
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7.
Under Options, select Maintain tangency, Advanced smoothing, or Close loft, if needed. •
Clear Show preview to display only the profiles and the path.
•
Merge result merges all the loft elements.
8.
To create a loft with thin walls, select the Thin Feature check box.
9.
Click OK
.
Loft with Split Line You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. To create a loft using a split line:
1.
Use a split line to create a non-planar profile on a model face.
2.
Set up the planes needed for the profile sketches. Use existing planes, or create new planes. The planes do not have to be parallel.
3.
Sketch the profiles.
4.
Click one of the following: • •
Loft on the Features toolbar or Insert, Boss, Loft Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar or Insert, Surface, Loft
The planar profile is a circle created on plane 4.
5.
The face created by the split line is projected onto a non-planar face.
Under Profile, do the following: •
Select the Profiles
to loft in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. •
Click Move Up
or Move Down
6.
To control tangency, click Start/End Tangency.
7.
Under Guide Curves
to reorder the profiles.
select guide curves from the graphics area, if needed.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type.
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8.
9.
Under Options, select Maintain tangency, Advanced smoothing, or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
To create a loft with thin walls, click Thin Feature.
10. Click OK
.
Loft with Guide Curve and Planar Profile You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles. The profiles can be either planar or non-planar. The guide curves help you control the intermediate profiles that are generated. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. After you create a loft, you can add and edit additional loft sections. To create a loft using guide curves and planar profiles:
1.
Sketch one or more guide curves.
2.
Sketch the profiles. See recommendations for using guide curves with a loft.
3.
Add relations between the guide curves and the profiles. You can use a combination of: •
•
•
4.
5.
Pierce relations between the guide curves and vertices, user-defined sketch points, or both, on the profile. Coincident relations between vertices, userdefined sketch points, or both, of the guide curves and the profiles. Add these relations to the profile sketches.
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar or Insert, Surface, Loft
Under Profile, do the following: •
Select the Profiles
to loft in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. •
Click Move Up
SolidWorks 2004 Reference Guide
or Move Down
to reorder the profiles.
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6.
You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. To control Start/End Tangency, do the following: •
For Start tangency type select either Normal to Profile, Direction Vector, or All Faces. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
.
•
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
•
Examine the preview and click Reverse Tangent Direction tangent.
•
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
to reverse the direction of the
.
Examine the preview and click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options Example of controlling the tangency magnitude and direction: 7.
Under Guide Curves, do the following: •
Select the Guide Curves
•
Click Move Up
in the graphics area.
or Move Down
to change the order in which to use the guide curves.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type. 8.
9.
Under Options, select Maintain tangency, Advanced smoothing or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness Thickness
10. Click OK
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.
.
, if necessary.
and if using Two-Direction as the Type, a Direction 2
Loft with Guide Curve and non-Planar Profile You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles. The profiles can be either planar or non-planar. The guide curves help you control the intermediate profiles that are generated. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. After you create a loft, you can add and edit additional loft sections. To create a loft using guide curves and non-planar profiles:
1.
Use a split line to create a non-planar profile on a model face.
2.
Sketch one or more guide curves. See recommendations for using guide curves with a loft.
3.
Add a Pierce relation between the guide curves and an edge or vertex on the non-planar face.
4.
Sketch the remaining profiles needed to create the loft. Add Pierce relations between the profiles and the guide curves. The relations should be added to the profile sketches.
Non-planar profile with split line and guide curve 5.
6.
Non-planar profile with split line and guide curve leading to planar profile
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar or Insert, Surface, Loft
Under Profile, do the following: •
In the graphics area, select the split line face and the planar Profiles
in order.
In the graphics area, a shaded preview connecting the selected entities appears. • 7.
Click Move Up
or Move Down
to reorder the profiles.
Under Start/End Tangency: You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. To control Start/End Tangency, do the following: •
For Start tangency type select either Normal to Profile, Direction Vector, or All Faces. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
.
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
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•
Examine the preview and click Reverse Tangent Direction tangent.
•
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
to reverse the direction of the
.
Examine the preview and click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options Example of controlling the tangency magnitude and direction 8.
Under Guide Curves, do the following: •
Select the Guide Curves
•
Click Move Up
in the graphics area.
or Move Down
to change the order in which to use the guide curves.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type. 9.
Under Options, select Maintain tangency, Advanced smoothing or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
10. To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness Thickness
11. Click OK
, if necessary.
and if using Two-Direction as the Type, a Direction 2
.
.
Example of Using Control Tangency in Lofts
Loft between adjacent edges of two surfaces
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Loft preview using zero Start tangency and End tangency
Loft using Normal to profile for both Start tangency and End tangency
Recommendations for Lofts with Guide Curves Consider the following when creating lofts with guide curves. •
Guide curves must intersect all the profiles.
•
There is no limit to the number of guide curves you may use.
•
Guide curves can intersect at points.
•
You can use any of the following items as a guide curve: sketched curves, model edges, or curves of any kind.
•
If a loft fails or twists: o
o
Use loft synchronization to modify the synchronization between loft profiles. You adjust the synchronization by changing the alignment between the profiles. To adjust the alignment, you manipulate the handles which appear in the graphics area as part of the connector. The connector is the poly line connecting corresponding points in both directions. Add a Curve Through Reference Points as a guide curve, selecting corresponding vertices of the profiles to create the curve.
•
Guide curves can be longer than the resulting loft. The loft stops at the end of the smallest guide curve.
•
You can further control the behavior of the loft by creating the same number of segments on all the guide curves. The endpoints of each segment mark corresponding points for transition of the profiles.
Loft Side Tangency You can add side tangency between adjacent faces that lie along the path of a guide curve. This creates a smoother transition between the adjacent faces. NOTE: For best results when using side tangency, the profiles should also be tangent to the tangency faces at the point where each profile meets the guide curve. The ideal tolerance is 2 degrees or less. You can use profiles with connection points up to 30 degrees off tangency before the loft fails. To add side tangency:
1.
Under Profiles
2.
Under Guide Curves
3.
, select the loft profiles in the graphics area. , do the following:
•
Select the guide curves in the graphics area.
•
Select All Faces from the Guide tangency type list.
Click OK
.
Loft with Centerline You can create a loft that uses a variation of a guide curve that acts as a centerline. The sketch planes of all the intermediate sections are normal to the centerline. The centerline may be a sketched curve, a model edge, or a curve. After you create a loft, you can add and edit additional loft sections. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. To use a center line to guide a loft:
1.
Create the profiles.
2.
Sketch a curve, or create a curve. The curve must intersect the area inside each closed profile and any split line faces.
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3.
4.
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar, or Insert, Surface, Loft
Under Profile, do the following: •
Select the Profiles
to loft in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. • 5.
Click Move Up
or Move Down
to reorder the profiles.
Under Start/End Tangency: You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. To control Start/End Tangency, do the following: •
For Start tangency type select either Normal to Profile, Direction Vector, or All Faces. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
.
•
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
•
Examine the preview and click Reverse Tangent Direction tangent.
•
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
to reverse the direction of the
.
Examine the preview and click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options Example of controlling the tangency magnitude and direction 6.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type.
7.
Under Options, select Maintain tangency, Advanced smoothing, or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
8.
Under Centerline Parameters, select the Centerline
sketch in the graphics area.
9.
You can preview the effect of the centerline. Click Number of Sections and adjust the slider to change the number of previews to display in the graphics area. Then click Show Sections
to display the previews
by using the arrows . NOTE: The number of sections you specify affects the shape of the loft. You may need to increase, or decrease, the number of sections to get the desired shape.
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10. To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness Thickness
11. Click OK
, if necessary.
and if using Two-Direction as the Type, a Direction 2
.
.
Loft with Start and End Tangency Control You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. To control Start/End Tangency, do the following:
1.
Under Start/End tangency type select either Normal to Profile, Direction Vector. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
.
2.
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
3.
Examine the preview and if necessary, click Reverse Tangent Direction tangent.
4.
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
5.
to reverse the direction of the
.
Examine the preview and if necessary, click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options
Loft preview using no Start tangency and End tangency
SolidWorks 2004 Reference Guide
Loft using All Faces for both Start tangency and End tangency
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Chapter 6 Features
Add Loft Section You can add one or more loft sections to an existing loft. When you add a section, it creates a loft section and a temporary plane. You can drag the plane to position the new loft section along the axis of the path. You can also use a pre-existing plane (created before the loft feature) to position the new loft section. Once you position the new loft section, you can use the shortcut menu to edit the new loft section. Edit the loft section as you would any other sketch element (dimension, add relations, modify shape, and so on). You can view the loft using zebra stripes as you add the new loft section. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. To add a loft section:
1.
Right-click along the path of the existing loft where you want to add the new loft section, and select Add Loft Section. The Add Loft Section PropertyManager appears with the current loft sections listed. In the graphics area, a temporary plane appears with the new loft section. NOTE: You can click OK in the PropertyManager after adding the new loft section if you do not need to specify a different plane, reposition the loft section, or use the edit functions.
2.
If you want to use the temporary plane, position the plane along the path of the existing loft by doing one of the following: •
Drag the plane along the axis of the path of the existing loft.
•
Place the pointer at one of edges of the plane. The pointer changes to . This allows you to change the angle of the plane and modify the shape of the new loft section.
Drag plane 3.
Rotate plane
If you want to use another previously created plane, click the Use selected plane check box, and select a plane
.
NOTE: The plane you use to add a new loft section must appear before the loft section in the FeatureManager design tree. 4.
Once you position the new loft section, you can do either of the following: •
Click OK
in the PropertyManager to create the loft section.
•
Use the shortcut menu and select Edit Loft Section to add relations, dimension, and so on
If you select Edit Loft Section, a dialog box appears, allowing you to go Back (to reposition the plane), Cancel (the add section process), or Finish.
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5.
Once you define the new loft section, click Finish. The sketch used to add the new loft section appears in the loft feature.
You can delete any sketch you added using Add Loft Section. To delete a new loft section from a loft:
1.
Right click the loft icon in the FeatureManager design tree and select Edit Definition.
2.
In the Loft PropertyManager, select the new sketch in the Profiles box, and press Delete.
3.
Click OK
.
This removes the loft sketch from the loft section, and places it above the loft feature in the FeatureManager design tree. It does not remove the loft section. 4.
To permanently remove the loft section and the sketch from the model, do the following: •
Select the sketch from the FeatureManager design tree.
•
Press Delete.
Example of Loft Add Sections
Add a loft section
Position a loft section
Modify a loft section
Finish a loft section
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Chapter 6 Features
Loft Synchronization This capability allows you to modify the synchronization between loft profiles. You adjust the synchronization by changing the alignment between the profiles. To adjust the alignment, you manipulate the handles which appear in the graphics area as part of the connector. The connector is the poly line connecting corresponding points in both directions. Loft synchronization is available with new or legacy models. The type of control you can apply to connectors depends on: •
Selection sequence. Whether it is the first connector you modify, or whether you modify connectors added to the profile.
•
Type of profile. Connectors in smooth contour profiles react differently than connectors on profiles with non-tangent edges.
•
Guide curves. With guide curves and closed contour profiles, the guide curve defines the start point for the profiles.
Connector control is either global or local: •
Global twist control. The first connector on a profile with non-tangent edges moves from vertex to vertex along an edge. When you select a handle, it moves the connector to the next vertex.
•
Local twist control. When you add connectors to profiles with vertices, those connectors have local twist control. Local twist control means that you can select the handle and drag it along the profile to modify the synchronization between the profiles.
To control connectors using global twist control:
1.
Click a handle
on one of the profiles.
The handle changes color
.
Regardless of the profile you select, the behavior is identical. However, the shape of the loft varies accordingly. 2.
Start to drag towards the vertex on which you want to relocate the connector. The connector moves to the next vertex along the edge you specified. The loft preview updates with the new synchronization.
To add a connector:
1.
Select and edge.
2.
Right-click and chose Add Connector. Once you add connectors to profiles, you can reposition each of these connectors. The number of connectors you can add is based on the number of vertices in the profile.
Once you add new connectors to profiles with vertices, or with smooth contour profiles, you can drag the handles to reposition the connector.
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To control connectors using local twist control:
1.
Click a handle
on one of the profiles.
The handle changes color
.
2.
Drag the connector along the edge to the location you want.
3.
Release the handle. The loft preview updates with the new synchronization.
To move additional connectors:
1.
Select a handle on the new connector.
2.
Drag the connector along the edge in between the vertices.
If you have coincident vertices, you need to select the corresponding vertex to move the initial handle. To move connectors with coincident vertices:
Press Shift and select the handle to twist the corresponding connector. You can also right-click to manipulate connectors using the following techniques: •
Show All Connectors.
•
Reset Connectors. Removes all changes implemented by moving connectors.
•
Hide Connector. Select a handle to remove a connector from the profiles, without deleting it.
•
Hide All Connectors. Hides all connectors, but does not delete them.
Show All Connectors
Hide All Connectors
Hide Connector
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Chapter 6 Features
Example of Loft Synchronization Handles
Loft synchronization handles: The Connector includes two handles linked by poly line.
Patterns and Mirroring Pattern and Mirror Overview Pattern repeats the selected features in an array based on a seed feature. You can create a linear pattern, a circular pattern, a curve driven pattern, or use sketch points or table coordinates to create the pattern. Mirror copies the selected features or all features, mirroring them about the selected plane or face. With multibody parts, you can use the pattern or the mirror feature to pattern or mirror multiple bodies within the same document.
Mirror multibody parts about a plane
Linear pattern in two directions with multibody parts
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•
For a Linear Pattern, select the features, then specify the direction, the linear spacing, and the total number of instances.
•
For a Circular Pattern, select the features and an edge or axis as the center of rotation, then specify: The total number of instances and the angular spacing between instances. – or – The total number of instances and the total angle in which to create the pattern.
•
For a Curve Driven Pattern, select the features and an edge or sketch segment on which to pattern the feature. Then you can specify the type of curve, the curve method, and the alignment method.
•
For a Sketch Pattern, select where to populate a seed feature by sketching points on model face.
•
For a Table Pattern, add or retrieve previously created X-Y coordinates to populate a seed feature on the face of the model.
•
For a Mirror Feature, select the features to copy and a plane about which to mirror them. If you select a planar face on the model, you mirror the entire model about the selected face.
You can also create patterns of patterns, and mirrored copies of patterns, as well as control and modify patterns. For information about using a pattern of components in an assembly, see adding a component pattern.
Patterns of Patterns With multibody parts, you can create a pattern that includes some or all of the multibody parts that you used to create the original multibody part pattern. You can use any of the patterns such as linear, circular, sketch driven, and so on. You have the same options with patterns of patterns in the multibody part environment as you have in the single body environment. For example, you can use more than one direction, skip instances, and so on.
Pattern from existing linear pattern. Some bodies and a single direction selected.
Pattern from existing linear pattern. Some bodies, single direction, and instance to skip selected.
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Chapter 6 Features
To create a pattern of patterns:
1.
Click Mirror on the Features toolbar, or click Insert, Pattern/Mirror. Then select either linear, circular, or curve driven pattern. You can also use a pattern you created using X-Y coordinates (table pattern) or sketch points.
2.
Do one of the following:
3.
•
For a single body pattern, select the pattern feature in the FeatureManager design tree, or select a face on a pattern instance in the model.
•
For a multibody part pattern, under Bodies to Pattern , select the individual instances from the existing pattern that you want to include in the new pattern.
Proceed as described in Linear Pattern, Circular Pattern, or curve driven pattern.
Curve Driven Pattern Overview The Curve Driven Pattern tool on the Features toolbar allows you to create patterns along a planar curve. To define the pattern, you can use any sketch segment, or the edge of a face (solid or surface), that lies along the plane. Like other pattern types, such as linear or circular, you can skip pattern instances, and pattern in one or two directions. Elements specific to curve driven patterns include the following: •
Type of curve. The type of curve you use to create your pattern determines how you specify the number of instances to pattern for both directions. You can base your pattern on an open curve or a closed curve (such as a circle). o
o
o
Direction 1. You can equally space the pattern instances by applying the Equal spacing option. Alternatively, you can specify a distance along the curve between each pattern instance. The distance between the curve or sketch segment and the Feature to Pattern is measured normal to the curve. Direction 2. For Direction 2, you can also apply the Equal spacing option or specify step distances. If you use a closed curve, you can create patterns of concentric rings or rows of identically patterned features. Implicit Direction 2. If you select the Direction 2 check box without specifying a sketch element or edge, an implicit pattern is created. The implicit Direction 2 is based on what you specified for Direction 1.
•
Curve method. You can define the direction of the pattern by transforming how you use the reference curve (an edge, sketch, or curve) on which your pattern is based. The default method is Transform curve, in which the feature you pattern follows the shape of the reference curve. Using Offset curve, the feature you pattern is offset from the reference curve.
•
Alignment method. You can align the features to the original alignment of the seed feature. Alternatively, you can align the features tangent to the direction reference.
Curve Driven Pattern You can create patterns based on a curve. Although curve driven patterns have similarities to linear and circular patterns, they include unique options. Bodies to Pattern. For multibody parts, select a separate body to create a curve driven pattern. You can use all functions such as Direction 2 or Instances to Skip with Bodies to Pattern. Example
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To create a curve driven pattern:
1.
Create a part that includes a feature you want to pattern along a curve.
2.
Click Curve Driven Pattern Pattern.
3.
Under Direction 1, do the following: •
on the Features toolbar, or Insert, Pattern/Mirror, Curve Driven
In the graphics area, click a curve, edge, or a sketch entity, or select a sketch from the FeatureManager to use as the pattern. If necessary, click Reverse Direction to change the direction of the pattern. The examples below use the upper edge of the model as Direction 1.
•
Specify the Number of Instances
•
Specify the Spacing
.
between pattern instances.
- or Select the Equal spacing check box. With equal spacing, the separation between each pattern instance depends on the the curve you select as the pattern, and the Curve method.
Equal spacing check box cleared
Equal spacing check box selected
•
Under Curve method, click either Transform curve or Offset curve.
•
Under Alignment method, click either Tangent to curve or Align to seed.
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Chapter 6 Features
Curve: Transform curve Alignment: Align to seed
Curve: Offset curve Alignment: Align to seed
Curve: Offset curve Alignment: Tangent to curve
Curve: Transform curve Alignment: Tangent to curve
4.
If you want to skip pattern instances, click Instances to Skip, and in the graphics area, select each of the pattern instances to skip. The pointer changes to when you mouse over each pattern instance. Click to select a pattern instance. The coordinates of the pattern instance appear. To restore a pattern instance, click the instance again, or delete the pattern instance from the Instances to Skip box. If you want to pattern only the geometry (faces and edges) of the features, rather than patterning and solving each instance of the feature, under Options, click to clear Geometry Pattern. NOTE: In some cases, the geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.
5.
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
NOTE: If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern , select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself. NOTE: When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
•
6.
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To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
Click OK
to create the curve driven pattern.
, select the the body to
To create a curve pattern in two directions: Example
1.
Follow steps 1-5 above to create a linear pattern in Direction 1. NOTE: You can select the Features to Pattern, Faces to Pattern, or Bodies to Pattern, and the Options before or after you select Direction 2.
2.
Under Direction 2, do the following: •
In the graphics area, click a curve or an edge to use as the pattern direction. In the example below, the right edge is selected. If necessary, click Reverse Direction pattern.
to change the direction of the
•
Set the Spacing
between pattern instances.
•
Set the Number of Instances
•
Select the Pattern seed only check box to replicate only the seed pattern. Selecting the Pattern seed only check box, creates a curve pattern under Direction 2, without replicating the curve pattern created under Direction 1.
.
TIP: The Pattern seed only option is especially useful when creating patterns in two opposite directions. Use Pattern seed only to prevent duplicate copies of the feature in the same location. 3.
4.
If you want to include specific pattern instances to skip, do the following: •
Click Instances to Skip
•
In the graphics area, select each pattern instance you want to skip. The pattern instances along with their coordinates are listed in the Instances to Skip box.
Click OK
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.
.
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Chapter 6 Features
Example of Multibody Part with Curve Driven Patterns
Multibody part with Body to Pattern
Curve driven pattern applied
Example of Curve Pattern in Two Directions
Pattern seed only
Pattern all instances
Linear Pattern Creates multiple instances of selected features along one or two linear paths. You can specify the following with linear patterns: •
Bodies to Pattern. For multibody parts, select a separate body to create a linear pattern. You can use all functions such as Direction 2 or Instances to Skip with Bodies to Pattern. Example
•
Direction of the pattern.
•
Number of pattern instances in each direction.
•
Distance between pattern instances.
•
Pattern instances to skip.
•
Pattern only the seed feature. If you modify the original feature (seed feature), all instances in the pattern are updated to reflect the changes.
•
Faces to Pattern. You can select the faces that make up a feature to create the pattern. This is useful with models that import only the faces that make up the feature, and not the feature itself. When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
•
Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
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To create a linear pattern in one direction: Example
1.
Create a base part and on the base part, create one or more cut, hole, or boss features that you want to repeat.
2.
Click Linear Pattern
3.
Under Direction 1, do the following:
4.
on the Features toolbar or click Insert, Pattern/Mirror, Linear Pattern.
•
Click a model edge or a dimension to indicate the first direction for the pattern. The name of the edge or dimension appears in the Direction 1 box.
•
Click Reverse Direction
•
Set the Spacing
•
Set the Number of Instances
if the arrow on the model points in the wrong direction.
between pattern instances. .
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern select all the faces in the graphics area.
•
To create a feature pattern on multibody parts:
• 5.
6.
,
a.
Under Features to Pattern design tree.
, select the feature to pattern from the FeatureManager
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
, select the body to
If you want to include specific pattern instances to skip, do the following: Example •
Click Instances to Skip
.
•
In the graphics area, select each pattern instance you want to skip. The pattern instances along with their coordinates are listed in the Instances to Skip box.
•
To restore pattern instances, select the pattern instances again, or select the coordinates in the Instances to Skip box and press Delete.
Under Options, do the following: •
Click Vary sketch if you want the pattern to change as it is repeated. Click Geometry Pattern if you want to pattern only the geometry (faces and edges) of the features, rather than solving each instance of the feature. In some cases, the geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.
7.
Click OK
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to create a linear pattern in Direction 1.
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Chapter 6 Features
To create a linear pattern in two directions: Example
1.
Follow steps 1-6 above to create a linear pattern in Direction 1. NOTE: You can select the Features to Pattern and the Options before or after you select Direction 2.
2.
Under Direction 2, do the following: •
Click a model edge or a dimension to indicate the second direction for the pattern. The name of the edge or dimension appears in the Pattern Direction box.
•
Click Reverse Direction
•
Set the Spacing
•
Set the Number of Instances
•
Select the Pattern seed only check box to replicate only the seed pattern. Selecting the Pattern seed only check box, creates a linear pattern under Direction 2, without replicating the linear pattern created under Direction 1.
if the arrow on the model points in the wrong direction.
between pattern instances. .
The Pattern seed only option is especially useful when creating patterns in two opposite directions. Use Pattern seed only, to prevent duplicate copies of the feature in the same location. • 3.
4.
• •
•
To create a feature pattern on multibody parts, follow the same steps from the procedure above.
If you want to include specific pattern instances to skip, do the following: •
Click Instances to Skip
•
In the graphics area, select each pattern instance you want to skip. The pattern instances along with their coordinates are listed in the Instances to Skip box.
Click OK
.
.
The following applies to linear patterns: When you create a pattern using a Shape feature, all pattern instances must be on the same face. Pattern instances inherit the feature color of the original feature as long as: o the pattern is based on one feature. o the color of the pattern or any faces on any pattern instances has not been changed. The feature colors are not inherited if you pattern or mirror multibody parts.
Example of Linear Patterns Single Direction
Linear pattern Direction 1 preview
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Linear pattern Direction 1 applied
Example of Linear Pattern Instances to Skip
Instances to Skip selected
Instances to Skip restored
Example of Linear Patterns Two Directions
Linear pattern both directions preview
Linear pattern both directions applied
Example of Linear Pattern Seed Feature
Linear pattern Pattern seed only not applied
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Linear pattern Pattern seed only applied
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Chapter 6 Features
Example of Multibody Part with Linear Patterns
Multibody part with Body to Pattern
Linear pattern applied
Example of Feature Scope Linear Pattern
Extrude and dome features applied to selected body
Extrude and dome feature applied to all bodies
Example of Boundaries and Faces to Pattern
Boundary causes pattern to fail
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Pattern suceeds without boundary
Circular Pattern Creates multiple instances of one or more features which you can space uniformly around an axis. Circular pattern includes the following: •
Bodies to Pattern. For multibody parts, select a separate body to create a circular pattern. You can use all functions such as Instances to Skip with Bodies to Pattern. Example
•
Seed feature. Modify the original feature (seed feature), and all instances in the pattern are updated to reflect the change.
•
Select pattern instances to skip as you create the circular pattern.
•
Faces to Pattern. Select the faces that make up a feature to create the pattern. This is useful with models that import only the faces that make up the feature, and not the feature itself. When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
•
Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
To create a circular pattern:
1.
Create one or more features to replicate.
2.
Create an axis around which to pattern the features. For information about how to create an axis, see Reference Axis.
3.
Click Circular Pattern
4.
Under Parameters, do the following:
on the Features toolbar, or Insert, Pattern/Mirror, Circular Pattern.
•
In the graphics area, select an axis, model edge or an angular dimension as the Pattern Axis.
•
If necessary click Reverse Direction
•
Specify the Number of instances
•
Specify the Angle
to change the direction of the circular pattern. .
between each instance.
- or Select the Equal spacing check box. With equal spacing, the Total Angle defaults to 360°. You can change the Angle the graphics area.
in which to create the pattern, using the PropertyManager or the callout in
If you change Number of instances or the Angle using the PropertyManager or the callout box, a preview of the resulting pattern is automatically displayed in the graphics area.
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Chapter 6 Features
5.
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern select all the faces in the graphics area.
•
To create a feature pattern on multibody parts:
• 6.
,
a.
Under Features to Pattern design tree.
, select the feature to pattern from the FeatureManager
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
, select the body to
If you want to skip circular pattern instances, click Instances to Skip, and in the graphics area, select each of the pattern instances to skip. The pointer changes to when you mouse over each pattern instance. Click to select a pattern instance. The coordinates of the pattern instance appear. To restore a pattern instance, click the instance again. If you want to pattern only the geometry (faces and edges) of the features, rather than patterning and solving each instance of the feature, under Options, click to clear Geometry Pattern. In some cases, the geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.
7.
Click OK
.
When you create a pattern using a Shape feature, all pattern instances must be on the same face. Pattern instances inherit the feature color of the original feature as long as: • the pattern is based on one feature. • the color of the pattern or any faces on any pattern instances has not been changed. The feature colors are not inherited if you pattern or mirror multibody parts.
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Example of Multibody Part with Circular Patterns
Multibody part with Body to Pattern
Circular pattern applied
Example of Feature Scope Circular Pattern
Cut extrude feature applied to all multibody parts.
Cut extrude feature using circular pattern applied to single body
Cut extrude feature using circular pattern applied to all bodies
Sketch Driven Patterns Using sketch points within a sketch, you can specify a feature pattern. The seed feature propagates throughout the pattern to each point in the sketch. You can use sketch-driven patterns for holes or other feature instances. Bodies to Pattern. For multibody parts, select a separate body to create a sketch driven pattern. Example To build a sketch-driven pattern:
1.
Open a sketch on the face of a part.
2.
If necessary, create a seed feature on the model.
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Chapter 6 Features
3.
Click Point or Tools, Sketch Entity, Point and add multiple sketch points to represent the pattern you want to create, based on the seed feature.
4.
Click Sketch Driven Pattern Pattern.
5.
Under Selections, do the following:
on the Features toolbar, or click Insert, Pattern/Mirror, Sketch Driven
•
If necessary, use the flyout FeatureManager design tree to select a Reference Sketch the pattern.
to use as
•
Click either Centroid to use the centroid of the seed feature, or Selected point to use another point as the reference point.
•
If you chose Selected point as the reference point, select a Reference Vertex area.
in the graphics
NOTE: You can use the centroid of the seed feature, the sketch origin, a vertex, or another sketch point as a reference point in a sketch-driven pattern. 6.
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
NOTE: If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern , select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself. NOTE: When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
• 7.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
Under Options, select the Geometry pattern check box (see Geometry Pattern). NOTE: The Geometry pattern is not available with Bodies to Pattern.
8.
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Click OK
to create the sketch pattern.
, select the the body to
The sketch-driven pattern is displayed.
Sketch pattern with Centroid as the reference point
Sketch pattern the Selected point as the reference point
Example of Multibody Part with Sketch Driven Patterns
Multibody part with Body to Pattern and sketch points
Sketch driven pattern applied
Reference Points for Sketch Driven Patterns Depending on what you select as your Reference point, the position of the features you propagate will change.
Origin used as the Reference point
Selected Vertex used as the Reference point
NOTE: You can also alter the relative position of the features you propagate when using a table driven pattern.
Table Driven Patterns Using X-Y coordinates, you can specify a feature pattern. Hole patterns using X-Y coordinates are a common application for table driven patterns. However, you can use other seed features, such as a boss, with table driven patterns. You can also save and load the X-Y coordinates of a feature pattern, and apply them to a new part. Bodies to copy. For multibody parts, select a separate body to create a table driven pattern. Example
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Chapter 6 Features
To build a table-driven pattern:
1.
Open a sketch on the face of a part or on a plane, and add a point to identify the reference point for the table pattern.
2.
Close the sketch.
3.
Create a coordinate system (see Coordinate System) based on the point in the previous sketch.
4.
If necessary, create a seed feature.
5.
Click Table Driven Pattern Pattern.
6.
In the Reference point box, select Centroid to use the centroid of the seed feature or Selected point, to use another point as the Reference point.
on the Features toolbar, or click Insert, Pattern/Mirror, Table Driven
NOTE: You can use the centroid of the seed feature, the sketch origin, a vertex, or another sketch point as a reference point in table driven pattern. See Centroid for more information on how the system determines the centroid of a seed feature. 7.
In the Coordinate system box, select the Coordinate System you created from the FeatureManager design tree.
8.
Do one of the following: •
To create the pattern based on the feature, under Features to copy, select the feature in the graphics area. NOTE: If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features.
•
To create the pattern based on the faces that make up the feature, under Faces to copy, select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself. NOTE: When using Faces to Copy, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
• 9.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
, select the the body to
Select the Geometry pattern check box (see Geometry Pattern). NOTE: The Geometry pattern is not available with Bodies to Pattern.
10. Double-click the area under Point 0 to enter the X-Y coordinates for each instance of the table pattern. Note that the X-Y coordinates of your seed feature are displayed for Point 0. NOTE: You can use positive or negative coordinates. To enter a negative coordinate, precede the value with a minus (-). 11. Click OK to create the table pattern. The table driven pattern is displayed.
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Example of Multibody Part with Table Driven Patterns
Save Table Pattern Coordinates You can also save and load (see Load Table Pattern Coordinates) the X-Y coordinates of a feature pattern, and apply them to a new part. To save a table-driven pattern instance:
1.
Create a part with a seed feature and create a table pattern.
2.
In the Table Driven Pattern dialog box, click Save. (If you use an existing set of X-Y coordinates that you modified, use Save As to rename the new pattern).
3.
Browse to the folder where you want to save the Table Pattern, and enter a name. The .sldptab extension is added automatically.
4.
Click Save to save the Table Pattern (.sldptab), and OK in the Table Driven Pattern dialog box to save the part.
Load Table Pattern Coordinates You can load the X-Y coordinates of a feature pattern that you saved (see Save Table Pattern Coordinates), and apply them to a new part. To load a table-driven pattern instance:
1.
With a part open, click Table Driven Pattern Table Driven Pattern.
on the Features toolbar, or click Insert, Pattern/Mirror,
2.
Click Browse to locate the .sldptab file, then click Open. The file name appears in the Read a file from box, along with the X-Y coordinates.
3.
Enter the appropriate Reference point and Coordinate system.
4.
Click OK to apply the Table Pattern to the part.
Mirror Pattern You can select one or more features, the faces that comprise a feature, or with multibody parts, select a body to create a mirror pattern. Multibody parts. Apply features to one or more by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
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To create a mirrored copy of a pattern:
1.
Click Mirror
on the Features toolbar or click Insert, Pattern/Mirror, Mirror.
2.
Under Mirror Face/Plane
, select a face or a plane in the graphics area.
You can select features or the faces that comprise features. •
To use features: Under Features to Mirror flyout FeatureManager design tree.
, click one or more features in the model or use the
•
To use faces: Under Faces to Mirror , in the graphics area click the faces that comprise the feature you want to mirror. Faces to Mirror is useful with imported parts where the import process included the faces of the feature, but not the feature itself.
•
To mirror a feature pattern on multibody parts: a.
Under Features to Pattern design tree.
, select the feature to pattern from the FeatureManager
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
•
To use bodies: Under Bodies to Mirror , in the graphics area select the body you want to mirror. If you select Bodies to Mirror, the following Options appear:
•
Merge solids. When you select a face on a solid part, and clear the Merge solids check box, you can create a mirrored body that is attached to the original body, but is a separate entity. If you select Merge solid, the original part and the mirrored part become a single entity.
•
Knit surfaces. If you select to mirror a surface by appending the mirror face to the original face without intersecting it, you can select Knit surfaces to knit the surfaces together. A preview of the mirrored pattern appears.
3.
Click Geometry pattern if you want to make an exact, geometric copy of the faces and edges of the original feature. Under certain conditions, when using Faces to Mirror, you may not be able to use the Geometry Pattern option. The Geometry Pattern is not available with Bodies to Mirror. To mirror a feature pattern on multibody parts, you must select Geometry Pattern.
4.
Click OK
.
Control and Modify Patterns You can control and modify feature patterns in the following ways: •
Use the Geometry pattern option to make exact patterned and mirrored copies of features, and to improve system performance when using patterned and mirrored features.
•
Use the Vary sketch option to adjust the profile of the patterned feature based on its dimensions and relations to other features.
•
Use a mathematical Equation to calculate values that define the pattern.
•
Use edit Seed Feature to modify the original feature of a pattern or mirrored feature based on a single feature.
•
Use Delete Pattern Instances to remove selected instances in a pattern.
•
Modify the Curve method and the Alignment method when applying curve-driven patterns.
Pattern instances inherit the feature color of the original feature as long as:
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•
the pattern is based on one feature.
•
the color of the pattern or any faces on any pattern instances has not been changed.
Geometry Pattern The Geometry Pattern option speeds up the creation and rebuilding of a pattern. Individual instances of the feature being copied are not solved; end conditions and calculations are ignored. Each instance is an exact copy of the faces and edges of the original feature. By default, the Geometry Pattern option is not selected except when you create a pattern using a Shape or Dome feature. In this example, the cut is extruded with the Offset from Surface end condition, and the bottom face selected.
With Geometry Pattern not selected, each instance is offset from the selected surface by the same amount (the end condition is solved).
With Geometry Pattern selected, each instance is an exact copy of the original feature (the end condition is ignored).
NOTE: You cannot create geometry patterns of features that have faces merged with the rest of the part.
Geometry Pattern must be cleared to create this pattern.
The Geometry Pattern option is available when creating any type of pattern: •
Circular Pattern
•
Linear Pattern
•
Curve-Driven Pattern
•
Table Pattern
•
Sketch Pattern
•
Mirror Feature
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Vary Sketch Use the Vary Sketch option if you want the pattern to change its dimensions as it is repeated. For example, you may want to maintain a specific distance between the edges of the base part and the patterned features. In this example, the first feature (the hole feature) is patterned three times.
When Vary Sketch is not checked, the pattern remains the same regardless of the defining geometry.
When Vary Sketch is checked, the pattern maintains its relation to the sloping edge, based on the dimensions and constraints of the first instance of the pattern.
To create a variable pattern:
1.
2.
Create a sketch for the first feature in the pattern, observing the following recommendations: •
The feature sketch must be constrained to the boundary that defines the variation of the pattern instances. For example, in the illustrated pattern, the angled top edge of the first feature is parallel and dimensioned to the angled edge on the base part.
•
The feature sketch should be fully defined.
Double-click one of the feature dimensions and click the arrows in the Modify box to change the dimension. This gives you a preview of the way this dimension will drive the feature when you create the pattern. Try a different dimension for a different result.
3.
When you are satisfied that the dimensions are correct and the pattern will repeat as you wish, click Insert, Cut, Extrude (or Insert, Boss, Extrude) to create the first feature.
4.
In the FeatureManager design tree, select the feature to repeat.
5.
From the Features toolbar, click Linear Pattern
6.
Click the dimension that you want to use to drive the pattern. Notice the preview arrow.
7.
Click the Vary Sketch check box.
8.
Specify the values for the Spacing and Total Instances of the pattern.
9.
Click OK to create the pattern.
, or click Insert, Pattern/Mirror, Linear Pattern.
Pattern Deletion To delete pattern instances:
1.
Select a face of the pattern instance that you want to delete. Edges cannot be selected because they are shared by more than one feature.
2.
Press the Delete key.
3.
In the Pattern Deletion dialog box, select one of the following:
4.
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•
Delete Pattern Instances. Only the selected instances are deleted. The instance locations are displayed in the Instances Deleted box.
•
Delete Pattern Feature. The complete pattern is deleted, not including the initial feature.
Click OK to delete, or click Cancel to exit the dialog box.
To restore deleted pattern instances:
1.
Right-click the pattern feature, and select Edit Definition.
2.
Select the coordinates of the deleted instance in the Instances to Skip box, and press Delete to restore that instance.
3.
Click OK
.
To delete a table driven pattern instance:
1.
Right-click the pattern in the FeatureManager design tree and select Edit Definition.
2.
In the Table Driven Pattern dialog box, click the number of the pattern you want to delete to highlight the X-Y coordinates.
3.
Press Delete.
4.
Click OK.
To delete a sketch driven pattern instance:
1.
Right click the sketch used by the sketch-driven pattern in the FeatureManager design tree, and select Edit Sketch.
2.
Select the sketch points you want to delete and press Delete.
3.
Click Rebuild
to close the sketch and update the pattern.
To delete a feature from a multi-feature pattern:
1.
Select the feature in the FeatureManager design tree that you want to delete.
2.
Press Delete.
3.
In the Confirm Delete dialog box, select the Also delete absorbed features check box, if available.
4.
Click Yes to delete the feature from the pattern and to close the dialog box. The feature is deleted from the pattern.
Seed Feature The original feature for any type of pattern (linear, circular, sketch driven and so on) or mirrored pattern, is called the seed feature. You can edit this feature. To edit the definition of the original feature:
1.
Right-click a pattern or mirrored instance, and select Edit Seed Feature.
2.
Change the desired parameters.
3.
Click OK.
Mirror Feature Creates a copy of a feature, (or multiple features), mirrored about a face or a plane. You can select the feature or you can select the faces that comprise the feature. •
Bodies to Mirror. Select a body in a single model or multibody part to create a mirror entity.
•
Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
Example If you modify the original feature (seed feature), the mirrored copy is updated to reflect the changes.
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To mirror a feature:
1.
Click Mirror
on the Features toolbar or Insert, Pattern/Mirror, Mirror.
2.
Under Mirror Face/Plane
, select a face or a plane in the graphics area.
You can select features, the faces that comprise features, or a body with multibody parts. •
To use features: Under Features to Mirror flyout in the FeatureManager design tree.
, click one or more features in the model or use the
•
To mirror the entire model: Under Bodies to Mirror
, select a model in the graphics area.
The mirrored model attaches to the face you select. •
To use faces: Under Faces to Mirror feature you want to mirror.
•
To mirror a feature pattern on multibody parts:
• 3.
, in the graphics area click the faces that comprise the
a.
Under Features to Pattern design tree.
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
To use bodies: Under Bodies to Mirror mirror.
, select the feature to pattern from the FeatureManager
, in the graphics area select the body you want to
If you select Bodies to Mirror, the following Options appear: •
Merge solids. When you select a face on a solid part, and clear the Merge solids check box, you can create a mirrored body that is attached to the original body, but is a separate entity. If you select Merge solid, the original part and the mirrored part become a single entity.
•
Knit surfaces. If you select to mirror a surface by attaching the mirror face to the original face without intersections or gaps between the surfaces, you can select Knit surfaces to knit the two surfaces together.
Example 4.
If you want to mirror only the geometry (faces and edges) of the features, rather than solving the whole feature, select Geometry Pattern. The geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part. To mirror a feature pattern on multibody parts, you must select Geometry Pattern. The geometry pattern is only available with Features to Mirror and Faces to Mirror.
5.
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Click OK
.
Example of Feature Scope Mirror Pattern
Plane used to mirror pattern
Pattern mirrored on body
Example of Multibody Part with Mirror
Select the body to mirror
Body mirrorred
Example of Multibody Surface with Knit Surface
Surface created on Front plane
Surface mirrored using Front plane. Knit surface option is available.
Surface mirrored using Top plane. Knit surface option is not available.
Surface mirrored using Right plane. Knit surface option is not available.
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Chapter 6 Features
Revolves Revolved Boss/Base Revolve creates a base or boss by revolving a sketch around a centerline. The default angle is 360°. You can also create revolved cut or revolved surface. With the Selected Contours pointer, you can choose different sketches from among intersecting or non-intersecting sketches to create the revolve. Example To create a revolve feature, use the following guidelines:
•
The sketch for a solid revolved feature can contain multiple intersecting profiles. With the Selected
•
Contours pointer, you can select one or more intersecting profiles. The sketch for a thin or surface revolved feature can contain multiple open or closed intersecting profiles.
•
Profiles cannot cross the centerline. If the sketch contains more than one centerline, select the centerline you want to use as the axis of revolution.
•
When you dimension a revolve feature inside the centerline, you produce a radius dimension for the revolve feature. If you dimension across the centerline, you produce a diameter dimension for the revolve feature.
To create a revolve feature, use one of the following tools:
•
Revolved Boss/Base
•
Revolved Cut
•
Revolved Surface
on the Features toolbar, or Insert, Boss/Base, Revolve
on the Features toolbar, or Insert, Cut, Revolve on the Surfaces toolbar, or Insert, Surface, Revolve
To define a revolve feature, specify the following parameters:
•
Revolve Type (One-Direction, Mid-Plane, or Two-Direction)
•
Angle
•
Reverse Direction
•
Thin Feature
•
Selected Contours
Revolve Features Revolve creates a feature that adds or removes material by revolving one or more profiles around a centerline. The feature can be either a solid, a thin feature, or a surface. With the Selected Contours pointer, you can choose different sketches from among intersecting or non-intersecting sketches to create the revolve. Example
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To create a revolved feature:
1.
Create a sketch containing one or more profiles and a centerline.
Sketching Tips for Revolves
•
The sketch for a solid revolved feature can contain multiple intersecting profiles. With the Selected Contours
pointer, you can select to revolve one or more intersecting profiles.
•
The sketch for a thin or surface revolved feature can contain multiple open or closed intersecting profiles.
•
Profiles cannot cross the centerline. If the sketch contains more than one centerline, select the centerline you want to use as the axis of the revolution.
•
When you dimension a revolve feature inside the centerline, you produce a radius dimension for the revolve feature. If you dimension across the centerline, you produce a diameter dimension for the revolve feature.
2.
Click one of the following:
3.
•
Revolved Boss/Base Revolve
•
Revolved Cut
•
Revolved Surface
in the Features toolbar, or Insert, Base, Revolve, or Insert, Boss,
in the Features toolbar, or Insert, Cut, Revolve in the Surfaces toolbar, Insert, Surface, Revolve
Under Revolve Parameters, do the following: •
Select a Revolve Type. Click Reverse Direction
•
The angle defaults to 360°. If necessary, change the Angle area.
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, if necessary , or drag the handles in the graphics
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4.
5.
If creating a Thin Feature, click the Thin Feature check box, and do the following: •
Select a Type. If necessary, click Reverse Direction
•
Click the Direction 1 Thickness
.
and enter a value. If necessary, click Direction 2 Thickness
and enter a value. If creating a revolve with multiple contours, click Selected Contours, and do the following: a.
Hover over the region with the pointer , and select the contours you want to revolve, You can select any combination of regions to create single or multibody parts. The selected region becomes red.
b.
Click to create a preview of the revolve. The selected region becomes yellow, and the region of the sketch appears in the Selected Contours box.
Select region 3.
Click OK
Preview contour
Create revolve
Revolve thin feature
Revolve from multiple contours
.
Revolve solid
Example of Revolve with Multiple Contours
Select top region (contour)
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Select top and mid regions (contours)
Select mid region (contour)
Select bottom region (contour)
Select bottom and mid regions (contours)
Select all regions (contours)
Ribs Rib Overview Rib is a special type of extruded feature created from an open sketched contour. It adds material of a specified thickness in a specified direction between the contour and an existing part. Elements that control the type of rib you create include: •
Specifying single open or closed sketch elements on a plane or a face
•
Selecting the type of the plane such as parallel
•
Changing the extrusion direction
•
Selecting either a linear or natural extension
•
Creating multiple open sketch elements on a plane
•
Using multiple drafts
•
Using the Detailed Preview PropertyManager with multibody parts to enhance detail and select entities to display
For additional information and examples of the rib feature, see the following topics: •
Creating a simple rib
•
Creating a rib using Normal to Sketch
•
Using multiple open sketch elements
•
Using the multiple drafts feature
•
Reversing the direction of the rib extrusion
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The examples below display some of the methods and results you can apply to create the rib feature.
Single open sketch on face. The arrow indicates the direction of the rib feature
Rib feature applied using Parallel
Rib feature applied using
Sketch on plane, parallel to the plane used for the Base-Extrude (15mm). The arrow indicates the direction of the rib feature.
Normal to Sketch Extrusion direction.
as the
Multiple open sketches on parallel plane, same distance as used for the Base-Extrude (30mm). The arrow indicates the direction of the rib feature.
to Sketch direction.
as the Extrusion
Sketch on parallel plane, same distance as used for the BaseExtrude (30mm). The arrow indicates the direction of the rib feature.
Rib feature applied using Parallel to Sketch direction.
Rib feature applied using Normal to Sketch direction.
as the Extrusion
as the Extrusion
Type: Natural Type: Linear
Example of Ribs with Open Sketches With an open sketch, you can create ribs in the following ways:
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•
Use one or multiple open sketches
•
Create sketches on intersecting, parallel, or other planes
•
Select Parallel to Sketch or Normal to Sketch model and the position of the bounding edges
as the Extrusion Direction, depending on your
Multiple open and closed contours sketched on a plane
Rib feature applied using Normal to Sketch
Single open contour sketch on a plane using
Single open contour sketch on a plane using
Parallel to Sketch Direction
Normal to Sketch Direction
as the Extrusion
as the Extrusion Direction
as the Extrusion
Single open contour sketch on a face. With an open contour sketch on a face, you can only use Parallel to Sketch
as the Extrusion Direction.
Using multiple open contour sketches on a plane, you can select only Normal to Sketch as the Extrusion Direction. However, you can select either of the following: •
Type: Natural
•
Type: Linear
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Chapter 6 Features
Example of Ribs and Direction of Extrusion
Flip material side Example of Rib Feature with Multiple Drafts To create a rib using multiple drafts, see rib feature.
Click Next Reference
Repeat and click Next Reference, until you have selected the contour you wish to use as the reference.
Apply a draft Angle and apply rib with multiple drafts.
Rib - Linear and Natural Type When you specify Normal to Sketch types.
under Parameters, you have the option to create Linear or Natural rib
You can use the Detailed Preview PropertyManager with multibody parts to enhance detail and select entities to display. To create a rib using Normal to Sketch:
1.
Create a plane on which to sketch. NOTE: In the example below, the base feature uses plane 2, and plane 4, which is Offset 10 mm from plane 2, is used to sketch the rib profile. You can also use other types of planes, such as Parallel Plane at Point, to achieve results.
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2.
Sketch a profile as a basis for the rib feature.
3.
Click Rib
on the Features toolbar, or click Insert, Features, Rib.
4.
Under Parameters, do the following. Select a Thickness from the following options: •
Create rib on the left of the sketch
•
Create rib on both sides of the sketch
•
Create rib on the right of the sketch
Enter a Rib Thickness
- adds material only to the left side of the sketch. - adds material equally to both sides of the sketch. - adds material only to the right side of sketch.
.
Select Normal to Sketch as the Extrusion direction, and choose either of the following: • Linear creates a rib that extends the sketch contours normal to the direction of the sketch until they meet a boundary. •
Natural creates a rib that extends the sketch contours in the same directions as the contour until they meet a boundary.
Linear
Natural
Select the Flip material side check box to change the direction of the extrusion. Click Draft On/Off 5.
Click OK
to add a draft, and enter the Draft Angle.
.
Rib Feature You can create a rib using either single or multiple open, or closed, sketches. Detailed Preview
is available from the Rib PropertyManager.
To create the rib:
1.
Using a plane that intersects the part, sketch the contour to use as the rib feature. NOTE: you can also do the following to create a rib feature: o
Use planes that are parallel or at an angle to existing planes
o
Sketch a single element, or multiple elements, using either closed or open contours
Sketch for rib feature created on an intersecting plane
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Rib applied selecting Parallel to sketch
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Chapter 6 Features
Sketch for rib using open sketch elements created on a parallel plane. With this type of sketch, you can either select: Normal to Sketch Parallel to Sketch
Rib using open sketch elements, selecting
Rib using open sketch elements, selecting
Normal to sketch
Parallel to sketch
2.
Click Rib
on the Features toolbar or click Insert, Features, Rib.
3.
Select a Thickness from the following choices: •
Create rib on the left of the sketch
•
Create rib on both sides of the sketch
•
Create rib on the right of the sketch
- adds material only to the left side of the sketch. - adds material equally to both sides of the sketch. - adds material only to the right side of sketch.
4.
Enter a Rib Thickness
5.
Select an Extrusion direction from the following choices: •
.
Parallel to Sketch
- creates the rib extrusion parallel to the sketch.
NOTE: If you select Parallel to Sketch as the Extrusion direction, you can select only Linear as an Extension Type.
6.
•
Normal to Sketch
•
With Normal to Sketch, select a Type, either Linear or Natural.
•
Select the Flip material side check box to change the direction of the extrusion.
Click Draft On/Off
- creates the rib extrusion normal to the sketch.
to add a draft, and enter the Draft Angle.
You can also create drafts using multiple drafts. 7.
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Click OK
.
Scaling You can scale a part or surface model about its centroid or about the model origin. The Scale feature scales only the geometry of the model, for use in data export, cavities, and so on. It does not scale dimensions, sketches, or reference geometry. With multibody parts, you can select to scale one or more models. A Scale feature is like any other feature in the FeatureManager design tree: it manipulates the geometry, but it does not change the definitions of features created before it was added. To temporarily restore the model to its unscaled size, you can roll back or suppress the Scale feature. You can select to scale a model using a uniform or non-uniform scaling by selecting X-Y-Z coordinate values. To scale a single solid or surface model:
1.
In a part document, click Scale
on the Features toolbar or click Insert, Features, Scale.
The Scale PropertyManager appears. 2.
From the Scale about list, select: Centroid, Coordinate System, or Origin.
3.
If you want uniform scaling, specify a scaling value in the Scale factor box.
4.
If you want non-uniform scaling, click to clear the Uniform scaling check box., and enter values for X, Y, and Z.
5.
Click OK
.
Solid model: uniform scaling
Solid model: non-uniform scaling
Surface: uniform scaling
Surface: non-uniform scaling
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To scale multibody parts or multiple surfaces:
1.
In a part document, click Scale
on the Features toolbar or click Insert, Features, Scale.
The Scale PropertyManager appears. 2.
Under Scale Parameters, select a solid or surface body in the graphics area.
3.
From the Scale about list, select: Centroid, Coordinate System, or Origin.
4.
If you want uniform scaling, specify a scaling value in the Scale factor box.
5.
If you want non-uniform scaling, clear the Uniform scaling check box and enter values for X, Y, and Z.
6.
Click OK
.
Multibody parts: uniform scaling
Multibody parts: non-uniform scaling
Shapes Shape Feature Creates a deformed surface on a model by expanding, constraining, and tightening the selected surface. A deformed surface is flexible, much like a membrane. It can be expanded, constrained, and tightened using the sliders on the Controls tab on the Shape Feature dialog box. To create a shape feature:
1.
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Sketch one or more entities with which to constrain the shape feature. You can create the constraining entities directly on the face or on a plane. Valid entities are as follows: •
Points (sketch points, endpoints, vertices, and so on)
•
Sketches
•
Edges
•
Curves
Example of Shape Constraints
Sketch points on face
Using Bend to change shape
Sketch rectangle on face
Using multiple controls to change shape
Sketch shape on separate plane
Using Resolution to change shape
2.
Click Shape
on the Features toolbar or click Insert, Features, Shape.
3.
Select a face on a model. (You can only select one face.)
4.
Click the Constrain to check box and select entities to constrain the shape.
5.
If desired, click to clear Maintain Boundary Tangents.
Maintain Boundary Tangents, selected
Maintain Boundary Tangents, cleared
6.
Click Preview. Rotate the part and examine the shape from different angles.
7.
Use the sliders on the Controls tab to adjust the shape.
8.
When you are satisfied with the shape, click OK. NOTE: If you constrain the shape using a vertex of a 3D sketch, you can use a feature handle to adjust the shape. See Move/Size Features with Feature Handles.
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Shape Feature Controls Tab The Shape Features Controls tab lets you adjust the shape of the deformed surface. After adjusting a slider, observe the preview. Experiment until you are satisfied with the results. Under Gains: •
Pressure. Deflates or inflates the shape.
•
Curve influence. Moves the shape away from or toward the constraining entities. The Curve influence control is grayed out if Constrain to is not selected on the Shape Feature tab.
Pressure and Curve Influence Sliders example. Under Characteristics: •
Stretch. Adjusts the degree of stretching.
•
Bend. Adjusts the degree of bending.
Stretch and Bend Sliders example. Under Advanced controls: •
Resolution. Adjusts the precision of the shape by changing how many points on the face are deformed. Higher Resolution often smooths the flat areas and sharpens the shape near the constraining entities. Lower Resolution provides better performance and a coarser shape; however, some details may be omitted.
Resolution Slider example. After making the first adjustment to the shape, the icon is displayed. Click adjustment. You can undo an unlimited number of adjustments.
to undo the previous
Pressure and Curve Influence Sliders The following illustrations show how you can get different results by adjusting the Pressure and Curve influence sliders. In each case, this same base feature and sketch are used.
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Pressure decreased
Pressure increased
Curve influence decreased
Curve influence increased
Stretch and Bend Sliders The following illustrations show how you can get different results by adjusting the Stretch and Bend sliders. Each illustration is derived from this same base feature, which was shaped by increasing Pressure on the front face.
Stretch decreased
Stretch increased
Bend decreased
Bend increased
Resolution Slider The following illustrations show how you can get different results by adjusting the Resolution slider.
Increase resolution
Shells Shell Features The shell tool hollows out the part, leaves open the faces you select, and creates thin-walled features on the remaining faces. If you do not select any face on the model, you can shell a solid part, creating a closed, hollow model. If you plan on adding fillets to the part, you should fillet the part before you shell it. If you have problems shelling a model, you can run the error diagnostics. To create a shell feature:
1.
Click Shell
on the Features toolbar or Insert, Features, Shell.
2.
To shell using uniform thickness, under Parameters, do the following: •
Enter the Thickness
•
Click on the Faces to remove one or more open faces.
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to control the thickness of the wall. , and select the faces from the graphics area to create a part with
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•
Select the Shell Outward check box if you want the shell feature to increase the outside dimensions of the part. NOTE: You also have the option to shell a model using multiple thicknesses.
3.
Click OK
.
Example of Shell Hollow Model
Shelled model with no faces removed
Shell with Multi-Thickness Faces To set a different shell thickness for each face:
1.
Click Shell
on the Features toolbar or click Insert, Features, Shell.
2.
Click the faces you want to remove in the graphics area. - or Click Multi-thickness Settings, and under Multi-thickness Faces remove in the graphics area. The faces are listed in the Multi-thickness Faces
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box.
, select the faces you want to
3.
Select Face <1> in the Multi-thickness Faces thickness(es)
4.
box, and enter a wall thickness in the Multi-
box.
Select each remaining Face <> in the the Multi-thickness Faces Multi-thickness (es)
box, and enter a wall thickness in the
box for that Face <>.
NOTE: You can add additional faces to the Multi-thickness Faces
box.
5.
Under Parameters, select the Shell outward check box if you want the shell thickness added to the outside.
6.
Click OK
.
Shell with variable thickness and face removed
Shell with variable thickness and model hollow (no faces removed)
Shell Feature Diagnostics The shell feature displays error messages and includes tools to help you identify why the shell feature failed. The diagnostic tool Error Diagnostics is available in the Shell PropertyManager. To run error diagnostics:
1.
Under Error Diagnostics: •
Select Entire body to diagnose all areas of the model - or -
• 2.
Select Failing faces to diagnose and identify the faces that failed to shell.
Click Check body/faces to run the diagnostic tool. The results display in the graphics area, using a callout to pinpoint the specific area on the model that needs correction.
For example, the shell feature can fail because the Thickness at a point is too large relative to one of the selected faces. A message that displays the minimum radius of curvature indicates that the shelling thickness is too large at that point. You can also select Display mesh or Display curvature. •
Display mesh shows a uv mesh. This mesh operates in the same manner as the Preview mesh option in Filled Surface.
•
Display curvature shows a curvature plot for the bodies.
Because problems related to surface gaps and curvature often relate to surface inconsistencies, you can click Go to offset surface. This opens the Offset Surface PropertyManager where the offset surfaces in the model are displayed. Return to Shell feature.
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Surfaces Surfaces Overview Surfaces are a type of geometry that can be used to create solid features. Surface tools are available on the Surfaces toolbar. You can create surfaces by these methods: •
Insert a planar surface from a sketch or from a set of closed edges that lie on a plane
•
Extrude, revolve, sweep, or loft from sketches
•
Offset from existing faces or surfaces
•
Import a file
•
Create mid-surfaces
You can modify surfaces in the following ways: •
Extend
•
Trim existing surfaces
•
Untrim surfaces
•
Fillet surfaces
•
Repair surfaces using Fill Surface
•
Move/Copy surfaces
•
Delete and patch a face
You can use surfaces in the following ways: •
Select surface edges and vertices to use as a sweep guide curve and path.
•
Create a solid or cut feature by thickening a surface.
•
Extrude a solid or cut feature with the end condition Up to Surface or Offset from Surface.
•
Create a solid feature by thickening surfaces that have been knit into a closed volume.
•
Replace a face with a surface
Surfaces Toolbar The Surfaces toolbar provides tools for creating and modifying surfaces. Extruded Surface Revolved Surface Swept Surface Lofted Surface Offset Surface Radiate Surface Knit Surface Planar Surface
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Extended Surface Trimmed Surface Filled Surface Mid-Surface Replace Face Delete Face Untrim Surface
Surface Bodies Surface body is a general term that describes connected zero-thickness geometries such as single surfaces, knit surfaces, trimmed and filleted surfaces, and so on. You can have multiple surface bodies in a single part. You can select a surface body from the graphics area using Filter Surface Bodies You can select all types of surfaces with Filter Surface Bodies. The cursor changes to
on the Selection Filter toolbar.
, indicating when the pointer is over a surface body. Surface bodies can include:
•
Single face surfaces
•
Multiple face surfaces
•
Knit surfaces
•
Filleted surfaces
•
Trimmed and extended surfaces
•
Imported surfaces
•
Planar surfaces and mid surfaces
•
Surfaces made by extrude, revolve, loft, sweep, offset, radiate, or fill
To select a single face in a complex surface body, use Filter Faces
on the Selection Filter toolbar.
Surface Features Planar Surface To create a bounded planar surface from a sketch:
1.
Create a non-intersecting, single contour, closed sketch.
2.
Click Planar Surface
on the Surfaces toolbar, or Insert, Surface, Planar.
The Planar Surface PropertyManager appears. 3.
Select the sketch in the FeatureManager design tree or in the graphics area. The sketch name appears under Bounding Entities
4.
Click OK
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To create a planar surface bounded by a set of closed edges in a part or assembly:
1.
Click Planar Surface
on the Surfaces toolbar, or Insert, Surface, Planar.
2.
Select a set of closed edges in a part or assembly. (All edges in the set must be on the same plane.)
The names of the edges appear under Bounding Entities 3.
Click OK
.
.
To edit the planar surface:
•
If the planar surface is created from a sketch, you can edit the sketch.
•
If the planar surface is created from a set of closed edges, right-click the surface and select Edit Definition.
Extruded Surface To extrude a surface:
1.
Sketch the profile of the surface.
2.
Click Extruded Surface
3.
Under Direction 1, do the following:
on the Surfaces toolbar or Insert, Surface, Extrude.
•
Select an End Condition.
•
If necessary, click Reverse Direction
•
If using Offset from surface, select a Face/Plane in the graphics area. Examine the preview. If the offset is in the wrong direction, click the Reverse offset check box.
•
Enter a Depth
to extrude the surface in the opposite direction.
.
Extruded surface using Mid Plane from sketched spline
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4.
If necessary, click Direction 2 and repeat the same process you followed under Direction 1.
5.
Click OK
.
Resulting extruded surface Revolved Surface Choose different sketches from intersecting or non-intersecting sketches to create the revolve with the Selected Contours pointer
.
Example To revolve a surface:
1.
Sketch a profile and a centerline around which to revolve the profile.
2.
Click Revolved Surface
3.
Under Revolve Parameters, do the following:
4.
5.
on the Surfaces toolbar or click Insert, Surface, Revolve.
•
Select a Revolve type: One-Direction, Two-Direction, or Mid-Plane.
•
Click Reverse Direction
•
Enter an Angle
to change the direction of the revolve.
.
When creating a revolve with multiple contours do the following: a.
Hover over the region with the pointer , and select the contours you want to revolve, You can select any combination of regions to create single or multiple revolved surfaces. The selected region becomes red.
b.
As you drag the pointer over the contours, the color of the contours changes to pink, then yellow when you select them. The region of the sketch appears in the Selected Contours box.
Click OK
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Example of Surface Revolves with Selected Contours
Non-intersecting profiles
Selected Contours
Intersecting profiles
Selected Contours
Swept Surface To sweep a surface:
1.
Create planes as needed for sketching the sweep profile, sweep path, and the guide curves (if any are needed).
2.
Sketch the sweep profile and path on the planes that you created. NOTE: You can also sketch the sweep path on a model face or use a model edge for the path.
Profile sketch
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Profile sketch with path sketch
Preview of sweep
3.
If you are using one or more guide curves, create coincident or pierce relations between the guide curves and the profile.
4.
Click Swept Surface
5.
Under Profile and Path, do the following:
on the Surfaces toolbar or click Insert, Surface, Sweep.
•
Click Profile
and select the profile sketch in the graphics area.
•
Click Path and select the path sketch in the graphics area. NOTE: If you preselect either the profile sketch or the path sketch, the sketch appears in the appropriate box of the PropertyManager.
6.
Apply Options if needed. NOTE: Some of these Options apply only to sweeps using a guide curve.
7.
Under Guide Curves, do the following: •
Select the Guide Curves
in the graphics area.
• •
Click Move Up or Move Down to change the order in which to use the guide curves. If necessary, clear the Merge smooth faces check box. Example
•
Click Show Sections Section Number.
, and click the arrows
8.
Apply Start/End Tangency if necessary.
9.
Click OK
to view and troubleshoot the profile by
.
Lofted Surface To loft a surface:
1.
Create a plane for each profile section of the loft. (The planes do not need to be parallel.)
2.
Sketch the section profiles on the planes. You need a separate sketch for each profile.
3.
Create guide curves, if needed. You need a separate sketch for each guide curve.
Profiles
Profiles with Guide Curves
4.
Click Lofted Surface
5.
Click Profiles , then in the graphics area select the profiles in the order you want to connect them. Select corresponding segments on each profile; the vertex closest to the selection point is used to connect the profiles. Examine the preview curve.
6.
on the Surfaces toolbar or Insert, Surface, Loft.
•
If the preview curve looks wrong, you may have selected the sketches in the wrong order. Use
•
Move Up or Move Down to rearrange the profiles. If the preview curve indicates that the wrong vertices will be connected, click the profile with the wrong vertex connected to clear it, then click again to select a different point on the profile.
•
To clear all selections and start over, right-click in the graphics area, select Clear Selections, and try again.
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7.
Under Options, select from the following as needed: •
Maintain tangency
•
Advanced smoothing obtains smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs. The sections are approximated, and sketch arcs can be converted to splines.
•
Close loft
•
Show preview
8.
If you are using guide curves, select the Guide Curves
9.
Move Down to change the order in which to use the guide curves. To control tangency, click Start/End Tangency.
Simple loft 10. Click OK
in the graphics area. Click Move Up
Loft using guide curve
.
Offset Surface 1.
Click Offset Surface
or Insert, Surface, Offset.
The Offset Surface PropertyManager appears. 2.
Select the surfaces or faces to offset. The name of the surfaces appear under Offset Parameters
.
NOTE: If you select multiple faces, they must be contiguous. 3.
Enter an offset distance in the Offset Distance box. NOTE: You can create an offset surface with a distance of zero.
The selected faces are listed under Offset parameters, and a preview of the offset is displayed.
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4.
Click Flip Offset Direction
5.
Click OK
.
to change the direction of the offset.
or
Radiating a Surface from a Parting Line You can create surfaces by radiating a parting line, an edge, or a set of contiguous edges inwards or outwards, and parallel to a selected plane. To create a surface by radiating a parting line:
1.
Sketch a curve on the face of a part.
2.
Project the curve as a Split Line.
3.
Click Radiate Surface
4.
Under Radiate Parameters, do the following: •
on the Surfaces toolbar or Insert, Surface, Radiate.
Select a plane that is parallel to the direction in which you want the surface to radiate. The name of the plane appears in the Radiate Direction Reference box.
•
Select the split line in the graphics area to place it in the Edges to radiate box. Note the arrow
•
direction. If necessary, click the Reverse direction check box. Set the width of the surface in the Radiate distance box.
• 5.
Click Propagate along tangent faces if you want the surface to continue around the tangent faces of the part.
Click OK
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Surface Face Blend Fillet To create a face blend fillet between surfaces:
1.
Create two surfaces (the surfaces need not be adjacent).
2.
Click Fillet
3.
Under Fillet Type, click Face Fillet.
4.
Under Items to Fillet, enter the Radius
5.
In the graphics area, select the first face to fillet.
6.
on the Features toolbar or click Insert, Surface, Fillet/Round.
•
The face you selected appears in the Face Set 1 box. The preview arrow indicates the direction of the face blend.
•
If the preview arrow points away from the second face, click Reverse Face Set direction of the face blend.
to change the
In the graphics area, select the second face to fillet. •
The face you selected appears in the Face Set 2 box.
•
Click Reverse Face Set
, if necessary, so that the arrows point towards each other.
7.
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces.
8.
Under Fillet Options, you can do the following: •
Click under Hold line then click an edge on one of the faces to define the size of the fillet. You cannot pick a laminar edge as a hold line. (A laminar edge is an edge with only one attached face.)
•
Click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes.
•
Click the Help point check box to resolve an ambiguous selection. Then click a vertex close to the location where you want to insert the fillet.
•
Under Trim surfaces, select one of the following: o
o
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.
Trim and attach. Trim the filleted faces and knit the surfaces into one surface body. This is the default. Don't trim or attach. Add a new fillet surface, but do not trim the faces or knit the surfaces.
9.
Click OK
.
The face blend fillet combines the two separate surface bodies into a single surface body.
Surface Controls Extend Surface You can extend a surface by either selecting an edge, multiple edges, or a face. To extend a surface:
1.
Click Extended Surface
on the Surfaces toolbar or click Insert, Surface, Extend.
2.
In the graphics area, select one or more edges (to extend those edges), or a face (to extend the entire surface an equal amount on all edges). The edge or face you select displays in the Edges/Faces to Extend box.
3.
4.
Select an End Condition. •
Distance. Enter a value under Distance to extend the surface that distance. Use the handles or enter the Distance in the PropertyManager.
•
Up to point. Select a Vertex
•
Up to surface. Select a Surface/face surface ends.
in the graphics area where the extended surface ends. (or a plane) in the graphics area where the extended
Select an Extension Type. •
Same surface extends the surface along the geometry of the surface.
•
Linear extends the surface tangent to the original surface along the edges.
Extend edge using Same surface as the Extension Type.
Extend edge using Linear as the Extension Type.
Extend surface using the face as the Edges/Faces to Extend and Same surface as the Extension Type.
TIP: To extend a surface up to another surface or reference plane, click FeatureManager design tree to select the surface or plane.
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5.
Click OK
.
To extend one or more tangent surfaces:
1.
Create a surface composed of multiple tangent surfaces.
2.
Select to extend individual adjacent tangent surfaces, non-adjacent tangent surfaces, or all tangent surfaces (see tangent surfaces sample). •
To extend individual or multiple (adjacent or non-adjacent) tangent surfaces, select any edge or face.
•
To extend all tangent surfaces, select an edge, and click Propagate tangent edges. Propagate
•
to highlight and extend all
changes color, indicating that you can extend all tangent edges.
Click Propagate again
to cancel the extension of all additional tangent edges.
NOTE: Propagate only displays when you select an edge. If you select the face, the surface extends in all directions. 3.
Select an Extension Type and End Condition.
4.
Click OK
.
Example of Extend Tangent Surfaces
Extend tangent surfaces selecting a single edge
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Click Propagate to highlight and extend all tangent surfaces
Extend tangent surfaces selecting multiple adjacent edges
Extend tangent surfaces selecting multiple non-adjacent edges
Fillet Surface You can use a fillet to smooth the edge between two adjacent faces in a surface body that meet at an angle. Select a Partial preview, a Full preview, or No preview in the Fillet PropertyManager. Fillets now include previews with all fillet types except face fillets and full round illets.
Constant radius surface fillet with Full preview
Constant radius surface fillet applied
Multiple radius surface fillet with Partial preview
Multiple radius surface fillet applied
Surface filleting works as it does for solid bodies with a few exceptions. You can do the following: •
Fillet the edges of a surface body.
•
Make multiple radius surface fillets.
•
Make fillets between two surfaces, or face blend fillets.
•
Add setback parameters to the surface fillets.
•
Make surface fillets with hold lines.
•
Trim or keep the filleted surfaces in a face blend fillet.
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You can not do the following: •
Make a variable radius fillet on a surface.
•
Preserve a cut in a surface body with the Keep features option.
•
Select a surface to fillet by feature.
To fillet edges on a surface body:
1.
Click Fillet
on the Features toolbar or Insert, Surface, Fillet/Round.
2.
Under Fillet Type, select Constant radius.
3.
Under Items to Fillet, enter the Radius
4.
In the graphics area, highlight the edges to fillet. The edge or loop and the radius is listed in the Edges, Faces, Features and Loops
.
box.
NOTE: Make sure that the edges you select have two attached faces. You should knit adjacent surfaces prior to filleting. 5.
Choose options such as Multiple radius fillets, Setback parameters, Keep features, Round corners, and Overflow type, as you would for a fillet on a solid body.
6.
Click OK
.
Example of Keep Features in Surface Fillet The Keep Features option in surface filleting works differently than it does in solid filleting. In a solid part, if you have a boss or cut feature in the area of a fillet, you can preserve the features when filleting. In a surface body, you can preserve a boss, but not a cut.
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Knit Surface Use the Knit Surface function to combine two or more faces and surfaces into one. Note the following about knit surfaces: Edges of the surfaces must be adjacent and not overlapping. Surfaces do not need to be on the same plane. Select the entire surface body, or select one or more adjacent surface bodies. •
Knit surfaces do not absorb the surfaces you used to create them.
•
Create a solid body when the knit surfaces form a closed volume, or leave as a surface body.
To knit surfaces:
1.
Click Knit Surface
or Insert, Surface, Knit.
In the PropertyManager, under Selections: a.
Select the faces and surfaces to knit in the graphics area or in the FeatureManager design tree. The result is a single surface listed in the FeatureManager design tree as SurfaceKnit.
Create adjacent, non-intersecting surfaces
There is no difference in the appearance of the faces and surfaces after knitting. b.
Select Try to form solid if you want to create a solid model from the enclosed surfaces. Select the faces to knit
2.
Click OK
.
The surfaces are knit.
To use the Seed face option:
To knit surfaces with the Seed option, you must use Radiate Surface. 1.
Create a radiated surface.
2.
Click Knit Surface
3.
In the Faces and surfaces box, select the radiated surface.
4.
Click the Seed face box, and click any face on the model you want to knit with the radiated surface.
5.
Click OK
or Insert, Surface, Knit.
.
The seed face and all adjacent faces are knitted to the radiated surface.
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Chapter 6 Features
Mid Surface The Mid Surface tool enables you to create mid surfaces between suitable selected face pairs. Suitable face pairs should be offset from each other. Examples of suitable face pairs include two parallel planes, or two concentric cylindrical faces. Mid surface is useful for generating meshes of two-dimensional elements in finite element modeling.
You can create any of the following mid surfaces: •
Single. Select a single pair of offset faces from the graphics area.
•
Multiple. Select multiple pairs of offset faces from the graphics area.
•
All. Click Find Face Pairs to have the system select all suitable offset faces on the model .
The resulting surface includes all the same attributes as any surface created in SolidWorks. To create a mid surface:
1.
Click Mid-Surface
on the Surfaces toolbar, or click Insert, Surface, Mid Surface.
2.
Under Selections, choose one of the following: from the graphics area an individual set of face pairs, multiple sets of face pairs - or from the PropertyManager, click Find Face Pairs to have the system scan the model for all suitable face pairs. Find Face Pairs automatically filters out any unsuitable face pairs.
Individual face pair selected
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All face pairs selected (Find Face Pairs)
3.
Use Position to place the mid surface between the face pair. The default is 50%. The position is the distance between the faces that appear in the Face 1 and Face 2 boxes, starting from Face 1. mid surface face 1 face 2 face 3 Position 50%
face 4 4.
Position 75%
When you use Find Face Pairs, you can specify a Recognition threshold to filter the results. The Recognition threshold is based on combining the following: •
The Threshold Operator function (= equal, < less than, <= less than or equal to, > greater than, >= greater than or equal to), is the mathematical operative.
•
The Threshold Thickness is the wall thickness. For example, you can set the system to recognize all suitable face pairs that have a wall thickness of less than or equal to (<=) 3 millimeters. Any face pair not meeting this criteria is not included in the results.
5.
If necessary, under Options, click the Knit surfaces check box to clear the default which creates a knit surface.
6.
Click OK
.
You can either add new face pairs, delete existing ones, or update face pairs. To delete face pairs:
1.
Select a set in Face Pairs and press Delete.
2.
Click OK
.
To add face pairs:
1.
Select Face 1 in the PropertyManager, and choose a face in the graphics area.
2.
Choose an offset face as Face 2. The selected faces are highlighted in the graphics area, and listed under Face Pairs.
3.
Click OK
.
To update face pairs:
1.
Select a set in Face Pairs. The face pair is displayed in Face 1 and Face 2.
2.
Select another pair of offset faces in the graphics area. NOTE: You can also amend one selection of the offset pair, provided the new face you select is offset to the first face.
3.
Click Update Pair to update Face pairs with the new set of faces.
4.
Click OK
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Chapter 6 Features
Fill Surface The Fill Surface feature constructs a surface patch with any number of sides, within a boundary defined by existing model edges, sketches, or curves. You can use this feature to construct a surface to fill a gap in a model. You can apply Fill Surface in one or more of the following cases: •
Correct a part that does not import correctly into SolidWorks (where there are missing faces).
•
Fill the holes in a part used for core and cavity molding.
•
Construct a surface for industrial design applications.
•
Create a solid.
•
Include features as separate entities, or merge those features.
Fill Surface includes the following capabilities in the PropertyManager. Patch Boundary Patch Boundary capabilities.
defines the edges of the patch you apply. Boundaries include the following properties and
•
You can use surfaces or solid edges, as well as 2D or 3D sketches as boundaries for the patch.
•
For all sketch boundaries, you can select only a Contact patch as the type of Curvature Control.
Alternate Face Example With Alternate Face, you can flip the boundary face for the curvature control of the patch. Alternate Face is used only when creating a patch on a solid model. Curvature Control Curvature Control defines the type of control you want to exert on the patch you create. The types of Curvature Control include: •
Contact. Creates a surface within the selected boundary.
•
Tangent. Creates a surface within the selected boundary, but maintains the tangency of the patch edges.
You can apply different types of Curvature Control in the same patch. Example Apply to all edges The Apply to all edges check box enables you to apply the same curvature control to all edges. If you select the function after applying both Contact and Tangent to different edges, it applies the current selection to all edges. Optimize surface Select the Optimize surface option with two, three, or four-sided surfaces. The Optimize surface option applies a simplified surface patch that is similar to a lofted surface. Potential advantages of the optimized surface patch include faster build times, and increased stability when used in conjunction with other features in the model. Show preview Display a shaded preview of the surface fill. Preview mesh Display a grid on the patch to help you visualize the curvature. The Preview mesh is available only when you select Show preview.
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Reverse Surface Change the direction of the surface patch. The Reverse Surface button is dynamic, and only displays under these conditions: •
All boundary curves are coplanar
•
No constraint points exist
•
No interior constraints
•
Fill surface is non-planar Example
Constraint Curves Constraint Curves allow you to add slope control to the patch. They are used primarily with industrial design applications. You can create a constraint curve using sketch elements such as sketch points or splines. Click on the images below to see examples of applying Fill Surface
Imported surface example
Industrial design example
Resolution Control If your fill surface is not smooth, you can improve its quality by adjusting the Resolution Control
slider.
The Resolution Control is available only when the Optimize Surface check box is cleared. The resolution is set to 1 by default. Change the setting to 2 or 4 to increase the number of patches defining the surface. A higher setting improves the quality of the surface profile. Changing the resolution increases the model size and processing time. You should not change the default setting if your surface is satisfactory.
Quality set to 1
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Quality set to 2
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Options You can create a solid model with the Filled Surface tool. Options include: •
Merge result
•
Try to form solid
•
Reverse direction
Merge result The behavior for this option depends on the boundaries. When all the boundaries belong to the same solid body, you can use the surface fill to patch the solid. If at least one of the edges is an open sheet edge and you select Merge result, then the Surface Fill knits with the surfaces to which the edges belong. If all the boundary entities are open edges, then a solid may optionally be created.
Model without Filled Surface applied. Note the features inside.
Model with Filled Surface applied and Merge result selected. The surface fill joins the solid, removing the features inside.
Model with Filled Surface applied and Merge result cleared. The surface fill creates a new surface, and the features inside remain. Merge result option allows: •
Streamline operation, eliminating Replace face.
•
Hide solid details within the model.
Try to form solid Forming a solid is possible if all the boundary entities are open surface edges. The option Try to form solid is cleared by default. Reverse direction When patching a solid with a fill surface there are often two possible results. Click Reverse direction to correct if the fill surface displays in an unwanted direction.
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Example of Using Alternate Face Example of a solid model, using Contact as the Curvature Control. The fill surface feature automatically selects a direction when you pick a boundary. In some cases, there is more than one possible direction option. To choose other directions, select Alternate Face.
Example of Multiple Curvature Control This example of an imported surface has a gap along the front face. To patch the surface correctly, you must apply a different curvature control type to the different boundary edges. 1.
Import model and click Filled Surface on the Surfaces toolbar, or Insert, Surface, Fill.
2.
In the graphics area, under Patch Boundary, select the boundary edges. •
Apply Contact patch to the two curved edges.
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•
3.
Apply Tangent patch to the two horizontal edges.
Click OK
to apply Fill Surface.
Example of Surface Fill with Reverse Surface
Left image: You select the top profile for the tangent surface fill (orange arrow), but the surface is attached to the bottom profile (black arrow). Correction is required. NOTE: The red section is the top of the fill surface extruding from the bottom profile through the top (blue).
Right image: You select the top profile for the tangent surface fill (orange arrow), and click Reverse Surface. Correction is applied. NOTE: The tangent fill surface (green), is correctly attached to the top profile.
Fill Surface Imported Surface Example This example of a casing is an imported surface. One of the faces in this example has failed. You can repair it by using fill surface. Creating a fill surface from an imported part:
1.
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Import the part.
2.
Click Filled Surface
on the Surfaces toolbar, or Insert, Surface, Fill.
3.
In the graphics area, under Patch Boundary, select each of the tangent edges around the hole.
The edges, along with the curvature type are listed in the Patch Boundaries
box.
NOTE: In this case use Tangent to apply constraints to the patch. 4.
Click OK
.
Fill Surface Industrial Design Example This model uses sketches as patch boundaries for the fill surface. To help shape the patch, it also uses sketch points and a spline as constraint curves. Creating a fill surface using constraint curves:
1.
Sketch1 - Sketch an arc on Plane1 (Front) and dimension.
2.
Sketch2 - Sketch an arc on Plane3 (Right), dimension, and add the necessary relations.
Sketch1
Sketch2
3.
Sketch3 - Sketch an arc to connect Sketch1 and Sketch2 on Plane2 (Top). Dimension and add the necessary relations.
4.
Create Plane4 (at angle to Plane1) and add sketch points (Sketch4), as shown, to use as constraint curves.
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5.
Create Plane5 (offset from Plane2) and sketch spline (Sketch5), as shown, to use as a constraint curve.
Sketch3
Sketch4
Sketch5
6.
Click Filled Surface
on the Surfaces toolbar, or Insert, Surface, Fill.
7.
In the graphics area, under Patch Boundary, select the edges created by Sketch1, Sketch2, and Sketch3. The edges, along with the curvature type are listed in the Patch Boundaries
box.
NOTE: The curvature control defaults to Contact, since only contact surfaces are eligible with sketch boundaries. 8.
Under Constraint Curves, select Sketch4 and Sketch5 in the graphics area. Sketch4 and Sketch5 are listed in Constraint Curves box
9.
Click OK
.
.
Three views of the industrial design example with fill surface applied Trim Surface You can use a surface, plane, or sketch as a trim tool to trim other surfaces where they intersect. You can also use a surface in conjunction with additional surfaces, as mutual trim tools. Trim surface includes the following options:
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•
Trim type: Standard or Mutual.
•
Keep selections Retains trimmed surfaces.
•
Remove selections. Discards trimmed surfaces.
•
Natural. Trims and forces the boundary edges to follow the shape of the surface.
•
Linear. Trims and forces the boundary edges to follow a linear direction from the trim point.
•
Split All. Displays all possible splits on the surface.
To trim a surface:
1.
Create two surfaces which intersect at one or more points.
2.
Click Trimmed Surface
3.
Under Trim Type, select Standard.
4.
Under Selections:
5.
6.
on the Surfaces toolbar or Insert, Surface, Trim.
•
In the graphics area, select a surface, plane, or sketch as the Trim tool
•
In the graphics area, select a surface as the Pieces to keep based on the following:
.
, or as the Pieces to remove
,
o
Keep selections. Select to retain the surface bodies listed under Pieces to keep.
o
Remove selections. Select to discard the surface bodies listed under Pieces to remove.
Under Surface Split Options, select an item: •
Natural. Boundary edges follow shape of the surface.
•
Linear. Boundary edges follow linear direction from trim point.
•
Split All. Display all splits in the surface.
Click OK
.
Trim tool
Pieces to keep
Trimmed surface
To trim a surface using mutual trim:
1.
Create two or more surfaces which intersect at one or more points.
2.
Click Trimmed Surface on the Surfaces toolbar or Insert, Surface, Trim.
3.
Under Trim type, select Mutual.
4.
Under Selections, do the following: •
In the graphics area, select at least two intersecting surfaces you want to use as the Trimming surfaces
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•
In the graphics area, select the areas you want as the Pieces to keep
, or as the
Pieces to remove , based on the following: o Keep selections. Select to retain the surface bodies listed under Pieces to keep. o Remove selections. Select to discard the surface bodies listed under Pieces to remove.
You can select one or more areas to keep, depending on the intersecting surfaces. 5.
Under Surface Split Options, select an item: • • •
6.
Natural. Boundary edges follow shape of the surface. Linear. Boundary edges follow linear direction from trim point. Split All. Display all splits in the surface.
Click OK
.
Two different sets of results.
Untrim Surface With Untrim Surface, you can patch surface holes and external edges by extending an existing surface along its natural boundaries. You can also extend the natural boundaries of the surface by a given percentage, or connect the end points to fill the surface. Use the Untrim Surface tool with any imported surface or surfaces that you create. Note: Untrim Surface extends an existing surface, whereas Surface Fill creates different surfaces, applies a patch between multiple faces, uses constraint curves, and so on.
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Example of Untrim Surface
Select the edges as shown and under Options, choose Extend edges
Select the edges as shown, and under Options, choose Extend edges.
Select edges as shown, and under Options, choose Connect endpoints.
Select the edge as shown, keep the
Select the edge as shown, change the Distance
Distance at the default 0%. Under Options, choose Extend edges.
to 30%. Under Options, choose Extend edges.
Select the face, and under Options, choose Internal edges.
Select the face, and under Options, choose External edges. You can also select All edges to untrim both internal and external edges.
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To use Untrim Surface:
1.
Open the surface part that you want to untrim.
2.
Click Untrim Surface on the Surfaces toolbar, or Insert, Surface, Untrim.
3.
Under Selections , choose the face or the edges you want to untrim. Note: Depending on the edge you select, the surface can extend to its natural boundary. To constrain the edge, select the adjacent edge, as show below.
Extend edges. If you select the edge as shown, the surface extends to its natural boundaries. 4.
To constrain the surface extension, select both edges, as shown above.
Under Options, as the Edge untrim type, you can accept the default Extend edges to extend all edges to their natural boundaries. Or you can select both edges and choose Connect endpoints, as shown at right. To create a surface extension that merges with the original surface, select the Merge with original check box (default). To create a new, separate surface body, clear the Merge with original check box. Both the original and the new surface body appear in the FeatureManager design tree.
5.
Click OK
to untrim the surface.
Surface untrim, select both left edges and the inner edge. Under Options, select Connect endpoints.
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Surface untrim, select the face. Under Options, select All edges. All edges are extended to their natural boundaries.
Radiate Surface Radiate surface works on edges, parting lines, or planar and non-planar curves. To radiate a surface:
1.
Click Radiate Surface
or Insert, Surface, Radiate.
The Radiate Surface PropertyManager appears. 2.
Select a reference plane that is parallel to the direction in which you want the surface to radiate.
3.
Click the Edges To Radiate box
4.
Note the arrow direction. To specify the opposite direction, click Flip Radiate Direction
5.
Select Propagate along tangent faces if the part has tangent faces and you want the surface to continue around the part.
6.
Specify the width of the surface in the Radiate Distance
7.
Click OK
, then click a parting line, an edge, or a set of contiguous edges. .
box.
.
Hide and Show Bodies With multibody parts, the solid bodies can be independent of other solid bodies or surfaces. You can hide or show surface (or solid) bodies, using View, Hide/Show Bodies. In the PropertyManager, you can select one or more surface bodies or a solid body from the graphics area. To hide bodies:
1.
Open a document containing multiple surface or solid bodies.
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2.
Click View, Hide/Show Bodies. The Hide/Show Bodies PropertyManager appears.
3.
Select one or more entities in the graphics area. Your selections appear under Hidden Bodies. When you select a solid body or a surface body, it becomes translucent in the graphics area.
4.
Click OK
.
The entities you selected remain hidden.
To show hidden bodies:
1.
Click View, Hide/Show Bodies again to open the PropertyManager.
2.
Select the translucent bodies in the graphics area. You can select some or all of the translucent bodies.
3.
Click OK
.
The translucent entities you selected are visible again.
You can also use the shortcut menu to hide a surface without using the PropertyManager to preview the entities you select. To show the hidden surface again, click View, Hide/Show Bodies, select the translucent bodies in the graphics area and click OK
.
NOTES:
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•
You can still select from the FeatureManager design tree to Hide or Show, but it does not open the PropertyManager or display the model in a translucent state.
•
To hide or show an assembly component, click Hide/Show Component
on the Assembly toolbar.
Delete Face With Delete Face
tool, you can do the following:
•
Delete. Deletes a face from a surface body, or deletes one or more faces from a solid body to create surfaces.
•
Delete and Patch. Deletes a face from a surface body or solid body and automatically patches and trims the body.
•
Delete and Fill. Deletes faces and generates a single face to close any gap.
To delete faces from a surface body:
1.
Click Delete Face
on the Surfaces toolbar, or Insert, Face, Delete.
The Delete Face PropertyManager appears. 2.
In the graphics area, click the faces you want to delete. The names of the faces appear under Faces to delete
3.
Under Options, click Delete.
4.
Click OK
.
.
The faces disappear.
Select gray faces to delete
Faces deleted
To delete and patch faces on a surface body:
1.
Follow steps 1 and 2 from the previous procedure.
2.
Under Options, click Delete and Patch.
3.
Click OK
.
The faces disappear, and the adjoining faces extend to form an unbroken surface.
Select gray faces to delete
Blue faces patched
To delete and fill surfaces:
1.
Follow steps 1 and 2 from the previous procedure.
2.
Under Options, click Delete and Fill. The system deletes the faces and replaces them with a single face •
Tangent fill cleared. The fill use contact edges.
•
Tangent fill selected. The fill uses tangent edges.
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3.
Click OK
.
The faces are deleted, and are filled by a single unbroken surface.
Before Delete and Fill To delete faces from a solid body and create surfaces:
1.
Using a solid body, click Delete Face on the Surfaces toolbar, or Insert, Face, Delete. The Delete Face PropertyManager appears.
2.
In the graphics area, click the faces you want to delete. The names of the faces appear under Faces to delete
.
3.
Under Options, click Delete.
4.
Click OK
.
The faces disappear, and a new DeleteFace1 surface body is added to the Surface Bodies folder
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in the FeatureManager design tree.
After Delete and Fill
Delete Hole The Delete Hole dialog box lists any closed profile instances previously deleted from a surface. It allows you to remove one or more instances, without deleting the entire Delete Hole feature from the FeatureManager design tree. NOTE: All entities must be on the same body.
Valid. Both holes are on the same body.
Invalid. Each set of holes is on a separate body. You need to create two instances of Delete Hole to remove all holes.
To edit delete hole instances:
1.
Click the Delete Hole feature in the FeatureManager design tree, right-click and select Edit Definition.
2.
Select the closed profile instance you want to restore from the Hole Edge(s) to remove list.
3.
Press Delete.
4.
Click OK to restore the closed profile to the surface.
To delete a hole from a surface:
1.
Select the closed profile instance on the surface.
2.
Click Delete.
3.
In the Choose Option dialog box, select Delete Holes(s).
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Replace Face You can replace faces in a surface or solid body with new surface bodies. The replacement surface body does not need to have the same boundaries as the old faces. When you replace a face, adjacent faces in the original body automatically extend and trim to the replacement surface body, and the new face trims. Replace Face allows you to do the following:
•
Replace a single face or set of connected faces with a surface body. Example
•
Replace more than one set of connected faces with the same number of surface bodies in a single operation. Example You must list the faces for replacement in the same order as the corresponding replacement surface bodies. Replace Face identifies the pairs of original and replacement faces and performs the replacement.
•
Replace a face in a solid or surface body.
The replacement surface body can be of the following types:
•
Any type of surface feature such as an extrude, loft, fill, and so on.
•
A knit surface body, or a complex imported surface body.
•
Usually wider and longer than the faces you are replacing. However, in some cases when the replacement surface body is smaller than the faces for replacement, the replacement surface body extends to meet the adjacent faces.
The faces for replacement have the following characteristics:
•
Must be connected.
•
Do not need to be tangent.
Replace Face Example - Single Set of Faces To replace a set of connected faces with a surface body:
1.
Make sure that your replacement surface body is wider and longer than the faces you are replacing.
2.
Click Replace Face
, or Insert, Face, Replace.
The Replace Face PropertyManager appears. 3.
Under Replace Parameters do the following: •
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Click the faces you want to replace to place them in the Target faces for replacement box. The faces must be connected, but they do not have to be tangent. If you cannot see the faces, rightclick the replacement surface body and select Hide Surface Body.
•
4.
Click the Replacement surfaces box, then click the replacement surface body to place it in the box. If the replacement surface body is hidden, select it in the FeatureManager design tree.
Click OK
.
The faces are replaced, and the adjacent faces of the original body are trimmed and extended to fit. The new face is trimmed to fit the adacent faces of the original body.
NOTE: If the replacement surface body is still visible, right-click it and select Hide Surface Body. Replace Face Example - Multiple Sets of Faces To replace more than one set of connected faces with surface bodies:
1.
Click Replace Face
2.
Under Replace Parameters do the following: •
, or Insert, Face, Replace.
Click the first set of faces you want to replace to place them in the Target faces for replacement box. You do not have to click them in order, but you need to place the first set together in the list. In this example, select the five faces along the top of the "H", including the vertical faces.
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•
Click the second set of faces to place them in the Target faces for replacement
box.
In this example, select the five faces along the bottom of the "H".
•
3.
Click to highlight the Replacement surfaces box, then click first the replacement surface body for the first group of faces, then the replacement surface body for the second group of faces.
Click OK
.
The faces are replaced, and the adjacent faces of the original body are trimmed and extended to fit. The new faces are trimmed to fit the adjacent faces of the original body.
Sweeps Sweep Overview Sweep creates a base, boss, cut, or surface by moving a profile (section) along a path, according to these rules: •
The profile must be closed for a base or boss sweep feature; the profile may be open or closed for a surface sweep feature.
•
The path may be open or closed.
•
The path may be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
•
The start point of the path must lie on the plane of the profile.
•
Neither the section, the path, nor the resulting solid can be self-intersecting.
You can view the sweep using zebra stripes as you create the sweep. Place the pointer on the sweep, open the shortcut menu, and select View zebra stripes. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear View zebra stripes.
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Sweeps can include: •
Simple sweeps
•
Sweeps using guide curves
•
Sweeps using multiple profiles
•
Sweeps using thin features
Simple Sweep To create a simple sweep:
Sketch on multiple planes, following the tips outlined below: Tips for creating a sweep:
Profile •
The profile must be closed for a base or boss sweep feature.
•
The profile can be open or closed for a surface sweep feature.
Path •
The path can be open or closed.
•
The path can be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
•
The start point of the path must lie on the plane of the profile. Neither the section, the path, nor the resulting solid can be self-intersecting.
You can create a sweep using multiple profiles. You can view the sweep using zebra stripes as you create it. Place the pointer on the sweep, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear View zebra stripes. 1.
Sketch a closed, non-intersecting profile on one plane or on a face.
2.
Create the path that the profile will follow. Use a sketch, existing model edges, or curves.
3.
Click one of the following: • • •
Sweep on the Features toolbar or Insert, Boss/Base, Sweep Insert, Cut, Sweep Swept Surface on the Surfaces toolbar or Insert, Surface, Sweep 1 = Profile 2 = Path
4.
Under Profile and Path, do the following: •
Click Profile
•
Click Path
and select the profile sketch in the graphics area. and select the path sketch in the graphics area.
NOTE: If you preselect either the profile sketch or the path sketch, the sketch is displayed in the appropriate box of the PropertyManager.
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5.
Apply Options if needed.
Sweep preview
Orientation/twist Type: Keep normal constant
Orientation/twist Type: Follow path
Under Options, clear Show preview if you do not want to display a shaded preview of the sweep. Under Orientation and Twist Control, only Keep normal constant and Follow path apply to simple sweeps. The other selections apply only to sweeps using a guide curve. When you select Follow path as the Orientation/twist type, you can select parameters to stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign. 6.
Apply Start/End Tangency if needed.
7.
You can create a Thin Feature sweep.
To create a thin feature sweep: o
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
o
Examine the preview and click Reverse Direction
o
Enter a Direction 1 Thickness Thickness
Click OK
and if using Two-Direction as the Type, a Direction 2
.
Sweep with solid feature 8.
, if necessary.
Sweep with thin feature
.
Example of Shaded Sweep Preview
Sweep shaded preview
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Sweep feature applied
Sweeps Feature A sweep creates a base, boss, cut, or surface by moving a profile (section) along a path. You can view the sweep using zebra stripes as you create it. Place the pointer on the sweep, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear View zebra stripes. Sweeps with guide curves. An option allows you to clear Merge smooth faces for sweeps with guide curves. Clearing Merge smooth faces results in the following: •
The performance of sweeps with guide curves improves. Sweeps generate faster and merge between adjacent geometry and edges.
•
The swept body is segmented at all points where the guide curve or the path is not curvature continuous (see the example below). Consequently, the lines and arcs in the guide curves are more accurately matched.
Merge smooth faces check box checked
Merge smooth faces check box cleared
When you clear the Merge smooth faces check box, the potential exists that some features created later might fail due to changed geometry. Orientation/twist type option. When you select Follow path as the Orientation/twist type, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign. Profiles always maintain a normal to the path. Profile fluctuations are due to uneven curvature fluctuations along the path. Unless you correct the fluctuations by selecting one of the Orientation/twist type options, the profiles follow the path and shift to adjust to the misaligned path: To create a sweep:
1.
Sketch a profile and a path.
You can create sweeps using multiple profiles.
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Tips for creating a sweep:
Profile •
The profile must be closed for a base or boss sweep feature.
•
The profile may be open or closed for a surface sweep feature.
Path •
The path may be open or closed.
•
The path may be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
•
The start point of the path must lie on the plane of the profile.
Neither the section, the path, nor the resulting solid can be self-intersecting. 2. 3.
Click Swept Boss/Base on the Features toolbar, or Insert, Boss/Base Sweep. Under Profile and Path, do the following: •
Click Profile
•
Click Path
and select the profile sketch in the graphics area. and select the path sketch in the graphics area.
If you preselect either the profile sketch or the path sketch, the sketch is displayed in the appropriate box of the PropertyManager. Clear the Show preview check box if you want to only display the profile and path.
4.
5.
6.
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Under Options, apply any of the following: •
Orientation/twist Type
•
Maintain tangency
•
Advanced smoothing
•
Align with end faces
The following functionality is also available: •
Guide Curves
•
Start/End Tangency
•
Thin Feature
Click OK
.
Sweeps with Mulltiple Profiles
Sweep with multiple separate profiles
Sweep with multiple nested profiles
Sweeps with Guide Curves You can use guide curves to control the intermediate profiles as the sketch is swept along the path. You can view the sweep using zebra stripes as you create it. Place the pointer on the sweep, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear View zebra stripes. To create a sweep using guide curves:
If you have already created the profiles for a sweep with guide curves, skip to step 4. 1.
Create the guide curves, either as a sketch, a curve, or a model edge.
2.
Create a path for the sweep. This also can be a sketch, curve, or model edge. NOTE: When using guide curves to create a sweep, the path must be a single entity (line, arc, and so on) or the path segments must be tangent (no angled corners). Path - vertical sketch through ellipse Guide curve - spline Profile - ellipse
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3.
Sketch the sweep profile. See some recommendations for creating sweeps with guide curves. You can create a sweep using multiple profiles. The Pierce Point relation is not required for sweeps with guide curves. You can use guide curves without specifying a pierce point between the guide curve and the profile sketch. You can also create the guide curves and the profile sketches in any order.
4.
5.
Click one of the following: •
Swept Boss/Base
•
Swept Cut
•
Swept Surface
on the Features toolbar or Insert, Boss/Base, Sweep
on the Features toolbar, or Insert, Cut, Sweep on the Surfaces toolbar or Insert, Surface, Sweep
Under Profile and Path, do the following: •
Click Profile
•
Click Path
and select the profile sketch in the graphics area. and select the path sketch in the graphics area.
NOTE: If you preselect either the profile sketch or the path sketch, the sketch is displayed in the appropriate box of the PropertyManager. 6.
Click Options to apply the following, if necessary: •
Clear the Show preview check box if you want to only display the profile, path and guide curves.
•
Orientation/twist Type If the sweep includes guide curves, end tangency is controlled by choosing either: Follow path and 1st guide curve or Follow 1st and 2nd guide curves.
•
Maintain tangency If the sweep section has tangent segments, selecting this option causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs can be converted to splines.
•
Advanced smoothing If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces. Sketch arcs can be converted to splines.
7.
8.
Under Guide Curves, do the following: •
Select the Guide Curves
in the graphics area.
•
Click Move Up
•
Click Show Sections Section Number.
•
If necessary, clear the Merge smooth faces check box. Example
or Move Down
to change the order in which to use the guide curves.
, and click the arrows
to view and troubleshoot the profile by
Click Start/End Tangency to apply the following, if necessary: •
None. No tangency is applied.
•
Path tangent. The sweep is normal to the path at the start or end.
•
Direction vector. The sweep is tangent to a selected linear edge or axis, or to the normal of a selected plane. Select Direction vector, then click the edge, axis, or plane.
•
All faces. The sweep is tangent to the adjacent faces of existing geometry at the start or end. This selection is only available when the sweep is attached to existing geometry. NOTE: Tangency options for sweeps are similar to tangency options for lofts. See Loft Tangency Options for examples.
9.
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Click OK
.
Recommendations for Sweeps with Guide Curves The following recommendations will help you when creating a sweep with guide curves. Path and guide curve sketch Create the path and guide curves first; then create the section. A Pierce relation is not required for sweeps with guide curves. The intermediate profiles of the sweep are dependent on both the path and guide curves for their definition. Relations Note that relations such as Horizontal or Vertical may be added automatically as you sketch the section. These relations influence the shape of the intermediate sections, and may produce results that are not what you want. Use Display/Delete Relations desired.
to delete the unwanted relations. This allows the intermediate sections to twist as
Path and guide curve length The path and the guide curves may differ in length. •
If the guide curves are longer than the path, the sweep is as long as the path.
•
If the guide curves are shorter than the path, the sweep is as long as the shortest guide curve.
Guide curves Guide curves may meet at a common point, which is the apex of the swept surface. You can use any of the following items as a guide curve: sketched curves, model edges, or curves.
Preview Intermediate Sweep Sections Intermediate sections in a sweep incrementally preview the section, as the section follows the trajectory set by the path and guide curves. To view the intermediate sections in the sweep:
NOTE: You can activate this option before creating the sweep, if desired. 1.
Right-click the Sweep feature in the FeatureManager design tree and select Edit Definition.
2.
Under Guide Curves, click Show Sections
3.
Click the Up and Down arrows
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Sweeps Options Sweep Options Under Options, you can do the following: Orientation/twist Type •
With a simple sweep, end tangency is controlled by choosing either Follow path or Keep normal constant.
•
When you select Follow path as the Orientation/twist type, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign.
•
If the sweep includes guide curves, end tangency is controlled by choosing either: Follow path and 1st guide curve or Follow 1st and 2nd guide curves.
Maintain tangency If the sweep section has tangent segments, selecting this option causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs can be converted to splines. Advanced smoothing If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces. Sketch arcs can be converted to splines. Align with end faces Continues the sweep profile to the last face encountered by the path. Sweep Options Align with End Faces Use Align with end faces to continue the sweep profile up to the last face encountered by the path. With Align with end faces selected, the faces of the sweep are extended or truncated to match the faces at the ends of the sweep, without requiring addtional geometry. Align with end faces selected
Align with end faces not selected
Top of helix
Bottom of helix
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Example of Sweep with Thin Features
Sweep with solid feature
Sweep with thin feature
Example of Merge Smooth Faces Option in Sweeps A new option allows you to clear the Merge smooth faces check box for sweeps with guide curves. Previously, there was no check box, and all sweeps merged smooth faces by default. Clearing the Merge smooth faces check box results in the following: •
The performance of sweeps with guide curves improves. Sweeps generate faster and merge between adjacent geometry and edges.
•
The swept body is segmented at all points where the guide curve or the path is not curvature continuous (see the example below). Consequently, the lines and arcs in the guide curves are more accurately matched.
Merge smooth faces check box checked
Merge smooth faces check box cleared
The entities that comprise the Path for sweeps with guide curves need not be tangent. NOTE: When you clear the Merge smooth faces check box, the potential exists that some features created later might fail due to the changed geometry. Sweep Options Advanced Smoothing Advanced smoothing. If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces. Sketch arcs may be converted to splines. Sweep Options Maintain Tangency Maintain tangency. If the sweep section has tangent segments, selecting this option causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs may be converted to splines.
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Loft Tangency Options Controls the tangency of a loft at the starting and ending profiles. You specify the Start and End Tangency on the Advanced tab of the Loft dialog box. •
None. No tangency is applied.
•
Normal to Profile. The loft is normal to the sketch plane of the profile at the start or end.
•
Direction Vector. The loft is tangent to a selected linear edge or axis, or to the normal of a selected plane. Click the Direction Vector button, then click the edge, axis, or plane.
•
All Faces. The loft is tangent to the adjacent faces of existing geometry at the start or end. This selection is only available when the loft is attached to existing geometry. The examples in this table were created from these profiles. The start profile is the converted face of the existing geometry; the selected model edge is the direction vector.
Start Tangency
Start Tangency
None
None
End Tangency
End Tangency
None
Normal to Profile
Start Tangency
Start Tangency
Normal to Profile
Normal to Profile
End Tangency
Normal to Profile
End Tangency
None
Start Tangency
Start Tangency
All Faces
All Faces
End Tangency
End Tangency
None
Normal to Profile
Start Tangency
Start Tangency
Direction Vector
Direction Vector
End Tangency
Normal to Profile
None
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End Tangency
Start and End Tangency Options for Sweeps With a simple sweep, end tangency is controlled by choosing either Follow path or Keep normal constant in the Orientation/twist Type list. When you use guide curves to create a sweep, you have additional options for controlling the tangency at the ends of the path. You specify the Start tangency type and End tangency type under Start/End Tangency. These tangency options are only effective when you use guide curves in the sweep. Choose from these start and end tangency types: •
None. No tangency is applied.
•
Path tangent. The sweep is normal to the path at the start or end.
•
Direction vector. The sweep is tangent to a selected linear edge or axis, or to the normal of a selected plane. Click the Direction vector button, then click the edge, axis, or plane.
•
All faces. The sweep is tangent to the adjacent faces of existing geometry at the start or end. This selection is only available when the sweep is attached to existing geometry. All faces is available only as a Start tangency type.
Orientation/Twist Control Option
Select Follow path and the section remains at the same angle with respect to the path at all times.
Select Keep normal constant and the section remains parallel to the beginning section at all times.
When you select Follow path, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign.
Select Follow path and 1st guide curve and the twist of the intermediate sections is determined by the vector from the path to the first guide curve. The angle between the horizontal plane and the vector remains constant in the sketch planes of all of the intermediate sections.
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Select Follow 1st and 2nd guide curves and the twist of the intermediate section is determined by the vector from the first to the second guide curve. The angle between the horizontal plane and the vector remains constant in the sketch planes of all of the intermediate sections.
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Orientation/Twist Type - Follow Path Under sweep Options, when you select Follow path as the Orientation/twist type, you can select parameters to stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign. Profiles always maintain a normal to the path. Profile fluctuations are due to uneven curvature fluctuations along the path. Unless you correct the fluctuations by selecting one of the new options, the profiles follow the path and shift to adjust to the misaligned path. The three parameters are: •
None. The default value, indicating that no correction is applied.
With None selected, the profile fluctuates, preventing a smooth sweep. •
Direction vector. Select a plane, planar face, or line to define the vector. When you select a plane or planar face, the normal of the plane or planar face is applied. If you select a line, the line direction provides the direction vector. The section plane (along which the sweep is created), always includes the direction vector as its X-axis. The normal of the plane, the Z-axis, is the plane that contains the direction vector and the path tangent at that point.
The Front plane (shown) is the Direction vector. The profiles do not fluctuate, remaining aligned along the entire path, and creating a smooth sweep. •
All faces. If the path includes neighboring faces, you can select All faces. When the path includes 2 alternative faces, click Next Face to switch faces. The section plane (along which the sweep is created), always includes the face normal as its Y-axis. The normal of the plane, the Z-axis, is the tangent of the path at that point.
All faces selected (as shown). The profiles do not fluctuate, remaining aligned along the entire path, and creating a smooth sweep.
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Thicken Thickens a selected surface. If the surface you want to thicken is comprised of multiple adjacent surfaces, you must first knit the surfaces together before you thicken the surface. To thicken a surface:
1.
Click Thicken
on the Features toolbar, or click Insert, Base (or Boss), Thicken.
2.
Under Thicken Parameters, do the following: •
In the graphics area, select a Surface to Thicken
•
Examine the preview, and select the side of the surface you want to thicken, as shown below.
Thicken Side 1 •
.
Thicken Both Sides
Thicken Side 2
Enter the Thickness . Note that when you select Thicken Both Sides Thickness you specify to both sides.
, it adds the
NOTE: To create a solid, click Create solid from enclosed volume. This option is available only if you created a volume that is fully enclosed by surfaces. 3.
Click OK
.
Original surface
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To cut an existing solid by thickening a surface:
You can thicken a surface to cut a solid and create multibody parts. 1.
Click Thickened Cut
on the Features toolbar, or click Insert, Cut, Thicken.
2.
Under Thicken Parameters, do the following: •
In the graphics area, select a Surface to Thicken
•
Examine the preview, and select the side of the surface you want to thicken. The following example shows the Thicken Both Sides
3.
Click OK
.
option.
.
The Bodies to Keep dialog box appears, which gives you the option to create a multibody part. 4.
You can choose All bodies or Selected bodies. If you chose Selected bodies, the dialog box expands to display the number of bodies available. Click the check boxes of the bodies you want to keep.
5.
Click OK.
Keep Body 1
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Keep Body 2
All bodies
To change the thicken feature:
You can edit the side to thicken, the thickness of the feature, and the bodies you selected to keep. 1.
Right click the feature’s name in the FeatureManager design tree and select Edit Feature.
2.
Examine the preview, and if necessary select one of the following to change the side to thicken: •
Thicken Side 1
•
Thicken Both sides
•
Thicken Side 2
3.
Change the Thickness
4.
Click OK
as necessary.
.
The Bodies to Keep dialog box appears. 5.
Change the bodies to keep, as necessary.
6.
Click OK.
To fill a volume with a loft between two surfaces:
1.
Create adjacent surfaces.
2.
Open a new sketch, sketch a guide curve, and close the sketch.
3.
Click Loft
4.
Click the Profiles box and select the surfaces.
5.
Click the Guide Curve(s) box and select the guide curve sketch.
6.
Click OK
or Insert, Boss/Base, Loft.
. The resulting lofted body is solid.
To cut a part with a surface:
1.
Create a surface in the part model, or import one.
2.
Select the surface in the graphics area.
3.
Click Cut with Surface
on the Features toolbar, or click Insert, Cut, With Surface.
In the PropertyManager, under Surface Cut Parameters, choose the Selected surface for cut. 4.
Note the preview arrow, indicating which side of the part will be cut away and click Flip Cut reverse the direction of the cut, if necessary.
to
5.
Click OK
6.
To hide the surface, if desired, right-click the Surface feature in the FeatureManager design tree and select Hide.
.
You can also cut a part with a surface by using the Up To Surface option when extruding a cut.
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Tools for Features Analysis of Features Draft Analysis Overview Designers of plastic parts and mold tooling manufacturers can use the Draft Analysis tool to check the correct application of draft to the faces of their part. With draft analysis, you can verify draft angles, examine angle changes within a face, as well as locate parting lines, injection, and ejection surfaces in parts. Criteria To perform a draft analysis, specify the following criteria:
•
Direction of Pull. Select the plane used to conduct the draft analysis.
•
Draft analysis types. You can select either of the following: o o
Contour map. The analysis generates a contour map of the face angles. Face classification. The analysis examines each face on the model, based on the draft angle. When you select the Face classification check box and click Calculate, each face is displayed in a different color. NOTE: You must specify both the Direction of Pull and the Draft Angle with either type of analysis.
•
Reverse Direction you selected.
. Change the direction of the draw normal to the Direction of Pull (plane or face)
•
Draft Angle. Enter a reference draft angle, and then compare that reference angle to those currently existing on the model.
Categories The results displayed when you click Calculate depend on the type of draft analysis you select. Each time you change the type of analysis or the parameters, you need to re-calculate. Face Classification In the graphics area, each face displays a color based on the Draft angle you selected. Draft analysis results listed under Color Settings are grouped into four categories, when you specify Face classification: •
•
•
•
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Positive draft. Displays any faces with a positive draft, based on the reference draft angle you specified. A positive draft means the angle of the face, with respect to the direction of pull, is more than the reference angle. Negative draft. Displays any faces with a negative draft, based on the reference draft angle you specified. A negative draft means the angle of the face, with respect to the direction of the pull, is less than the negative reference angle. Draft required. Displays any faces that require correction. These are faces with an angle greater than the negative reference angle, and less than the positive reference angle. Straddle faces. Displays any faces that contain both positive and negative types of draft. Typically, these are faces that requires you to create a split line. NOTE: Display colors may vary. The first time you use draft analysis, the system uses default colors. If you modify the colors, the system will use the new colors you specified.
Find Steep Faces This option is used only to analyze the curved faces on a model where a draft was added. Based on the reference angle, there are points on a curved face that meet the criteria, and other points on the curve that do not meet the criteria specified by the reference angle. On some models that include curved faces, all areas along the curve may meet or exceed the reference angle. In such cases, selecting Find steep faces will not register any results, since any point along the curved face meets or exceeds the reference angle. •
Positive draft. Displays any steep faces with a positive draft, based on the reference draft angle you specified.
•
Negative draft. Displays any steep faces with a negative draft, based on the reference draft angle you specified.
Surfaces When analyzing the draft for surfaces, an additional Face classification criterion is added: Surface faces with draft. Since a surface includes an inside and an outside face, surface faces are not added to the numerical part of the classification (Positive draft and Negative draft). Surface faces with draft lists all positive and negative surfaces that include draft.
Negative draft
Positive draft
No steep faces, as all points along curved face are greater than the reference angle
In the examples below, a draft analysis using Face classification was applied to the model.
No draft analysis applied
Positive draft
Negative draft
Draft required
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Each category includes the following information and capability: •
Number of faces included in the category, shown as the number on the color swatch for that category
•
Toggle display using Show
•
Change the default display colors
•
Save the color classifications with the part when you click OK
or Hide
.
Color Contour Color contour displays the uniform or graduated changes within each face on the model as the angle on the face changes. Based on the reference angle (Draft angle ), the scale in the PropertyManager displays a positive to negative range, with 0 degrees at the center. You can select two display modes: •
Uniform display. The uniform display uses three colors to represent the areas within the faces that have positive draft, negative draft, and that require draft. You can modify the three colors.
•
Transition display. Select the Gradual transition check box to display the variations in the angles on the model where the draft is required. TIP: You can see the individual faces of the model during a color contour calculation by specifying Display HLR edges in shaded mode
on the Views toolbar.
The next time you analyze a model using Color contour, these midrange values appear as the default. NOTE: Using either display mode, move the pointer over an area on the model to display the value of the draft angle dynamically.
Gradual transition check box checked. Note the circled area.
Gradual transition check box cleared. Note the circled area.
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Draft Analysis Using the settings in draft analysis, you can verify draft angles on model faces or you can examine angle changes within a face. To apply a draft analysis to verify draft angles:
1.
Open the model, and click
in the Mold Tools toolbar, or click Tools, Draft Analysis.
2.
Under Analysis Parameters, do the following: •
Select a planar face, a linear edge or an axis to indicate the Direction of Pull.
•
Note the draw direction. To change the draw direction, click Reverse Direction use the handle in the graphics area to reverse direction.
•
Enter a Draft Angle
•
Click Face classification to conduct a face-based draft analysis.
•
If necessary, click the Find steep faces check box. Use steep faces when the model includes curved faces. Selecting Find steep faces separately displays faces that have a portion of the face with less angle than the specified draft angle to the direction of pull.
. You can also
.
When you select Find steep faces, two additional categories, are displayed: o
Positive steep faces
o
Negative steep faces These categories function in the same manner as other face categories (positive draft, negative draft, and so on), but only apply to steep faces.
•
Click Calculate.
The regions of the model display the colors appropriate to their draft angle.
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3.
Examine the results. Note that the colors may not exactly match with the images below, and will depend on your computer settings.
Positive draft
Negative draft Requires draft
Draft Required. Displays faces that require correction. These are faces with an angle less than the specified draft angle. If the model includes curved faces and you checked the Find steep faces check box, examine steep faces as well. When analyzing the draft for surfaces, an additional Face classification criterion is added: Surface faces with draft. Since a surface includes an inside and an outside face, surface faces are not added to the numerical part of the classification (Positive draft and Negative draft). Surface faces with draft lists all positive and negative surfaces that include draft.
Draft Required
Negative steep faces
Positive steep faces Straddle faces. Displays faces that include a combination of positive and negative draft. TIP: To examine draft angles within a face in more detail, use a contour map. Perform the analysis without using Face classification. See "To apply a contour map of draft angles" below. 4.
You can change the default colors, and toggle between Show
or Hide
.
NOTE: You can change colors or toggle the display before or after you complete the steps under Analysis Parameters. •
To change colors: Click Edit Color, select a color from the Color dialog box, and click OK.
•
To Show/Hide a draft category: Click Show
or Hide
to toggle. The default is Show
. TIP: You can combine the Show or Hide function with the number on the color swatch in each draft category to help identify small faces that have a draft problem. 5.
Click OK
to exit the draft analysis. If you want to save the draft analysis colors with the part, click OK.
The next time you open the part, it will use the colors used with the draft analysis.
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To apply a contour map of draft angles:
1.
Open the model, and click
2.
Under Analysis Parameters, do the following:
3.
in the Mold Tools toolbar, or click Tools, Draft Analysis.
•
Select a plane, a planar face, a linear edge or an axis from the graphics area to indicate the Direction of Pull.
•
Note the draw direction. To change the draw direction, click Reverse Direction
•
Enter a Draft Angle
.
.
Click Calculate. The regions of the model display a color according to their draft angle.
Move the pointer over the different areas on the model to display the draft angle at that location.
4.
Under Color Settings, you can toggle between two display modes, and change the colors. •
Clear the Gradual transition check box to display a uniform color gradient. This is the default display.
•
Check the Gradual transition check box to display color variations that reflect the transitions in the draft angles on the model. This displays the range of angles (positive draft through negative draft), based on the Draft Angle you specified. Gradual transition is especially useful with complex models with numerous variations in the draft angle. TIP: You can see the individual faces of the model during a color contour calculation by specifying Display HLR edges in shaded mode
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Gradual transition check box cleared 5.
Gradual transition check box checked.
To change the color display, click Edit Color, select a color from the Color dialog box, and click OK. NOTE: If you selected Gradual transition, you can change only the colors for Positive draft and Negative draft.
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6.
If necessary, under Draft Angle, enter a new value to view angular changes in smaller steps.
7.
If you changed the values under Draft Angle or changed the type of display, click Calculate to re-examine the results.
8.
Click OK
.
Example of Draft Analysis
Part with no draft analysis applied
Positive draft
Negative draft
Draft required
Deviation Analysis The Deviation Analysis tool is a diagnostic tool that calculates the angle between faces. You can select a single edge or a series of edges. The edges can be between faces on a surface, or any edges on a solid. The analysis is based on the number of sample points that you select along the edges. You can examine operations which fail or have the potential for failure in any of the following situations: •
Molds. Investigate problems with mold tooling along the split line of the mold, in conjunction with the Draft Analysis tool. Example
•
Fillets. Identify potential problems along tangent faces where a fillet operation fails. Example
•
Tangency requirements. Check along the edges of lofts, sweeps, or surface fills and verify that tangency requirements are met.
•
Maximum deviation. Identify problem areas along the edges of sweeps, lofts, or surface fills where there is maximum deviation. Example
After you use the Deviation Analysis tool, you can modify the results by controlling the appropriate entities within the model. For example, when you examine an edge along a surface fill, deviation analysis results vary according to the following: •
Curvature Control. Select Contact or Tangent. Normally, Tangent yields a lower deviation between adjoining faces.
•
Optimize surface. Use the standard patch, or, with two, three, and four sided edges, apply the Optimize surface option to use the more efficient simplified patch.
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To apply a deviation analysis:
1.
Open the model with the edges you want to examine. Note: The sample model on the right uses a surface fill.
2.
Click Deviation Analysis Tools, Deviation Analysis.
on the Tools toolbar, or
The Deviation Analysis PropertyManager appears.
3.
Under Analysis Parameters
, select the edges in the graphics area that you want to examine.
4.
Use the slider to select the Number of Sample Points
to include in the analysis.
NOTE: The number of points is based on the size of the window client area. If you select more than one edge, the sample points are distributed across the selected edges, proportional to the edge length. 5.
Click Calculate. The colored arrows display the amount of deviation. The results appear for the following criteria between the adjacent faces: • • •
Maximum Deviation - the maximum deviation error along the selected edge. Minimum Deviation - the minimum deviation error along the selected edge. Average Deviation - the average between the maximum and the minimum values along the selected edge.
NOTE: You can change the display colors for Maximum Deviation and for Minimum Deviation. To change the colors, click Edit Color to display the Color palettes, select a color for each deviation type, and click OK or Calculate to apply the new colors.
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Example of Deviation Analysis with Mold Part
Deviation analysis along edges of mold parts
Example of Deviation Analysis with Fillets
Sweep with edges to fillet
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Example of Deviation Analysis with Lofts
Deviation analysis along edge of loft using 3D sketches Example of Deviation Analysis with Surface Fill
Deviation analysis along edge of surface fill
Manipulation of Features Move/Size Features with Feature Handles Provides handles so you can move, rotate, and resize extruded and revolved features. With multibody parts, you can use Move/Size Features to individually move, resize, or rotate each body in the multibody part document. To display and use the feature handles:
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1.
Click Move/Size Features
on the Features toolbar.
2.
Click the feature you want to work with, either in the FeatureManager design tree or in the graphics area. Double-click the feature to display both the handles and the dimensions of the feature.
3.
Drag the rotate handle
or the resize handle
, to rotate or resize the feature.
4.
To move a feature, you can either: •
Drag the feature to a new location with the move handle. If the feature has locating dimensions or relations that restrict its movement, a message asks you if you want to delete or keep the relations or dimensions. - or -
•
Hold the Alt key as you drag to maintain the dimensions and relations on the feature. The feature is allowed to move, but only in the directions not already controlled by dimensions or relations.
NOTE: When you drag a feature with the move handle, any child feature moves with its parent. When you hold down Shift and drag the child feature, the software tries to maintain the position of the child relative to the parent. This position is based on the child’s dimensions and relations. However, in some cases (for example, when the child feature is under defined, or dimensioned to something other than its parent), the child may not move with the parent as expected. Move/Copy Bodies With multibody parts, you can move, rotate, and copy bodies and surfaces. To move a body or a surface:
1.
Click Move/Copy Bodies
on the Features toolbar, or click Insert, Features, Move/Copy.
The Move/Copy Body PropertyManager appears. 2.
Select the surface or the body in the graphics area. The name of the selected item appears under Bodies to Move/Copy.
3.
Under Translate: Enter values for Delta X
, Delta Y
, and Delta Z
.
- or a.
Click to highlight the Translation Reference box
.
b.
Select an edge in the graphics area to define the translation direction.
c.
Type a Distance
. Type a negative number to switch the translation direction.
- or a.
Click to highlight the Translation Reference box
b.
Select a vertex in the graphics area.
c.
If necessary, click To Vertex
.
to select a second vertex.
The surface moves the direction and distance defined by the vertices. Both the original position of the surface or body and a preview of the moved surface or body appear. NOTE: All changes you make in the PropertyManager are reflected dynamically in the graphics area. 4.
Click OK
.
The surface or body appears in the moved position. Example of move body parts and move multibody parts
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To rotate a body or a surface:
1.
Click Move/Copy Bodies
2.
Select a surface or a body in the graphics area.
3.
Under Rotate: •
Enter values for X Rotation Origin A square marker
•
on the Features toolbar, or click Insert, Features, Move/Copy.
, Y Rotation Origin
, and Z Rotation Origin
.
appears in the graphics area to show the location of the origin.
Enter values for X Rotation Angle Rotation Angle - or -
(angle around the X axis), Y Rotation Angle
, and Z
.
•
Click to highlight the Rotation Reference Entity box
.
•
Select an edge in the graphics area to define the rotation axis.
•
Enter an Angle
.
The original position of the surface or the body and a preview of the rotated surface or the body appear. 4.
Click OK
.
The surface or body appears in the rotated position. Example of rotate solid bodies or surfaces To copy bodies or surfaces:
1.
During moving or rotating a surface or a body, select the Copy check box in the Move/Copy Bodies PropertyManager.
2.
Enter the Number of Copies
.
Previews of the copied surfaces or bodies appear in the graphics area. Each copy increments by the values entered for translation and rotation. Example of copy and rotate bodies Example of Move Bodies
Preview of move multibody solid parts Delta X: 10mm Delta Y: 40mm Delta Z: -30mm
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Preview of move multibody solid parts Translation Reference: vertex indicated To Vertex: vertex indicated
Preview of move multibody surface parts Delta X: 20mm Delta Y: 50mm Delta Z: 0mm
Preview of move multibody surface parts Translation Reference: Point at origin To Vertex: Vertex indicated
Example of Rotate Bodies
Preview of rotate multibody solid parts (the arrow indicates the X-Y rotation origin) X Rotation Origin: 10mm
Preview of rotate multibody solid parts Rotation Reference: Point at sketch origin, as indicated
Y Rotation Origin: 20mm
X Rotation Angle: 12°
X Rotation Angle: 80°
Y Rotation Angle: 16°
Preview of rotate surface (the arrow indicates the X-Y rotation origin) X Rotation Origin: 40mm
Preview of rotate surface Translation Reference: Point at sketch origin, as indicated
Y Rotation Origin: -50mm
X Rotation Angle: 20°
X Rotation Angle: 20°
Z Rotation Angle: -5°
Z Rotation Angle: -5°
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Example of Rotate and Copy Bodies
Preview of rotate and copy multibody solid parts X Rotation Origin: 40mm
Preview of rotate and copy multibody solid parts Rotation Reference: Coordinate system created at the sketch origin
Y Rotation Origin: 40mm X Rotation Angle: 12° X Rotation Angle: 45° Y Rotation Angle: 16°
Preview of rotate and copy surface Rotation Reference: Coordinate system created at the sketch origin
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Preview of rotate and copy multibody surfaces Rotation Reference: Sketch point on plane, parallel to top plane
X Rotation Angle: 30°
X Rotation Angle: -23°
Y Rotation Angle: 5°
Y Rotation Angle: -5°
Z Rotation Angle: 15°
Z Rotation Angle: 0°
Combine Bodies You can combine multiple solid bodies to create a singled-bodied part or another multibody part. There are three ways to combine multiple solid bodies: •
Add. Combines solids of all selected bodies to create a single body.
•
Subtract. Removes overlapping material from a selected main body.
•
Common. Removes all material except that which overlaps.
To use the Add or Common operation type:
1.
Click Combine
on the Features toolbar, or click Insert, Features, Combine.
The Combine1 PropertyManager appears. 2.
Under Operation Type, click Add or Common.
3.
Under Bodies to Combine, select the bodies in the graphics area, or select the bodies from the Solid Bodies folder in the FeatureManager design tree.
4.
Click Show Preview to preview the feature.
5.
Click OK
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To use the Subtraction operation type:
1.
Click Combine
on the Features toolbar, or click Insert, Features, Combine.
The Combine1 PropertyManager appears. 2.
Under Operation Type, click Subtract.
3.
Under Main Body, select the body to keep from the graphics area, or select the body from the Solid Bodies folder in the FeatureManager design tree.
4.
Under Bodies to Subtract, select the bodies whose material you want to remove.
5.
Click Show Preview to preview the feature.
6.
Click OK
.
Delete Body You can delete bodies using the Delete Body feature. To use Delete Body:
1.
Click Delete Solid/Surface
on the Features toolbar, or click Insert, Features, Delete Body.
The Body-Delete PropertyManager appears. 2.
Under Bodies to Delete, select the bodies from the graphics area.
3.
Click OK
.
Choose Option The Choose Option dialog box appears when you select several entities on a model and press Delete. The dialog box is dynamic, with the appropriate selections available depending on what entities you select on the model. Options include the following: •
Delete Feature. Deletes the entire feature and any associated features.
•
Delete Face(s). Displays the Delete Face PropertyManager.
•
Delete Hole(s). Deletes any holes created with a sketch, the Simple Hole, or the Hole Wizard features. From the Delete Face PropertyManager, you can select one or more faces on the solid model to create surfaces.
For example, if you select the two items on the model, as shown below, and press Delete, the Choose Option dialog box appears. Because the Hole Wizard holes were drilled on the non-planar surface prior to creating the offset surface feature, the holes on the offset surface do not appear on the FeatureManager design tree. •
•
•
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Delete Feature. Select to delete the surface offset. You can also delete the cut and the fillet along the edges of the cut. Delete Face(s). Select to display the Delete Face PropertyManager, from which you can delete any other faces on the model. Delete Hole(s). Select to delete the hole on the offset surface.
Select Detailed Preview Detailed Preview •
Ribs
•
Extrudes
•
Draft
is available from the PropertyManager with the following features:
You can use the Detailed Preview PropertyManager with multibody parts to enhance detail and select entities to display: •
Highlight new or modified faces. Inspect what was changed from the previous edit. New or modified faces are highlighted in color, as opposed to appearing shaded.
•
Show only new or modified bodies. Display only new or modified bodies. All other bodies are hidden.
New sketch prior to extrusion
Selected Contours for extrude feature
With the Detailed Preview PropertyManager, the selected options control what displays in the graphics area:
Neither option selected
Show only new or modified bodies selected
Highlight new or modified faces selected
Both options selected
Extrude feature applied to new sketch
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To use detailed preview:
1.
Click Detailed Preview
in the PropertyManager.
2.
In the Detailed View PropertyManager: Click Highlight new or modified faces or Show only new or modified bodies.
3.
Click Detailed Preview
to return to the original PropertyManager.
Wrap This feature wraps a sketch onto a planar or non-planar face. You can create a planar face from cylindrical, conical, or extruded models. You can also select a planar profile to add multiple, closed spline sketches. The wrap feature supports contour selection and sketch reuse. The sketch plane must be tangent to the face, allowing the face normal and the sketch normal to be parallel at the closest point. To create a wrap feature:
1.
Select the sketch you want to wrap from the FeatureManager design tree.
2.
Click Wrap
3.
In the PropertyManager, under Wrap Parameters: a.
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on the Features toolbar, or click Insert, Feature, Wrap.
Select an option: •
Emboss. Create a raised feature on the face.
•
Deboss. Creates an indented feature on the face.
•
Scribe. Creates an imprint of the sketch contours on the face.
b.
Select a non-planar face in the graphics area for Face for Wrap Sketch
c.
Set a value for Thickness
d.
Select Reverse direction, if necessary.
.
.
4.
Under Pull Direction, if Emboss or Deboss is selected, click Pull Direction edge, or a plane. If you select a plane, the direction is normal to the plane.
5.
Click OK
, and select a line, linear
.
Example of Pull Direction Wrap Feature
Pull direction - Plane A
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Pull direction - Plane B
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7 Parts
Overview and Editing Parts Parts Overview The 3D part is the basic building block of the SolidWorks mechanical design software. This section describes parts and some ways to work with them, including: •
Modeling solid multibody parts
•
Applying custom properties
•
Editing properties of features and faces
•
Editing, moving, and copying
•
Using color
•
Controlling material properties
•
Using equations
•
Dependency editing using suppress and unsuppress
•
Derived parts and external references
•
Splitting parts
•
Displaying a section view of the model
•
Annotating parts
•
Specifying lighting characteristics and material properties
Edit Definition In a parts document, you can perform the following types of feature editing operations: •
Edit the definition, the sketch, or the properties of a feature.
•
View the parent and child relationships of a feature.
•
Use the feature handles to move and resize features.
•
Control the access to selected dimensions.
•
Change the order in which features are reconstructed when the part is rebuilt (see Drag and Drop Features).
•
Roll back the part to the state it was in before a selected feature was added.
To perform some of these operations, you use the icons in the FeatureManager design tree, where the features are listed in the order in which they are created. See also color and appearance of parts.
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To edit the definition of a feature:
You can edit the definition of a feature to change its parameters. For example, you can edit the depth of an extruded feature, or the selected edges for a fillet. 1.
Click a feature in the FeatureManager design tree or the graphics area.
2.
Click Edit, Definition or right-click and select Edit Definition, and depending on the selected feature type, the appropriate dialog box appears.
3.
Edit the definition in the dialog box by specifying new values or options.
4.
Click Apply or OK to accept the changes; click Cancel to discard the changes.
Properties of Features and Faces Feature and face properties include: •
Name
•
Color
Feature properties also include the capability to suppress (and then unsuppress) the feature. Suppressing temporarily removes the feature from the model, without deleting it. This can be used to simplify the model, or to create part configurations. See creating a configuration manually. To edit feature properties:
1.
In the FeatureManager design tree or in the graphics area, select one or more features, then click Edit, Properties, or right-click the features and select Feature Properties. (To select multiple features, hold down Ctrl while selecting.)
2.
Enter a new Name if desired in the Feature Properties dialog box.
3.
To suppress the feature, select the Suppressed check box.
4.
To change the appearance of the feature, click Color. The Entity Property dialog box appears.
5.
•
To change the feature color, click Change Color. Select a color from the Color palette or define a custom color.
•
To change material properties such as shininess and transparency, click Advanced.
•
To restore the feature to the original color of the part, click Remove Color.
Click OK.
To edit face properties:
1.
Right-click one or more faces and select Face Properties. The Entity Property dialog box appears.
2.
Enter a face Name if desired. (Face names are used under certain conditions when replacing components in an assembly. See replacing components in an assembly.
3.
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•
To change the face color, click Change Color. Select a color from the color palette or define a custom color.
•
To change material properties such as shininess and transparency, click Advanced.
•
To restore the face to the original color of the feature it belongs to, click Remove Color. (Face colors override colors specified for the feature.)
Click OK.
Dynamic Feature Editing You can see a dynamic feature preview when you drag the entities of a sketch, either with or without opening the sketch itself. The preview updates when you release the mouse button after dragging. To display a dynamic preview without opening a sketch:
1.
Click Move/Size Features
on the Features toolbar.
2.
Click the feature you want to edit. The sketch is highlighted in the graphics area. If more than one sketch is used to create the feature (for example, if the selected feature is a loft or a sweep), all the sketches used in the feature are highlighted. Notice that the model is not rolled back when you edit a feature this way.
3.
Drag the sketch entities as needed. As you modify the sketch, the preview shows you what the resulting feature will look like.
4.
When you are satisfied with the feature, click an empty area of the document window or press Esc to clear the selected sketch entity.
Select feature
Resize feature
Feature resized
NOTE: Even though the fillet feature was created separately from the cut extrude, it moves and changes size with the cut extrude because of parent and child relations. To display a dynamic preview while editing a sketch:
1.
Click Move/Size Features
on the Features toolbar.
2.
Double-click a sketch to open the sketch for editing. The model is rolled back to the selected feature.
3.
Modify the sketch by dragging the sketch entities, changing the dimensions, adding relations, and so on. As you modify the sketch, the preview shows you what the resulting feature will look like.
4.
Exit the sketch to update the feature. See Edit Sketch for more information.
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Chapter 7 Parts
Copying Features You can copy features from one face to another on the same model. You can also copy features from model to model. To copy a feature:
1.
With your cursor highlighting the feature, hold down Ctrl and drag the feature where needed. To copy more than one feature, hold down Ctrl as you select the features.
2.
Drop the feature on the same face or to a different face. If the feature includes locating dimensions or relations that restrict its movement, a dialog box is displayed. You can Delete the relations or dimension, Dangle them, or Cancel copy.
To re-attach dangling dimensions:
1.
Select the sketch and click Edit Sketch. The dangling dimensions are displayed in a different shade.
2.
Click the dangling dimension and drag the red handle to a new attachment point. As you drag, the pointer is displayed until you are on an edge or a vertex that is suitable to re-attach the dimension.
Cut extrude feature with location dimensions 3.
Copy of cut extrude feature with dangling dimensions
Red handle indicates the dangling attachment point
Release the pointer to re-attach the dimension to the new edge or vertex.
To copy features from one part to another part:
Tile the windows, then drag the features from one window to another, or use the Copy tools on the Standard toolbar.
and Paste
Color of Parts You can apply a color to the entire part, selected features (including surfaces or curves), or selected model faces. You can also modify the color by manipulating the shaded appearance of the model. NOTE: Color selections made with the Edit Color tool supercedes colors set on the Document Properties tab. To change the shaded appearance of a part:
7-4
1.
Click Tools, Options, Document Properties, Colors.
2.
Under Model\Feature colors, select Shading.
3.
Click Edit and select a color from the Color palette or click Define Custom Colors and define a color of a new shade or hue.
4.
Click OK to close the Color palette, and click OK to close the Document Properties - Colors dialog box.
To change the color of selected features or the entire part:
1.
Select each feature from the FeatureManager design tree or from the graphics area (use Ctrl to select multiple features).
2.
Click Edit Color color.
3.
If you selected items from the graphics area, in Apply to select Face, Feature, Body, or Part.
4.
Click Apply to see a preview then click OK.
on the Standard toolbar, and select a color from the Color palette or select a Custom
All features selected on the model
Color applied to all features
Color applied to selected features
Material Properties and Appearance of Parts You can change the way light affects any shaded model by changing the material properties. You can apply different properties to the entire model, to a face on the model, or to a feature. Material properties are independent of color. You can also combine the controls in the Material Properties dialog box with lighting, to create different effects. NOTE: The shape of the model, the shading, as well as the lighting, affects material properties. The system comes with a default settings which make the model appear "normal". With some models, changing material properties displays negligible differences between a minimum and a maximum setting. Setting Material properties and lighting both require user experimentation. To change material properties for a part:
1.
Click Tools, Options, on the Document Properties tab, Colors or right-click the icon in the FeatureManager design tree and select Document Properties.
2.
In Model/Feature colors, select Shaded.
3.
Click Advanced to display the Material Properties dialog box.
4.
Use the sliders to control material display properties: •
Ambient. How light is reflected and scattered by other objects
•
Diffuse. How light is scattered equally in all directions on the surface
•
Specularity. How surfaces exhibit highlights
•
Shininess. How solid object alternate between a glossy, reflective surface and a dull, matte surface
•
Transparency. How much light passes through the surface
•
Emission. How light projects from the surface
5.
Click Apply and click OK.
6.
Click OK to close the Document Properties - Colors dialog box.
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Appearance and Material Properties
7-6
All values set to default
Diffuse. Slider set to midpoint (default is maximum)
Ambient. Slider set to minimum (default is maximum)
Shininess. Slider set close to maximum (default is 1/3 of maximum)
Transparency. Slider set to halfway between maximum and minimum (default is minimum)
Emission. Slider set towards maximum (default is minimum)
Edit Color Use Edit Color to change the color of a face, feature, part, or assembly when in shaded mode. NOTE: Colors selelections made with the following procedures supercede colors set on the Document Properties tab. To edit the color of one or more faces in a part document:
1.
Click Edit Color
on the Standard toolbar.
2.
In the graphics area, select one or more faces.
3.
Select a color from the Color palette or define a custom color.
4.
In the Apply To box, make sure Face is selected.
5.
Click OK. Face selected
To edit the color of one or more features in a part document:
1.
Click Edit Color
on the Standard toolbar.
2.
In the FeatureManager design tree, click the name of one or more features. - or In the graphics area, click one or more features.
3.
Select a color from the Color palette or define a custom color.
4.
In the Apply To box, make sure Feature is selected.
5.
Click OK.
Feature (base revolve) selected
To edit the color of a part, component, or assembly:
1.
Click Edit Color
on the Standard toolbar.
2.
In the FeatureManager design tree, click the name of the part, component or assembly.
3.
In the Edit Color dialog box, select a color from the Color palette or define a custom color. - or To restore the default color, click Remove.
4.
Click OK.
Assembly with colors applied to parts
To edit the color of a component in an assembly:
1.
Select the component in the FeatureManager design tree or in the graphics area.
2.
Click Edit Color
3.
In the Edit Color dialog box, select a color from the Color palette or define a custom color and click OK.
on the Standard toolbar.
- or To use the assembly’s default color, click Use assembly, and click OK. NOTE: To remove the color layers that you applied, click Undo
SolidWorks 2004 Reference Guide
or click Edit, Undo Edit Color.
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Chapter 7 Parts
Entity Property Displays the properties of faces, surfaces, or edges. To change the color of a face or surface (or multiple faces or surfaces):
1.
Right-click a face or surface, and select Face Properties - or To change the color of multiple faces or surfaces, hold down the Ctrl key and click the faces or surfaces, then right-click and select Face Properties.
2.
Change the color with one of the following methods: •
Change the numeric values for Red, Green, or Blue.
•
Click Remove Color to use the part color.
•
Click Change Color and select a color from the Color palette or click Define Custom Colors and define a new color.
•
Click Advanced and use the sliders to increase or decrease advanced material property values such as ambient, shininess, transparency, and so on.
Example 3.
Under Entity Information, type a name for the face in the Name box, or change the name by typing a new name, if desired.
4.
Click OK.
To change the name of an edge, face, or surface:
1.
Right-click an edge, face, or surface.
2.
Select Edge Properties or Face Properties. The Entity Property dialog box appears.
3.
Under Entity Information, change the name for the edge, face, or surface in the Name box.
4.
Click OK. The name of the edge, face, or surface is changed.
Change Value for Red Change the color of the selected face by changing the numeric value for red. The color displays when you select Shaded view. Change Value for Green Change the color of the selected face by changing the numeric value for green. The color displays when you select Shaded view. Change Value for Blue Change the color of the selected face by changing the numeric value for blue. The color displays when you select Shaded view. Change Color To change the color for the selected face when in Shaded view, click this button. Select a color from the color blocks or create a color with the custom color palette. Use Part Color To use the default part color for the selected face when in Shaded view, click this button. The part color is displayed in the preview box.
7-8
Advanced Properties Use the slider controls to change the material display properties of the selected face. For example, you can make the face more or less transparent (Transparency), or control how much light is projected from the face (Emission). The material display properties are independent of color. You can also combine the controls in the Advanced Properties dialog box with lighting, to create different effects. To set Advanced Properties for a model face:
1.
Right-click a model face and select Face Properties.
2.
In the Entity Property dialog box, click Advanced.
3.
Set the sliders as needed. •
Ambient - light reflected and scattered by other objects
•
Diffuse - light scattered equally in all directions on the surface
•
Specularity - ability to reflect light from a surface
•
Shininess - a glossy, highly reflective surface
•
Transparency - ability to pass light through the surface
•
Emission - ability to project light from the surface
4.
Click Apply to see a preview, or click OK to set the value.
5.
Click OK to close the Entity Property dialog box.
NOTE: The values displayed in the Advanced Properties dialog box are initially system defaults. You have the option to change the values in the Advanced Properties dialog box, and save the new values to a document template. Sample Advanced Properties
System default setting for all sliders
Diffuse slider set to minimum (0%)
Transparency slider set to 50%
Emission slider set to 50%
Only the individually specified slider was moved in each of the examples above. System default were as follows: • • •
Ambient - 100% Diffuse - 100% Specularity - 100%
SolidWorks 2004 Reference Guide
• • •
Shininess - 25% Transparency- 0% Emission - 0%
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Chapter 7 Parts
Multibody Parts Multibody Overview Part documents can now contain multiple solid bodies. A folder named Solid Bodies
appears in the
FeatureManager design tree when there are solid bodies in a single part document. The number of solid bodies in the part document is displayed in parentheses next to the Solid Bodies
folder.
For example, when you design a spoked wheel, you know the requirements of the rim and the axle. However, you do not know how to design the spoke. With multibody parts, you can create the rim and axle, then create the spoke to connect the bodies.
You can manipulate multibody solids the same ways you manipulate single solid bodies. For example, you can add and modify features, and change the names and colors of each solid body. You can hide and show solid bodies in the FeatureManager design tree. You can create multiple solid bodies from a single feature with the following commands: •
Extrude boss and cut (including thin features)
•
Revolve boss and cut (including thin features)
•
Sweep boss and cut (including thin features)
•
Surface cut
•
Boss and cut thicken
•
Cavity
Modeling techniques that you can use in a multibody environment include the following: •
Bridging
•
Local Operations
•
Symmetry Modeling
•
Body Intersection
•
Tool Body Modeling
•
Multibody Versus Assemblies
Multibody Parts Versus Assemblies Multibody parts should not replace the use of assemblies. A general rule to follow is that one part (multibody or not) should represent one part number in a Bill of Materials. A multibody part consists of multiple solid bodies that are not dynamic. If you need to represent dynamic motion among bodies, use an assembly. Tools such as Move Component, Dynamic Clearance, Mates, and Collision Detection are available only with assembly documents. You can save an assembly as a multibody part document. This enables you to save complex assemblies as smaller part documents to facilitate sharing files. For example, you have a design of an intricate motor assembly and a potential customer wants to know if it fits in their frame. You can save the motor assembly as a part document and send the part file to potential customers without risking design integrity or transmitting a large assembly document file.
7-10
To save an assembly as a multibody part document:
1.
Open an assembly document.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set the Save as type to Part (*.prt, *.sldprt). A set of options appears at the bottom of the dialog box.
4.
Select one of the following: •
Exterior Faces to save the exterior faces as Surface Bodies
.
•
Exterior Components to save the visible components as Solid Bodies
•
All Components to save all components as Solid Bodies
.
.
NOTE: Components that are hidden or suppressed are not saved when you select All Components. 5.
Click Save.
Modeling Techniques Body Intersection For the body intersection multibody technique, you use the Combine feature and its Common option. Body intersection is a quick way to create complex parts with very few operations, which can result in faster performance. The operation takes multiple solid bodies that overlap one another and leaves only the intersecting volumes of the bodies. For most models that can be represented fully by two or three drawing views, this technique can be used by intersecting either two or three extruded solids. The extrusion sketches are the solid lines represented in the two or three views. The following example shows this technique with the intersection of two extrusions.
Front
Top
Isometric
To create the part described above, you begin with the base part:
And then select the Common option of the Combine feature to use only the overlapping material of the base part.
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Chapter 7 Parts
Bridging Bridging is a commonly used technique in a multbody environment. Bridging creates a solid that connects multiple solid bodies. This technique is useful when you create portions of the model first and create the connecting geometry afterwards.
For example, when designing a golf club, you might know the specifics of the head and shaft design, but not necessarily how they are connected. You can design the head and the shaft first, then bridge the two bodies. Local Operations You use local operations when you want to perform operations on certain portions of a mulitbody model, but not on others. For example, you design a double-ended measuring cup. You need to shell the two cups and fillet them. However, you do not want to shell the piece that connects the two cups. You can create the part and perform the feature operations on the separate bodies.
When modeling the double ended measuring cups, first create the cups as two separate solid bodies.
Next, shell each body.
Model the connection bar and merge bodies.
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Lastly, fillet the edges. Symmetry Modeling Symmetry modeling simplifies the creation of axis-symmetric parts and also speeds performance for these types of parts. In this approach you make one symmetric body, pattern the bodies to obtain the remaining geometry, then use the Combine feature to glue all of the bodies together. You can use multiple patterns and combine features to create an entire model. For instance, the example below shows the design progression of a symmetrical part. Begin by building the basic piece that you pattern later.
Next, add the end piece, keeping this body separate, but adjacent.
Then pattern the basic piece.
Lastly, mirror the entire part, including the end piece, and combine the bodies.
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Chapter 7 Parts
Tool Body Modeling Use tool body modeling to create complex multibody tools to remove material from a solid body, or add complex shapes to geometry. You create common geometrically shaped bodies in separate part documents, then use the Insert, Part tool to create a multibody part document.
Initial part
Insert part
Use the Combine feature to remove material of inserted part.
Controlling Parts Parent and Child Relations Features are normally built upon other existing features. For example, you create a base extrude feature and then create additional features such as a boss or cut extrude. The original base extrude is the parent feature; the boss or cut extrude is a child feature. The existence of a child feature depends on the parent. A parent feature is an existing feature upon which others depend. Parent/Child include the following characteristics: •
You can only view the relations; you cannot edit them.
•
You cannot reorder a child feature before it’s parent.
To view Parent/Child relations:
1.
In the FeatureManager design tree or in the graphics area, right-click the feature whose relationships you want to see.
2.
Select Parent/Child from the menu.
Equations Creates mathematical relations between model dimensions, using dimension names as variables. When using equations in an assembly, you can set equations between parts, between a part and a sub-assembly, with mating dimensions, and so forth. When you delete a feature or dimension that is used in an equation, you have the option of deleting the equation or not. NOTE: Dimensions driven by equations cannot be changed by editing the dimension value in the model.
7-14
To add an equation:
1.
Click
or Tools, Equations.
2.
Click Add.
3.
In the model or the FeatureManager design tree, double-click on the feature that contains the first dimension you want to use in the equation.
4.
Click on the dimension to paste its name into the equation. (Dimension names are in the form dimension name @ feature or sketch name.)
5.
Complete the equation by typing or clicking on the calculator buttons, or by clicking on other dimensions to paste their names. Equations are solved left to right (i.e., the dimension on the left is driven by the value on the right), in the order in which they appear in the equation list. You can use additional supported functions. You can also insert comments in equations.
6.
Click OK. The equation appears in the Equations window, and the value of the solution is shown in the Evaluates To column.
7.
Click OK, then click or Edit, Rebuild to update the model. (All equations are solved before the geometry is regenerated.) An equation folder appears in the FeatureManager design tree. Right-click the folder to delete or edit existing equations or add a new equation to the document. NOTE: When using any trig function in an equation or dimension dialogue, the value of the angle is interpreted as radians. For example, sin(90) is evaluated as .89 (90radians) not 1.0 (90deg).
To edit equations:
1.
Click
or Tools, Equations, and click Edit All, or right-click
and select Edit equation.
2.
Edit the equations. Each equation must be on a separate line, and dimension names must be enclosed in quotes.
3.
Click OK to close the Edit Equations window.
4.
Click OK to close the Equations window.
5.
Click
or Edit, Rebuild.
Edit and Delete Equations To edit an equation:
1.
Click Equations
or click Tools, Equations and then click Edit All.
- or Right-click the Equations folder 2.
, and select Edit Equation.
In the Edit Equations dialog box, edit the text of the equations as needed, and click OK. The revised equation is displayed in the Equations dialog box. You can also cut and paste equations here to change the order, if necessary. If you make a mistake, click Undo to clear each consecutive value in the New Equation dialog box. You can clear one value each time you click Undo.
3.
Click OK, then click Rebuild
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.
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Chapter 7 Parts
To delete an equation:
1.
Click Equations - or -
or click Tools, Equations.
Right-click the Equations folder
, and select Delete Equation.
2.
Click the equation number or the status marker for the equation to delete, and click Delete in the Equations dialog box.
3.
Click OK, then click Rebuild
.
Operators and Constants Function
Name
Notes
sin (a)
sine
a is the angle expressed in radians; returns the sine ratio
cos (a)
cosine
a is the angle expressed in radians; returns the cosine ratio
tan (a)
tangent
a is the angle expressed in radians; returns the tangent ratio
atn (a)
inverse tangent
a is the tangent ratio; returns the angle in radians
abs (a)
absolute value
returns the absolute value of a
exp (n)
exponential
returns e raised to the power of n
log (a)
logarithmic
returns the natural log of a to the base e
sqr (a)
square root
returns the square root of a
int (a)
integer
returns a as an integer
sgn (a)
sign
returns the sign of a as -1 or 1 For example: sgn(-21) returns -1
pi
3.14...
Constant pi
Equation Comments and Status Comments in Equations You can add comments to equations, to document your design intent. You can also use comment syntax to prevent an equation from being evaluated. To add a comment to an existing equation:
1.
Click Equations
or click Tools, Equations.
- or Right-click the Equations 2.
folder and select Edit Equation.
If there is only one equation, the Equations and the Edit Equations dialog boxes are displayed. If there is more than one equation, select the equation and click Edit all to display the Edit Equations dialog box.
3.
Type a single quote (‘) at the end of the equation, then enter the comment. Anything after the single quote is ignored when the equation is evaluated. For example: "D2@Sketch1" = "D1@Sketch1" / 2 ‘height is 1/2 width
7-16
To add a comment to a new equation:
1.
Click Equations
or click Tools, Equations.
Click Add and enter the equation. 2.
Type a single quote (‘) at the end of the equation, then enter the comment. Anything after the single quote is ignored when the equation is evaluated. If you want to temporarily prevent an equation from being evaluated, but you do not want to delete it, place a single quote before the equation. The equation is then interpreted as a comment, and it is ignored.
Operators and Functions The following operators and functions are supported: + (plus sign) addition – (minus sign) subtraction * (asterisk) multiplication / (forward slash) division ^ (caret) exponentiation You can also use pi in equations. Its value is calculated to the number of decimal places specified for the document. Equations can also use additional operators and constants. Equation Status When you delete a feature or a dimension that is used in an equation, the software asks you if you want to delete the equation also. Because the order of solving equations is important, you may prefer to keep the equation, and edit it later. If you keep the equation, it has Not Solved status, and is marked with a red exclamation point dialog box. Equations with Solved status are marked with green check marks .
in the Equations
When you rename an assembly that includes an equation between assembly components, the equation is marked with a Read Only status .
Shared Values Using shared values, enables you to link dimension values using named variables. You can set the value of several dimensions to be equal without using multiple equations or relations. When dimensions are linked in this way, any member of the group can be used as a driving dimension. Changing any one of the linked values changes all others to which it is linked. The variable name you specify becomes the name of the linked dimensions, and appears in the Name box of the Dimension Properties dialog box. To link dimension values:
1.
Right-click one of the dimensions that you want to link, and select Link values. The Shared Values dialog box appears. The Value box displays the value of the selected dimension, but you may not change it here.
2.
Enter a Name. This is the variable name that will be used as the dimension name for the linked items. NOTE: You can delete unused dimension names from the Name list. Select the name and press Delete. You cannot delete a name used by another dimension.
3.
Click OK.
4.
Right-click one of the dimensions that you want to link to the first dimension, and select Link Values.
5.
Select the variable name from the list in the Name box, and click OK.
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Chapter 7 Parts
6.
Repeat for as many dimensions as needed. The values of the selected dimensions become linked to the first one. Changing any of the linked values causes the others to change.
The two linked dimensions are the side of the cube (25) and the depth of the cut extrude feature (25). When you change the side of the cube to 10, the linked value changes accordingly. To unlink dimension values:
Right-click the dimension that you want to unlink, and select Unlink value.
Measure Measures distance, angle, radius, and size of and between lines, points, surfaces, and planes in sketches, 3D models, assemblies, or drawings. When you measure the distance between two points, the delta x, y, and z distances are also displayed. When you select a vertex or sketch point, the x, y, and z coordinates are displayed. See Coordinate Systems. To use the measure tool:
1.
Click Measure
on the Tools toolbar or Tools, Measure.
The Measure dialog box appears. NOTE: While the Measure dialog box is in place, you can switch among different documents without closing the dialog box. The name of the currently active document displays in the title bar of the Measure dialog box. If you activate a document that has items already selected, the measurement information updates automatically. 2.
Under Projection on, click Screen to measure the projection on the screen, or click Plane/Face to measure the projection on a selected plane or planar face. When you measure a distance, the program calculates the projected distance (on the plane you selected), and the normal distance (normal to the plane you selected). In Detached drawings, if the model is not loaded, all measurements are reported as 2D projected data.
3.
Select the items to measure. Right-click an edge to use the Select Other, Select Midpoint, Select Tangency, Select Loop, or Clear Selections commands. The selected items appear in the Selected items list, and appropriate values are displayed in the Measurements box. New measurements update dynamically when you change selections. If you select a curve, one of the measured values is chord length. Chord length is the distance between the end points of the curve.
7-18
If you select a single entity, the size of the entity (the length of an edge, the area of a face, and so on) is displayed in the Measurements box.
If you select two entities, the smallest distance between the entities is displayed in the Measurements box.
If a valid measurement cannot be performed with the selected entities, a message in the Measurements box states: Invalid combination of selected entities. 4.
To delete an item from the Selected items list, click the item’s name in the list and press the Delete key, or click the selected item again in the graphics area.
5.
To clear all items from the Selected items list, right-click in the graphics area, and select Clear Selections.
6.
To display the results based on a coordinate system that you defined, select the name from the Output coordinate system list.
7.
To display the results in scientific notation or using different measurement units than the units specified for the active document, click Options to display the Measurement Options dialog box. To change other material properties, click Tools, Options, on the Document Properties tab, select Material Properties.
8.
To temporarily turn off the measure function, right-click in the graphics area, and choose Select from the menu. To turn the measure function back on, click inside the Measure dialog box.
9.
Click Close to close the dialog box.
Measurement Options Use the Measurement Options dialog box to modify measurement units and the material density of parts. Units You can change the measurement units. •
Use Length unit for linear dimensions.
•
Use Angular unit for angular dimensions.
•
Select the Scientific notation check box to display measurements in scientific notation.
When you change the Length unit, the dialog box reacts dynamically depending on which Length unit you select. For example, if you select microinches, mils, inches, or feet & inches, you can also select Fractions, Denominator, and Round to nearest fraction. Display Units To display the results with units other than the units specified for the active document, select one of the following: •
View measurement settings. Displays the units specified in the Measurement Options dialog box.
•
View global settings. Displays the units specified for the active document set in Tools, Options, Document Properties, Units.
•
View system defaults. Displays the system default units for new documents set in the document template.
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Material Properties In Material Properties, select Density to change the density of the material for this document. You can enter the density value using any units. For example, if the units of the part are grams and millimeters, you can enter a density value using pounds and inches. The software converts the value to the document’s units when you click OK. You can also change the density, as well as change options for cross hatch patterns through the Tools menu. Click Tools, Options, on the Document Properties, tab click Material Properties. Accuracy Level You can select between two accuracy level settings: •
Default mass/section property precision. Calculation used in versions previous to 2003 of the SolidWorks software.
•
Maximum property precision (Slower). Provides greater accuracy of the calculation, but the computation is slower.
Dependency Editing You can suppress a feature so you can work on the model with the selected feature temporarily removed from the model. Suppressing a feature not only removes it from the display, but also from any calculations in which it may be involved. Rebuilding complex models occurs faster when features with a large amount of detail are suppressed. The Features toolbar contains the following tools to suppress and unsuppress features of the model. See Suppress and unsuppress. Suppression is governed by the parent and child relations of the features.
Tooth Cut
Unsuppressed
Suppressed
Unsuppressed
Tooth Pattern
Unsuppressed
Suppressed - The child feature is suppressed because it is dependent on the parent feature, and the parent feature is suppressed.
Suppressed - If you unsuppress the parent feature, the child feature is not automatically unsuppressed. If you unsuppress the child feature, however, the parent feature is also unsuppressed.
Dependency editing is one way to control parts. Others methods of controlling parts include:
7-20
•
Rollback
•
Configurations
•
Design tables
Suppress and Unsuppress Features To suppress a feature:
1.
Select the feature in the FeatureManager design tree, or select a face of the feature in the graphics area. To select multiple features, hold down Ctrl as you select.
2.
Click Suppress
on the Features toolbar, or click Edit, Suppress.
- or 1.
In the FeatureManager design tree, right-click a feature, and select Properties.
2.
In the Feature Properties dialog box, select the Suppressed check box, and click OK. The selected feature is removed from the model (but not deleted). The feature disappears from the model view and is shown in gray in the FeatureManager design tree.
To unsuppress a feature:
1.
Select the suppressed feature in the FeatureManager design tree.
2.
Click Unsuppress
on the Features toolbar, or click Edit, Unsuppress.
- or 1.
In the FeatureManager design tree, right-click a feature, and select Properties.
2.
In the Feature Properties dialog box, clear the Suppressed check box, and click OK. If you want to unsuppress a suppressed feature, you must select it using the FeatureManager design tree.
To unsuppress a feature and its dependents:
1.
Select the suppressed parent feature in the FeatureManager design tree.
2.
Click Unsuppress with Dependents Dependents.
on the Features toolbar, or click Edit, Unsuppress with
The selected feature and any features that are dependent on it are returned to the model. - or 1.
Select the child feature in the FeatureManager design tree.
2.
Click Unsuppress with Dependents Dependents.
on the Features toolbar, or click Edit, Unsuppress with
The selected feature and its parent feature are returned to the model.
Derived Parts You can create a new part directly from an existing part. The new part, called a derived part, has the original part as its first feature, and it is linked to that part by means of an external reference. This means that any changes you make to the original part are reflected in the derived part. When a part has an external reference, its name in the FeatureManager design tree is followed by an arrow ->. To see the name, location, and status of the externally referenced document, right-click the derived part, and select List External Refs. There are three types of derived parts: •
Insert part
•
Mirror part
•
Derived component part
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Insert Part Use Insert Part to insert one or more base parts multiple times into a part document. Under Locate Part, select the Launch Move Dialog check box on the Insert Part PropertyManager to define a location for the inserted part. When you insert more than one part, the Locate Part PropertyManager appears automatically. To insert a part:
1.
With a part document open, click Insert Part
2.
Browse to a part document and click Open.
on the Features toolbar, or click Insert, Part.
The Insert Part PropertyManager appears. 3.
4.
Under Transfer, select any combination of the following: •
Axis. Transfers the axis information.
•
Plane. Transfers all planes from the original part.
•
Cosmetic Thread. Transfers cosmetic threads.
•
Surface. Transfers surfaces.
Click OK
.
To change the configuration of the inserted part:
1.
Right-click the part and select List External Refs.
2.
Select Use named configuration, select a configuration from the list, and click OK.
Mirror Part Mirror Part creates a mirrored version of an existing part. This is a good way to create a left-hand version and a right-hand version of a part. Because the mirrored version is derived from the original version, the two parts always match.
This type of mirroring produces a different result than using a mirror pattern. To create a mirrored, derived part:
1.
In an open part document, click a model face or plane about which to mirror the part.
2.
Click Insert, Mirror Part.
3.
In the PropertyManager, select one or more items:
4.
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•
Axis. Select to use an axis as a reference point for the new, mirror part.
•
Plane. Select to use a plane as a reference point for the new, mirror part.
•
Cosmetic Thread. Select to use cosmetic thread, when present, as a reference point for the new, mirror part.
•
Surface. Select to use a surface as a reference point for the new, mirror part.
The mirrored part is opened in a new part window.
Derive Component Part Derive Component Part creates a part from an assembly component. Derived parts created this way include any features created in the context of the assembly. For example, you can create a cavity in a mold assembly, then derive and cut the pieces of the mold. The derived parts maintain the necessary references to the components in the assembly. However, you cannot insert the derived component part back into the assembly. To create a derived part from an assembly component:
1.
In an assembly document, select a component.
2.
Click File, Derive Component Part. The derived part is opened in a new part window. TIP: If you need to include assembly features, use a derived component part. Otherwise, use a base part to optimize system performance.
Split and Save Bodies Use Split to create multiple parts from an existing part. You can create separate part files, and form an assembly from the new parts if needed. With multibody parts, you can use Split to create separate bodies. Create split parts by building separate parts, or by building a single part, and using a trim tool to separate the single part into multiple parts. When you create separate parts, you have the option to Show Bodies, Hide Bodies, or Consume Bodies.
To split a part:
1.
Click Split
on the Features toolbar, or click Insert, Features, Split.
The Split PropertyManager appears. 2.
Select one or more of the following as trimming surfaces: •
Reference planes (Planes extend infinitely in all directions.)
•
Planar model faces (Faces extend infinitely in all directions.)
Original Part •
Revised Original Part
New Part
Sketches (Sketches extrude through all in both directions.)
Original Part
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New Part
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•
Reference surfaces and non-planar model faces (These do not extend their boundaries. Note that internal holes on reference surfaces or non-planar model faces are closed when splitting the part.)
Original Part
New Parts
The entities appear under Trim Tool. 3.
Click Cut Part. Split lines appear on the part, showing the different bodies formed by the split. Callout boxes appear in the graphics area for up to 10 bodies. As you move your pointer
4.
over a body, the body highlights.
Select a body. The Save As dialog box appears.
5.
Type a name for the new part and click Save. The new part name appears in the Resulting Bodies list and in the callout box. NOTE: You can choose the same name for two different bodies if they are identical. If the bodies are not identical, the software does not let you choose the same name.
6.
Continue selecting bodies in the graphics area and naming new parts as needed. You can save all the bodies as new parts. The bodies that you do not save are not split. They remain with the original part.
7.
Callout boxes are displayed for 10 bodies at a time. Click Next 10 or Previous 10 to scroll through all the callout boxes for a part.
8.
Click OK
.
The new part documents open beneath the original document. Minimize the original document to see them. To split a part into multibody parts: 1.
Click Split on the Features toolbar, or click Insert, Features, Split. The Split PropertyManager appears.
2.
Select a Trim Tool in the graphics area. You can use reference planes, planar model faces, sketches, or reference surfaces as trim tools to create multibody parts. The entities appear under Trim Tool
7-24
.
In the example above, a sketch is the Trim Tool.
3.
Click Cut Part. Split lines appear on the part, showing the different bodies formed by the split. Callout boxes appear in the graphics area for up to 10 bodies. As you move the pointer body, the body highlights.
4.
over a
Select a body. The bodies you choose are listed under Resulting Bodies, and the check box selected. NOTE: Under
In the example above, there are three bodies. The center ring is selected.
is
, you can also select the
check box to choose the bodies. The bodies selected are the bodies you split. 5.
Continue selecting bodies in the graphics area or by selecting the appropriate check box
.
In the File column, double-click each split part to select it and to display the Save As dialog box. 6.
Type a name for the new part and click Save. The new part name appears in the Resulting Bodies list, and, with the complete path, in the callout box.
In the example above, the middle section was split, creating a multibody part.
NOTE: If you clear the check box for a split part after you save it, that part is no longer saved as a separate entity. It remains with the original part.
7.
Under Resultant bodies state, select one of the following: •
Show bodies. All bodies appear in the graphics area. All of the bodies are listed in the
•
FeatureManager design tree under Solid Bodies, and the icons are filled . Hide bodies. Only the bodies that you did not split appear in the graphics area. Bodies that are selected
•
are hidden. All the split bodies are listed in the FeatureManager design tree
under Solid Bodies, but the icons for hidden bodies are blank . Consume bodies. Removes the body from the part. Consumed bodies are not listed in the FeatureManager design tree under
8.
Click OK
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.
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Chapter 7 Parts
New Parts The new parts are derived; they contain a reference to the parent part. Each new part contains a single feature named Stock-<parent part name>-n->. If you change the geometry of the original part, the new parts also change. With multibody parts, the various split parts are listed in the FeatureManager design tree under Bodies.
Solid
Original Part The original part contains all its original features plus a new feature called Split. The solid body displayed in the graphics area is the original solid body minus the new parts. If all bodies in the original part were saved as split bodies, no solid body is displayed. To see the original solid body, move the rollback bar in the FeatureManager design tree above the split feature, or suppress the split feature. If you delete the split feature in the original part, the new parts still exist, but the status of the external reference in the new parts is dangling. You can also save solid bodies after you split the model using the Save Bodies feature. This enables you to save the bodies from a split part to a different folder or with different names to the same folder. To save bodies from multi-body parts:
1.
Click Insert, Features, Save Bodies. The pointer changes to
2.
and the Save Bodies PropertyManager appears.
Select each of the body parts from the graphics area to include in the assembly. •
Callouts. Display the default path and file names.
•
Path. Location of your multibody part.
•
File names. Listed in the Solid Bodies
•
You can also select each part from the File list under Resulting Parts.
folder in the FeatureManager design tree.
3.
Under Resulting Parts, click each file to activate and open the Save As dialog box. You can select a new location and file name for each part.
4.
Under Create Assembly, click Browse, and select a folder to save the assembly as SplitAssembly type (*.sldasm).
5.
Click OK
.
In the FeatureManager design tree, the entities are listed under Solid Bodies
.
Edit Derived Parts Derived part documents have some limitations: •
You can only add features in a derived part document.
•
You cannot delete or modify the features of the original part in the derived part document.
•
You can only edit the original part in its own window.
•
You cannot change the configuration of a derived part using the External References For dialog box.
To edit the original part from which another part is derived:
1.
Right-click the derived part, and select Edit In Context. If the part was derived using an insert part or a mirror part, the original part document is opened. If the part was derived from an assembly component, the assembly document is opened.
2.
Change the original part as needed. The changes are reflected in any derived parts that have an external reference to the original part.
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Create Assembly You can create an assembly from split part in a single step using the Create Assembly feature. The assembly you create is identical to an assembly created manually by opening an assembly document and dragging the part files individually into the assembly document. You can create additional features in the multibody part after using the Create Assembly command. However, these additional features do not appear as individual part files and are not part of the assembly document. To form split parts into an assembly:
1.
Select one or more Split features from the FeatureManager design tree.
2.
Click Insert, Features, Create Assembly.
3.
In the PropertyManager, under Split Features, select a Split part from the FeatureManager design tree.
4.
Click Browse. The Save As dialog box appears.
5.
Browse to the folder where you want to save the assembly, and type a name for the assembly in the File name box.
6.
Click Save.
7.
Click OK
.
The new assembly document opens.
Resolve Ambiguity The Resolve Ambiguity dialog box is displayed when the SolidWorks software identifies two or more valid solutions. Since more than one solution is valid, you are prompted to select the most appropriate solution from the list the solution. The Resolve Ambiguity dialog box can appear in any of the following scenarios. Editing a part within an assembly If you open an assembly and edit a part in that assembly, the Resolve Ambiguity dialog box is displayed when you try to save the changes. Saving the file creates an ambiguity because SolidWorks cannot determine whether you want to save the part or the assembly. To resolve the ambiguity:
1.
Select the part file or the assembly file in the Resolve Ambiguity dialog box.
2.
Click OK to save the selected element.
Converting entities with a closed contour If you select one side of a closed contour sketch (such as a rectangle), and click Convert Entities Ambiguity dialog box is displayed. There are two valid solutions: •
Single segment - only the line segment is converted
•
Closed contour - the entire closed contour sketch is converted
, the Resolve
To resolve the ambiguity:
1.
Select either Single segment or Closed contour from the list.
2.
Click OK to convert the entity you selected.
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File Management with External References When you save a part that has external references to another document, the path and the internal ID of the referenced document are saved with the current part. The software needs this information to locate and verify the original document the next time you open the derived part. You can specify whether or not referenced documents are opened when you open a part that has external references. Locating Derived Parts Suppose you create a derived part, then you inadvertently move or rename the original document. When you try to open the derived part, the software notifies you that the externally referenced document (the original) was not found, and you are given a chance to look for it. If you choose not to look, the operation is cancelled. If you decide to look for the referenced document, you have the following choices: •
If you locate and select the original document (in a different directory, or with a new name), the derived part opens using the new name or path. Because the internal ID matches, the external reference updates as expected. When you save the part, the new name or path is saved also.
•
If you select a different document, you are notified that the internal ID does not match. Then you can either accept the selected document anyway, or keep looking.
Rebuild Errors If you accept the selected document, the model may have rebuild errors, especially if you have added features in the derived part document. If the geometry of the document you selected is not the same as the geometry of the original referenced document, the additional features may have rebuild errors.
Feature Statistics Feature Statistics is a tool that displays the amount of time it takes to rebuild each feature in a part. Use this tool to reduce rebuild time by suppressing features that take a long time to rebuild. This tool is available in all part documents. To use feature statistics:
1.
Open a part document.
2.
Click Statistics
on the Tools toolbar, or click Tools, Feature Statistics.
The Feature Statistics dialog box appears with a list of all features and their rebuild times in descending order.
3.
•
Feature Order. Lists each item in the FeatureManager design tree: features, sketches, and derived planes. Use the shortcut menu to edit feature definition, suppress features, and so on.
•
Time %. Displays the percentage of the total part rebuild time to regenerate each item.
•
Time(s). Displays the amount of time in seconds that each item takes to rebuild.
Click Feature Order. This sorts the features to match the FeatureManager design tree.
4.
5.
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Click one of the following: •
Print. Prints the Feature Statistics.
•
Copy. Copies the Feature Statistics so you can paste them into another file.
•
Refresh. Refreshes Feature Statistics.
Click Close.
Model Geometry Overview The Check Entity dialog box enables you to identify undesirable geometry and check model geometry. It is divided into two sections, Check and Check for. •
Check allows you to check Solids, Surfaces, or Features.
•
Click Selected items to display the Items to check box.
This checks a selected face or edge, for the items listed in the Items to check list. Use as a fast check of the selected items to report any errors on faces or edges. You can use this option first, to determine if the model geometry is valid. If you design very complex models, it is a good idea to use this option regularly, after creating several features. Sample of selected items check •
Click All to check some or all of the Solid or Surface features from the model. You can select all Solids, all Surfaces, or both.
It is a fast check of the whole model (or the selected items). It reports any errors on faces or edges. You can also use this option, to determine if the model geometry is valid. •
Click Features to select all the features in the model.
This is slower, especially for complex models, because it examines the model feature by feature, to locate the source of the problem. If any errors are found when you use Selected items, you can use this option to identify which features contain errors •
Check for allows you to select the types of problems that you want to check for:
•
Invalid face(s)
•
Invalid edge(s)
•
Short edge(s)
When you check for Short edge(s), you must specify a minimum edge length. The software reports any edges that are less than the specified length. The number of errors is listed in the Found column. The items are displayed in the Result list box. Additional information is in the message area. You can also check model geometry: •
Maximum radius of curvature
•
Maximum edge gap
•
Maximum vertex gap
The items are displayed in the Result list box. Additional information is in the message area.
Selected Items Check Entity Selected items: Surface body (created with Offset Surface) Check for: • Maximum edge gap • Maximum vertex gap Results: • No errors • 1 open surface found • 4 edges and vertices found with maximum gaps
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Chapter 7 Parts
Checking Model Geometry The SolidWorks software automatically checks the model geometry as you create each feature, to prevent invalid geometry. It also provides additional tools for checking the model, which you can use for the following purposes: •
To examine imported geometry (when you import the body as a whole, from another system, such as an IGES or STEP file)
•
To make sure that the model exports properly to other formats
•
To determine the cause when the model looks wrong
Force Regeneration with Verification on Rebuild By default, each time you add or modify a feature, the feature is checked against any adjacent faces and edges. For most situations, this default level of error checking is adequate, and results in fast rebuilding of the model. However, under certain circumstances, it is recommended that you perform more rigorous checks on the model: •
When the model looks wrong (and you have determined that it is not the result of a display problem)
•
When you have problem exporting the model in different formats
To increase the level of error checking, turn on the Verification on rebuild option. When this option is turned on, the software checks every new or changed feature against all existing faces and edges, not just adjacent faces and edges. Features that cause invalid geometry fail when this option is turned on. NOTE: This option has a negative effect on performance. Rebuilding the model is considerably slower and more CPU-intensive. This option applies to all documents, not just the active document. Use this option only when needed, then be sure to turn it off when you are done. To verify the model with a higher level of error checking:
1.
Click Tools, Options, on the System Options tab, select Performance, and the Verification on rebuild check box.
2.
Press Ctrl + Q to regenerate the entire model. NOTE: When you press Ctrl + Q, it causes a complete rebuild of all the features in the model. The Edit, Rebuild
operation (Ctrl + B) only rebuilds new or changed features and their children.
3.
Examine and correct any features that fail, beginning with the first failed feature in the FeatureManager design tree. Often fixing one failed feature allows subsequent failed features to rebuild successfully.
4.
When you are satisfied that all the errors are corrected, click Tools, Options, on the System Options tab, select Performance, clear the Verification on rebuild check box.
Checking a Planar Surface To check a planar surface:
1.
In the Check Entity dialog box, click Check selected items, select the surface in the FeatureManager design tree, and click Check.
2.
The message reports if the surface is open or closed, and the surface boundary edges are highlighted.
3.
7-30
•
The Result list identifies any invalid edges or faces.
•
The message area lists a description of the results. To highlight an individual result, select the item displayed in the selection box.
Click OK to close the message, then click Close to close the dialog box.
Checking Part Faces or Edges To check a face or edge of a part:
1.
Click Tools, Check to display the Check Entity dialog box.
2.
In Check, click Selected items and select a face or an edge in the graphics area. The name of the item appears in the Item to check box.
3.
In Check for, select the types of problems that you want to review: Invalid face(s), Invalid edge(s), and/or Short edge(s), or any combination of the three.
4.
If you selected Short edge(s), specify a minimum edge length in the spin box. The software reports any edges that are less than the specified length.
5.
Click Check. After checking, the dialog box remains open so you can check additional entities.
6.
•
The Found column displays the number of items found with the specified error.
•
The Result list box displays the items that are either invalid or too short.
•
A message area lists a description of the results. To highlight the individual result, select the item displayed in the selection box.
Click Close to close the dialog box.
Check Entity To check a model for correct geometry:
1.
With a part document active, click Tools, Check.
2.
In the dialog box, select the entity type that you want to verify.
3.
•
All. Checks the entire model. Specify Solids, Surfaces, or both.
•
Selected items. Select items, such as faces, edges, and so on from the graphics area.
•
Features. Select features from the graphics area. As you select each feature, it is highlighted in the FeatureManager design tree.
In the Check for area, check the model for errors or report on the model’s geometry. •
Invalid face(s)
•
Invalid edge(s)
•
Short edge(s)
When you check for Short edge(s), you must specify a minimum edge length. The software reports any edges that are less than the specified length. 4.
Click Check (The dialog box remains open so that you can change the options or select different items to check.)
5.
Click Close to exit the Check Entity dialog box.
Finding the Minimum Radius of Curvature To find the smallest radius of curvature for the model:
1.
Click Tools, Check to display the Check Entity dialog box.
2.
In Check for, select the Minimum radius of curvature check box to determine the face with the smallest radius of curvature.
3.
In Check, you can choose Selected items and then select model faces, splines, or curves in the graphics area. If you select All, the entire part is checked.
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Chapter 7 Parts
4.
5.
Click Check. (The dialog box remains open so that you can change the options or select different items to check.) •
The Item to check box displays the items you selected from the graphics area.
•
The Result list box displays the minimum radius. In the graphics area, an arrow points to the place on the curve where the minimum radius of curvature is found. (If there are two locations with the same minimum radius, only one is reported.)
•
The message area lists a description of results (the minimum curvature). To highlight the individual result, select the item displayed in the selection box.
Click Close to exit the Check Entity dialog box.
Interrupt Regeneration Press Esc to interrupt the regeneration of parts. This also works with opening parts, rollbacks, and so on. NOTE: When you interrupt the regeneration of a part, the system completes regeneration of the current feature and then places the rollback bar after the feature.
Send To Send the current part document to another system using electronic mail. To mail a part document to another computer:
1.
Click File, Send To.
2.
Enter your mail password, the mailing address, and any other information requested by your mail application. To send an assembly or drawing document, see Send Mail.
Displaying Parts Information Displaying Annotations in Parts You can add annotations to your model to further clarify the information the part document provides. This includes dimensions, notes, symbols, and so on. Then you can import the dimensions and annotations from the model into a drawing (see Detailing Overview). You can control the display of annotations in the part window using shortcut menu selections on the Annotations folder
in the FeatureManager design tree.
To select the types of annotations to display:
1.
In the FeatureManager design tree, right-click Annotations Properties dialog box appears.
2.
Under Display filter, select the annotation types to display (Notes, Datums, and so on), or select the Display all types check box to show all types of annotations available for the part.
3.
Change the values in the Text scale boxes to modify the scale of the text used in the annotation.
4.
Select from the following options:
5.
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and select Details. The Annotation
•
Always display text at the same size. Annotations and dimensions are displayed at the same size regardless of zoom.
•
Display items only in the view orientation in which they are created. An annotation is only displayed when the part is in the same view orientation as when the annotation was inserted. Rotating the part or selecting a different view orientation removes the annotation from the display.
•
Display annotations. All annotation types that are selected in the display filter are displayed.
Click OK.
To toggle the display of annotations:
Right-click Annotations
and select (or clear) the items to display:
•
Display Annotations. All annotation types that are selected in the Annotation Properties dialog box are displayed. This is the same as selecting the Display Annotations check box in the Annotation Properties dialog box.
•
Show Feature Dimensions. This is the same as selecting the Feature dimensions check box in the Display filter of the Annotation Properties dialog box.
•
Show Reference Dimensions. This is the same as selecting the Reference dimensions check box in the Display filter of the Annotation Properties dialog box.
To toggle the display of selected feature dimensions:
To hide an individual dimension, right-click it, and select Hide. To hide all the dimensions of a selected feature, right-click the feature in the FeatureManager design tree, or right-click one of its faces, and select Hide All Dimensions. To re-display the dimensions, right-click the feature or one of its faces, and select Show All Dimensions.
Summary Information You can use the Summary Information dialog box to add more information to a part or assembly document, or to a configuration of the model in the document. Use this type of custom information in the followings ways: •
Apply in a Bill of Materials
•
Add associative dimensions in parts that dynamically update in a Bill of Materials
•
Use as advanced selection criteria for managing assembly configurations
•
Integrate with drawing sheet formats and link notes to document properties
•
Add system-defined, configuration-specific mass properties
To enter or display summary information:
1.
Click File, Properties. The Summary Information dialog box appears.
2.
On the Summary tab, type the appropriate information in the boxes provided for: Author, Keywords, Comments, Title, and Subject. The system provides read-only Statistics about the document’s creation date, the date last saved, and the name of the person who saved the document last. NOTE: If you insert a part identification number in the Title box, you can use that number automatically when you create a bill of materials in an assembly drawing that contains that part.
Summary Info – Custom and Configuration Specific Access to the Summary Information dialog box is through File, Properties. The Custom and the Configuration Specific tabs in the Summary Information dialog box allow you to: •
Specify custom properties for the active part, assembly, or drawing document.
•
Apply configuration-specific properties for the active part or assembly configuration.
•
Add associative dimensions. The dimensions can come from sketches, part features, assembly features, or assembly mates. Since part dimensions are associative, values in the Bill of Materials (BOM) are updated when the dimensions are changed.
•
Edit the list of custom properties.
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• • •
When you type a Name and a Value to add a new Property, you can click OK to add the new property without first clicking Add. If you type a Name and a Value to add a new Property, and then select another name from the list without clicking Add, the first property is automatically added. When you modify an existing custom property, those changes are saved when you click OK. You no longer need to click Modify to apply the changes.
In addition to the BOM, you can use the properties in the following ways: •
As advanced selection criteria for managing assembly configurations
•
In drawing sheet formats and to link notes to document properties If you plan to use the property as a custom column in a Bill of Materials, do not include any spaces in the Name.
To specify custom properties:
1.
Enter a Name for the property, or choose one from the list. You can now specify a Description name, which appears in the Open and Save As dialog boxes.
2.
Select the Type from the list.
3.
Enter a Value for the custom property that is compatible with the selection in the Type box.
4.
Click Add. The Properties box displays the name, values, and type of the custom properties.
To add associative dimensions into custom properties:
1.
Open the part and display the dimensions to add to Custom Properties.
2.
Enter a Name for the property, or choose one from the list.
3.
Select the Type from the list.
4.
Click the dimension in the graphics area. The dimension name @ feature is displayed in Value.
5.
Place your cursor at the end of the dimension name and add additional text, such millimeters. NOTE: Values are cumulative unless you clear the content in the Value box. Cumulative values enable you to include dimensions, units, and other text. For example: Click one dimension in the graphics area, type x in the Value box, and click additional dimensions in the graphics area to display: dimension name1 @ feature x dimension name2 @ feature, and so on.
6.
Click Add. The Properties box displays the name, values, and type of the custom property. Any dimension included in Custom Properties is updated when you modify the dimension in the part.
To edit custom properties:
1.
In the Name box, click the property that you want to change.
2.
Edit the Type or Value as needed.
3.
Click Modify. NOTE: This modifies the custom properties for the current document only. Edit the global custom properties with the Edit List dialog box.
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To delete custom properties:
1.
Click the property in the Properties box that you want to delete.
2.
Click Delete. NOTE: This deletes the custom properties from the current document only. Delete the global custom properties with the Edit List dialog box.
You can add system-defined, configuration-specific mass properties as a custom property, using either the Custom or Configuration Specific tabs. Use the Configuration Specific tab to display with other configuration-specific properties. Mass properties use the following, system-generated format: SW<mass property>@ @configuration@model To add mass properties:
1.
Enter a Name for the mass property.
2.
Select the Type from the list.
3.
Click Mass Properties and select the appropriate mass property from the list.
4.
Click Add. The Properties box displays the name, values, and type of the mass property.
5.
Click OK.
Edit List You can edit the list of custom properties. You can also edit the text file where the properties are stored in any text editor. The default file location is install_dir\lang\english\properties.txt. To edit custom properties:
1.
Click Edit List on the Custom tab of the Summary Information dialog box. The Edit List dialog box with the list of properties appears.
2.
You can do one of the following: •
Add. Type a name in the box and click Add.
•
Delete. Select a property from the list and click Delete.
•
Move Up. Select a property from the list and click Move Up.
•
Move Down. Select a property from the list and click Move Down.
Section Views Overview You can display a view of the model cut through the part or assembly. You can cut through a model or assembly using one of the following: • •
One or more standard planes. You can pre-select a plane, or if no plane is selected, the Front plane is selected by default. One or more planes you create.
•
One or more planar faces, by selecting any planar face on the model.
•
Viewing plane, which is the invisible plane parallel to the screen.
You can view both the section view and the complete view of the model at the same time by splitting your screen into two windows. (Drag the split bars on the bottom or right side of the window frame.) You can now select faces, edges, and vertices formed by a section view. See Section View Selection. Before you can display a section view of an assembly, you must fully resolve any lightweight parts that it contains. Displaying and creating views include: •
Creating section views
•
Using viewing planes
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Section View Selection You can select the faces, edges, and vertices that are created by a section view of a part or assembly. In earlier versions, the section view was for visualization only, and you could not select faces or edges that were cut by the section plane.
NOTE: You cannot open a sketch on a section view face. Measure and Section Properties •
Select a face on the section plane to calculate its section properties. Select edges or vertices to measure.
•
Select truncated faces to measure lengths or calculate section properties. Truncated faces are faces cut by the section plane.
Truncated Faces Convert Entities For functions other than Measure and Section Properties, the truncated faces act as if they are not truncated. For example, if you open a sketch on a truncated face and convert the edges, the edges of the full face are converted.
Full Face is Converted
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Section Views in Models Section views use a plane to display a cutaway of a part or assembly. To create a section view of the model:
1.
Click Section View
on the View toolbar or click View, Display, Section View.
The Section View dialog box appears. 2.
Click one or more planes in the FeatureManager design tree, or click one or more planar faces on the model. Alternatively, you can pre-select planes or planar faces before you click View, Display, Section View. If nothing is selected, the Front plane is used by default. To pre-select multiple planes or faces, hold down the Ctrl key as you select.
3.
Click a plane in the Section Plane(s)/Face(s) box, then use the arrows to set a value in the Section Position box to move the plane and change the section cut. You can also use the viewing plane.
4.
Click the Flip the Side to View check box to reverse the viewing direction of the section cut. (Not available if you are using the viewing plane.)
5.
Select a Preview/Display mode:
6.
•
When Preview is selected, the section view is updated whenever any item in the dialog box is changed. If you need to adjust more than one setting, especially with a large part or assembly, this option may not be efficient.
•
When Preview is cleared, click Display to update the section view. You can make multiple changes to the settings, then click Display again to update the view with all the changes at once.
Click OK.Example NOTE: You can view both the section view and the complete view of the model at the same time by splitting your screen into two windows. (Drag the split controls on the bottom or right side of the window frame.) You can revolve, size, and shade the views independently.
Using Viewing Planes for Section Views Instead of model faces and planes, you can use a viewing plane to cut the section view. The viewing plane is an invisible plane that is parallel to the screen, and normal to your line of sight. The initial position for this plane is the center of the part body bounding box. As you rotate the part, the angle of the viewing plane relative to the part body changes, cutting the part at a different angle. To use the viewing plane to cut a section view:
To use the viewing plane to make a section cut, click Use Viewing Plane in the Section View dialog box. You can offset the Section Position of the viewing plane. The Flip the Side to View option is not available when you use the viewing plane. To change the section view:
1.
Click Section View
or click View, Modify, Section View.
2.
Change the settings in the Edit Section View dialog box, and select a different plane if needed.
3.
Click OK.
To return to a normal view of the model:
Click Section View
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or click View, Modify, Section View again to deselect the command.
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Sample Section Views
Model with no section view
Model using plane 45° to Plane1 and Section Position -5.00mm
Model using plane 45° to Plane1, Section Position -5.00mm, and Flip side to view
Model using Viewing Plane and Section Position 26.50mm
Mass Properties and Section Properties Displays the density, mass, volume, surface area, center of mass, inertia tensor, and principal axes of inertia of a part or assembly model. A tri-colored reference 3D triad displays at the origin. A red 3D triad displays at the centroid of the part or assembly along with the mass properties and section properties.
Before you can calculate mass properties or section properties of an assembly, you must fully resolve any lightweight parts that it contains. See also Loading Additional Model Data. Mass Properties To evaluate components or solid bodies in assembly and multibody part documents, click the component or body, and click Recalculate. If no component or solid body is selected, the mass properties for the entire assembly or multibody part are reported.
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To display mass properties:
1.
Click Mass Properties
on the Tools toolbar or click Tools, Mass Properties.
NOTES: •
You evaluate different entities without closing the Mass Properties dialog box. Clear the selections, then select the entity, and click Recalculate.
•
The results are displayed in the Mass Properties dialog box, and the principal axes and center of mass are displayed graphically on the model.
2.
Click Options if you want to display the Measurement Options dialog box and to display the results using different units than the units specified for the active document.
3.
Click Print if you want to print the results directly from this dialog box.
4.
Click Copy if you want to copy the information to the clipboard, then paste it into another document.
5.
Click Close to close the dialog box.
NOTE: When you save the document, you can update the mass properties information. This enhances system performance, since the next time you access mass properties, the system does not need to recalculate the values (if the document is unchanged). To set this option, click Tools, Options, on the System Options tab, click Performance, and click the Update mass properties while saving document check box. Section Properties You can evaluate section properties for multiple faces and sketches that lie in parallel planes. Clear the selections, then select the entity, and click Recalculate. NOTE: When you evaluate more than one entity, the first selected face defines the plane for section property calculation. To display section properties for multiple entities:
1.
2.
Select any of the following that lie in parallel planes: •
one or more planar model faces
•
a face on a section plane
•
the crosshatch section face in a section view of a drawing
•
a sketch (click the sketch in the FeatureManager design tree or right-click the feature and select Edit Sketch)
Click Tools, Section Properties. The results are displayed in the Section Properties dialog box.
Curvature You can display a part or assembly with the surfaces rendered in different colors according to the local radius of curvature. Curvature is defined as the reciprocal of the radius (1/radius), in current model units. By default, the greatest curvature value displayed is 1.0000, and the smallest value is 0.0010. As the radius of curvature decreases, the curvature value increases, and the corresponding color changes from black (0.0010), through blue, green, and red (1.0000). As the radius of curvature increases, the curvature value decreases. A planar surface has a curvature value of zero (1/8). To render curved surfaces in colors and display curvature radius:
1.
Click Tools, Options. The Options dialog box appears with the System Options tab active.
2.
On the System Options tab, click Display/Selection, and make sure that the Dynamic highlight from graphics view check box is selected.
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3.
Click View, Display, Curvature. The curvature of the model is displayed in color. When you point to a model surface, a spline, or a curve, the curvature value and the radius of curvature are displayed beside the pointer.
4.
To remove the color, click View, Display, Curvature to clear the check mark.
To render an individual model face in colors:
1.
Right-click the model face and select Face Curvature. The curvature of the selected face is displayed. When you point to the model face, the curvature value and the radius of curvature are shown beside the pointer.
Model with no color applied to curved surface 2.
Model with color applied to selected curved surfaces (zero curvature is black)
To remove the color, right-click the model face and click Face Curvature to clear the check mark.
To set values for the color scale for displaying curvature:
1.
Click Tools, Options. The Options dialog box appears with the System Options tab active.
2.
On the Document Properties tab, click Colors.
3.
Click Curvature.
4.
Select the curvature value edit boxes that you want to change and enter new values. You can modify the values at five intervals on the color scale; values are interpolated for the intermediate colors in the range. See sample of curvature values for some common radius values.
5.
Click Apply to preview the color scale changes with the new values.
6.
Click OK to save the new settings.
Curvature Values for Common Radius Values
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Radius
Curvature
Radius
Curvature
0.125
8
10
0.1
0.25
4
20
0.05
0.5
2
25
0.04
0.75
1.333
30
0.033
1
1
40
0.025
1.5
0.667
50
0.02
2
0.5
75
0.013
2.5
0.4
100
0.01
3
0.333
125
0.008
4
0.25
200
0.005
5
0.2
250
0.004
7.5
0.133
500
0.002
Curvature Options Defines the colors associated with the curvature of models. Curvature is equal to the inverse of the radius of the curve (curvature = 1/radius). By default, the greatest curvature is represented by red, and the least curvature is represented by black. For example, if you display curvature on a cube, all sides display as black. This is because the radii of flat faces are infinite and the curvature is zero. As the curvature increases (and the radius decreases), the corresponding color values change from black, through blue, green, and red. You can change the curvature values at both ends of the scale and at three points in the middle so that the curvature values increment within a narrower or wider range, or increment more or less rapidly. To set the curvature values:
1.
Click Tools, Options, click the Document Properties tab, and click Colors.
2.
Click Curvature.
3.
Select the curvature value edit boxes that you want to change and enter new values.
4.
Click Apply to see how the color scale changes in response to the new curvature values. The intermediate curvature values also change appropriately.
5.
Click OK to save the new settings, and click OK again to close the Color dialog box.
Curvature Display You can display a surface, part, or assembly with the curved surfaces rendered in different colors according to their local radius of curvature. To define the colors, click Tools, Options, and click the Document Properties tab. Select Colors and click Curvature. You can also display the curvature value of sketch segments and curves in a closed sketch. To render curved surfaces in colors, and to display the radius of curvature values:
Click View, Display, Curvature. While the Curvature menu item remains selected, •
The value of the curvature radii is displayed next to the pointer when you point at curved surfaces.
•
The curvature of the model is displayed in colors related to the radii of the curvature. To remove the curvature display, click View, Display, Curvature again (to clear the check mark).
To toggle curvature display for individual faces:
Right-click a curved face and select Face Curvature from the menu. NOTE: The curvature display for faces can be toggled on or off using the shortcut menu, except when Curvature is turned on with View, Display, Curvature.
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To display curvature values for sketch entities in a closed sketch:
1.
Click Tools, System Options, Display/Selection, and select Dynamic highlight from graphics view.
2.
Click OK.
3.
Now you can click View, Display, Curvature in the main menu. The curvature value is displayed next to the pointer when you point at sketches or curves.
Zebra Stripes Zebra stripes allow you to see small changes in a surface that may be hard to see with a standard display. Zebra stripes simulate the reflection of long strips of light on a very shiny surface. With zebra stripes, you can easily see wrinkles or defects in a surface, and you can verify that two adjacent faces are in contact, are tangent, or have continuous curvature. See Zebra Stripes on Boundaries for more information.
Part Zebra Stripes To view a part with zebra stripes:
1.
Click View, Display, Zebra Stripes. The Zebra Stripes PropertyManager appears, and the part is displayed with zebra stripes.
2.
Under Settings, do the following: •
Adjust the Number Of Stripes
•
Adjust the Width Of Stripes
•
Adjust the Stripe Accuracy . Move the slider from low accuracy (left) to high accuracy (right) to improve the quality of the display. Note that increasing the display accuracy also increases the display calculation time.
•
Change the Color Of Stripes and Color Of Background. Click Edit Color, choose a new color from the Color palette, and click OK. The new color appears in the color box and in the graphics area.
•
Select one of the following: •
.
Spherical Map. Available on all systems. The part appears to be inside a large sphere that is covered on the inside with strips of light. The zebra stripes are always curved (even on flat faces) and display singularities.
Singularities
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.
•
Cube Map. Available on systems with a graphics card that supports cube texture maps. If your computer does not have this type of graphics card, SolidWorks does not allow you to select this option. The part appears to be inside a large square room that is covered with strips of light on the walls, ceiling, and floors. The zebra stripes are straight on flat faces, and do not display singularities. The cube map display shows unstriped bands. Unstriped bands are the reflections of the corners of the "room."
No stripes 3.
Click OK
Spherical Map
Cube Map
.
To turn off zebra stripes:
Click View, Display, Zebra Stripes, or right-click the part in the graphics area and click Zebra Stripes. Zebra Stripes are deselected. Face Zebra Stripes You can improve the accuracy of your display by selecting only those faces that you want displayed with zebra stripes. To view a face with zebra stripes:
1.
Right-click a face in the graphics area and select Face Zebra Stripes. The Zebra Stripes PropertyManager appears, and the face is displayed with zebra stripes.
2.
Adjust the display as described previously.
3.
Click OK
.
To turn off face zebra stripes:
Click View, Display, Zebra Stripes, or right-click in the graphics area and click Face Zebra Stripes. Zebra Stripes are deselected. NOTE: It may be helpful to use zebra stripes in conjuction with the Curvature display.
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Zebra Stripes on Boundaries You can visually determine what type of boundary exists between surfaces by using zebra stripes. Contact Zebra stripes do not match at the boundary.
Tangency Zebra stripes match at the boundary, but there is an abrupt change in direction.
Curvature Continuous Zebra stripes continue smoothly across the boundary. Curvature continuity is an option when creating face blend fillets.
Fillet
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Tangent
Curvature Continuous
Lighting Lighting Overview You can adjust the direction, intensity, and color of light in the shaded view of a model. You can add light sources of various types, and modify their characteristics to illuminate the model as needed. The properties of the light sources work with the material properties of the model. If you change material properties of the model, you can enhance or reduce the effect of the light properties. Light Types There are several types of light source: •
Ambient light. Illuminates the model evenly from all directions. In a room with white walls, the level of ambient light is high, because the light reflects off the walls and other objects.
•
Directional light. Comes from a source that is infinitely far away from the model. It is a columned light source consisting of parallel rays from a single direction, like the sun. The rays of a Directional light point toward the center of the model.
•
Point light. Comes from a very small light source located at a specific coordinate in the model space. This type of light source emits light in all directions. The effect is like a tiny light bulb floating in space.
•
Spot light. Come from a restricted, focused light with a cone-shaped beam that is brightest at its center. A spot light can be aimed at a specific area of the model. You can adjust the position and distance of the light source relative to the model, and you can adjust the angle through which the beam spreads.
System Lighting Defaults By default, the Lighting folder light.
in the FeatureManager design tree contains one Ambient light and one Directional
•
You can turn the Ambient light on or off, but you cannot delete it or add additional Ambient lights.
•
You can turn the Directional light source on or off, or delete it. You can also add additional Directional light sources.
•
The maximum number of light sources in any document is nine (the Ambient light and eight others in any combination).
Basic Lighting Controls To add a light source:
1. 2.
Right-click the Lighting folder
or any existing light.
Select Add Spot Light (or Add Directional Light, or Add Point Light) - or Click View, Lighting, Add Spot (or Add Directional, or Add Point).
To delete a light source:
1.
Click the
to expand the Lighting folder
and display the light sources.
2.
Select Spot Light (or Directional Light, or Point Light) and press Delete. - or Click View, Lighting, Delete, Spot (or Directional, or Point).
To turn off a light, without deleting it:
1. 2.
Click the
to expand the Lighting folder
and right-click the light source.
Select Properties. - or Click View, Lighting, Properties (Ambient, Directional, Spot, or Point).
3.
In the Ambient, Directional, Spot, or Point Light Properties dialog box, click to clear the On check box.
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To modify the lighting properties:
1.
Right-click the light source in the Lighting folder
2.
Edit the properties as needed. The light properties that are available depend on the type of light source. See: •
Ambient Light Properties
•
Directional Light Properties
•
Point Light Properties
•
Spot Light Properties
and select Properties.
3.
As you edit each light, a graphical representation of the light source is displayed, indicating the color and direction of the light.
4.
Click OK.
Ambient Light You can control the intensity and the color of ambient light. To control ambient light:
1.
In the FeatureManager design tree, click
2.
Right-click Ambient and select Properties.
3.
In the Ambient Light Properties dialog box, you can do the following: •
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Slider right: high ambience
Click Edit to display the Color palette, and select colored ambient light rather than the default white light.
White ambient light •
Ambient Off
Move the slider from left (for low intensity) to right (for high intensity).
Slider left: low ambience •
folder.
Clear the On check box to eliminate the ambient light from the model. You can turn ambient light off, but you cannot delete the ambient light.
Ambient On •
to expand the Lighting
Red ambient light
Click Use as default to save the current ambient setting as your default setting.
NOTE: The results vary widely. They depend on multiple combinations, including the color of the model, the degree of ambience (intensity), as well as the color of the light. For example, changing the color of the ambient light produces more noticeable results with high ambience than with low ambience.
Directional Light Properties Basic Tab On the Basic tab, a Directional light source has the following Intensity properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
See also Ambient light for information on Basic properties. Direction Tab On the Direction tab, specify the following properties: •
Direction. Specify the direction from which the light arrives, relative to the origin. You can use the sliders to specify the values for Longitude and Latitude, or you can enter a value in degrees.
Directional light with default placement •
Directional light with change in Latitude
Directional light with change in Latitude and Longitude
Lock to model. When this check box is selected, the light moves along with the model when you rotate the model. The light always shines on the same area of the model because the position of the light relative to the model is maintained.
To keep the light in the same position in the model space, clear the Lock to model check box. When you rotate the model, the light shines on different areas of the model because the position of the light remains fixed in space. As you edit the Directional light, a graphical representation of the light source is displayed, indicating the color and direction of the light. After you finish, click OK.
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Point Light Properties Basic Tab On the Basic tab, a Point light includes the following Intensity properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
See also Ambient light for information on Basic properties. Position Tab On the Position tab, specify the Position of the light source relative to the origin. Select the type of coordinate system, and specify the values: •
Spherical (Longitude, Latitude, Distance)
•
Cartesian (X, Y, Z)
Point light with default placement and default values
•
Point light with default placement, change to green color and Specularity at maximum
Point light with increase in Brightness (Basic) and changes to Position, using Cartesian coordinates
Lock to model. When this check box is selected, the light moves along with the model when you rotate the model. The light always shines on the same area of the model because the position of the light relative to the model is maintained.
To keep the light in the same position in the model space, clear the Lock to model check box. When you rotate the model, the light shines on different areas of the model because the position of the light remains fixed in space. As you edit the Point light, a graphical representation of the light source is displayed, indicating the color and direction of the light. After you finish, click OK.
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Spot Light Properties Basic Tab On the Basic tab, a Spot light includes the following Intensity properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
See also Ambient light for information on Basic properties. Position Tab On the Position tab: •
Position. The Position is the location of the light source relative to the center of the scene. Like a Point light, you can use either Spherical or Cartesian coordinates.
•
Target. The Target is where the light strikes the model or the surrounding scene. Only Cartesian coordinates (X, Y, Z) are available.
The Spot light also includes an Advanced tab where you can set Cone Angle, Exponent, and Attenuation. As you edit each light, a graphical representation of the light source is displayed, indicating the color and direction of the light. After you finish, click OK.
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Lighting - Basic All light sources have the following properties: •
Color. To change the color, click Edit, select a new color from the palette, and click OK.
•
On. To turn the light on or off, select or clear the On check box.
•
Configurations. Select This Configuration, All Configurations, or Specify Configurations.
•
Use as default. If you want to save the settings for the current light, and use them in new documents, click Use as default.
•
Intensity. Move the Ambient slider to adjust the level of light. The level changes equally on all sides of the model.
Directional, Point, and Spot lights have these additional properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
Lighting - Advanced Exponent. The exponent controls how tightly the beam of light is concentrated. A low exponent value produces a focused, cone-shaped beam of light with sharp edges. The intensity of the light is similar at the center of the beam and at the edges. With a high exponent value, the beam is brightest at the center. The intensity decreases toward the edges of the beam, and the edges of the beam appear softer. Cone Angle. The cone angle specifies the angle through which the beam spreads. A small angle produces a narrow beam of light. Attenuation. The attenuation is the property that decreases the intensity of the light as the distance increases. The values A, B, and C are multipliers in the following equation (D is the distance): attenuation = 1 / A + (B * D) + (C * D2) As the values for A, B, and C increase, the amount of light that reaches the target decreases.
Low values
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High values
Lighting - Position and Direction Direction. For a Directional light, specify the direction from which the light arrives, relative to the origin. You can use the sliders to specify the values for Longitude and Latitude, or you can enter a value in degrees. For a Point or Spot light, select the type of coordinate system, then specify the values: •
Spherical (Longitude, Latitude, Distance)
•
Cartesian (X, Y, Z)
For a Directional light, type a position or use the sliders to set values for the following: •
Latitude
•
Longitude Lock to model. • In these examples, notice the position of the Spot light relative to the model when the model is rotated. Original position •
When selected, the light moves along with the model when you rotate the model. The light always shines on the same area of the model because the position of the light relative to the model is maintained.
Lock to model selected •
To keep the light in the same position in the model space, clear this check box. When you rotate the model, the light shines on different areas of the model because the position of the light remains fixed in space. Lock to Model cleared
Target. (Spot light only). • The Target is where the light strikes the model or the surrounding scene. Only Cartesian coordinates (X, Y, Z) are available.
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8 Mold Design
Mold Tools Toolbar The Mold Tools toolbar provides tools for creating molded parts and assemblies. Scale Parting Lines Ruled Surface Parting Surfaces Tooling Split Cavity Draft Split Line Offset Surface Ruled Surface Radiate Surface Planar Surface Knit Surface Draft Analysis Undercut Detection
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Chapter 8 Mold Design
Understanding Mold Design Creating a mold design in the SolidWorks software requires the following items: •
Design parts - The parts that you want to mold.
•
A mold base - The part that holds the cavity feature of the design part.
•
An interim assembly - The assembly in which the cavity is created.
•
Derived component parts - The parts that become the halves of the mold after you cut them (recommended).
You can create a mold using a sequence of integrated tools that control the mold creation process. With the model finished, you can use these mold tools to analyze and correct deficiencies with either SolidWorks or imported models. Mold tools span from initial analysis to creating the tooling split. The process is as follows: •
Undercut Detection model from ejecting.
•
Parting Lines . This tool has two functions: o Verifies the you have draft on your model, based on the angle you specify. o
. Use the Undercut Detection tool to identify trapped areas that prevent the
Creates a parting line from which you create a parting surface. The Parting Lines tool includes the option to select an edge and have the system Propagate
to all edges.
. Models often include openings which you need to shut-off to prevent leakage from
•
Shut-off Surfaces core-to-cavity.
•
Parting Surfaces . Parting surfaces extrude from the parting line to separate mold cavity from core. You can also use a parting surface to create an interlock surface. In such instances, you can create a separate surface to separate mold cavity from core.
•
Ruled Surface . Ruled surfaces are used with imported parts when the draft analysis shows that sections of the model require draft. You can also use the Ruled Surface tool to create an interlock surface.
•
Tooling Split . The Tooling Split tool creates the core and cavity by automatically populating the core, cavity and parting surface, based on the steps followed earlier.
The Mold Tools toolbar also includes additional tools common to the mold process, such as Scale as well surface modeling tools such as Planar Surface
and Knit Surface
, Cavity
,
.
You combine the design parts and mold base in the interim assembly. Then, you create a cavity feature in the context of the interim assembly. This relates the mold base to the design part in the event that the design part changes shape. You cannot edit mold features within an assembly.
8-2
Mold Tools - Undercut Detection The Undercut Detection tool finds trapped areas in a model that cannot be ejected from the mold. These areas require a slide, which usually slides in a perpendicular direction to the core and cavity segments as these are separated. Undercut detection does not detect with imported surface parts, or surface parts generated in SolidWorks. Undercut analysis is not based on the parting line. To run an undercut detection:
1.
Click Undercut Detection
2.
In the PropertyManager, under Analysis Parameters: •
in the Molds toolbar, or click Insert, Molds, Undercut Detection.
Click Coordinate input to set coordinates along the X, Y and Z axes. This controls the Direction of Pull. - or -
•
3.
Select a plane, face, or edge as the Direction of Pull
.
Click Calculate.
Under Undercut Faces, the number of faces appears. 4.
5.
Under Undercut Faces: •
Click Show
•
Click Edit Color to display the Color palette and change the color for either the undercut faces or the normal faces.
•
Clear Save color if you do not want to save the new color definition upon exit.
Click OK
SolidWorks 2004 Reference Guide
, or Hide
for either the undercut faces or the normal faces.
.
8-3
Chapter 8 Mold Design
Scaling Factor and Draft in Mold Design Scaling Factor When you create a mold you must account for the scaling factor. The scaling factor is the amount the material in the mold shrinks or expands as it solidifies. The scaling factor depends on the type of material used and the shape of the mold, and is expressed as a percentage of the linear size (not volume) of the design part. The software scales the cavity by the specified scaling factor, using this formula: Cavity size = part size * (1 + scaling factor/100) For example: Desired adjustment
Scaling factor in % (enter this number)
Resulting cavity size
2% material shrinkage (cavity larger than part)
2.0
part size * 1.02
2% material expansion (cavity smaller than part)
-2.0
part size * 0.98
Creating Drafts for Molds You may need to add draft angles to molded design parts to make it possible to remove the finished part from the mold. If you have a SolidWorks model, you can use the Split Line
tool to split faces and the Draft
tool to add
tool with either SolidWorks or imported models to add draft, correct
draft. You can also used the Ruled Surface flawed surfaces, or create interlock surfaces.
Mold Tools - Parting Lines Parting lines lie along the edge of the molded part, between the core and the cavity surfaces. They are used to create the parting surfaces, and to separate the surfaces. You create the parting lines after the model is scaled and proper draft is applied. To create parting lines:
8-4
1.
Click Parting Lines
on the Mold toolbar, or click Insert, Molds, Parting Line.
2.
In the PropertyManager, under Mold Parameters: •
Select a flat face or a plane as the Direction of Pull.
•
Note the direction of the arrow, and click Reverse
•
Set a value for Draft Angle
•
Click Draft Analysis.
.
if necessary.
3.
Inspect the model for draft, and compare the colors to those displayed under Mold Parameters. You should have a combination of Positive and Negative draft. If draft is required:
Positive and Negative draft
4.
•
With a SolidWorks model, click Draft
on the Molds toolbar, or click Insert, Molds, Draft.
•
With an imported model, click Ruled Surface Ruled Surface.
on the Molds toolbar, or click Insert, Molds,
Under Parting Lines, do one of the following: •
If the model includes a chain of edges that runs between positive and negative faces (that includes no straddle faces), the parting lines are selected automatically.
•
If the model includes multiple chains, the longest chain is selected automatically.
•
If you want to automatically select a different chain of edges: a. b.
Right-click and select Clear Selections. Select an edge.
c.
Click Propagate
to display all the edges under Edges.
Propagate to all edges automatically •
5.
If you want to manually select each edge: a.
Click Add selected edge
b.
Click Select next edge
c.
Click Zoom to the selected edge
Click OK
SolidWorks 2004 Reference Guide
. , and repeat until all the edges appear under Edges. for detail of the edge selection area.
.
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Chapter 8 Mold Design
Mold Tools - Ruled Surfaces With imported geometry, you cannot use draft tools from the SolidWorks application to correct surfaces that require draft. The Ruled Surface command can create ruled surfaces that are either perpendicular or tapered from the selected edges. You can also use the ruled surfaces to create interlock surfaces. To create a ruled surface:
1.
Click Ruled Surface
2.
In the PropertyManager, under Type, select an option:
3.
4.
5.
6.
on the Molds toolbar, or click Insert, Molds, Ruled Surface.
•
Tangent to Surface. Ruled surface is tangent to the surfaces that share an edge.
•
Normal to surface. Ruled surface is normal to the surfaces that share an edge.
•
Tapered to Vector. Ruled surface is tapered to the specified vector.
•
Perpendicular to Vector. Ruled surface is perpendicular to the specified vector.
•
Sweep. Ruled surface is built by creating a swept surface using selected edges as guide curves.
Under Distance/Direction: •
Set a value for Distance
.
•
With Tapered to Vector, or Perpendicular to Vector: o
Select an edge, a face, or a plane as the Reference Vector.
o
Click Reverse Direction
o
With Tapered to Vector only, set an Angle
, if necessary. .
Under Edge Selection: •
Select the edges used as the base for the ruled surfaces
•
Click Alternate Side, if necessary.
Under Options: •
Clear Trim and knit to manually trim and knit the surfaces.
•
Clear Connecting Surface to remove any connecting surfaces. Connecting surfaces are usually created between sharp corners.
Click OK
.
Mold Tools - Shut Off Surfaces After you create the parting lines, you need to shut off any open areas to prevent leakage. The liquid filling the mold must not connect the cavity side of the part with the core side of the part. To create shut off surfaces:
1.
Click Shut-off Surfaces
on the Mold toolbar, or click Insert, Molds, Shut-off Surfaces.
In the PropertyManager, under Edges, all the edges that belong to open surfaces appear. 2.
8-6
Inspect the arrows that show the direction of the shut-off surface.
Incorrect direction
Correct direction
Incorrect direction: note the uneven surface
Correct direction: note the smooth surface
3.
If necessary, click the arrow to shift the direction.
4.
Click OK
.
Mold Tools - Parting Surfaces After you determine the parting lines and create the shut off surfaces, you create the parting surfaces. Parting surfaces extrude from the parting lines, and are used to separate the mold cavity from the core. To create a tooling split (the next step in the process), you need at least three surface bodies in the Surface Bodies
folder.
To create parting surfaces:
1.
Click Parting Surfaces
on the Molds toolbar, or click Insert, Molds, Parting Surface.
2.
In the PropertyManager, under Mold Parameters, select an option: •
Tangent to surface. Parting surface is tangent to the surface of the parting line.
•
Normal to surface. Parting surface is normal to the surface of the parting line.
•
Perpendicular to pull. Parting surface is perpendicular to the direction of pull. This is the most common.
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Chapter 8 Mold Design
Tangent to surface 3.
Normal to surface
Perpendicular to pull
Under Parting Surfaces: •
Set a value for Distance.
•
Click Reverse offset direction
•
If you selected Tangent to surface or Normal to surface, you can set a value for Angle changes the angle from perpendicular to the direction of pull.
•
Smoothing. You can apply a smoother transition between adjacent surfaces. o
Sharp
, if necessary. . This
is the default value.
Smooth gives you the option to set a value for Distance between adjacent edges. A higher value creates a smoother transition between adjacent edges. Under Options: o
4.
•
Clear knit all surfaces to prevent surfaces from knitting by default. With most models, the surfaces are created correctly. However, if you need to repair a gap between adjacent surfaces, you can use surface tools such as Lofted Surface
• 5.
on the Surfaces toolbar, or Ruled Surface
on the Molds
toolbar. When you clear knit all surfaces, use Knit Surface in the Molds toolbar to manually knit the surfaces after the repairs. Clear Show Preview if you want to optimize system performance.
Click OK
.
With most mold parts, you need to also create interlocking surfaces. Interlock surfaces help prevent the core and cavity blocks from shifting, and are located along the perimeter of the parting surfaces. Usually, they have a 5 degree taper. With simpler models, you can create interlock surfaces using the same tools you used to create the parting surface.
8-8
Mold Tools - Tooling Split After you define a parting surface, use the Tooling Split tool to create the core and cavity blocks for the model. To create a tooling split, you need at least three surface bodies in the Surface Bodies folder. This model includes an interlock surface. It was created using the Ruled Surface tool using other surface modeling tools.
and it was finished
To create the tooling split:
1.
Select a face or plane on which to sketch an outline that separates the core and cavity segments.
2.
Click Tooling Split
3.
Orient the model so that the surface or plane you selected is normal to.
4.
Sketch a rectangle that extends beyond the model edge, but is within the parting surface boundaries.
5.
Close the sketch to open the Tooling Split PropertyManager. Under Core
, the Core Surface Bodies appear.
Under Cavity 6.
on the Molds Tools toolbar, or click Insert, Molds, Tooling Split.
, the Cavity Surface Bodies appear.
In the PropertyManager, under Block Size: •
Set a value for Depth in Direction 1
.
•
Set a value for Depth in Direction 2
.
•
Select Interlock surface if you want the system to create an interlock surface.
With most models, creating an interlock surface manually provides better control than relying on automatic creation. 7.
Under Parting Surface
8.
Click OK
SolidWorks 2004 Reference Guide
, select the parting surface created earlier.
.
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Chapter 8 Mold Design
Tooling split preview
Tooling split applied
Interlock Surface With most mold parts, you need to create interlock surfaces. Interlock surfaces help prevent the core and cavity blocks from shifting, and are located along the perimeter of the parting surfaces. Usually, they have a 5 degree taper.
Finishing the Interlock Surface
Lofted Surface
Ruled Surface Use Ruled Surface, rather than Extend Surface to maintain the correct taper.
Extend Surface To facilitate Trim Surface.
Trim Surface , using Mutual to remove material adjacent to the horizontal ruled surface. Knit Surface
8-10
after trim.
Create a plane, parallel to Top Plane. Sketch rectangle to create a planar surface.
Planar Surface
Trim Surface , using Standard to trim below the planar surface.
After trim, the planar surface is ready as the basis for tooling split operation.
Mold Tools - Insert Cavity To create a mold cavity:
1.
Prepare the interim assembly.
2.
In the assembly window, right-click the mold base in the graphics area or in the FeatureManager design tree and select Edit Part. - or Click the mold base, and click Edit Component
on the Assembly toolbar.
You are editing the part, not the assembly. The changes you make are reflected in the original part file of the mold base. If you do not want to affect the original mold base, use Save As in the mold base part document to save it with a different name for use in each new mold assembly. Otherwise, the original mold base includes the cavity you are about to insert. See also Editing Referenced File Locations. 3.
Click Cavity
4.
In the PropertyManager, under Design Components, select the design parts from the FeatureManager design tree.
SolidWorks 2004 Reference Guide
on the Mold Tools toolbar, or click Insert, Mold, Cavity.
8-11
Chapter 8 Mold Design
5.
Under Scale Parameters: a.
b.
6.
Select the point about which scaling occurs for Scale About. •
Component Centroids. Scales the cavity for each part about its own centroid.
•
Component Origins. Scales the cavity for each part about its own origin.
•
Mold Base Origin. Scales the cavity for each part about the origin of the mold base part.
•
Coordinate System. Scales the cavity for each part about the selected coordinate system.
Enter the Scaling Factor in %. A positive value expands the cavity, a negative value shrinks the cavity. See Scaling Factor. •
Uniform scaling. Select Uniform scaling, and enter a value to scale in all directions.
•
Non-uniform scaling. Clear Uniform scaling, and enter a scaling value for the X, Y, and Z directions.
Click OK
.
A cavity in the shape of the design part is created. The cavity size reflects the scaling factor you specified.
Any changes you make to the design part automatically update the cavity in the mold base, as long as the update path is available. See also External References.
8-12
9 Assemblies
Assemblies You can build complex assemblies consisting of many components. The components of an assembly can include both individual parts and other assemblies, called sub-assemblies. For most operations, the behavior of components is the same for both types. Components are linked to the assembly file. Assembly documents have the .sldasm extension. To create an assembly from a part:
1.
Click Make Assembly from Part/Assembly from Part.
on the Standard toolbar, or click File, Make Assembly
An assembly opens with the Insert Component PropertyManager active. 2.
Click in the graphics area to add the part to the assembly.
The following topics describe the basics of creating an assembly from components you have already built, and general information about working with assemblies of any kind. •
Design methods
•
Adding assembly components
•
Assembly mating
•
Working with sub-assemblies
•
Simplifying large assemblies
•
Using advanced component selection methods
•
Exploding an assembly view
•
Customizing the appearance of an assembly
•
Smart Fasteners
Design Methods You can create an assembly using bottom-up design, top-down design, or a combination of both methods. Bottom-up Design Bottom-up design is the traditional method. In bottom-up design, you create parts, insert them into an assembly, and mate them as required by your design. Bottom-up design is the preferred technique when you are using previously constructed, off-the-shelf parts. An advantage of bottom-up design is that because components are designed independently, their relationships and regeneration behavior are simpler than in top-down design. Working bottom-up allows you to focus on the individual parts. It is a good method to use if you do not need to create references that control the size or shape of parts with respect to each other.
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Chapter 9 Assemblies
Top-down Design Top-down design is different because you start your work in the assembly. You can use the geometry of one part to help define other parts, or to create machined features that are added only after the parts are assembled. You can start with a layout sketch, define fixed part locations, planes, and so on, then design the parts referencing these definitions. For example, you can insert a part in an assembly, then build a fixture based on this part. Working top-down, creating the fixture in context, allows you to reference model geometry, so you can control the dimensions of the fixture by creating geometric relations to the original part. That way, if you change a dimension of the part, the fixture automatically is updated.
The FeatureManager Design Tree in an Assembly FeatureManager Design Tree Conventions The FeatureManager design tree displays the names of these items in an assembly window: •
Top-level assembly (the first item in the tree)
•
Lighting
•
Assembly planes and origin
•
Components (sub-assemblies and individual parts)
•
Mategroup and mating relations
•
Assembly features (cuts or holes) and component patterns
, Annotations
, MateReferences
, and Simulation
folders
You can expand or collapse each component to view its detail by clicking beside the component name. To collapse all the items in the tree, right-click the assembly icon at the top of the tree, and select Collapse Items. You can use the same component multiple times within an assembly. Each component has the suffix. For each occurrence of the component in the assembly, the number n is incremented. In the FeatureManager design tree, a component name may have a prefix that provides information about the state of its relationships to other components. The prefixes are: (-) under defined (+) over defined (f) fixed (?) not solved The absence of a prefix indicates that the component’s position is fully defined. Display of Components in the FeatureManager Design Tree There are times when you want to focus on the structure or hierarchy of the design rather than the details of the sketches and features. In addition, you may want to focus on the design of the assembly without all of the features of the components. Each of these ways of viewing the assembly affects only the level of detail displayed in the FeatureManager design tree. The assembly itself is not affected. To display the hierarchy or feature detail of an assembly:
•
To display the hierarchy, right-click the assembly name in the FeatureManager design tree, and select Show Hierarchy Only. The FeatureManager design tree displays only the components (both parts and sub-assemblies), but no lower level detail.
•
9-2
To display the detail again, repeat the procedure, selecting Show Feature Detail.
To view an assembly by dependencies or by features:
•
To display the dependencies, right-click the assembly name in the FeatureManager design tree and select Tree Display, View Mates and Dependencies or click View, FeatureManager Tree, By Dependencies. Dependent items (instead of features) are listed under each component. Dependent items include mates and component patterns. You can view a component's features and planes by expanding the Features under the component.
•
folder
To display the features again, right-click the assembly name in the FeatureManager design tree, and select Tree Display, View Features or click View, FeatureManager Tree, By Features.
Component Icons in the FeatureManager Design Tree Resolved. The component is fully loaded into memory and all of its features and mates are editable. Lightweight. A feather overlay appears on the icon of a lightweight part. Out-of-Date Lightweight. A red feather overlay appears on the icon of an out-of-date lightweight part. Suppressed. A gray icon indicates that the component is not in use in the active configuration. Hidden. A transparent icon indicates that the component is active, but invisible. Hidden Lightweight. A transparent feather over a transparent component indicates that the component is lightweight and hidden. Hidden, Out-of-Date, and Lightweight. A transparent icon with a red feather overlay indicates that the component is hidden, out-of-date, and lightweight.
Viewing Mates View Mates displays a list of the mates for one or more components or sub-assemblies in an assembly. It is a useful tool to use when the number of mates gets large. To view the mates for a component:
1.
Right-click a component and select View Mates. The left panel splits to show the FeatureManager design tree and a list of the component's mates. TIP: To view the mates for more than one component, hold down Ctrl and select the components, then right-click and select View Mates. Mates between selected components are listed in bold.
2.
Click a mate to highlight the mated entities in the graphics area.
To view the mates for a sub-assembly:
Right-click a sub-assembly and select View Mates. Mates between sub-assembly reference geometry (such as planes), and reference geometry or components outside the sub-assembly are listed. Mates between the components of a sub-assembly are not listed. Mates between sub-assembly components and components outside the sub-assembly are not listed.
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Chapter 9 Assemblies
To view mates between the components of a sub-assembly:
1.
Expand
the sub-assembly in the FeatureManager design tree.
2.
Expand
the mategroup.
The mates are listed in the split panel display. To view the mates for a sub-assembly component:
1.
Expand
the sub-assembly.
2.
Right-click the component and select View Mates. The component's mates are listed.
Adding Components to an Assembly When you place a component (either an individual part or a sub-assembly) in an assembly, the component file is linked to the assembly file. The component appears in the assembly; the component data remains in the source component file. Any changes you make to the component file update the assembly. There are many ways to add components to a new or existing assembly: •
Use the Insert Component PropertyManager.
•
Drag from an open document window.
•
Drag from Windows Explorer.
•
Drag a hyperlink from Internet Explorer.
•
Drag within the assembly for additional instances of existing components.
•
Drag from the Feature Palette window.
•
Use Insert, Smart Fasteners to add bolts, screws, nuts, pins, and washers.
Insert Components To insert components into an assembly:
1.
Click Insert Components Assembly.
on the Assembly toolbar, or click Insert, Component, Existing Part/
Open documents that you previously saved appear under Part/Assembly to Insert. 2.
Select a part or assembly from the list, or click Browse to open an existing document.
3.
Click Keep Visible
4.
Click in the graphics area to place the component.
to add more than one instance of a component or more than one component.
If Keep Visible is not selected, the PropertyManager closes. If Keep Visible is selected, click again in the graphics area to add another instance of the selected component. Alternatively, you can repeat steps 2 through 4 to add a different component. Options
9-4
•
Start command when creating new assembly. Select to open this PropertyManager when you create a new assembly. Clear if your first assembly task is commonly something other than inserting components.
•
Graphics preview. Select to see a preview of the selected document in the graphics area under your pointer.
Adding Components from an Open Document Window To add components by dragging and dropping from an open document window:
1.
Open the destination assembly document, and open the source document (either the component document itself, or another assembly document that contains the component.)
2.
Click Window, Tile Horizontally (or Tile Vertically).
3.
Drag the component icon from the FeatureManager design tree of the source window, and drop it in the destination assembly window. If you are adding an individual part (not a sub-assembly), you can also drag the part from the graphics area of the source window. You can inference the assembly origin. If the component has multiple configurations, you can select which configuration to insert. Click the ConfigurationManager tab configuration.
in the source window, then drag and drop the name of the desired
Adding Components from Windows Explorer To add components by dragging and dropping from Windows Explorer:
1.
Open an assembly.
2.
Open Windows Explorer. Browse to the folder that contains the desired component.
3.
Drag the document icon from the Explorer window. A preview of the component appears.
4.
Drop it in the graphics area of the assembly window. You can inference the assembly origin. If the component has multiple configurations, the Select a configuration dialog box appears. Select the configuration you want to insert, and click OK.
Adding Components from Internet Explorer You can add a part from a hyperlink to an assembly. You can also drag and drop assemblies and .zip files from hyperlinks, but they open in their own window rather than as components of the assembly. To add a part from a hyperlink in Internet Explorer:
1.
In Internet Explorer, navigate to a location that contains hyperlinks to SolidWorks part files.
2.
Drag a hyperlink from the Internet Explorer window. A preview of the component appears.
3.
Drop it in the graphics area of the assembly window. The Save As dialog box appears.
4.
Browse to the folder where you want to save the part, enter a new name if desired, and click Save. The part document is saved to the specified folder.
5.
If the part has multiple configurations, the Select a configuration dialog box appears. Select the configuration you want to insert, and click OK. The part is added to the assembly.
Adding Components by Dragging and Dropping To add another component instance by dragging and dropping:
1.
With an assembly open, hold the Ctrl or Shift key, then drag a component either from the FeatureManager design tree, or from within the graphics area. A preview of the component appears.
2.
Drop it in the graphics area. You can inference the assembly origin. When you add a new instance of a component, the instance number suffix (component) is incremented.
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Chapter 9 Assemblies
Inferencing to the Assembly Origin When you insert a component by various means, you can inference the assembly origin. Look for the pointer shown here when you point to the origin.
When you inference the assembly origin: •
the component is fixed (f)
•
the component origin is coincident with the assembly origin
•
the planes of the component and the assembly are aligned
You can also drop a component in the tree of the assembly window to inference the origin. The component is fixed only if it is the first component in the assembly.
Deleting Components from an Assembly To delete a component from an assembly:
1.
Click the component in the graphics area or in the FeatureManager design tree.
2.
Press the Delete key, click Edit, Delete, or right-click and select Delete.
3.
Click Yes to confirm the deletion. The component and all its dependent items (mates, component patterns, explode steps, and so on) are removed.
Saving an Assembly and Its Components When you save an assembly, the path and name of each referenced component is saved in the assembly document. For this reason, you must exercise caution when you save or rename a component document, or move it to a different folder. Under the File menu, there are several ways to save an assembly document. Whichever method you use, the current locations of all referenced components (parts and sub-assemblies) are saved with the assembly document.
9-6
•
Save. When you use Save, you save the assembly document, and any referenced component documents that have changed.
•
Save As. When you use Save As, you save a copy of the assembly document with a new name or path. You can create a new folder in the Save As dialog box if needed. After you use Save As, you are working in the new assembly document. The original assembly document is closed without saving.
•
Save as copy. Click the Save as copy check box in the Save As dialog box to save a copy of the assembly document, with a new name or path, without replacing the active document. You continue to work in the original assembly document.
•
With both Save As and Save as copy, if any of the components have changed since the last Save operation, you are notified that they need to be saved also. If you agree to save them, they are saved in their original referenced locations.
Saving an Assembly in Various Ways The following table lists the effects of saving an assembly in various ways. For this example, assume that these are the active documents: Assembly document
c:\test\Assem1
Referenced part documents
c:\test\PartA c:\test\PartB (changed since the last save)
Saved files
Active assembly after saving
Referenced File Locations
Save
c:\test\Assem1 c:\test\PartB
c:\test\Assem1
c:\test\PartA c:\test\PartB
Save As c:\final\Assem2
c:\final\Assem2 c:\test\PartB
c:\final\Assem2
c:\test\PartA c:\test\PartB
Save as copy c:\final\Assem2
c:\final\Assem2 c:\test\PartB
c:\test\Assem1
c:\test\PartA c:\test\PartB
Find References, then Copy files to c:\final
c:\final\PartA c:\final\PartB
c:\test\Assem1
c:\test\PartA c:\test\PartB
Replace Components An assembly and its components may go through many revisions during the course of a design cycle. This is especially true in a multi-user environment where several users can work on the individual parts and sub-assemblies. A safe, efficient way to update the assembly is to replace the components as needed. NOTES: •
You can replace a part with a sub-assembly or vice versa.
•
You can replace one, more than one, or all instances of a component at the same time.
To replace one or more components:
1.
Click Replace Components on the Assembly toolbar, click File, Replace, or right-click a component and select Replace Components. The Replace PropertyManager appears.
2.
Select the components to replace in the Replace these component(s) check box to replace all the instances of the selected component.
box. Select the All instances
3.
Click Browse to locate the replacement component for the With this one
4.
Under Configuration, select Match name to allow the software to try to match the configuration name of the old component with a configuration in the replacement component. Select Manually select to choose the matching configuration in the replacement component.
5.
Select Re-attach mates to allow the software to try to re-attach existing mates to the replacement component.
6.
Click OK
box.
.
The selected component instances are replaced. If you chose Manually select, choose the configuration to open in the Configurations dialog box. If you selected the Re-attach mates check box, the Mated Entities PropertyManager appears.
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Chapter 9 Assemblies
Reload Documents Allows you to Reload documents. This is useful if you have read-only access to a document and you want to reload the latest version with any changes made by a colleague. To reload a document:
1.
Click File, Reload in a part or assembly document, or right-click a component in an assembly and select Reload.
2.
Select Open as read-only if you do not want to save any changes to the file. NOTE: If you have write-access to a sub-assembly then you reload it as read-only, you still have writeaccess to the individual components of the sub-assembly. You must reload each of the sub-assembly components as read-only to relinquish write-access privileges.
3.
Click OK. See also Replace Components.
Edit Referenced File Locations You can edit the locations of referenced parts: •
To open different parts for an assembly or drawing, - or -
•
To save selected assembly or drawing parts to a new location or filename.
NOTES: •
When saving, if the part filename already exists in the new location, you are prompted to confirm that you want to replace the part.
•
Only open documents appear in the list. For example, you must resolve lightweight components to see them in the list.
To edit part location:
1.
Click File, Open, References, or click File, Save As, References.
2.
In the New pathname list, select a path or filename that you want to edit , or click Select All.
3.
You can edit the path or filename using one of the following methods:
4.
•
Select a list entry by double-clicking. Browse to a new folder or type a new name in the Open dialog box, then click Open.
•
Select the check box for a list entry and click Browse to change to a new drive or directory path. The new drive or path appears in the New folder box.
•
Click Replace and enter a word to find and a word to replace with. (For example, change "\samples" to "\archive" to move one or all part files to the archive directory.) Click the Match case check box if the case is significant in the search.
Click OK to make the changes and exit the dialog. Click Cancel to exit without saving your changes.
Replace Mated Entities The Mated Entities PropertyManager helps you reattach dangling mate entities. You can list all of the mated entities in the assembly or in a particular component. Then you can replace any of the mated entities to satisfy the mates. For example, if you have a mate between two faces and you remove one of the faces from a model (by a cut or a fillet), the mate becomes dangling. You can use the Mated Entities PropertyManager to select a replacement face to satisfy the mate again.
9-8
To replace dangling mate entities:
1.
Right-click a mate, a component, or a mategroup and select Replace Mate Entities to replace the entities for a single mate, all the mates on a component, or all the mates in the assembly, respectively. - or Select a mate, a component, or a mategroup, then click Replace Mate Entities toolbar to replace the mate entities for the selected entity.
on the Assembly
The Mated Entities PropertyManager appears. Dangling mates appear with an X and satisfied mates appear with a checkmark in the Mate Entities list. 2.
Select an entity to replace in the Mate Entities list, then select a replacement entity. The replacement entity appears in Replacement Mate Entity
.
3.
Select Show all mates to show all satisfied and dangling mates. When cleared, only the dangling mates are shown.
4.
Click Flip Mate Alignment to toggle the alignment of the mate.
5.
Click Disable Preview to turn off the preview of the replacement mate.
6.
Click OK
to accept the new entities.
Assembly Statistics You can generate a report of the components and mates in an assembly. To generate a report of assembly statistics:
Click Statistics following items:
on the Tools menu, or click Tools, Assembly Statistics. The report includes the
•
total number of components
•
number of unique parts and sub-assemblies
•
number of suppressed, resolved and lightweight components
•
number of top-level mates
•
maximum depth of the assembly hierarchy (for nested sub-assemblies). When you are finished reading the report, click OK to close the dialog box.
Component Properties Lets you view or change the properties of a component. To view or change component properties:
1.
Right-click the component in the FeatureManager design tree and select Component Properties.
2.
Under General properties: o
o
o
Component Name. The part name is displayed, but usually is read-only. (If you want to change a component name, you must clear the Update component names when documents are replaced check box in the External References Options dialog box. Instance ID. The instance is 1 for the first time the component is used in the assembly; if it is used more than once, each occurrence is assigned a consecutive instance identification number. Full Name. The combination of the Component Name and Instance ID. You can copy the full name from this box, and paste it into table cells when creating a design table.
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o
o
Component Description. The description is read-only in this dialog box. You set it in the Summary Information dialog box of the component. Model Document Path. The path to the component document is displayed. You can click Browse to search for a replacement component. The last saved or in-use configuration of the replacement component is used.
3.
Select Configuration specific properties. The properties available depend on the type of assembly component you selected.
4.
Click OK when you finish making your changes.
Assembly Instance Color Lets you specify the color for selected component instances. •
Click Use Assembly to use the default color specified for the current assembly document, and override the color specified in the referenced part document. If different colors are specified for individual faces in the part document, these are overridden also.
•
Click Change Color to select a different color from the color palette, or to define a custom color for the selected instance.
•
Click Remove Color to return the selected component to the color specified in the referenced part document. This includes any colors specified for individual faces in the part document.
•
Click Advanced to set lighting display characteristics, such as transparency, shininess, and so on.
Arranging Components Assembly PropertyManager From this PropertyManager, you can do the following: •
Move a component.
•
Rotate a component.
•
Detect collisions with other components.
•
Activate Physical Dynamics
•
Dynamically detect the clearance between components. NOTE: The selections under Options appear in each of the topics listed above, as necessary for that topic.
Positioning Components in an Assembly Once a component is in an assembly, you can move it, rotate it, or fix its location. This is useful for rough placement of the components in the assembly. You can then position the components precisely using mating relationships. As you add mating relationships, you can move the components within the unconstrained degrees of freedom, visualizing the mechanism’s behavior. You can position a component in any of the following ways:
9-10
•
Fix the position of a component.
•
Move or rotate a component.
•
Add mates to a component.
•
Add SmartMates.
•
Use Physical Simulation.
Fixing the Position of a Component You can fix the position of a component so that it cannot move with respect to the assembly origin. By default, the first part in an assembly is fixed; however, you can float it at any time. It is recommended that at least one assembly component is either fixed, or mated to the assembly planes or origin. This gives a frame of reference for all other mates, and helps prevent unexpected movement of components when mates are added. •
A fixed component has a (f) before its name in the FeatureManager design tree.
•
A floating, under defined component has a (-) before its name in the FeatureManager design tree.
•
A fully defined component does not have a prefix.
To fix or float an assembly component:
1.
Right-click the component in the graphics area or the component’s name in the FeatureManager design tree.
2.
Select Fix or Float from the menu, depending on how you want the component to behave. NOTE: You cannot fix or float an instance in a component pattern.
Moving a Component To move components by dragging:
Drag a component in the graphics area. The component moves within its degrees of freedom. To prevent this behavior, click Tools, Options, System Options, Assemblies. Clear Move components by dragging, then click OK. To move components with a triad:
1.
Right-click a component and select Move with Triad.
2.
Drag the arm
3.
Drag the wing
4.
Drag the center sphere
5.
Right-click the center sphere and select from the following:
of the triad to move along the axis coincident with the arm. of the triad to move along the plane coincident with the wing. to a linear or planar entity to align the triad with the entity.
•
Show Translate XYZ Box. Moves the component to a specific XYZ coordinate.
•
Show Translate Delta XYZ Box. Moves the component by a specific amount.
•
Align to Component or Align to Assembly. Aligns the triad's axes to the component's or assembly's axes.
To move components with the PropertyManager:
1.
Click Move Component
on the Assembly toolbar, or click Tools, Component, Move.
The Move Component PropertyManager appears, and the pointer changes to 2.
Select one or more components in the graphics area.
3.
Select an item from the Move o o
.
list to move the components in one of following manners:
Free Drag - Select a component and drag in any direction. Along Assembly XYZ - Select a component and drag in the X, Y, or Z direction of the assembly. The coordinate system appears in the graphics area to help orient you. To select the axis you want to drag along, click near that axis before dragging.
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o
o
o
Along Entity - Select an entity, then select a component to drag along that entity. If the entity is a line, an edge, or an axis, the component you move has one degree of freedom. If the entity is a plane or a planar face, the component you move has two degrees of freedom. By Delta XYZ - Type an X, Y, or Z value in the PropertyManager, and click Apply. The component moves by the amount you specify. To XYZ Position - Select a point of a component, type an X, Y, or Z coordinate in the PropertyManager, and click Apply. The component’s point moves to the coordinate you specify. If you select something other than a vertex or point, the component’s origin is placed at the coordinate you specify.
You can select and move one component or group of components after another while the Move Component tool is active. 4.
Under Advanced Options, select This configuration to apply the movement of the components to only the active configuration.
5.
Click OK
or click Move Component
again when finished.
NOTES: •
You cannot move a component whose position is fixed or fully defined.
•
You can only move a component within the degrees of freedom allowed by its mating relationships.
Rotating a Component To rotate a component by dragging:
Right-click a component, hold down the right mouse button, and drag the component. The component rotates within its degrees of freedom. To prevent this behavior, click Tools, Options, System Options, Assemblies. Clear Move components by dragging, then click OK. To rotate a component with a triad:
1.
Right-click a component and select Move with Triad.
2.
Use the right-mouse button to drag the arm arm.
of the triad to rotate about the axis coincident with the
3.
Drag the center sphere
4.
Right-click the center sphere and select from the following:
to a linear or planar entity to align the triad with the entity.
•
Show Rotate Delta XYZ Box. Rotates the component by a specific amount about the specified arm of the triad.
•
Align to Component or Align to Assembly. Aligns the triad's axes to the component's or assembly's axes.
To rotate a component with the PropertyManager:
1.
Click Rotate Component
on the Assembly toolbar, or click Tools, Component, Rotate.
The Rotate Component PropertyManager appears, and the pointer changes to 2.
9-12
Select one or more components in the graphics area.
.
3.
Select an item from the Rotate
list to rotate the components in one of the following manners:
o
Free Drag - Select a component and drag in any direction.
o
About Entity - Select a line, an edge, or an axis, then drag a component around the selected entity.
o
By Delta XYZ - Type an X, Y, or Z value in the PropertyManager, and click Apply. The component moves around the assembly’s axes by the angular value you specify.
You can rotate one component or group of components after another; the tool remains active until you click it again, or select another tool. 4.
Under Advanced Options, select This configuration to apply the rotation of the components to only the active configuration.
5.
Click OK
or click Rotate Component
again when finished.
NOTES: •
You cannot rotate a component whose position is fixed or fully defined.
•
You can only rotate a component within the degrees of freedom allowed by its mating relationships.
Assembly Mates Mates create geometric relationships between assembly components. As you add mates, you define the allowable directions of linear or rotational motion of the components. You can move a component within its degrees of freedom, visualizing the assembly's behavior. Some examples include: •
A coincident mate forces two planar faces to become coplanar. The faces can move along one another, but cannot be pulled apart.
•
A concentric mate forces two cylindrical faces to become concentric. The faces can move along the common axis, but cannot be moved away from this axis.
Other topics about mates include: •
Mate PropertyManager
•
Standard Mates
•
Advanced mates including Cam Follower Mates, Gear Mates, Limit Mates, and Symmetry Mates.
•
SmartMates
Mate PropertyManager Mate Selections Select the faces, edges, planes, and so on that you want to mate together. See Standard Mates by Entity or see one of the mate types listed below. Standard Mates Angle, Coincident, Concentric, Distance, Parallel, Perpendicular, and Tangent mates are under Standard Mates. All the mate types are always shown in the PropertyManager, but only the mates that are applicable to the current selections are available. Toggle the Mate Alignment as necessary. Advanced Mates Cam, Gear, Limit, and Symmetric mates are under Advanced Mates. Toggle the Mate Alignment as necessary.
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Mates The Mates box contains all the mates added while the PropertyManager is open or all of the mates that you are editing. When there are multiple mates in the Mates box, you can select one to edit that mate. To edit more than one mate at a time, select multiple mates in the FeatureManager design tree, then right-click and select Edit Feature. All the mates appear in the Mates box. Options •
Add to new folder. When selected, new mates appear in a folder in the mategroup in the FeatureManager design tree. When cleared, new mates appear in the mategroup.
•
Show pop-up toolbar. When selected, the Mate pop-up toolbar appears when you add standard mates. When cleared, you add standard mates in hte PropertyManager.
•
Show preview. When selected, a preview of a mate occurs when you make enough selections for a valid mate.
•
Use for positioning only. When selected, components move to the position defined by the mate, but a mate is not added to the FeatureManager design tree. A mate appears in the Mates box so you can edit and position the components, but nothing appears in the FeatureManager design tree when you close the Mate PropertyManager. This check box is an alternative to adding many mates, then later deleting those mates in the FeatureManager design tree.
Standard Mates The valid mating relationships are: •
Coincident: positions selected faces, edges, and planes (in combination with each other or combined with a single vertex) so they share the same infinite line. Positions two vertices so they touch
•
Parallel: places the selected items so they lie in the same direction and remain a constant distance apart from each other
•
Perpendicular: places the selected items at a 90 degree angle to each other
•
Tangent: places the selected items in a tangent mate (at least one selection must be a cylindrical, conical, or spherical face)
•
Concentric: places the selections so that they share the same center point
•
Distance: places the selected items with the specified distance between them
•
Angle: places the selected items at the specified angle to each other
To add a standard mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
In the PropertyManager, under Mate Selections, select the entities that you want to mate together for Entities to Mate . The Mate pop-up toolbar appears with a default mate selected and the components move into place to preview the mate. The preceding occurs if you select Show pop-up toolbar and Show preview under Options in the PropertyManager.
9-14
3.
Click Add/Finish Mate
4.
Click OK
or select a different mate type.
to close the PropertyManager.
Standard Mates by Entity Mates create geometric relationships, such as coincident, perpendicular, tangent, and so on. Each mate is valid for specific combinations of geometry. Select one of the geometry types below to view its valid mates. Cam
•
Cam/Cylinder - Tangent
•
Cam/Plane - Tangent
•
Cam/Point - Coincident
Circular or Arc Edge
•
Circular or Arc Edge/Cone - Coincident, Concentric
•
Circular or Arc Edge/Line - Concentric
•
Circular or Arc Edge/Cylinder - Concentric, Coincident
•
Circular or Arc Edge/Plane - Coincident
•
Circular or Arc Edge/Circular or Arc Edge - Coincident
•
Cone/Circular or Arc Edge - Coincident, Concentric
•
Cone/Cone - Angle, Coincident, Concentric, Distance, Parallel, Perpendicular
•
Cone/Cylinder - Angle, Concentric, Parallel, Perpendicular
•
Cone/Extrusion - Angle, Parallel, Perpendicular
•
Cone/Line - Angle, Concentric, Parallel, Perpendicular
•
Cone/Plane - Tangent
•
Cone/Point - Coincident, Concentric
•
Cone/Sphere - Tangent
Cone
Cylinder
•
Cylinder/Cam - Tangent
•
Cylinder/Cone - Angle, Concentric, Parallel, Perpendicular
•
Cylinder/Cylinder - Angle, Concentric, Distance, Parallel, Perpendicular, Tangent
•
Cylinder/Extrusion - Angle, Parallel, Perpendicular, Tangent
•
Cylinder/Line - Angle, Coincident, Concentric, Distance, Parallel, Perpendicular, Tangent
•
Cylinder/Plane - Distance, Tangent
•
Cylinder/Point - Coincident, Concentric, Distance
•
Cylinder/Sphere - Concentric, Tangent
•
Cylinder/Circular Edge - Concentric, Coincident
•
Cylinder/Surface - Tangent
Extrusion
•
Extrusion/Cone - Angle, Parallel, Perpendicular
•
Extrusion/Cylinder - Angle, Parallel, Perpendicular, Tangent
•
Extrusion/Extrusion - Angle, Parallel, Perpendicular
•
Extrusion/Line - Angle, Parallel, Perpendicular
•
Extrusion/Plane - Tangent
•
Extrusion/Point - Coincident
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Line
•
Line/Cone - Angle, Concentric, Parallel, Perpendicular
•
Line/Cylinder - Angle, Coincident, Concentric, Distance, Parallel, Perpendicular, Tangent
•
Line/Extrusion - Angle, Parallel, Perpendicular
•
Line/Line - Angle, Coincident, Distance, Parallel, Perpendicular
•
Line/Plane - Coincident, Distance, Parallel, Perpendicular
•
Line/Point - Coincident, Distance
•
Line/Sphere - Concentric, Distance, Tangent
•
Line/Circular Edge - Concentric
•
Plane/Cam- Tangent
•
Plane/Cone - Tangent
•
Plane/Cylinder - Distance, Tangent
•
Plane/Extrusion - Tangent
•
Plane/Line - Coincident, Distance, Parallel, Perpendicular
•
Plane/Plane - Angle, Coincident, Distance, Parallel, Perpendicular
•
Plane/Point - Coincident, Distance
•
Plane/Sphere - Distance, Tangent
•
Plane/Circular Edge - Coincident
•
Plane/Surface - Tangent
•
Point/Cam - Coincident
•
Point/Cone - Coincident, Concentric
•
Point/Cylinder - Coincident, Concentric, Distance
•
Point/Extrusion - Coincident
•
Point/Line - Coincident, Distance
•
Point/Plane - Coincident, Distance
•
Point/Point - Coincident, Distance
•
Point/Sphere - Coincident, Concentric, Distance
•
Point/Surface - Coincident
•
Sphere/Cone - Tangent
•
Sphere/Cylinder - Concentric, Tangent
•
Sphere/Line - Concentric, Distance, Tangent
•
Sphere/Plane - Distance, Tangent
•
Sphere/Point - Coincident, Concentric, Distance
•
Sphere/Sphere - Concentric, Distance, Tangent
•
Surface/Cylinder - Tangent
•
Surface/Plane - Tangent
•
Surface/Point - Coincident
Plane
Point
Sphere
Surface
9-16
Mate Alignment You can set the alignment condition of standard and advanced mates in the Mate PropertyManager. The alignment conditions for a mate are: •
Aligned direction.
: places the components so the normal or axis vectors for the selected faces point in the same
•
Anti-Aligned : places the components so the normal or axis vectors for the selected faces point in opposite directions. These examples show the effect of changing the alignment condition for Coincident and Distance mates.
Aligned
Anti-aligned
Coincident
Distance
Mate Reference Mate references specify one or more entities of a component to use for automatic mating. When you drag a component with a mate reference into an assembly, the SolidWorks software tries to find other combinations of the same mate reference name and mate type. If the name is the same, but the type does not match, the software does not add the mate. Here are some items to note about mate references: •
Components. You can add mate references to part and assembly components. In assemblies, you can select assembly geometry (such as a plane in the assembly) or component geometry (such as the face of a component.)
•
Multiple mate references. A component can contain more than one mate reference. The MateReferences folder in the FeatureManager design tree holds all mate references. For example, you can have a component in an assembly with two mate references, bolt and washer. When you drag a fastener with a mate reference named bolt into the assembly, mates are added between the entities with the same mate reference name.
•
Multiple mated entities. Each mate reference can contain up to three mated entities: a primary, secondary, and tertiary reference entity. Each of these entities can have an assigned mate type and alignment. The primary reference entity on one component must mate to the primary reference entity on another component. For example, a shaft can have its cylindrical face assigned to a concentric mate and its planar end face assigned to a coincident mate. When you drag that component into an appropriate location in an assembly, the SolidWorks software adds both mates.
•
SmartMates. When the SmartMates PropertyManager is open, the software adds mates via mate references before it adds geometric SmartMates.
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To define a mate reference:
1.
In a part or an assembly, click Mate Reference Reference Geometry, Mate Reference.
on the Reference Geometry toolbar, or click Insert,
The Mate Reference PropertyManager appears. 2.
Under Reference Name, type a name for the mate reference.
3.
Under Primary Reference Entity: o
o
Select a face, edge, vertex, or plane for the Primary reference entity potential mates when dragging a component into an assembly. Select a Mate Reference Type mate for the reference entity.
. The entity is used for
and a Mate Reference Alignment
4.
If desired, repeat Step 3 to add secondary and tertiary entities.
5.
Click OK
to define the default
.
The mate reference is added to the FeatureManager design tree in the MateReferences
folder.
To capture a mate reference from an existing mate:
1.
Edit a component in the context of an assembly.
2.
Click Mate Reference
3.
In the PropertyManager, under References to Capture, select an entity or a mate.
.
The entity, mate, and alignment of the mate appear under Primary Reference Entity. 4.
Type a name under Reference Name and click OK
to add the mate reference to the component.
Mategroups When you create a new assembly, an empty mategroup is automatically included in the FeatureManager design tree. Each mating relationship that you create is added to this mategroup. The entry for each mating relationship includes the names of the components involved. All the mates within a mategroup are solved together; the order in which they appear within the mategroup does not matter. You can perform operations such as Replace Mate Entities on all the mates in a mategroup by selecting the mategroup in the FeatureManager design tree. You can add mates to a folder within a mategroup to sort the mates. Right-click the mates and select Add to New Folder or drag the mates into an existing folder. Additionally, you can select the Add to new folder check box under Options in the Mate PropertyManager.
9-18
Modifying a Mating Relationship To modify a mating relationship:
1.
Expand the mategroup in the FeatureManager design tree. Right-click one or more mates, and select Edit Feature. The mates appear under Mates in the PropertyManager and the related geometry is highlighted in the graphics area.
2.
In the PropertyManager, select the mate to edit under Mates and change the desired options. •
Mate Alignment (Aligned or Anti-aligned) on mates which imply a direction
•
Flip Dimension to reverse the direction in which a Distance or Angle mate is measured
•
Value of an Angle or Distance mate
•
Select a different mate type.
3.
To replace one entity with another, click the entity to replace in the Mate Selections then select the new entity.
4.
Click OK
box, press Delete,
to make the change.
NOTE: To change only the dimension value of a Distance or Angle mate, double-click the mate in the FeatureManager design tree, then double-click the dimension to edit. Enter the new value in the Modify box, then click Rebuild
.
Angle Mate You can add an angle mate between the combinations shown below: Cone - Cone - Cylinder - Extrusion - Line Cylinder - Cone - Cylinder - Extrusion - Line Extrusion - Cone - Cylinder - Extrusion - Line
Line - Cone - Cylinder - Extrusion - Line Plane - Plane
NOTE: •
A Cylinder refers to the cylinder's axis.
•
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
•
You must type an angle value in the Angle box in the Mate PropertyManager. The default value is the current angle between the selected entities.
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Coincident Mate You can add a coincident mate between the combinations shown below: Cone - Circular/Arc Edge - Cone - Point Cylinder - Line - Point - Circular/Arc Edge Extrusion - Point Line - Cylinder - Line - Plane - Point
Plane - Line - Plane - Point - Circular/Arc Edge Point - Cam - Cone - Cylinder - Extrusion - Line - Plane - Point - Sphere - Surface Sphere - Point
Circular/Arc Edge - Cone - Plane - Cylinder - Circular/Arc Edge Surface - Point
NOTE: •
Mates between two cones must use cones of the same half-angle.
•
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
Concentric Mate You can add a concentric mate between the combinations shown below: Cone - Circular/Arc Edge - Cone - Cylinder - Line - Point Cylinder - Cone - Cylinder - Line - Point - Sphere - Circular/Arc Edge
9-20
Line - Cone - Cylinder - Sphere - Circular/Arc Edge Point - Cone - Cylinder - Sphere Sphere - Cylinder - Line - Point - Sphere
Circular/Arc Edge - Cone - Line - Cylinder - Circular/Arc Edge
Distance Mate You can add a distance mate between the combinations shown below: Cone - Cone Cylinder - Cylinder - Line - Plane - Point Line - Cylinder - Line - Plane - Point - Sphere
Plane - Cylinder - Line - Plane - Point - Sphere Point - Cylinder - Line - Plane - Point - Sphere Sphere - Line - Plane - Point - Sphere
NOTES: •
A Line can also refer to an axis in this instance.
•
You must type a distance value in the Distance box in the Mate PropertyManager. The default value is the current distance between the selected entities.
•
Mates between two cones must use cones of the same half-angle.
Parallel and Perpendicular Mates You can add a parallel or perpendicular mate between the combinations shown below: Cone - Cone - Cylinder - Extrusion - Line Cylinder - Cone - Cylinder - Extrusion - Line Extrusion - Cone - Cylinder - Extrusion - Line
Line - Cone - Cylinder - Extrusion - Line - Plane Plane - Line - Plane
NOTE: •
A Cylinder refers to the cylinder's axis.
•
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
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Tangent Mate You can add a tangent mate between the combinations shown below: Surface - Plane - Cylinder
Line - Cylinder - Sphere Plane - Cam - Cone - Cylinder - Extrusion - Sphere - Surface Sphere - Cone - Cylinder - Line - Plane - Sphere
Cone - Plane - Sphere Cylinder - Cam - Cylinder - Extrusion - Line - Plane - Sphere - Surface Extrusion - Cylinder - Plane
NOTE: •
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
Cam-Follower Mates A cam-follower mate is a type of tangent or coincident mate. It allows you to mate a cylinder, plane, or point to a series of tangent extruded faces, such as you would find on a cam. You can make the profile of the cam from lines, arcs, and splines, as long as they are tangent and form a closed loop. The following picture shows three followers which stay in contact with the cam as it rotates.
To add a cam-follower mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
Under Advanced Mates, click Cam
3.
Under Mate Selections, select the tangent faces on the cam for Entities to Mate
. .
Right-click one of the faces and click Select Tangency. This selects all the tangent faces in one step.
9-22
4.
Click in Cam Follower and select a face or vertex on the cam follower.
5.
Click OK
.
6.
The follower is mated to all of the cam surfaces, allowing the follower to stay in contact with the cam as it rotates. A cam-follower mate for a cam made from a set of tangent surfaces appears in the FeatureManager design tree as CamMateCoincident or CamMateTangent. A cam-follower mate for a cam made from a single surface appears as Coincident or Tangent.
Gear Mates Gear mates force two components to rotate relative to one another about selected axes. Valid selections for the axis of rotation for gear mates include cylindrical and conical faces, axes, and linear edges. Other notes include: •
You can mate any two components that you want to rotate relative to one another. You do not have to mate two gears.
•
Similar to other mate types, gear mates do not prevent interference or collisions between components. To prevent interference, use Collision Detection or Interference Detection.
To add a gear mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
In the PropertyManager, under Advanced Mates: •
Click Gear
.
•
Type a value for Ratio to set the gear ratio.
•
Select Reverse to change the direction of rotation of the gears relative to one another.
3.
Under Mate Selections, select the rotation axes on the two gears for Entities to Mate
4.
Click OK
.
.
Limit Mates Limit mates allow components to move within a range of values for distance and angle mates. You specify a starting distance or angle as well as a maximum and minimum value.
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To add a limit mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
In the PropertyManager, under Advanced Mates: •
Click Distance
or Angle
.
•
Set Distance or Angle to define the starting distance or angle.
•
Select Flip Dimension to move the entities to opposite sides of the dimension.
•
Set Maximum Value extents of the limit mate.
and Minimum Value
to define the maximum and minimum
3.
Under Mate Selections, select the entities to mate together for Entities to Mate
4.
Click OK
.
.
A LimitDistance or LimitAngle mate is added to the assembly. Symmetry Mate A symmetry mate forces two similar entities to be symmetric about a plane or planar face of a component or a plane of the assembly. The following entities are allowed in symmetry mates: •
Points such as vertices or sketch points
•
Lines such as edges, axes, or sketch lines
•
Planes or planar faces
•
Spheres of equal radii
•
Cylinders of equal radii
Please note the following items about symmetry mates: • Symmetry mates do not mirror the entire component about the plane of symmetry. • Symmetry mates only relate the selected entities to one another. In the illustration, the two highlighted faces are symmetric about the highlighted plane. Notice the two components are upside down with respect to one another. That is because the highlighted faces only are symmetric, not all of the faces of both components. To add a symmetry mate:
9-24
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
Under Advanced Mates, click Symmetric
3.
Under Mate Selections, select the two entities to be symmetric for Entities to Mate
4.
Click in Symmetry Plane and select the plane of symmetry.
5.
Click OK
.
. .
SmartMates You can create some types of mating relationships automatically. Mates created with these methods are referred to as SmartMates. •
You can create mates when you insert a part in the assembly, by dragging the part in specific ways from an open part window. The entity that you use to drag determines the types of mates that are added. See Geometry-Based Mates, Feature-Based Mates, and Pattern-Based Mates.
•
You can specify a mate reference in the part document. A mate reference identifies the entity to use for mating when you insert the part from a file. See Defining a Mate Reference.
•
You can create mates by inferring potential mate partners when you move a part within the assembly. See Adding SmartMates While Moving Components.
Geometry-Based Mates You can create some types of SmartMates by dragging parts into assemblies using certain model geometry. You inference the geometry of existing components to create mates as you drop the new parts. To create mates automatically, based on model geometry:
1.
Drag a part from an open part window into the graphics area of the assembly window, but do not drop it immediately. Use one of the following entities to drag the part: a linear or circular edge, a temporary axis, a vertex, a planar face, or a cylindrical/conical face. When the pointer is over an entity of another component that is a potential mate partner, the pointer changes to indicate the mate or mates that will result if the part is dropped at this location. A preview of the part snaps into place.
2.
If the preview indicates that you need to change the alignment condition, press the Tab key to flip the alignment (aligned/anti-aligned).
3.
Drop the part. The mates are added automatically. The following types of automatic mates are supported: Mating entities
Type of mate
2 linear edges
Coincident
2 planar faces
Coincident
2 vertices
Coincident
2 conical faces, or 2 axes, or 1 conical face and 1 axis
Concentric
2 circular edges (the edges do not have to be complete circles)
Concentric (conical faces) coincident (adjacent planar faces)
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Pointer
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Feature-Based Mates You can add mates automatically between features that have a "peg-in-hole" relationship. The requirements are as follows: •
One of the features must be a base or boss, and the other must be a hole or a cut.
•
The features may be extruded or revolved.
•
The conical faces that are used in the mate must both be of the same type (either a cone or a cylinder, not one of each type).
•
There must be a planar face adjacent to the conical face of both features.
Click for an example of feature-based mates. To create SmartMates using features:
1.
In the FeatureManager design tree of a part document, select a feature with a cylindrical or conical face. Drag the feature name into an assembly graphics window. When the pointer is over another cylindrical or conical face, it changes to indicate the mates that will result if the part is dropped at this location.
A preview of the part snaps into place. If the preview indicates that you need to change the alignment condition, press the Tab key to flip the alignment (aligned/anti-aligned). 2.
Drop the part. Two mates are applied: a Concentric mate between the cylindrical or conical faces, and a Coincident mate between the planar faces that are adjacent to the conical faces.
Example of Feature-Based Mates If you mate the cylindrical base of a screw to the cylindrical face of a countersunk hole, the planar face at the end of the screw mates to the planar face at the bottom of the hole. If you mate the conical boss of the screw to the conical face of the hole, the planar face on the head of the screw mates to the planar face at the top of the hole. If you create the whole screw as a single revolved base, then mate it to either face of the hole, the top planar faces are mated. When the set of faces matches this way, the coincident mate is applied where the faces meet at the largest circular edge.
Pattern-Based Mates In some special cases, you can create as many as three SmartMates at once. Each part must have a circular pattern of cylindrical holes (or bosses) on a planar face with a circular edge.
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To add SmartMates based on a feature pattern:
1.
Drag the component into the assembly using the circular edge. When the pointer is over another circular edge, it changes to to indicate the mates that will result if the component is dropped at this location. A preview of the part snaps into place.
2.
Press the Tab key to rotate the part that you are dragging, to align it with the desired pattern instance.
3.
Drop the component.
The following mates are added: o
A Concentric mate is added between the cylindrical faces.
o
A Coincident mate is added between the adjacent planar faces.
o
If possible, an additional Concentric mate is added between the pattern instance on the part that you are dragging and one on the part that is already in the assembly.
Adding SmartMates While Moving Components You can add SmartMates when you move a component in an assembly, even if the component is used in other mates. As you drag the component into place, you can infer potential mate partners for creating geometry-based SmartMates. NOTE: If a component is already used in other mates, you can only move it within the degrees of freedom allowed by those mates. Also, you cannot add SmartMates to an instance in a component pattern. To create SmartMates while moving a part:
1.
Hold down Alt and drag a component over potential mate pointers. The component becomes transparent and the pointer changes when it is over a valid mate partner.
2.
Drop the component to apply the mate.
To create SmartMates with the Move Component PropertyManager:
1.
Click Move Component
on the Assembly toolbar.
2.
In the PropertyManager, under Move, click SmartMates
3.
Double-click a component then click a valid mate partner.
.
The Mate pop-up toolbar appears and you can add a SmartMate.
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Deleting a Mating Relationship You can delete mates. When you delete a mate, it is deleted in all configurations of the assembly. To delete a mating relationship:
1.
Click the mate in the FeatureManager design tree.
2.
Press the Delete key, click Edit, Delete, or right-click and select Delete.
3.
Click Yes to confirm the deletion.
Suppressing a Mating Relationship You can suppress mates to prevent them from being solved. This allows you to experiment with different types of mates without over defining the assembly. To suppress a mate in the active configuration:
1.
Right-click the mate in the FeatureManager design tree, and select Properties.
2.
Select Suppressed, and click OK. To unsuppress the mate, repeat the process, and clear the Suppressed check box. You can also select one or more mates and click Suppress (or Unsuppress toolbar, or click Edit, Suppress (or Unsuppress), This Configuration.
) on the Features
To suppress a mate for one or more configurations:
1.
Select one or more mates and click Edit, Suppress (or Unsuppress), Specified Configurations (or All Configurations). If you select Specified Configurations, a dialog box appears.
2.
Select the configurations you want to change from the list, and click OK.
Mate Diagnostics Mate Diagnostics is a tool that allows you to identify mating problems in an assembly. You can examine the details of mates that are not satisfied, and identify groups of mates which over define the assembly. Versions of the software after SolidWorks 2001 may find a mating error that went undetected in earlier versions of SolidWorks. These are primarily conflicts between mates and in-context features. Remember that when this error occurs, it is important to understand that the mate problem is not a new one. It existed in earlier versions of SolidWorks but was not detected by the software. Mate Diagnostics can help you identify these errors. An assembly with one or more mates that are not satisfied has a red flag
next to the mategroup. An assembly with
one or more over defined mates and mates that are all satisfied has a yellow flag
next to the mategroup.
To diagnose mating problems:
1.
Expand
the mategroup
.
Mates which are not satisfied are highlighted with a red flag
.
Mates which are satisfied, but over define the assembly, are highlighted with a yellow exclamation point . 2.
Click Tools, Mate Diagnostics, or right-click the assembly, mategroup, or any mate in the mategroup, and select Mate Diagnostics.
3.
In the PropertyManager, under Analyze problem, click Diagnose. One or more subsets of mates with problems appear. In the graphics area, components that are not related to the current subset become transparent. A message appears with information on the mating problem.
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4.
Under Not satisfied mates, click a mate. The entities in the unsolved mate are highlighted in the graphics area. A message tells you the distance or angle by which the mated entities are currently misaligned. Mates that appear under Analyze Problem and Not Satisfied Mates appear in bold.
5.
6.
Right-click a mate in the PropertyManager and select: •
Suppress.
•
Edit Mates. Opens the Mate PropertyManager so you can edit the mate.
•
Toggle alignment. Toggles the mate alignment between aligned and anti-aligned. (Available only for mates with alignment problems.)
Click OK
.
NOTE: Mate Diagnostics analyzes only one mategroup at a time. Sub-assembly mategroups are not included in the analysis of a top-level assembly mategroup. You can analyze the mategroup in any sub-assembly separately. Conflicting Mates At times a mate can not be satisfied because the components are already constrained in such a way that they can not move into the mate. The components can be fixed or mated to other components. Example The bottom faces of these two blocks are mated to the same plane:
If you add a coincident mate between the side of one block and the side of the other, the blocks can move into the mate:
If you add a coincident mate between the bottom of one block and the top of the other, you get an error. The first block cannot be simultaneously mated to the plane and to the top of the second block, because the bottom of the second block is also mated to the plane. How Mate Diagnostics helps In this example, when you click Diagnose in Mate Diagnostics, the program lists three conflicting mates. These mates are the two Coincident mates to the plane and the bottom face to top face Coincident mate. When you click on the problem mate, Mate Diagnostics tells you that the mated faces are not coincident, that instead they are 40mm (the height of the block) apart. How you can fix the problem Delete or edit one of the conflicting mates.
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Design Errors and Mating Sometimes the geometry in or between your components appears to be accurate, but is slightly wrong. For example, you can have the following situations: •
Two components that look parallel, but are positioned to be slightly diverging.
•
An imported block that appears to have orthogonal sides, but the angle between two faces is actually 90.1 degrees.
•
Two components that appear to be the same height, but are slightly different.
•
Bolt holes in two components that should be the same distance apart, however one component was made using rounded metric units, and one using rounded English units.
These design errors (and others) can sometimes lead to mating errors. Example Suppose your intention is to align these two blocks so that they are coincident on one side and one end as shown. Your visual inspection makes you believe the blocks are each orthogonal.
You first add a coincident mate between the sides:
Then add a coincident mate between the ends:
The blocks do not move into the mate and a mating error appears in the FeatureManager design tree. How Mate Diagnostics helps When you click on the problem mate in Mate Diagnostics, a message appears which tells you that the faces in the mate are not parallel, and lists the angle between the faces. How you can fix the problem Change the geometry of one of the blocks so that the faces are parallel. Because your intention was for both blocks to be orthogonal, examine the blocks for the cause of the non-orthogonal geometry. In this case, the sketch for the base extrusion of one of the blocks was not a rectangle. You do not have to delete the problem mate. After you correct the geometry in your parts, the mate will be satisfied.
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Errors in Solving Mates If changes in a component remove an entity (face, edge, and so on,) that is involved in a mate, the mate cannot be solved. The mate is not deleted, however. The mate is suppressed, and is displayed in the FeatureManager design tree with an error symbol. Suppressed mates are not considered when the remaining mates are solved. Sometimes adding many mates can cause the position of a component to be over defined. To correct the situation, suppress the mates on the component individually, then test the degrees of freedom by dragging the component. That way you can identify and delete the mate that is causing the conflict. In-Context Mating Conflicts An in-context mating conflict can occur when you delete an Inplace mate then add a mate between a part that was created in the context of an assembly and another component. Example
Red block is in-context, blue block is fixed
Delete Inplace mate, add Distance mate
Mate solves by moving red block
Red block updates, but sketch origin moves
The red block was created in the context of the assembly by converting and extruding a face of the blue block. If you delete the Inplace mate and add a distance mate between the parts, the following occurs: 1.
SolidWorks tries to solve the distance mate by moving the red block. As the red block moves, the origin of the sketch for the base extrude of the red block moves.
2.
SolidWorks then updates the sketch for the base extrude of the red block by converting the sketch entities from the face of the blue block. The blocks appear exactly as they did previously, except that the origin of the sketch for the red block has moved relative to the blocks. If you have a drawing of the red block, the geometry may appear to have "walked" off the edge of the drawing.
In versions earlier than SolidWorks 2001Plus, the distance mate was not marked as an error, although it is clearly not satisfied. Mate Diagnostics detects this type of error, lists the Distance mate as not satisfied, and displays a message about the geometry of the mated faces. Mates to Dangling Geometry One type of mate error occurs when you change the geometry of a component so that the mate can no longer be satisfied. Example
Concentric Mate
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Dangling Concentric Mate
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Chapter 9 Assemblies
In this example, there is a concentric mate between the two cylinders. Then, the sketch for the base feature of the bottom component changes from a circle to a rectangle. The cylindrical face of the bottom component no longer exists. The concentric mate to that face can no longer be solved. How Mate Diagnostics helps When you click Diagnose in Mate Diagnostics, a message appears telling you that a mate has dangling geometry. The mate and the missing geometry (in the example above, the cylindrical face of the bottom component) are listed. How you can fix the problem Delete the mate, or edit its definition to include different entities. Mating Conflicts with Sketch Relations If you have a sketch relation between a part sketch entity and assembly-level geometry, that sketch relation may come into conflict with a mate. Example
Add Colinear relation between line and assembly-level plane.
Relation is satisfied.
Add Distance mate between side of component and assembly-level plane.
Mating error. Part origin (at red arrow) moves.
In this example, the assembly-level plane cannot be both colinear with one side of the rectangular sketch, and at a distance from the side of the part created from that sketch. When you apply the distance mate, the part moves into the mate, and then the sketch updates to place the edge of the rectangle back at the assembly-level plane. If you have a drawing of the block, the geometry may appear to have "walked" off the edge of the drawing, since the part origin has moved. Mate Diagnostics detects this type of error, lists the Distance mate as not satisfied, and displays a message about the geometry of the mated faces.
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Physical Simulation Physical Simulation allows you to simulate the effects of motors, springs, and gravity on your assemblies. Physical Simulation combines simulation elements with SolidWorks tools such as mates and Physical Dynamics to move components around your assembly. To create a simulation:
1.
Add simulation elements. See Linear or Rotary Motors, Springs, and Gravity.
2.
Record the simulation. See Recording and Replaying a Simulation.
3.
Playback the simulation. See Recording and Replaying a Simulation.
NOTES: •
A simulation that you record is valid for as long as you do not make changes to the assembly. If you delete, suppress, move, replace, fix, float, or change a component that is included in a recorded simulation, the simulation is no longer valid.
•
Physical Simulation uses the Sensitivity setting of Physical Dynamics to check for collisions. To change this setting, click Move Component slider.
•
, select Physical Dynamics under Options, then move the Sensitivity
You can suppress and configure the suppression state of the Simulation folder in the FeatureManager design tree and its simulation elements. Suppressing the folder also suppresses its elements.
Linear or Rotary Motors Linear and rotary motors are simulation elements that move components around an assembly using Physical Simulation. Physical Simulation combines simulation elements with other tools such as mates and Physical Dynamics to move components in a realistic manner within the components degrees of freedom. See Recording and Replaying a Simulation for more information on creating a simulation. NOTES: •
Motors move components in a selected direction, but they are not forces. Motor strength does not vary based on component size or mass. For example, a small cube moves at the same speed as a large cube if the Velocity slider is set to an equal value.
•
If another force (for example, a collision with another component) causes a motor's Direction Reference to change orientation, the motor will move the component in the new direction.
•
It is recommended that you do not add more than one motor of the same type to the same component.
•
Motion due to motors supersedes motion due to gravity or springs. If you have a motor moving a component to the left and a spring pulling a component to the right, the component moves to the left.
To add a linear motor:
1.
Click Linear Motor
on the Simulation toolbar, or click Insert, Simulation, Linear Motor.
The Linear Motor PropertyManager appears. 2.
Select a linear or circular edge, a planar, cylindrical, or conical face, or an axis or a plane of a component as the Direction Reference. Click Reverse Direction , if necessary. If you select a circular edge or conical face, the Direction Reference is parallel to the axis of the cylinder. If you select a plane or a planar face, the Direction Reference is normal to the entity.
3.
Move the Velocity slider to to the right to increase the speed of the motor or to the left to decrease the speed. The Velocity is the speed at which a component moves if no other force acts on it.
4.
Click OK
.
A LinearMotor
SolidWorks 2004 Reference Guide
icon is added to the FeatureManager design tree under the Simulation
icon.
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Chapter 9 Assemblies
To add a rotary motor:
1.
Click Rotary Motor
on the Simulation toolbar, or click Insert, Simulation, Rotary Motor.
The Rotary Motor PropertyManager appears. 2.
Select a linear or circular edge, a planar, cylindrical, or conical face, or an axis or a plane of a component as the Direction Reference. Click Reverse Direction
, if necessary.
The Direction Reference is the direction of rotation, not the axis of rotation. The Direction Reference is parallel to the axis of rotation. The software moves the component about its center of mass taking into account mates and other relations to the component. If you select a linear edge, the Direction Reference revolves around the edge. If you select a planar face, the Direction Reference revolves around the normal of the face. 3.
Move the Velocity slider to to the right to increase the speed of the motor or to the left to decrease the speed. The Velocity is the speed at which a component moves if no other force acts on it.
4.
Click OK
.
A RotaryMotor
icon is added to the FeatureManager design tree under the Simulation
icon.
Linear Springs Linear springs are simulation elements that move components around an assembly using Physical Simulation. Physical Simulation combines simulation elements with other tools such as mates and Physical Dynamics to move components in a realistic manner within the components degrees of freedom. NOTES: •
Springs apply a force to a component. A spring with a higher spring constant will move a component faster than a spring with a lower spring constant. Also, a component with a smaller mass will move faster than a component with a larger mass if acted upon by an equal strength spring.
•
Motion due to a spring stops when the spring reaches its free length.
•
Motion due to motors supersedes motion due to springs. If you have a motor moving a component to the left and a spring pulling a component to the right, the component moves to the left.
See Recording and Replaying a Simulation for more information on creating a simulation. To add a spring:
1.
Click Linear Spring
on the Simulation toolbar, or click Insert, Simulation, Linear Spring.
The Linear Spring PropertyManager appears. 2.
Select two Spring Endpoints points.
to connect the spring. You can select linear edges, vertices, or sketch
If you select an edge, the Spring Endpoint attaches to the midpoint of the edge. 3.
Type a value for Free Length to determine if the spring is stretched or compressed.
4.
Type a value for Spring Constant to determine the strength of the spring.
5.
Click OK
.
A LinearSpring
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icon is added to the FeatureManager design tree under the Simulation
icon.
Gravity Gravity is a simulation element that moves components around an assembly using Physical Simulation. Physical Simulation combines simulation elements with other tools such as mates and Physical Dynamics to move components in a realistic manner within the components degrees of freedom. See Recording and Replaying a Simulation for more information on creating a simulation. NOTES: •
You can define one gravity simulation element per assembly.
•
All components move at the same speed under the effect of gravity regardless of their mass.
•
Motion due to motors supersedes motion due to gravity. If you have a motor moving a component to the left and gravity pulling a component to the right, the component moves to the left without any pull to the right.
To add gravity:
1.
Click Gravity
on the Simulation toolbar, or click Insert, Simulation, Gravity.
The Gravity PropertyManager appears. 2.
Select a linear edge, a planar face, a plane, or an axis as the Direction Reference. Click Reverse Direction , if necessary. If you select a plane or a planar face, the Direction Reference is normal to the selected entity.
3.
Move the Strength slider to to the right to increase the gravitational strength or to the left to decrease the strength.
4.
Click OK
.
A Gravity
icon is added to the FeatureManager design tree under the Simulation
icon.
Recording and Replaying a Simulation Physical Simulation allows you to simulate the effects of motors, springs, and gravity on your assemblies. When you record a simulation, the affected components move to a new location in the assembly. You can then replay the simulation to view it again. NOTES: •
You cannot interact with the assembly components when you are recording a simulation. You cannot use the Move Component
or Rotate Component
tools to move components during the simulation.
•
If there is an initial collision between two or more components, Physical Simulation ignores collisions between these components while recording a simulation. If the components no longer collide due to the motion of a simulation, Physical Simulation takes subsequent collisions between the components into account.
•
When you record a simulation, components with in-context references may move if you do not fully define the position of the components. Be cautious when using Physical Simulation in an assembly with in-context references.
•
When replaying a simulation, the components do not actually move to their original positions. Temporarily, the components appear in their original positions in the graphics area to show the start of the simulation. The replay of the simulation is for graphical purposes only.
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To record a simulation:
1.
Add simulation elements. See Linear or Rotary Motors, Springs, and Gravity.
2.
Click Calculate Simulation
on the Simulation toolbar.
The components move within their degrees of freedom according to the simulation elements. The degrees of freedom are determined by the mates on the component and collisions with other components. 3.
Click Stop Record or Playback on the Simulation toolbar to end the simulation. Sometimes the simulation stops automatically if the components can no longer move within their degrees of freedom. The components are in their new position.
4.
If desired, click Reset Components original position.
on the Simulation toolbar to return the components to their
To replay a simulation:
1.
Click Replay Simulation
to replay the simulation from the beginning to the end.
2.
Click a tool on the Animation Controller pop-up toolbar. For example, you can continuously replay the simulation or replay it at one-half speed.
Sub-assemblies Working with Sub-assemblies When an assembly is a component of another assembly, it is referred to as a sub-assembly. You can nest subassemblies in multiple levels, to reflect the hierarchy of your design. Creating a Sub-assembly There are several ways to create a sub-assembly: •
You can create an assembly document as a separate operation, then make it a sub-assembly by inserting it as a component in a higher-level assembly.
•
You can insert a new, empty sub-assembly at any level of the assembly hierarchy while you are editing a top-level assembly, then add components to it in a variety of ways.
•
You can form a sub-assembly by selecting a group of components that are already in the assembly. This creates a sub-assembly and adds components to it in a single step.
Modifying a Sub-assembly •
As you develop an assembly, you can modify its sub-assemblies in these ways:
•
You can dissolve a sub-assembly into individual components, thereby moving the components up one level in the assembly hierarchy.
•
You can edit the assembly structure by moving components up or down in the hierarchy, or to a different branch of the hierarchy. There are two ways to do this:
•
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•
Drag and drop the components to move them from one assembly to another.
•
Click Tools, Reorganize Components. This method can be easier to use when the FeatureManager design tree is very long, and therefore requires a lot of scrolling.
You can change the order of the components within a level of the hierarchy.
Forming a New Assembly from Existing Components You can form a sub-assembly from components that are already in the assembly, thereby moving the components down one level in the assembly hierarchy. It is a good idea to position and mate at least one of the components before you begin, then select that component first. To form a new assembly from existing components:
1.
In the FeatureManager design tree, select the components (individual parts or sub-assemblies) that you want to group into a sub-assembly. Hold the Ctrl key while you select. All the components must be at the same level within a single parent assembly.
2.
Right-click one of the selected components, and select Form New Sub-assembly Here. - or Select the components, then click Insert, Component, Assembly from [Selected] Components. The Save As dialog box appears.
3.
Browse to a different folder if needed, enter a File name, and click Save. A new assembly document is saved in the folder you specify. A new sub-assembly is inserted at the level where the selected components were located, and the components are moved into the new sub-assembly.
Sub-assembly from Selected Components In this example, P1 and P2 are selected to form a new sub-assembly, S1.
Instead of referencing the individual component documents P1 and P2, assembly A now references the sub-assembly document S1. Any mates that exist between components P1 and P2 move from the mategroup of assembly A to the mategroup of sub-assembly S1.
Dragging Components to Edit the Assembly Structure To reorganize components in sub-assemblies by dragging components:
Drag the component icon in the FeatureManager design tree, and drop it on the icon for the destination assembly (either the top-level assembly, or a sub-assembly at any level of the hierarchy). If the destination assembly is expanded, you can also drop the icon in the component section of the destination assembly. As you drag, watch for the
pointer.
To move multiple components at once, hold Ctrl as you select the icons. All the components selected for a move operation must be from the same level of a single assembly. If any components or features will be deleted as a result of the move, the Assembly Structure Editing dialog box appears, with a list of the affected items. TIP: If you are removing the last component of a sub-assembly, the empty sub-assembly is left in the FeatureManager design tree. If you want to move the last component up a level and remove the empty sub-assembly at the same time, dissolve the sub-assembly instead.
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Assembly Structure Editing To modify the assembly structure:
1.
Click Tools, Reorganize Components.
2.
Select the components that you want to move, either in the FeatureManager design tree or in the graphics area. The selected components are listed in the Components to move box. All the components selected for a single operation must be at the same level in one parent assembly.
3.
Click the Destination assembly box, then click the appropriate assembly icon in the FeatureManager design tree. If any components or features will be deleted as a result of the move, the dialog box expands to display a list of the affected items. See Effects of Assembly Structure Editing.
4.
Click Move. The component icons appear at the end of the component section of the destination assembly.
Effects of Assembly Structure Editing When you dissolve a sub-assembly, or reorganize the components at any level, the mates and any features that reference the selected components are affected. Therefore, decisions about hierarchical groupings should be made early in development of a complex assembly, in order to minimize the effects on these items. •
Mates move to the mategroup of the lowest common parent. For example, assume that there is a mate between P1 and P2, in the mategroup of the nested sub-assembly S3. • If you move P1 up one level (into S1), the mate moves to the mategroup of S1, the lowest common parent on the same branch. • If you move P1 into S2 (a different branch), the mate moves to the mategroup of the top-level assembly A, because A is the only common parent. • If you dissolve S3, the mate moves to the mategroup of sub-assembly S1.
•
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Component patterns have these specific limitations: •
If you move the seed component of a pattern into a different assembly, the pattern feature and all the instances generated by the pattern are deleted.
•
If you dissolve a sub-assembly that has a component pattern, the pattern feature and pattern instances are deleted. The seed component becomes a component of the assembly at the next higher level.
•
You cannot move individual instances generated by the pattern.
•
Assembly feature cuts and holes are deleted.
•
Equations may not solve. This is because, in many cases, the instance number suffix of the components changes when you reorganize or dissolve an assembly. This is done automatically, to prevent conflicts with existing components in the destination assembly.
•
Explode steps that explode the reorganized component are deleted.
•
Piping sub-assemblies are subject to some special rules. See SolidWorks Piping Help for more information.
Changing the Order of Components You can change the order of the components within a level of the assembly hierarchy. By default, assembly components appear in the FeatureManager design tree in the order in which they are added. The same order is used in a bill of materials in a drawing of the assembly. By changing the order in the assembly, you can control the order in the bill of materials. To change the order of components:
Drag and drop the icons in the FeatureManager design tree to rearrange the order. The component is placed below the icon where you drop it (the highlighted icon). Watch for the
pointer.
To place a component directly below a sub-assembly, press Alt to change from a reorganize operation (with the pointer) to a reorder operation.
Inserting a New Sub-assembly You can insert a new, empty sub-assembly at any level of the assembly hierarchy. Then you can add components to it in a number of ways. To insert a new sub-assembly:
1.
In the FeatureManager design tree, right-click either the top-level assembly icon or the icon for an existing sub-assembly, and select Insert New Sub-assembly. - or Click New Assembly
on the Assembly toolbar, or click Insert, Component, New Assembly.
The Save As dialog box appears. 2.
Browse to a different folder if needed, enter a File name for the new assembly document, and click Save. An empty sub-assembly is inserted as the last component of the selected assembly, and a new assembly document (.sldasm) is created and saved in the folder you specify.
3.
Add components to the sub-assembly: •
To move a component that is already in the assembly into the sub-assembly, see Dragging Components to Edit the Assembly Structure or Assembly Structure Editing.
•
To add an existing, saved component to the sub-assembly, right-click the sub-assembly icon in the FeatureManager design tree, and select Edit Sub-assembly. Then insert components using any of the methods in Adding Components to an Assembly.
•
To insert a new component into a sub-assembly, you must edit the sub-assembly in its own window. You cannot insert a new component into a sub-assembly while you are editing the top-level assembly. Also, you cannot insert a new component while you are editing the sub-assembly in the context of a higher level assembly. Right-click the sub-assembly icon in the FeatureManager design tree, and select Open <subassembly.sldasm> to open the sub-assembly in its own window. Then add a new component.
Dissolving a Sub-assembly You can dissolve a sub-assembly into individual components, thereby moving the components up one level in the assembly hierarchy. To dissolve a sub-assembly:
In the FeatureManager design tree, right-click the sub-assembly you want to dissolve, and select Dissolve Subassembly. You can also select the sub-assembly icon and click Edit, Dissolve Assembly. The components become components of the immediate parent assembly, and the sub-assembly is removed. The assembly document itself is not deleted from the folder where it is stored.
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Example of Dissolving a Sub-assembly In this example, when you dissolve sub-assembly S1, components P1 and P2 become components of the top-level assembly A.
Instead of referencing the sub-assembly document S1, assembly A now references the individual component documents P1 and P2. Any mates that exist between components P1 and P2 move to the mategroup of assembly A.
Changing the Editing Focus Manually For some types of editing operations, you need to specify that the changes you are making belong to the subassembly, and not to the top-level assembly. This includes any case where the edits could be successfully applied to either one. For example, you can add an assembly feature hole either to a sub-assembly, or to the top-level assembly, with different results. You must activate the sub-assembly to perform these editing operations: •
Add a component into the sub-assembly. You cannot add a new component in the context of a sub-assembly.
•
Delete a component from a sub-assembly.
•
Add a component pattern, an assembly feature cut or hole, a sketch, or reference geometry to the subassembly.
•
Use dynamic assembly motion on sub-assembly components. You can fix, float, and move sub-assembly components when the sub-assembly is active, to visualize the movement within the sub-assembly.
•
Add a mate between components of the active sub-assembly (both at the same level in the hierarchy, or one at a lower level, in a nested sub-assembly of the active sub-assembly).
NOTE: While a sub-assembly is active, the mates in the top-level assembly that position the sub-assembly with respect to the top-level are temporarily ignored. Top-level mates are solved again when you return to editing the toplevel assembly and click Rebuild
.
You cannot add a mate between a component within an active sub-assembly and a component outside the active subassembly. To activate a sub-assembly for editing in context:
Right-click the sub-assembly icon in the FeatureManager design tree, and select Edit Sub-assembly. When you activate a sub-assembly, it turns pink, and the rest of the assembly turns gray, just as it does when you edit a part. When you edit a component of a sub-assembly, only the individual part being edited turns pink.
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Automatic Change of Editing Focus For some types of editing operations, the software recognizes that the changes you are making belong to the subassembly, and not to the top-level assembly. In those cases, the editing focus automatically changes from the top-level assembly to the sub-assembly. If you edit any of the following items that belong to a sub-assembly, the editing focus changes automatically: •
sketch
•
component pattern
•
mate
•
assembly feature (cut or hole)
•
reference geometry.
Similarly, if you edit a feature (the definition or the sketch) of a sub-assembly component, the software automatically changes to Editing Part mode. References that you make while editing a sub-assembly component are always made in the context of the top-level assembly, not the sub-assembly that contains it. If you add a mate between a sub-assembly component and some geometry outside that sub-assembly, the focus changes to the sub-assembly automatically. The mate is added to the lowest level assembly that contains both components (the lowest common parent).
Limitations in Sub-assembly Editing Most of the operations available for editing a sub-assembly on its own are available when editing a sub-assembly in context. However, there are a few operations that cannot be performed while editing a sub-assembly in context: •
creating a new component in context
•
inserting or modifying a weld bead
For these operations, you must open and edit the sub-assembly in its own window.
Flexible Sub-Assemblies You can make sub-assemblies flexible. This allows movement of the individual components of a sub-assembly within the parent assembly. An example of the benefit of this function is when you want to move the components of a piston sub-assembly in a motor assembly. You can move the individual components of the piston while still grouping the components as a subassembly. Please note the following regarding flexible sub-assemblies: •
Mates. The mates in a flexible sub-assembly are solved simultaneously with the mates of the parent assembly. Therefore, moving or rotating a sub-assembly component does not violate the mates in the subassembly or its parent. A component moves only within its degrees of freedom according to its mates.
•
Configurations. Each flexible sub-assembly must have its own unique configuration. This is because the position of a component in one flexible sub-assembly could be in a different position in another configuration of the flexible sub-assembly.
To make a sub-assembly flexible:
1.
Right-click a sub-assembly in the FeatureManager design tree and select Component Properties. The Component Properties dialog box appears.
2.
Under Solve as, click Flexible, then click OK.
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Working with Parts Within an Assembly Working with Parts within an Assembly In top-down assembly design, you build and modify parts within the context of an assembly. Parts created or modified in the context of an assembly contain external references and time-dependent features. Some of the techniques for working with parts in an assembly include: •
Create and edit components within the context of the assembly. That way, you can use the geometry of one component to help define another. When you create references between components, the models are fully associative. Changes you make to a referenced component cause the others to update accordingly.
•
Start with a layout sketch that defines fixed component locations, planes, and so on, then design the parts referencing these definitions.
•
Create assembly features that are added only after the components are assembled. These assembly features exist only in the context of the assembly.
•
Place patterns of components, either by referencing a pattern feature on one of the components, or by creating a pattern in the assembly.
•
Merge the bodies of assembly components by using a join operation.
External References An external reference is created when one document is dependent on another document for its solution. If the referenced document changes, the dependent document changes also. In an assembly, you can create an in-context feature on one component that references the geometry of another component. This in-context feature has an external reference to the other component. If you change the geometry on the referenced component, the associated in-context feature changes accordingly. An in-context feature updates automatically if the update path is available. The update path is contained in the assembly where you create the reference. Update paths for in-context features are displayed in the FeatureManager design tree. If the update path is not available (for example, if the assembly document is closed), updating occurs the next time you open the assembly that contains the update path. See Understanding the Update Path for more information. FeatureManager design tree conventions In the FeatureManager design tree, any item with an external reference has a suffix that indicates the status of the reference: •
The suffix -> means that the reference is in-context. It is solved and up-to-date.
•
The suffix ->? means that the reference is out-of-context. The feature is not solved or not up-to-date. To solve and update the feature, open the assembly that contains the update path.
•
The suffix ->* means that the reference is locked.
•
The suffix ->x means that the reference is broken.
See Locking and Breaking External References for more information. To list the external references on a part or feature:
Right-click the part or the feature with the external reference, and select List External Refs. The referenced components, features, and entities are listed, as well as the status of each reference. See Rules for External References for more information. TIP: To reduce the size of the FeatureManager design tree, you can hide all of these in-context icons. Rightclick the top-level assembly icon
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and select Hide Update Holders.
Understanding the Update Path Consider the example of an assembly that contains two components: a mold base and a design component. In the context of the assembly, you create a cavity feature in the mold base, with an external reference to the design component. The update path for the cavity feature is therefore contained in the assembly. Now, suppose that you need to change the design component and you need to update the mold base accordingly. •
If the assembly is open, the cavity feature in the mold base updates automatically when you make the changes to the design component.
•
If the assembly is closed, the cavity feature cannot be updated to reflect the changes until you open the assembly, thereby making the update path available.
Locking and Breaking External References You can lock, unlock, or break the external references of a component. When you lock the external references on a component, the existing references no longer update and you cannot add any new references to that component. Once you unlock the external references, you can add new references or edit the existing references. When you break the external references, the existing external references no longer update and you can add new references to the component. To lock, unlock, or break the external references:
1.
Right-click the feature or the component with the external references in the FeatureManager design tree and select List External Refs. The External References For dialog box appears.
2.
Click Lock All to lock all of the external references for this component. The suffix for the component changes from -> to ->*.
3.
Click Unlock All to unlock the references for this component. The suffix for the component changes back to ->.
4.
Click Break All to permanently break the external references for this component. The suffix for the component changes to ->x. To list the broken references in the External References For dialog box, select the List Broken References check box.
5.
Click OK to close the dialog box.
Rules for External References •
A component cannot have an external reference to itself (a circular reference).
•
You cannot reference one instance of a part to create a feature on another instance of the same part, even if the instances are in different configurations.
•
You cannot replace a part with another part created by deriving the second part from the first. See Derive Component Part for more information.
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List External References You can list the external references of any component or feature created in the context of an assembly. You can also list the references for various types of derived parts. To list the external references for a feature, an assembly component, or a derived part:
Right-click the feature, component, or part in the FeatureManager design tree and select List External Refs. This operation is only available for items that have external references. The External References For dialog box appears. o
The Part or Assembly box displays the path and name of the assembly in which the component or feature was created.
o
Configuration. Select the configuration of the referenced component to use for a derived part.
o
The Feature column lists each in-context item (sketches, features, and so on) in the selected part.
o
o o
o
The Data column describes the type of data used to create the item (converted edge or face, converted or offset sketch entity, body, and so on). The Status of each reference. This can be In context or Out of context, Locked, or Broken. The Referenced Entity describes the actual item being used, and the name of the document that contains the item. The Feature’s Component column displays the name of the component in which the affected feature exists. This information is displayed only when the Referenced entity is in a different component in an assembly; this column does not apply to derived parts.
To lock, unlock, or break external references, see Locking and Breaking External References.
Searching for Referenced Documents When opening a referenced document, SolidWorks performs a search to locate the document. For example, this search may occur when you open a drawing and the referenced assembly cannot be found or when you resolve a lightweight component in an assembly. When a referenced document is found, the software updates the path to the referenced document in the parent document. When you save the parent document, the updated path is saved as well. The Rules column below describes the search routine that the software uses to locate a missing referenced document. The Examples column shows the paths that the software checks using the following scenario:
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•
The assembly was last saved as C:\zz\a1.sldasm. You move the assembly to D:\ss\tt\a1.sldasm.
•
The first part in the assembly was last saved as C:\qq\p1.sldprt. You do not move this part.
•
The second part in the assembly was last saved as C:\zz\yy\xx\p2.sldprt. This part is missing either through deletion, renaming, or some other file management mistake.
•
There are two paths in the Folders list of the File Locations Options dialog box: D:\aa\bb\ and E:\cc\dd\
•
You click File, Open to open a1.sldasm in its new location.
Rules
Examples
1.
Uses any open document with the same name.
If p2.sldprt is in another open document, SolidWorks uses this version of p2.sldprt.
2.
Searches the first path that you specify in the Folders list in the File Locations Options dialog box.
D:\aa\bb\p2.sldprt
NOTE: You must select the Search file locations for external references check box in the External References Options dialog box or else SolidWorks ignores the paths that you specify. 3.
Searches the path in Step 2 plus the last folder in the path where the referenced document was last saved.
D:\aa\bb\xx\p2.sldprt
4.
Searches the path in Step 2 plus the last two folders in the path where the referenced document was last saved.
D:\aa\bb\yy\xx\p2.sldprt
5.
Repeats Step 4 until the full original path has been appended to the the path in Step 2.
D:\aa\bb\zz\yy\xx\p2.sldprt
NOTE: This concept of adding one folder at a time from the full path will be called "recursive searching" in the following steps. 6.
Recursively searches the first path in the Folders list, then recursively searches the path where the referenced document was last saved.
D:\aa\xx\p2.sldprt D:\aa\yy\xx\p2.sldprt D:\aa\zz\yy\xx\p2.sldprt D:\xx\p2.sldprt D:\yy\xx\p2.sldprt D:\zz\yy\xx\p2.sldprt
7.
Repeats Steps 2 through 6 for the other folders in the Folders list.
E:\cc\dd\p2.sldprt E:\cc\dd\xx\p2.sldprt E:\cc\dd\yy\xx\p2.sldprt E:\cc\dd\zz\yy\xx\p2.sldprt E:\cc\xx\p2.sldprt E:\cc\yy\xx\p2.sldprt E:\cc\zz\yy\xx\p2.sldprt E:\xx\p2.sldprt E:\yy\xx\p2.sldprt E:\zz\yy\xx\p2.sldprt
8.
Searches the path of the active document, then recursively searches the path where the referenced document was last saved.
D:\ss\tt\p2.sldprt D:\ss\tt\xx\p2.sldprt D:\ss\tt\yy\xx\p2.sldprt D:\ss\tt\zz\yy\xx\p2.sldprt D:\ss\xx\p2.sldprt D:\ss\yy\xx\p2.sldprt D:\ss\zz\yy\xx\p2.sldprt D:\xx\p2.sldprt D:\yy\xx\p2.sldprt D:\zz\yy\xx\p2.sldprt
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9.
Searches the path where you last opened a document, then recursively searches the path where the referenced document was last saved.
same as Step 8
NOTE: In most cases, the path of the active document and the path where you last opened a document are the same. The two paths are different if you click File, Open to open one document, then drag and drop an assembly from Windows Explorer into that document. The path of the active document is the path from Windows Explorer and the path where you last opened a document is the path from File, Open. 10. Searches the path where the software last found a referenced document.
C:\qq\p2.sldprt This is the location of p1.sldprt.
11. Searches the full path where the document was last saved without a drive designation.
This is useful if you save a part with a UNC path such as \\machine\folder\p2.sldprt.
12. Searches the full path where the document was last saved with its original drive designation.
C:\zz\yy\xx\p2.sldprt
13. Allows you to browse for the document yourself.
n/a
Search Results In an assembly document, lists the part and sub-assembly documents that are components of the active assembly. This is useful if you have several versions of the component files. In a part document, lists externally referenced documents, if they exist. To list the referenced files then copy the listed files to a new directory:
1.
Click File, Find References.
2.
In the dialog box, click Print to print the contents of the dialog box.
3.
Click Copy list to copy the contents of the dialog box to the Windows clipboard so you can paste the list into a text editor.
4.
To copy the files: a.
Click Copy files. NOTE: This option is not available for parts with in-context references. To copy files in this case, open the assembly that is listed, and click File, Find References.
5.
b.
To retain the directory structure of the file copies, click Yes when prompted to preserve directory structure. To copy all files to a single folder, click No.
c.
Browse to the desired folder in the Browse For Folder dialog box and click OK.
Click Close to close the dialog box.
Saving Assemblies with In-context Features There are some special considerations when you save an assembly with in-context features:
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•
Parts that have features defined in the context of an assembly must maintain the association with the parent assembly in order to update correctly, both inside and outside of the assembly context.
•
If you need two versions of the same part (one that includes the in-context features, and one that does not include them), you must edit the referenced file locations when you save the assembly. This prevents the incontext features from affecting the original part document.
Editing Parts in the Assembly Context While editing an assembly, you can: •
Create a new part in the assembly window
•
Edit an existing component in the assembly window
•
Open an existing component document in its own window
Creating a Part in an Assembly You can create a new part in the context of an assembly. That way you can use the geometry of other assembly components while designing the part. The new part has its own part file so you can modify it independently from the assembly. You can also create a new sub-assembly in the context of the top-level assembly. See Creating a Sub-assembly for more information. To create a part within an assembly:
1.
Click New Part on the Assembly toolbar, or click Insert, Component, New Part. The default part template on the Default Templates Options page is used.
2.
In the Save As dialog box, enter a name for the new part and click Save. The new part is saved in its own document so you can edit it separately. The component pointer
3.
appears.
If the assembly is empty, select a plane from the FeatureManager design tree. Otherwise, select a plane or planar face on which to position the new part. The name of the new part appears in the FeatureManager design tree, and a sketch is automatically opened in the new part. An Inplace (coincident) mate is added between the Front plane of the new part and the selected plane or face. The new part is fully positioned by the Inplace mate. No additional mates are required to position it. If you wish to reposition the component, you need to delete the Inplace mate first.
4.
Construct the part features, using the same techniques you use to build a part on its own. Reference the geometry of other components in the assembly as needed. NOTE: If you extrude a feature using the Up To Next option, the next geometry must be on the same part. You cannot use the Up To Next option to extrude to a surface on another component in the assembly or a surface of an assembly feature.
5.
Click File, Save, then select the part name in the Resolve Ambiguity dialog box, or select the assembly name to save the entire assembly and its components.
6.
To return to editing the assembly, right-click the assembly name in the FeatureManager design tree, or rightclick anywhere in the graphics area, and select Edit Assembly:assembly_name, or click Edit Part
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Editing a Part in an Assembly Editing a part while in an assembly allows you to modify a component without leaving the assembly. You can also reference surrounding geometry while creating new features. The sketches that you create while editing a part in the assembly can use any edge or can be dimensioned to any edge of any part. Features may use end conditions such as Up to Surface to another component. You can change the transparency of assembly components while editing a part. To edit a part while in an assembly:
1.
Right-click the part and select Edit Part, or click Edit Part
on the Assembly toolbar.
The title bar shows the name of the part in the assembly that is open for editing as part_name in assembly_name.sldasm. Note that the message in the status bar indicates that you are now editing the part document even though the entire assembly is visible. NOTE: When you edit a part in the context of an assembly, the referenced configuration in the assembly becomes the active configuration in all open windows (for example, if the part is open in its own window). If the part is used in another open assembly document, with the Use component’s in-use or last saved configuration option selected, those instances are also affected. For more information, see Component Configurations in an Assembly. 2.
Make the necessary changes to the part.
3.
To return to editing the assembly, right-click the assembly name in the FeatureManager design tree, or rightclick anywhere in the graphics area, and select Edit Assembly:assembly_name, or click Edit Part
.
Transparency During Part Editing There are several options for displaying component transparency while editing parts. These settings affect only the components that are not being edited. The illustrations below show the results of applying different settings during editing of the sphere in this assembly. The sphere is completely enclosed by blocks, some of which have transparency applied as a component property.
To set the scope of transparency to use during part editing:
1.
Click Tools, Options, System Options, Display/Selection.
2.
Under Assembly transparency for in-context edit, select Force assembly transparency, and move the slider to the desired transparency level.
3.
Click OK.
To set the transparency of the components you are not editing:
1.
Select a component and click Edit Part
on the Assembly toolbar.
The component you are editing turns opaque pink. The appearance of the other components depends on the assembly transparency settings you choose. 2.
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Click Change Assembly Transparency •
Opaque
•
Maintain Transparency
•
Force Transparency
on the Assembly toolbar, and select from the following:
. Components are opaque. . Components retain their individual transparency settings. . Components use the transparency level you set.
Opaque
Maintain Transparency
Force Transparency
TIP: Additionally, you can right-click any blank area and set Assembly Transparency on the shortcut menu to Opaque, Maintain Transparency, or Force Transparency. 3.
Edit the part as needed.
4.
Click Edit Part
to return to editing the assembly, and to turn off transparency.
Time-Dependent Features Time-dependent features are the basis of top-down design. They include: •
Assembly features (assembly feature cuts or holes, and weld beads)
•
Components that are created in the context of the assembly
•
In-context features, reference geometry, and sketches that reference other components
•
Component patterns
When a time-dependent feature references components that have already been positioned by mates, the features become dependent on both the components and the mates that position the components. To view these dependencies, right-click the feature and select Parent/Child. Mates are solved together as a system within a mategroup. Each assembly has a single default mategroup. The order in which mates are added to the mategroup does not matter; all the mates are solved at the same time.
Tips for Mating with Time-Dependent Features It is good design practice to only reference time-dependent features for mating when that is the only way you can achieve the design intent of the assembly. You can edit the positions of the components with more flexibility when time-dependent features are not involved because the order of evaluation does not matter. When positioning a component to geometry that depends on a time-dependent feature, it is good design practice to mate components to the time-dependent feature first, then add additional mates as needed.
Adding a Component Pattern You can create a pattern of components in the assembly in one of the following ways: •
You can create a local linear or circular pattern of components.
•
You can place a pattern of components in an assembly based on a feature pattern of an existing component. This is called a derived component pattern.
•
You can place a pattern of components in an assembly based on a feature pattern of assembly features.
To toggle the visibility or suppression state of all of the components in the pattern, right-click the pattern feature in the FeatureManager design tree, and select Hide components, Show components, Suppress, or Unsuppress. You can dissolve a component pattern to make its components independent. One benefit is that you can individually move and rotate components that were in the pattern. One drawback is that you cannot hide and suppress all the components in the pattern because the pattern feature is gone.
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Linear Component Pattern You can create a linear pattern of components in an assembly in one or two directions. To create a linear pattern of components:
1.
Click Insert, Component Pattern, Linear Pattern.
2.
In the PropertyManager, under Direction 1:
3.
•
Select a linear edge or a linear dimension for Pattern Direction.
•
Click Reverse Direction
if necessary.
•
Type a value for Spacing
. This is the value between the centers of the instances.
•
Type a value for Number of Instances seed components.
. This is the total number of instances including the
Repeat for Direction 2 for a bidirectional pattern. Select Pattern seed only to pattern the seed component only in the second direction. When cleared, SolidWorks patterns all of the instances generated by Direction 1 and the seed component in the second direction.
4.
Click in Components to Pattern
5.
To skip instances, click in Instances to Skip area. The pointer changes to
, then select the seed components. and select the preview of the instance in the graphics
when it is over a preview in the graphics area.
6.
To restore instances, select the instance in Instances to Skip and press Delete.
7.
Click OK
.
The new components appear under LocalLPattern in the FeatureManager design tree. By default, all instances use the same configuration as the seed components. To change the configuration, edit the component properties of an instance. Circular Component Pattern You can create a circular pattern of components in an assembly. To create a circular pattern of components:
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1.
Click Insert, Component Pattern, Circular Pattern.
2.
In the PropertyManager, under Parameters: •
Select an axis or a linear edge for Pattern Axis. The pattern revolves around this axis.
•
Click Reverse Direction
•
Type a value for Angle
•
Type a value for Number of Instances seed components.
•
Select Equal Spacing to set the Angle to 360°. You can change the value to a different angle. The instances equally space themselves along the total angle.
if necessary. . This is the angular value between the centers of the instances. . This is the total number of instances including the
3.
Click in Components to Pattern
4.
To skip instances, click in Instances to Skip area. The pointer changes to
, then select the seed components. and select the preview of the instance in the graphics
when it is over a preview in the graphics area.
5.
To restore instances, select the instance in Instances to Skip and press Delete.
6.
Click OK
.
The new components appear under LocalCirPattern in the FeatureManager design tree. By default, all instances use the same configuration as the seed components. To change the configuration, edit the component properties of an instance. Feature Driven Pattern You can create a pattern of components based on an existing pattern. To use an existing pattern to create a pattern of components:
1.
Click Insert, Component Pattern, Feature Driven.
2.
Select the seed components for Components to Pattern
3.
Click in Driving Feature and select the pattern feature in the FeatureManager design tree or a face of a pattern instance in the graphics area.
4.
Click OK
.
.
The new components appear under DerivedLPattern or DerivedCirPattern in the FeatureManager design tree. By default, all instances use the same configuration as the seed components. To change the configuration, edit the component properties of an instance. To skip instances:
1.
Right-click the pattern feature in the FeatureManager design tree and select Edit Feature.
2.
Click in Instances to Skip The pointer changes to
and select the preview of the instance in the graphics area. when it is over a preview in the graphics area.
You cannot skip instances when creating a derived component pattern; you must edit the feature.
Mirror Components - Overview You can create new components by mirroring existing part or sub-assembly components. The new components can either be a copy or a mirror of the original components. A mirrored component is sometimes called a "right-hand" version of the original "left-hand" version. Some important items to note include: •
If the original components change, so do the copied or mirrored components.
•
Mates between the original components can be preserved in the copied or mirrored components.
•
Configurations in the original components appear in the copied or mirrored components.
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The difference between a component that you copy and one that you mirror is described as follows: Copy
Mirror
No new documents are created.
A new document is created.
The geometry of the copied component is identical to the original component; only the orientation of the component is different.
The geometry of the new component is mirrored; thus it is different from the original component.
Here is an example of a sub-assembly that includes a mirrored and copied component. The support has been mirrored so the opening for the jaw is on the correct side. The jaw has been copied since the geometry did not need to change. The mates that hold the jaw to the support have been preserved.
Mirror Components Step 1: Selections You must select a plane of symmetry and the components to mirror or copy. To mirror or copy one or more components:
1.
Click Insert, Mirrored Components.
2.
In the PropertyManager, under Selections, select a plane or planar face for Mirror plane as the entity to mirror about.
3.
Select one or more components that you want to mirror or copy for Components to Mirror. You can select from the graphics area or from the FeatureManager design tree. If you select a sub-assembly in the FeatureManager design tree, all of its components are selected as well.
4.
Set the state (mirror or copy) for each component: •
Toggle between
and
where:
indicates that the component is copied. The geometry of a copied component is unchanged from the original, only the orientation of the component is different. indicates that the component is mirrored. The geometry of the mirrored component changes to create a truly mirrored component. •
•
Right-click the component name to select: o
Mirror All Children - Mirrors the sub-assembly and all of its children.
o
Mirror All Instances - Mirrors all instances of the selected component.
o
Copy All Instances - Copies all instances of the selected components.
Click
next to a sub-assembly to show its children. You can select
or
for each child.
5.
To preserve any mates between the selected components when you mirror more than one component, select Recreate mates to new components.
6.
Click Next
.
If you chose to mirror components, you go to Step 2: Filenames to choose names for your new parts. If you did not mirror components, you go to Step 3: Orientation.
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Mirror Components Step 2: Filenames Select a name and a location for each of the components you are mirroring. You can create a new part or subassembly from the component or use an existing part or sub-assembly. For example, if you previously made a mirror of your component in an earlier operation, you can use that part. To specify the name and location for a new part or subassembly:
1.
Select a component under Filenames. A proposed name for the mirrored part appears below.
2.
To change the part name, type a new name for the part over the proposed name or click existing part.
3.
Repeat steps 1 and 2 for the other components in the list.
4.
To place the new parts in a common folder:
5.
a.
Select Place files in one folder.
b.
Click Choose to browse to a new folder.
to browse to an
To change the name defaults: a.
Select prefix or suffix for Add.
b.
Type the prefix or suffix in the box below. The new part names automatically appear with the chosen prefix or suffix attached.
6.
Click Next
to go to Step 3: Orientation.
Mirror Components Step 3: Orientation Select an orientation for the components you are copying. To change the orientation of the components:
1.
Select a component from the list and click Reorient Component to toggle through the possible alignments until the desired preview appears. Repeat for all of your components.
2.
Click Apply to All to set all of the components to the same orientation.
3.
Click Reset Orientations to set all of the components back to the default orientation.
4.
To see a preview of the components, select the Preview mirrored components or Preview instanced components check boxes.
5.
Click OK
.
Reorder and Roll Back in Assemblies Reorder Changing the order of assembly items in the FeatureManager design tree is dictated by parent/child relationships, just as it is with features in parts. •
You can reorder sketches, features, and reference geometry that belong to the assembly.
•
You can reorder components within their own level of the assembly hierarchy. See Changing the order of components.
•
You can reorder mates within the mategroup.
•
You cannot reorder mategroups, component patterns, in-context features, or any default assembly items (default planes, Annotations or Lighting folders, and so on).
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Roll Back You can roll back reference geometry, sketches, component patterns, assembly features and in-context features. In general, rolling back assembly items behaves the same as rolling back features in parts. The following behaviors are specific to assemblies: •
If you roll back an assembly pattern, the components generated by that pattern are rolled back.
•
You cannot roll back into the section of the FeatureManager design tree that lists the components (that is, after some of the components are added, or before others). This is because components are not timedependent. Hide or suppress the components instead.
Assembly Layout Sketch You can design an assembly from the top-down using layout sketches. You can construct one or more sketches showing where each assembly component belongs. Then, you can create and modify the design before you create any parts. In addition, you can use the layout sketch to make changes in the assembly at any time. The major advantage of designing an assembly using a layout sketch is that if you change the layout sketch, the assembly and its parts are automatically updated. You can make changes quickly, and in just one place. To use an assembly layout sketch, do the following:
•
Create a sketch in the assembly in which various sketch entities represent parts in the assembly. Indicate a tentative location for each component, capturing the overall design intent.
•
Reference the geometry in the layout sketch when you create each component. Use the layout sketch to define the component size, shape, and location within the assembly; make sure that each part references the layout sketch.
Example of Using an Assembly Layout Sketch The following example is typical of an automobile engine accessory drive belt system. The system has several pulleys and idlers, connected by a serpentine belt. 1.
Create an assembly sketch. Use circles to represent the outer rims of the pulleys. Use tangent lines between the circles to represent the serpentine belt. Dimension the size and location of each pulley.
2.
For each pulley, insert a new part, sketch a circle, add a Coradial relation with the corresponding circle in the layout sketch, then extrude the sketch. Add other features to the pulley parts as needed.
3.
Using the layout sketch as a guide, create the belt around the pulleys as another new part.
You can change the location or the size of the pulleys by editing the layout sketch. The assembly now consists of a belt and a set of pulleys whose locations and sizes are driven by the layout sketch. The advantage of this type of design is clear when you have to make changes to the design.
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For example, working in the layout sketch, you can: •
Rearrange the pulleys so that a slipping pulley has more of its surface covered by the belt.
•
Make a driven pulley larger so less torque is required to turn it.
•
Drag the pulleys and belt to dynamically experiment with different locations.
•
Set an angle dimension to specify how much of each pulley must be covered by the belt.
•
When you exit the layout sketch, the assembly and the parts are updated.
If you designed this assembly without a layout sketch, you would need to change many dimensions, or move components in the assembly, then rebuild each time. The layout sketch does not have to be the master plan for a design. If you had a model of an engine with some fixed pulley locations, you could make the circles in the layout sketch coincident with the known locations of the pulleys in the model. You would still have the freedom to drag the other pulleys to different locations, and the assembly would update automatically when you made changes.
Assembly Features While in an assembly, you can create cut or hole features that exist in the assembly only. You determine which parts you want the feature to affect by setting the scope. You can create a pattern of assembly features in the same manner as you create a pattern of features in a part. This is useful for creating cuts or holes that are added after the components are actually assembled, and that affect more than one component. When you want to add a cut or hole to a single component in an assembly, it is better to edit the part in context than to use an assembly feature. While it is not a requirement, it is good practice to fully define the positions of the components of the assembly, or fix their locations before you add assembly features. This helps prevent unexpected results if the components are moved later.
Creating an Assembly Feature Assembly feature cuts and holes affect the assembly only; the individual part files are not affected. You can set the scope before you create an assembly feature, or you can edit the scope afterwards. To create an assembly feature cut :
1.
Open a sketch on a face or plane, and sketch a profile of the cut. The profile can contain more than one closed contour.
2.
Click Insert, Assembly Feature, Cut, Extrude or Revolve.
3.
Set the options as needed in the Cut-Extrude or Cut-Revolve PropertyManager.
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To create an assembly feature hole:
1.
Click the planar face approximately where you want to create the hole.
2.
Click Insert, Assembly Feature, Hole, Simple or Wizard.
3.
Set the options as needed in the Hole PropertyManager or Hole Definition dialog box.
To create an assembly feature pattern:
1.
Create an assembly cut or hole.
2.
Click Insert, Assembly Feature, and select one of the following: Linear Pattern, Circular Pattern, Table Driven Pattern, Sketch Driven Pattern.
To edit an assembly feature:
Right-click the assembly feature in the FeatureManager design tree, and select either Edit Sketch, Edit Definition, or Feature Scope.
Feature Scope When creating an feature in an assembly or a multibody part, you must determine which components or bodies you want to be affected by the feature. By setting the scope, you can selectively choose the components or bodies you want the feature to impact. To set the scope for an assembly feature:
1.
Select an assembly feature to set the scope for that feature. If you do not select a feature, you specify the feature scope for the next assembly feature that you create.
2.
In an assembly, select Edit, Feature Scope.
3.
Select the components that this assembly feature will affect by clicking the components or the component names in the FeatureManager design tree. The selected component names appear in the Edit Assembly Feature Scope dialog box.
4.
Click OK.
To set the scope for a feature in a multibody part:
1.
Create the feature as usual. Features that allow you to set the scope include Cut-Extrude and Cut-Revolve features.
2.
In the PropertyManager, under Feature Scope, select All bodies or Selected bodies.
3.
If you chose Selected bodies, click Auto-select to allow the software to determine which bodies to affect. Clear Auto-select to select bodies for Solid Bodies to Affect.
Joining Parts You can join two or more parts to create a new part. The join operation removes surfaces that intrude into each other's space, and merges the part bodies into a single solid volume. Creating a Joined Part To join parts:
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1.
Create the parts that you want to join, then create an assembly containing the parts.
2.
Position the parts as desired in the assembly. The parts may either touch each other or intrude into one another.
3.
Save the assembly but do not close the window.
4.
Insert a new part into the assembly: o o
o
5.
Click Insert, Component, New Part. Enter a name for the new part and click Save. Click a plane or planar face on a component on which to position the new part.
Click Insert, Features, Join. The Join PropertyManager appears.
6.
In either the FeatureManager design tree or the graphics area, click the components you want to join. The names appear under Parts to Join.
7.
Select the Hide Parts check box to hide the original components after the join is complete.
8.
Select the Force Surface Contact check box if you want to join any coincident faces (as well as intruding volumes). The software finds the affected faces, then extends the face with the smallest area into the other component, and fills in any resultant gaps.
9.
Click OK
to create the joined part.
Before join - coincident faces 10.
After Join - faces are removed
To exit from Editing Part mode, right-click in the graphics area, and select Edit Assembly:assembly_name.
Editing a Joined Part To edit the definition of the joined part to add or remove components:
1.
In the FeatureManager design tree of an assembly, right-click the Join feature of the joined part and select Edit Feature. - or In the graphics area of an assembly, right-click the joined component and select Edit Feature.
2.
Click the parts that you want to remove from the joined component, or click additional parts to be joined to the existing component. To remove all the parts, right-click in the graphics area, and select Clear Selections. The components that make up the joined component are listed under Parts to Join.
3.
Click OK
. The joined component updates to reflect the changes.
NOTE: The joined part is fully associative to the original parts and to the assembly. Any changes made to the original parts are reflected in the joined part. If the parts move relative to each other in the assembly, the joined part changes also.
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Identifying the Parts in a Joined Part To identify which parts are used to create a joined part, either:
•
Right-click the joined component and select List External Refs. The referenced components appear in the Referenced Entity column.
•
Expand the joined component in the FeatureManager design tree, then expand the Join feature to see the absorbed references.
Weld Beads You can add a variety of weld types to an assembly. The weld bead becomes a new assembly component created in the context of the assembly. See Working with Parts within an Assembly. You can do the following: •
View the available weld types
•
Create and edit weld beads
•
Select faces for weld beads more easily
•
Automatically create weld symbols
Weld Types The following weld types are supported for the ISO and ANSI dimensioning standards: ISO
ANSI
Butt
Square
Square Butt
Scarf
Single V Butt
V Groove
Single Bevel Butt
Bevel
Single V Butt with Root
U Groove
Single Bevel Butt with Root
J Groove
Single U Butt
Flare-V
Single J Butt
Flare-Bevel
Backing Run
Fillet
Fillet
Seam
Seam
Flange-Edge Flange-Corner
Creating and Editing Weld Beads To add a weld bead between components:
1.
Insert the components in an assembly, and add mates to position them as needed for the specific weld type you plan to use.
2.
Click Insert, Assembly Feature, Weld Bead.
3.
In the Weld Bead Type dialog box, select a weld Type from the list, then click Next.
4.
In the Weld Bead Surface dialog box:
5.
•
Select a Surface Shape from the list (Flat, Convex, or Concave).
•
Specify the Top Surface Delta, the Bottom Surface Delta and Radius as required for the Type and Surface Shape selected. See Surface Delta and Radius.
Click Next. The Weld Bead Mate Surfaces dialog box appears. Be sure to read the information in the dialog box about selecting faces for the weld type you have chosen.
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6.
Select the necessary faces. For all welds, you must select Contact Faces. Depending on the type of weld you are adding, you may also need to select Stop Faces and Top Faces. Click each box, then select the faces in the graphics area. See Weld Face Selection Tips for more information. Contact Faces are the faces that are joined by the weld bead. Select a face (or a set of adjacent faces) on each component. Stop Faces are the faces that define the beginning and the end of the weld bead. On each component, select two faces (or two sets of adjacent faces) that share an edge with the contact faces. Top Faces are the faces from which to measure the Top Surface Delta. On each component, select one face that shares an edge with a contact face.
7.
Click Next.
8.
In the Weld Bead Part dialog box, either accept the default name for the Weld Bead Part, or enter a new part name, and click Finish.
To edit a weld:
1.
In the FeatureManager design tree, expand the Bead component.
2.
Right-click the Weld Bead feature and select Edit Feature.
3.
In each of the dialog boxes, change the parameters as needed. Click Next to continue, then click Finish when you reach the last dialog box.
Surface Delta and Radius When you add a weld bead with a Surface Shape of Convex or Concave, you must specify the Top Surface Delta. For a backing run weld, you also specify the Bottom Surface Delta. If the Surface Shape is Flat, there is no surface delta. For a convex weld, the top surface delta is the distance between the highest point on the bead and the contact faces.
For a concave weld, the distance is measured below the top surface rather than above.
For a fillet weld, you also specify the Radius. The radius is measured as the radius of an imaginary ball rolling along the seam. The edges of the weld bead are at the points of tangency, where the ball meets the contact faces. In the illustrated fillet weld, the specified Radius is 10mm, and the Top Surface Delta is 2mm.
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Weld Face Selection Tips When components have complex shapes, or when the mates place the components very close to each other, selecting the faces for a weld can be difficult. There are several ways you can make it easier: •
Change the view to Wireframe
or Hidden Lines Visible
.
•
Rotate the model using Rotate View
•
Set the Selection Filter to Filter Faces
•
Temporarily add some space between the components. You can do this by editing the values of Angle and Distance mates or suppressing one or more mates, then moving the components apart slightly.
. You can change the orientation then select the faces. .
After you complete the weld bead, edit or unsuppress the mates as needed to restore the components to the correct positions. Then click Rebuild
to update the weld bead.
Automatic Weld Symbols When you create a weld, a weld symbol is automatically attached to the weld bead component in the assembly.
To add more detailed specifications to the default weld symbol:
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1.
In the assembly document or in a drawing document, right-click the symbol and select Properties, or double-click the symbol.
2.
Specify the dimensions, symbols, and other options that you want to include, and click OK.
Simplifying Assemblies Simplifying Large Assemblies Large assemblies can consist of hundreds of components. You can simplify a complex assembly by toggling the visibility of the components, and by changing the suppression state of components. Large Assembly Mode is a collection of system options that improves the performance of assemblies. You can turn on Large Assembly Mode at any time, or you can set a limit for the number of components, and have Large Assembly Mode turn on automatically when that limit is reached. You can customize Large Assembly Mode, and you can combine it with other simplification methods (such as toggling the visibility and changing the suppression state). There are several reasons to simplify an assembly: •
To improve system performance, and to reduce rebuild times, especially with very large assemblies.
•
To create simplified views of the assembly that include certain components, and exclude others.
•
To create design variations of the assembly, with different combinations of components, and different configurations of the components themselves.
Large Assembly Mode Large Assembly Mode is a collection of system options that improves the performance of assemblies. You can turn on Large Assembly Mode at any time, or you can set a limit for the number of components, and have Large Assembly Mode turn on automatically when that limit is reached. Two notes about saving an assembly with Large Assembly Mode active: •
If you save an assembly with Large Assembly Mode active, SolidWorks ignores the Automatically activate Large Assembly Mode option (Tools, Options, System Options, Large Assembly Mode) the next time you open the assembly. The assembly opens with Large Assembly Mode active.
•
If you save an assembly that contains sub-assemblies with Large Assembly Mode active, SolidWorks does not save the sub-assemblies in Large Assembly Mode. To save a sub-assembly in Large Assembly Mode, you must open the sub-assembly in its own window, activate Large Assembly Mode, and save.
SolidWorks is pre-set with recommended Large Assembly Mode options, but you can customize the options as needed. To turn on Large Assembly Mode:
Click Large Assembly Mode
on the Assembly toolbar, or click Tools, Large Assembly Mode.
The options are enabled.
Lightweight Components You can load an assembly with its active components fully resolved or lightweight. Both parts and sub-assemblies can be lightweight. •
When a component is fully resolved, all its model data is loaded in memory.
•
When a component is lightweight, only a subset of its model data is loaded in memory. The remaining model data is loaded on an as-needed basis.
You can improve performance of large assemblies significantly by using lightweight components. Loading an assembly with lightweight components is faster than loading the same assembly with fully resolved components. Lightweight components are efficient because the full model data for the components is loaded only as it is needed. Only components that you select, and components that are affected by changes that you make in the current editing session, become fully resolved. Assemblies with lightweight components rebuild faster because less data is evaluated. Mates on a lightweight component are solved, and you can edit existing mates.
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To enable lightweight loading of components:
1.
Click Tools, Options, System Options, Performance.
2.
Under Assemblies, select Automatically load components lightweight.
To open an assembly with lightweight components:
1.
Click File, Open. The Open dialog box appears.
2.
Select Lightweight, browse to the assembly file, and click Open. When this check box is selected, all components are loaded lightweight when you open an assembly. Components in the feature scope of an assembly feature can be loaded lightweight. When you point at a lightweight part in the graphics area, a feather pointer surrounded by a bounding box.
is displayed, and the body is
NOTE: Lightweight parts are only used when the model is in Shaded mode. If the model was last saved in Hidden Lines Removed, Hidden In Gray, or Wireframe mode, lightweight parts are not used. To set one or more resolved components to lightweight:
1.
For a single component, right-click the component and select Set to Lightweight.
2.
For an entire assembly, right-click the top level assembly icon and select Set Resolved to Lightweight. This option is available for a sub-assembly and its components when you right-click the sub-assembly.
Toggling the Visibility You can toggle the display of assembly components. You can remove the component completely from view or make it 75% transparent. Turning off the display of a component temporarily removes it from view, allowing you to work with underlying components. Hiding or showing a component affects only the visibility of the component. Hidden components have the same accessibility and behaviors as shown components in the same suppression state (see suppression states of components). Toggling the visibility does not affect the rebuild or evaluation speed. Display performance improves, however. To toggle the visibility of a component (part or sub-assembly):
1.
In the FeatureManager design tree or in the graphics area, right-click the component, and select Properties. To change several components at once, hold the Ctrl key as you select the components, then right-click and select Properties.
2.
In the dialog box, under Visibility, select Hide Model.
3.
Click OK. To show the components again, select the components in the FeatureManager design tree, then edit the Component Properties.
To toggle the transparency of a component:
Select the component, then click Change Transparency
on the Assembly toolbar.
Other ways to toggle the visibility:
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•
Right-click the component, and select Hide Component or Show Component. This method changes only the visibility of the active configuration.
•
Select the component, then click Hide/Show Components changes only the visibility of the active configuration.
•
Select the component, then click Edit, Hide (or Show, or Show with Dependents), This Configuration (or All Configurations, or Specified Configurations).
on the Assembly toolbar. This method
Component Suppression States Depending on the scope of the work you plan to do at any given time, you can specify an appropriate suppression state for the components. This can reduce the amount of data that is loaded and evaluated as you work. The assembly displays and rebuilds faster, and you make more efficient use of your system resources. There are three suppression states for assembly components: •
Resolved
•
Suppressed
•
Lightweight
To change the suppression state of components:
1.
In the FeatureManager design tree or the graphics area, right-click the desired component, and select Properties. To change several components at once, hold the Ctrl key as you select the components, then right-click and select Properties.
2.
In the dialog box, under Suppression State, select the desired state.
3.
Click OK.
Other ways to change the suppression state:
•
Click a component, then click Change Suppression State on the Assembly toolbar. This method changes only the suppression state of the active configuration. -orClick Edit, Suppress (or Unsuppress), This Configuration (All Configurations, Specified Configurations). If you select Specified Configurations, a dialog box appears. Select the configurations you want to change from the list, and click OK.
•
To fully resolve (unsuppress) a suppressed component, right-click the suppressed component, and select Set to Resolved. This resolves all configurations of the component.
•
To fully resolve all lightweight parts, right-click the assembly icon at the top of the FeatureManager design tree, and select Set Lightweight to Resolved.
NOTE: You cannot set specific configurations of components to lightweight. Resolved Resolved (or unsuppressed) is the normal state for assembly components. A resolved component is fully loaded in memory, fully functional, and fully accessible. All its model data is available, so its entities can be selected, referenced, edited, used in mates, and so on. Suppressed You can use the suppressed state to remove a component temporarily from the assembly, without deleting it. It is not loaded in memory, and it is no longer a functional member of the assembly. You cannot see a suppressed component, or select any of its entities. A suppressed component is removed from memory, so loading speed, rebuild speed, and display performance are improved. Because of the reduced complexity, evaluation of remaining components occurs faster. However, mates that involve the suppressed components are suppressed also. As a result, the positions of components in the assembly can become under defined. In-context features that reference suppressed components may also be affected. When you restore a suppressed component to the fully resolved state, conflicts can occur. Therefore, use the suppressed state carefully when modeling.
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Loading Additional Model Data When an operation requires model data that is not loaded for a lightweight component, the software fully resolves the part for you, to gain access to the additional data. This happens automatically when you do any of the following things: •
Click a part in the graphics area. When you click, the part becomes fully resolved, and the entity (face, edge, etc.) where you clicked is selected and highlighted.
•
Right-click a part or feature, and select Edit Part, Edit Sketch or Edit Feature. The part becomes fully resolved, and you are in Editing Part mode.
•
You can choose to automatically resolve any lightweight components that are out-of-date. Click Tools, Options, then Performance on the System Options tab. Select Always resolve from the Check out-ofdate lightweight parts list. If you select Indicate from the list then components that are out-of-date have a feather with red stripes next to them in the FeatureManager design tree.
Certain global operations require that many parts be fully resolved at once: •
Mass Properties
•
Interference Detection
•
Exploded View
•
Advanced Show/Hide, Advanced Selection
•
Section view of the assembly model
•
editing equations that involve lightweight parts
•
Physical Dynamics and Physical Simulation
•
exporting to other file types (IGES, SAT, and so on) You do not have to resolve parts before exporting to TIFF or JPEG.
To specify what you want to happen when you request one of these operations, click Tools, Options, then Performance on the System Options tab. Choose one of these options under Resolve lightweight components: •
Always. All lightweight parts are fully resolved for you, and they are included in the operation.
•
Prompt (default). A dialog box appears, asking if you want the software to resolve the lightweight parts for you. Click Yes to fully resolve the parts and continue, or click Cancel. If you also click Always resolve (before you click Yes or Cancel), the option is set to Always.
NOTE: When a lightweight part becomes fully resolved, all instances of the part, in any configuration, in any open assembly documents, become fully resolved.
Comparison of Components Suppression States
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Resolved
Lightweight
Suppressed
Hidden
Loaded in memory
Yes
Partially
No
Yes
Visible
Yes
Yes
No
No
Features available in FeatureManager design tree
Yes
Yes 3
No
No
Faces and edges accessible for adding mates
Yes
Yes 3
No
No
Mates solved
Yes
Yes
No
Yes
In-context features solved
Yes 1
Yes
No
Yes
Assembly features solved
Yes
Yes
No
Yes
Considered in global operations
Yes
On demand 2
No
Yes
May be edited in-context
Yes
Yes 3
No
No
Load and rebuild speed
Normal
Faster
Faster
Normal
Display speed
Normal
Normal
Faster
Faster
1 In-context features on resolved parts that reference lightweight parts update automatically. 2 Global operations include Mass Properties, Interference Detection, Exploded View, Advanced Selection and Advanced Show/Hide, solving equations, displaying section views, and exporting to other file formats. When lightweight components are present, the software prompts you to either resolve them, or cancel the operation. 3 Lightweight components are resolved automatically when selected for this operation.
Assembly Envelopes An assembly envelope is a special type of assembly component. It is a reference component, and it is ignored in global assembly operations (Bill of Materials, Mass Properties, and so on). This functionality allows you to select components based on their positions with respect to the envelope volume (inside, outside, or crossing). You can use an envelope by itself to quickly change the visibility of assembly components. You can also use an envelope (either alone or in combination with file properties), to select components for other editing operations, such as suppress, copy, or delete. The envelope component must be a solid volume (not shelled). This is because selection with envelopes is based on interference between the volumes of the functional assembly components and the envelope component. It is not based on the containment of components within the bounding box of the envelope component. Envelope components are displayed in a light blue transparent color when you use Shaded view mode. An Envelope feature is added to the ConfigurationManager for each envelope component that you create. Also, envelope components are identified in the FeatureManager design tree.
Apply Envelope Lets you specify selection criteria to hide or show assembly components, based on their positions relative to an envelope component. To apply criteria to an envelope:
1.
In the ConfigurationManager, right-click the Envelope component, and select Show/hide using envelope. The Apply Envelope dialog box appears.
2.
Choose one or more Criteria for selecting the components: •
Inside envelope. Components that are completely inside the envelope are selected. This includes components that are inside the envelope, but have a face that is coincident with the outside of the envelope.
•
Outside envelope. Components that are completely outside the envelope are selected. This includes components that are outside the envelope, but have a face that is coincident with the outside of the envelope.
•
Crossing envelope. Components that cross the boundary of the envelope are selected.
3.
Choose Show part components or Hide part components.
4.
Specify what to do with any component that does not meet the selection criteria:
5.
•
With Show part components, you can either Hide it (regardless of current display state), or Leave its show/hide state as is.
•
With Hide part components, you can either Show it (regardless of current display state), or Leave its show/hide state as is.
Click OK. The display is updated to hide or show components according to your selections.
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Creating Assembly Envelopes You can create an assembly envelope using an existing part file or in the context of the assembly. To create an assembly envelope from a file:
1.
Click Insert, Envelope, From File.
2.
In the Open dialog box, select the part file to use as an envelope, then click Open.
3.
Click in the assembly window where you want to place the envelope component. You can mate the envelope component to the other components in the assembly to position it precisely.
To create an assembly envelope in the assembly context:
1.
Click Insert, Envelope, New.
2.
In the Save As dialog box, enter a name for the new envelope component, then click Save. A part document with this name is created.
3.
Click a face or plane in the assembly window where you want to begin sketching the envelope component. The Front plane of the new envelope component is mated to the selected face or plane with an Inplace mating relation.
4.
Create the base feature and any additional features of the envelope component. You can reference the geometry of the assembly components as you create the envelope component. If any of the referenced entities changes, the envelope updates accordingly.
5.
When you are done defining the new envelope component, right-click anywhere in the graphics area, and select Edit Assembly:assembly_name.
Removing Assembly Envelopes To remove an assembly envelope:
1.
Select the envelope component in either the FeatureManager design tree or the graphics area. You can also select the Envelope feature in the ConfigurationManager.
2.
Press the Delete key or click Edit, Delete. Both the envelope component and the Envelope feature are deleted.
Select Using Envelope Lets you select components for editing operations, based on their positions relative to an envelope component.
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1.
In the ConfigurationManager, right-click the Envelope component and click Select using envelope. The Apply Envelope dialog box appears.
2.
Choose one or more check boxes for selecting the components: •
Inside envelope. Components that are completely inside the envelope are selected. This includes components that are inside the envelope, but have a face which is coincident with the outside of the envelope.
•
Outside envelope. Components that are completely outside the envelope are selected. This includes components that are outside the envelope, but have a face which is coincident with the outside of the envelope.
•
Crossing envelope. Components that cross the boundary of the envelope are selected.
3.
Click the Select Components in Top Assembly Only check box to treat sub-assemblies as a single entity for selection with envelopes. When this check box is selected, you can apply an envelope to an entire subassembly if one or more of its components meets the selection criteria.
4.
Click OK. Components that meet the selection criteria are selected and highlighted.
Component Selection by Properties You can select components for editing operations based on properties. Properties include those specified under File, Properties, Custom and Configuration Specific, as well as some properties that are specific to SolidWorks documents, including Part volume, Configuration name, Document name, and Part mass. For example, you assign the custom property System to each component in an assembly. You specify the name of the system the component belongs to as the value. Then you select all components that have the custom property System whose value is Cooling Or Heating. This selects all the components that belong to either the cooling system or the heating system of the assembly. Before you can use these component selection methods in an assembly, you must fully resolve any lightweight parts that it contains. See Lightweight Components and Loading Additional Model Data for more information.
Advanced Hide/Show Components For show and hide operations in an assembly, you can also control the visibility of components that do not meet the specified criteria. You use the same methods to select the components as described in the previous section, Component Selection by Properties. To define advanced visibility criteria:
1.
In the ConfigurationManager, right-click the active configuration, and select Advanced Show/Hide.
2.
Under Define additional criteria, select a Property from the list or type in a property name. Properties include those listed in the default list under File, Properties, on the Custom tab, plus several special SolidWorks properties. NOTE: Custom property names added by you do not show on the list, but you can enter them in the Property box.
3.
Select a Condition, and enter a Value. For most properties, conditions include is (exactly), is not, and contains (a text string which is part of the text of the value. For example, the value "simplified" contains the string "sim".) For the SolidWorks special property Part volume, conditions include is inside, is crossing, and is outside, and the values that are available include the names of any envelopes that you have defined.
4.
Click Add to include the selection criteria in the Criteria list.
5.
To add another criteria to the list, click And or Or as a logical operator for combining the criteria, then specify another Property, Condition, and Value. Click Add after specifying each new criteria.
6.
When you have specified all the necessary criteria, click Apply. The selected components are highlighted. If needed, you can modify the selection, and click Apply again.
7.
Under Operations, click Show part components or Hide part components to specify the visibility of the components that meet the criteria.
8.
Specify what to do with any component that does not meet the criteria:
9.
•
If you clicked Show part components in Step 7, you can either Hide it (regardless of current display state), or Leave its show/hide state as is.
•
If you clicked Hide part components in Step 7, you can either Show it (regardless of current display state), or Leave its show/hide state as is.
Click Apply. If needed, you can modify the selection, and click Apply again.
10. If you want, you can Save Criteria for future use, or Load Criteria that you saved earlier. See Saving and Reloading Selection Criteria. 11. Click Close when you are satisfied with the selections.
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Advanced Component Selection You define the selection criteria by specifying the properties, conditions, and property values of components you want to select. To define advanced selection criteria:
1.
Click Tools, Advanced Select.
2.
Under Define additional criteria, select a Property from the list. Properties include those listed under File, Properties, on the Custom or Configuration Specific tabs, plus several special SolidWorks properties.
3.
Select a Condition, and enter a Value. •
For most properties, conditions include standard mathematical operators.
•
For some properties, conditions include is (exactly), is not, and contains. You use contains to specify a text string which is part of the text of the value; for example, the value "simplified" contains the string "sim".
•
For the SolidWorks special property Part volume, conditions include is inside, is crossing, and is outside. The values that are available are the names of any envelopes that you have defined. See Assembly Envelopes.
4.
Click Add to include the selection criteria in the Criteria list.
5.
To add another criteria to the list, click And or Or as a logical operator for combining the criteria, then specify another Property, Condition, and Value. Click Add after specifying each new criteria.
6.
To delete a criteria from the list, click in the first column of the Criteria list box, beside the criteria to delete. A blue box appears beside the selection. Click Delete.
7.
When you have specified all the necessary criteria, click Apply. The selected components are highlighted. If needed, you can modify the selection, and click Apply again.
8.
If you want, you can Save Criteria for future use, or Load Criteria that you saved earlier. See Saving and Reloading Selection Criteria.
9.
Click the pushpin
if you want to keep the dialog box open for further selections and operations.
10. Perform the desired editing operation, such as Suppress, Hide, or Copy.
Saving and Reloading Selection Criteria When you use Advanced Component Selection or Advanced Show/Hide Components, you can save the selection criteria to a file. Then you can load the criteria later, to quickly apply the same set of selection criteria whenever you want. To save selection criteria:
1.
In the Advanced Component Selection or Advanced Show/Hide Components dialog box, specify a set of selection criteria.
2.
Click Save Criteria.
3.
In the Save Criteria dialog box, browse to the folder where you want the file to be stored, enter a file name, and click Save. The query is saved with the extension .sqy.
To reload selection criteria:
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1.
In the Advanced Component Selection or Advanced Show/Hide Components dialog box, click Load Criteria.
2.
In the Load Criteria dialog box, browse to and select the query file (.sqy), and click Open. The query is loaded, and the criteria are listed in the dialog box.
Displaying Assemblies Exploding an Assembly View For manufacturing purposes, it is often useful to separate the components of an assembly to visually analyze their relationships. Exploding the view of an assembly allows you to look at it with the components separated. While an assembly is exploded, you cannot add mates to the assembly. An exploded view consists of one or more explode steps. An exploded view is stored with the assembly configuration with which it is created. Each configuration can have one exploded view. You can add Explode Lines to an exploded view to indicate component relationships. Before you can explode an assembly, you must fully resolve any lightweight parts that it contains. See Lightweight Components and Loading Additional Model Data for more information.
Assembly Exploder To automatically explode an assembly with few components:
1.
Click Exploded View on the Assembly toolbar, or right-click the configuration name in the ConfigurationManager, and select New Exploded View.
2.
Click Auto Explode.
3.
Examine the Step Parameters, and modify if necessary.
4.
Click OK.
To create separate explode steps for an exploded view:
1.
Click New
. The Assembly Exploder dialog box expands.
2.
Click an edge or face that is parallel to the direction you want to explode for Direction to explode along.
3.
If the preview arrow points in the wrong direction, select Reverse direction.
4.
Click the components you want to explode for Components to explode.
5.
Select Explode related components together to reposition all components that are mated to the components in Components to explode.
6.
If you selected a component that is part of a sub-assembly: •
Click Entire sub-assembly to explode the selected component and all other components belonging to the sub-assembly.
•
Click Component part only to explode only the selected part, leaving the rest of the sub-assembly in place.
7.
Click Apply
8.
Drag the green drag handle to position the components as desired, or to explode the components by a precise distance, type a value for Distance.
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9.
Click Apply
to update the step.
10. To add more explode steps to the exploded view, repeat the process for each component or group of components. Remember to click Apply after defining each step. 11. When you are satisfied with the completely exploded view, click OK. To edit the explode steps:
1.
Select the Explode Step you want to edit, or use the
buttons to examine and edit each step in turn.
As you select each step, the drag handle appears and the components involved are highlighted or enclosed in bounding boxes. 2.
Edit the explode step by dragging the green handle, changing the distance or direction, and so on, until the component is positioned as desired.
3.
To change the Components to explode or the Direction to explode along, click the corresponding box, then click the desired entities to select or deselect them.
4.
To clear the contents of a box and start again, click the box, then right-click in the graphics area, and select Clear Selections.
5.
To undo the changes to a step, click Undo
6.
Click Apply
7.
To delete an explode step, click Delete
8.
Click OK to finish the view.
.
after editing each step. .
Exploding and Collapsing an Exploded View An exploded view is stored with the assembly configuration in which it is created. Each assembly configuration can only have one exploded view. TIPS: •
You can copy an exploded view from one configuration to another.
•
You can only drag an exploded view from the active configuration to another configuration.
•
You cannot delete an exploded view from an inactive configuration.
To explode and collapse an exploded view:
1.
Click the ConfigurationManager tab
2.
Click the
3.
To explode:
4.
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.
beside the desired configuration, and beside the ExplView feature to see the Explode Steps.
•
Double-click the ExplView feature.
•
Right-click the ExplView feature and select Explode.
•
Right-click the ExplView feature and select Animate explode to display the Animation Controller pop-up toolbar while the assembly explodes.
To collapse, repeat step 3 substituting Collapse in the second bullet and Animate collapse in the third bullet.
Alternative Method for Editing an Exploded View To edit an exploded view without the Assembly Exploder dialog box:
1.
Double-click the ExplView feature in the ConfigurationManager to explode the view.
2.
Right-click the component you want to reposition, and select Show Explode Steps. The drag handles for the explode steps on the selected component are displayed.
3.
Drag the component by the green drag handle to the new position.
4.
Repeat as needed for each component, then collapse the assembly.
Explode Line Sketch An Explode Line Sketch is a type of 3D sketch that you add to an exploded view in an assembly. In an explode line sketch, you can add explode lines to indicate the relationship between assembly components. To insert an explode line sketch:
1.
Create an exploded view in an assembly.
2.
Click Explode Line Sketch
on the Assembly toolbar, or click Insert, Explode Line Sketch.
The Route Line PropertyManager appears. and Jog Sketch Line
tools on the Explode
3.
Add explode lines as needed using the Route Line Sketch toolbar. The lines appear in phantom font.
4.
Add additional lines using the 3D sketch tools, if needed. All lines appear in phantom font.
5.
Close the sketch. The sketch appears in the ConfigurationManager under ExplView.
To edit an explode line sketch:
1.
In the ConfigurationManager, click
to expand ExplView.
2.
Right-click 3DExplode, and select Edit Sketch.
3.
Edit the sketch as you would for any 3D sketch, or add more explode lines.
4.
Close the sketch.
Jog Line You can jog sketch lines in 2D or 3D sketches in part, assembly, and drawing documents. Jog lines are automatically constrained to be parallel or perpedicular to the original sketch line. You can drag and dimension jog lines.
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To jog a sketch line:
1.
In an open sketch with a line, or in a drawing with a sketched line, click Jog Line Sketch toolbar, or click Tools, Sketch Tools, Jog Line.
2.
Click a line to begin the jog.
3.
Move the pointer to preview the width and depth of the jog.
on the Explode
In 3D sketches, press Tab to change the plane of the jog. 4.
Click again to complete the jog. The Jog Line tool stays active so you can insert multiple jogs.
Example of Jog Lines A jog with dimensions in a 2D sketch line.
Jogs in 3D sketch lines in different planes.
Image Quality in Assemblies You can control the Shaded and Wireframe quality of assembly components by changing the image quality of the assembly. When you change the image quality of the assembly, you can choose to apply the assembly’s settings to each of the referenced components. To change the image quality for all components in an assembly:
1.
Click Tools, Options, Document Properties, Image Quality.
2.
Select Apply to all referenced part documents.
3.
Move the Shaded and draft quality HLR/HLV resolution or Wireframe and high quality HLR/HLV resolution sliders.
4.
Click OK.
Color and Appearance in Assemblies By default, components that you add to an assembly are displayed using the color specified in the original part document. This is true for Shaded and all wireframe display modes. You can override the part color for selected instances, or use the default color for the assembly. You can also modify material properties such as Transparency and Shininess. These changes do not affect the original part document.
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To change the color of selected component instances:
1.
Click a component in the FeatureManager design tree or in the graphics area. To select multiple components, hold Ctrl as you select.
2.
Click Edit Color
3.
Click OK.
on the Standard toolbar. See Color and Optics.
To edit the color and advanced properties of selected component instances:
1.
Right-click a component and select Properties.
2.
Click Color. •
To apply a new color, click Change Color, choose a color from the palette, and click OK.
•
To use the default color for the assembly document, click Use Assembly.
•
To restore the component to the original color specified in the part document, click Remove Color.
3.
Click Advanced to set other properties for the selected component, such as Transparency and Shininess.
4.
Click OK. The color of the selected instances changes, but not the referenced part document.
To change the color of a component and its original part document:
1.
Right-click a component and select Edit Part.
2.
Click Tools, Options, Document Properties, Colors.
3.
Select Shading in Model\Feature colors, and click Edit.
4.
Select a new color, click OK to close the Color dialog box, and OK again to close the Options dialog box.
5.
To return to editing the assembly, right-click the assembly icon at the top of the FeatureManager design tree, and select Edit Assembly.
To toggle the wireframe display color of components:
Click View, Display, Use Component Color in HLR/HLV. •
When this menu item is selected, assembly components appear in the wireframe/HLR color of the component.
•
When this menu item is cleared, assembly components appear in the wireframe/HLR color of the assembly.
Annotations in Assemblies To specify the display of annotations in an assembly, right-click the Annotations folder in the FeatureManager design tree, and select Details. In the Annotation Properties dialog box, you have these options: •
Display filter. Select which annotation types, if any, to display by default. To select specific types, clear the Display all types check box, and select the types you want.
•
Text scale. Adjust the size of the text as needed.
•
Always display text at the same size. When checked, all annotations and dimensions are displayed at the same size, regardless of zoom.
•
Display items only in the view orientation in which they are created. When checked, any annotation is displayed only when the model is viewed in the same orientation as when the annotation was added.
•
Display assembly annotations. Toggles the display of annotations, including annotations that belong to the assembly, and annotations that are displayed in the individual part documents.
•
Use assembly’s setting for all components. Sets the display of all annotations to match the setting for the assembly document, regardless of the setting in the individual part documents. Use this option along with Display assembly annotations to display different combinations of annotations.
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Preventing Interference Between Components Interference Detection In a complex assembly, it may be difficult to visually determine whether components interfere with each other. You can determine the interference between components and examine the resulting interference volumes. To detect interference:
1.
Click Interference Detection
on the Assembly toolbar, or click Tools, Interference Detection.
By default, the top-level assembly appears under Selected Components unless you pre-selected other components. If you check an assembly for interference, all of its components are checked. 2.
Under Options, select Treat coincident as interference to report coincident entities as interference volumes. When cleared, coincident entities are ignored.
3.
Click OK
to check for interference.
The following occurs: •
The interference volumes appear under Results.
•
The components for the selected interference appear under Component 1 and Component 2.
•
The volume of the selected interference highlights in the graphics area. The volume of the interference is in the form of length, width, and height of the bounding box around the area of interference.
4.
Select other interference volumes under Results to examine other results.
5.
Clear the Selected Components box, select new components, and click OK for interference.
6.
Click Cancel
to check other components
when done.
Collision Detection You can detect collisions with other components when moving or rotating a component. The software can detect collisions with the entire assembly or a selected group of components. You can find collisions for either the selected components or for all of the components that move as a result of mates to the selected components. Physical Dynamics is an option in Collision Detection that allows you to see the motion of assembly components in a realistic way. With Physical Dynamics enabled, when you drag a component, the component applies a force to components that it touches, and moves the components if they are free to move. To detect collisions as you move or rotate components:
1.
Click Move Component
2.
In the PropertyManager, under Options, select Collision Detection.
3.
Under Check between, select: o
o
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or Rotate Component
on the Assembly toolbar.
All components - If the component you are moving touches any other component in the assembly, the collision is detected. These components - Select components for the Components for Collision Check box, then click Resume Drag. If the component you are moving touches a selected component, the collision is detected. Collisions with items that are not in the box are ignored.
4.
Select Dragged part only to check for collisions with only the components that you selected to move. When cleared, the components that you selected to move, plus any other components that move because of mates with the selected components, are checked.
5.
Select Stop at collision to stop the motion of the component when it touches any other entity.
6.
Under Options, select: o
Highlight faces - The faces that touch the component you are moving are highlighted.
o
Sound - The computer beeps when a collision is detected.
o
Ignore complex surfaces - Collisions are only detected on the following surface types: planar, cylindrical, conical, spherical, and torodial. NOTE: The This configuration check box does not apply to Collision Detection, Physical Dynamics, or Dynamic Clearance. It applies only to Move Component or Rotate Component.
7.
Move or rotate the component to detect collisions.
8.
Click OK
to finish and exit.
Physical Dynamics Physical Dynamics is an option in Collision Detection that allows you to see the motion of assembly components in a realistic way. With Physical Dynamics enabled, when you drag a component, the component applies a force to components that it touches. The effect is to move or rotate contacted components within their allowable degrees of freedom. The dragged component reacts to a collision by rotating within its allowable degrees of freedom or by sliding against a constrained or partially constrained component to allow the drag to continue. Physical Dynamics propagates throughout the assembly. The dragged component can push aside a component, which then moves into and pushes aside another component, and so on. Physical Dynamics works best and is most meaningful on assemblies that have only a few degrees of freedom. Add all appropriate mates prior to running Physical Dynamics. You cannot use Physical Dynamics and Dynamic Clearance at the same time. To move a component using physical dynamics:
1.
Click Move Component
or Rotate Component
on the Assembly toolbar.
2.
In the PropertyManager, under Options, select Physical Dynamics.
3.
Move the Sensitivity slider to change the frequency with which Physical Dynamics checks for collisions. Move the slider to the right to increase the sensitivity. At the most sensitive setting, the software checks for collisions every .02mm (in model units). At the least sensitive setting, the check interval is 20mm. Use the most sensitive settings only for very small components, or for components with complex geometry in the collision area. When you use the maximum sensitivity when checking for collisions between larger components, the drag is very slow. Use only the sensitivity setting you need to see the motion in your assembly.
4.
If needed, specify the components to participate in the collision: a.
Click These components.
b.
Select components for Components for Collision Check.
c.
Click Resume Drag. Choosing specific components in Collision Detection improves the performance of Physical Dynamics. Choose only those components that are directly involved in the motion you are testing.
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5.
Drag a component in the graphics area. When Physical Dynamics detects a collision it adds a contact force between the colliding parts and allows the drag to continue. The force remains as long as the two parts touch. When the two parts no longer touch, the force is removed. You can select one component after another within a single command.
6.
Click OK
.
Initial Collisions If the component you drag has an initial collision with another component, SolidWorks displays a message in the graphics area and all components involved in the collision turn transparent. Physical Dynamics is turned off for collisions between the transparent components. You can continue the drag, and collide with and apply a force to other components. To activate a collision between initially colliding components
1.
Drag your component until it no longer interferes.
2.
Release the drag.
3.
Drag again. The components are no longer transparent, and Physical Dynamics works.
Dragging by Center of Mass When you click a component to drag it, a center of mass symbol appears at the component's center of mass. If you click the symbol and drag the component, you are dragging by the center of mass. If you click outside the symbol and drag, you are dragging by the point on the body you clicked. You apply a moment arm to a component if you drag outside the center of mass, which causes the component to rotate within the allowable degrees of freedom. NOTE: The center of mass symbol appears during Move, but not during Rotate. The Free Drag option in Rotate Component is by definition rotation about the center of mass.
Dynamic Clearance You can dynamically detect the clearance between components when moving or rotating a component. As you move or rotate a component, a dimension appears indicating the minimum distance between the selected components. Additionally, you can prevent two components from moving or rotating within a specified distance of one another. To dynamically detect the clearance between components:
1.
Click Move Component
or Rotate Component
on the Assembly toolbar.
2.
In the PropertyManager, select Dynamic Clearance.
3.
Click in Components for Collision Check
4.
Click Stop at Specified Clearance and type a value in the box to prevent the selected components from moving within the specified distance.
5.
Drag one of the selected components in the graphics area.
, select the components to check, then click Resume Drag.
Notice a dimension appears in the graphics area and in the PropertyManager. This dimension is the minimum distance between the selected components; the dimension dynamically updates as you drag the component. Also, in the PropertyManager, a value appears in brackets. This is the minimum distance found during the drag operation.
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6.
Under Options, select: o
o
Sound - The computer beeps when the minimum distance in the Stop at Specified Clearance box is reached. Ignore complex surfaces - Clearances are only detected on the following surface types: planar, cylindrical, conical, spherical, and torodial. NOTE: The This configuration check box does not apply to Collision Detection, Physical Dynamics, or Dynamic Clearance. It applies only to Move Component or Rotate Component.
7.
Click OK
to finish and exit.
Smart Fasteners Smart Fasteners Overview Smart Fasteners automatically adds fasteners (bolts and screws) to your assembly if there is a hole, hole series, or pattern of holes, that is sized to accept standard hardware. It uses the SolidWorks Toolbox library of fasteners, which has a large variety of ANSI Inch, Metric and other standard hardware. Smart Fasteners follows the copy parts options in the SolidWorks Toolbox Configure Browser dialog box to determine if fasteners are added to an assembly as a configuration of an existing part or as a copy of an existing part.
Assembly with various types of holes
Assembly with Smart Fasteners
Holes for Smart Fasteners Smart Fasteners adds fasteners to available hole features in assemblies. The holes can be assembly or part features. You can add fasteners to specific holes or patterns, faces or components, or to all available holes. Smart Fasteners is feature-based. Fasteners are placed in Hole Wizard holes, simple holes, and cylindrical cut features. Smart Fasteners does not recognize holes in derived, mirrored, or imported bodies. If you extrude a sketch of a rectangle with a circle in it as a base feature, Smart Fasteners does not recognize the inside of the boss as a hole, because the cylinder is not a separate feature. See Unsupported Hole Types for more information on hole recognition.
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Fasteners Hole Wizard holes are fitted with matching bolts or screws. For other types of holes, you can configure Smart Fasteners to add any type of bolt or screw as a default. The fasteners are automatically mated to the holes with concentric and coincident mates. Hardware Stacks Smart Fasteners can add nuts and washers to your fasteners. Nuts and washers are automatically mated to the fastener with a concentric mate, and to the fastening surface with a coincident mate. Configurations The added fasteners are fully parameterized parts. Each Smart Fastener is shown in the FeatureManager, and can be expanded to show individual features. Smart Fasteners added to hole patterns use a fastener pattern derived from the hole pattern. The fasteners are all the same type and size, but you can use different configurations of the fastener in the pattern. For example you can make some bolts longer than others. Editing You can change your fasteners with the Edit Smart Fasteners command. It is not recommended to edit the individual parameters of a Toolbox part using Edit Sketch or Edit Definition. These functions do not update the Toolbox database.
Smart Fasteners PropertyManager Smart Fasteners inserts bolts and screws into selected holes in your assembly. The fasteners are fully parameterized SolidWorks parts from the Toolbox library. NOTE: You must enable Toolbox to use Smart Fasteners. To enable Toolbox:
1.
Click Tools, Add-ins.
2.
Select SolidWorks Toolbox and SolidWorks Toolbox Browser.
3.
Click OK.
To add Smart Fasteners to an assembly:
1.
Select one or more holes, face, or component. If you select a component, Smart Fasteners finds all available holes in that component. If you select a face, Smart Fasteners finds all available holes that pass through the surface.
2.
Click Smart Fasteners
on the Assembly toolbar, or click Insert, Smart Fasteners.
If you pre-selected a hole, face, or component, new fasteners appear in the assembly and under Fasteners in the PropertyManager. 3.
To add fasteners: a.
Select holes, faces, or components.
b.
Under Selection, click Add. New fasteners appear in the assembly and under Fasteners.
c.
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Click Populate All to add fasteners to all the holes in the assembly.
4.
Change the fastener parameters if needed.
5.
Add nuts and washers if needed.
6.
Click OK
.
Fastener Defaults The length of a new fastener is the next smallest national standard length for a blind hole, and the next longest national standard length for a through hole. When holes are deeper than the longest fastener length, the longest one is used. For a Hole Wizard hole, the fastener type matches the type of hole, and the diameter is the appropriate size. For a Simple Hole or cylindrical cut, you can specify a default fastener type. The fastener diameter is the next smallest national standard size. The PropertyManager Fasteners List The Fasteners list in the Smart Fasteners PropertyManager shows each fastener in your assembly. You can expand each item to show: •
Top Stack. Washers under the head of the fastener.
•
Bottom Stack. Washers and nuts at the end of the fastener.
•
Series 1, Series 2, and so on. Separate hole series that use this fastener. Expand a Series to show: o
Top Stack.
o
Hole features.
o
Bottom Stack. Available for through holes only.
Right-click a fastener to change fastener type, delete it, or change the fastener parameters. Drag and drop a hole feature to create a new series or assign it to a different fastener. Smart Fasteners does not automatically add nuts or washers. You must add these by editing the fastener or the series. See Smart Fasteners Hardware Stacks for more information on adding hardware to fasteners.
Smart Fasteners Bolts and Screws
Askew Head Bolt
Binding Head Screw
Binding Head Miniature Screw
Countersunk Bolt
Countersunk Elevator Bolt
Countersunk Square Neck Bolt
Fillister Head Screw
Fillister Head Chamfered Miniature Screw
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Fillister Head Oval Crown Miniature Screw
Flat Head Screw
Flat Head Miniature Screw
Heavy Hex Bolt
Heavy Hex Structural Bolt
Hex Lag Screw
Hex Screw
Hex Washer Screw
Oval Head Screw
Pan Cross Head Screw
Pan Head Miniature Screw
Pan Slot Head Screw
Round Head Bolt
Round Head Fin Neck Bolt
Round Head Ribbed Neck Bolt
Round Head Screw
Round Head Square Neck Bolt
Round Head Step Bolt
Socket Button Head Cap Screw
Socket Countersunk Head Cap Screw
Socket Head Cap Screw
Socket Head Shoulder Screw
Square Bolt
T-Head Bolt
Truss Head Screw
Hex Flange Screw
Square Lag Screw
Smart Fasteners Nuts Size comparison of Regular and Heavy Hex Nuts:
Styles: Both Hex Nuts and Heavy Hex Nuts are available in Hex, Hex Flat, Hex Flat Jam, Hex Jam, and Hex Slotted styles.
Hex
Hex Flat
Hex Jam
Hex Slotted
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Hex Flat Jam
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Miscellaneous Nut Styles:
Acorn High Crown
Hex Thick
Acorn High Crown 61
Acorn Low Crown
Heavy Hex Square
Hex Thick Slotted
Smart Fasteners Washers Type A Washers Selected washers have a smaller hole than preferred washers. Narrow washers are slightly thinner than wide washers.
Preferred Narrow Flat
Preferred Wide Flat
Selected Narrow Flat
Type B Washers Narrow washer is slightly thinner than wide and regular washers.
Wide Flat
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Regular Flat
Narrow Flat
Selected Wide Flat
Spring Lock Washers
Regular
Heavy
Hi-Collar
Extra Duty
Unsupported Hole Types Smart Fasteners inserts fasteners into series of holes in assemblies. •
Holes must be a supported type.
•
Not all hole types are supported by Smart Fasteners. Unsupported hole types include: o
Single holes
o
Base extrude formed from a sketch with inside circles
o
Mirrored Hole Wizard holes
o
Holes from imported, derived, or mirrored parts
o
Mismatched patterned holes
o
Holes with a large difference in radius
o
Misaligned holes
o
Aligned holes with large gaps between holes
Single holes The hole must pass through at least two components.
Unsupported
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Supported
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Base extrude with inside circles
A base extrude with inside circles appears to form holes. Although geometrically identical to holes, they are not separate features, and are not recognized by Smart Fasteners. Holes from imported, derived, or mirrored parts If holes in an imported part, derived base part, or mirrored part come from the parent part, they are not recognized by Smart Fasteners. However, holes you put into imported, derived, or mirrored parts are recognized because they are separate features. Mismatched patterned holes If a hole is part of a pattern in one component, it must be part of an identical pattern in the other components through which the fastener hole passes. The patterns must be identical in the number of holes. If a hole in one component is part of a pattern, it cannot form a series with a hole in another component that was created as a separate feature that is not part of a pattern.
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Unsupported
Unsupported
Supported
Supported
Large differences in radius If any hole in a series is more than twice the radius of the smallest hole in the series, Smart Fasteners does not recognize the holes.
Unsupported hole series - 45 > 2(20)
Supported hole series - 35 < 2(20)
Misaligned holes Holes are unsupported if they are misaligned. If Smart Fasteners does not insert a fastener into a hole series that appears aligned and is otherwise appropriate, check for a small geometric misalignment (see Measure). Large gaps between holes If the length of the series from start to finish is greater than 5 times the total depth of all the individual holes, the series is not recognized during Populate All. You can add Smart Fasteners into specific holes in the long series by selecting them during insert.
Editing Smart Fasteners You can change the type, size, length, and other editable dimensions of a Smart Fastener. You can flip Smart Fasteners in through holes. You can also change the type of fastener assigned to a hole, or split a bolt series by dragging a hole to a different fastener. To edit Smart Fasteners:
Right-click Smart Fastener in the FeatureManager design tree and select Edit Smart Fastener. The Smart Fasteners PropertyManager appears. To flip Smart Fasteners:
1.
Expand the fastener in the Smart Fasteners PropertyManager.
2.
Right-click the Series you want to flip and select Flip. The heads of the fasteners in the selected series flip to the other side of the joint.
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To change the type of Smart Fastener:
1.
Right-click a fastener in the Smart Fasteners PropertyManager and select Change fastener type. The Smart Fastener dialog box appears.
2.
3.
Select from the following: •
Standard. Select a national or user-defined standard.
•
Type. Choose a type of bolt or screw from the list.
•
Fastener. Choose from specific fasteners based on the Standard, Category, and Type you selected. The Toolbox Browser displays the full range of available fasteners. You can also view an online glossary of bolts and screws.
Click OK.
To change the parameters of Smart Fasteners:
1.
Right-click a fastener or Series and select Properties. A dialog box opens with a list of dimensions and features which can be changed. Dimensions that cannot be changed are not listed.
2.
Select a parameter to change and choose a new value or option from the list. Repeat for other parameters as needed.
3.
Click OK.
NOTE: It is not recommended to edit the individual parameters of a Toolbox part using Edit Sketch or Edit Definition. These functions do not update the Toolbox database.
Smart Fasteners Hardware Stacks Smart Fasteners does not automatically add nuts or washers to fasteners. You can add standard nuts and washers to Smart Fasteners in the Smart Fasteners PropertyManager. Each Series of fasteners has an associated Top Stack (washers added under the head of the fastener) and Bottom Stack (washers and nuts added to the end of the fastener). You can expand each fastener series to see its Top Stack and Bottom Stack. If you add hardware to the Top Stack or Bottom Stack at the fastener level, that hardware appears in each Series. If you add hardware to the Top Stack or Bottom Stack at the Series level, it appears in that Series only. NOTE: You cannot add hardware to a Bottom Stack for blind or tapped holes. See Smart Fastener Defaults for options to associate the size and length of a fastener to the hardware stack. To add washers under a bolt head:
1.
If you are not in the Smart Fasteners PropertyManager, right-click the Smart Fastener in the FeatureManager design tree, and select Edit Smart Fasteners. The Smart Fasteners PropertyManager appears.
2.
Click
to expand the fastener tree.
3.
If you want to add washers to one Series only, click
4.
Double-click Top Stack for either the fastener or the Series.
to expand that Series
The Top Stack Components dialog box appears. 5.
In row 1, select a Component and Quantity.
6.
Click the box under Properties. The properties dialog box appears, where you can change the component's properties and assign a part number.
7.
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If you want to add other sizes or types of washers to the Top Stack, select a second component in row 2 of the properties dialog box, a third component in row 3, and so on. If you add more than one type of washer, the first is next to the bolted surface, and the subsequent washers are added toward the bolt head.
NOTE: To remove a component from the stack, select None from the component list.
Top Stack Order
Bottom Stack Order
To add nuts and washers at the end of a bolt:
1.
Repeat steps 1 to 3 from the procedure above.
2.
Double-click Bottom Stack. The Bottom Stack dialog box appears.
3.
Add hardware as described in the procedure above. Add washers first, and the nut last. The hardware appears in order from the bolted surface toward the end of the bolt.
NOTE: If you add hardware at the Series level, and then add hardware at the fastener level, you overwrite the Serieslevel hardware.
Drag-and-Drop Editing of Smart Fasteners Splitting Hole Series In an assembly with a series of aligned holes, the design may call for a number of short fasteners or one long fastener. Smart Fasteners automatically assigns a single long fastener to the hole series. You can then split the hole series into multiple series, each with its own fastener. NOTE: To split the series, you must have separate hole features within the series. For example, you cannot split a series of holes formed from an assembly-level hole feature, since that is a single feature.
Single fastener assigned to hole series.
Hole series split. New fastener lengths.
To split a hole series:
1.
If you are not in the Smart Fasteners PropertyManager, right-click the Smart Fastener in the FeatureManager design tree, and select Edit Smart Fasteners. The Smart Fasteners PropertyManager appears.
2.
Under Fasteners, click
3.
Click
to expand the fastener tree.
to expand the Series.
Separate hole features are listed in order between Top Stack and Bottom Stack. In this example there are four hole features.
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4.
Select the first hole feature that you want to split off from the series, (in this example, the third hole feature), and drag it to the fastener name at the top level of the tree. The first and second hole features stay with the original series, and the third and fourth hole features form a new series. When you select a hole feature for a new series, that hole feature and all the ones following it in the fastener list move into the new series.
5.
A message box appears. Select one of the following options: •
Click Yes to calculate new fastener lengths for both series.
•
Click No to keep the original fastener length for both series.
A new Series is added to the list, and another set of fasteners appears in the graphics area in the selected holes. The fasteners have the same properties (except for length) as the parent fastener. You can edit the properties at the fastener level or at the Series level. Reassigning Holes One way to change the properties of Smart Fasteners is to reassign the fastener hole to a different fastener. See Editing Smart Fasteners for other ways to change fastener properties. To reassign a hole:
1.
If you are not in the Smart Fasteners PropertyManager, right-click the Smart Fastener in the FeatureManager design tree, and select Edit Smart Fasteners.
2.
Expand the fastener and Series for the hole you want to reassign.
3.
Select the hole series in the PropertyManager design tree and drag it to another Smart Fastener in the tree. The hole series moves under the new Smart Fastener in the tree, and the new fastener appears in the graphics area.
Smart Fasteners Part Numbers You can assign part numbers and descriptions to Smart Fasteners. The part numbers become part of the Toolbox database, and are available to you in other assemblies. To assign part numbers and descriptions to Smart Fasteners:
1.
In the Smart Fasteners PropertyManager, right-click a fastener group in the Fasteners list and select Properties.
2.
Select List by Part Number or List by Description.
3.
Click Add. The Toolbox - New Part Number dialog box appears.
4.
Accept the default part number or type your own in the Part Number box. Type a description in the Description box.
5.
Click OK
.
Mark Up-to-date If you change a hole containing Smart Fasteners, you might get the following warning: Hole series has changed. Please verify that current fastener is correct. The affected fastener is marked with a flag
in the FeatureManager design tree.
To clear the warning:
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1.
Check to see that the fastener is correct.
2.
Right-click the fastener in the FeatureManager design tree and select Mark upto date.
Configuring Bolt Patterns in Smart Fasteners Smart Fasteners added to hole patterns use a bolt pattern derived from the hole pattern. The fasteners are all the same and there is only one fastener listed in the Smart Fasteners PropertyManager. If you want to change the properties of some bolts in the pattern, (for example, make them longer), you can specify different configurations of the bolt. Each time you specify a Smart Fastener, you add it to your Toolbox database. Smart Fasteners follows the copy parts options in the SolidWorks Toolbox Configure Browser dialog box to determine if fasteners are added to an assembly as a configuration of an existing part or as a copy of an existing part. To change the parameters of an individual fastener in a pattern:
1.
Click
to expand the Smart Fastener in the FeatureManager design tree.
2.
Click
to expand the DerivedLPattern (or DerivedCPattern).
All fasteners in the pattern are listed. 3.
Right-click a fastener in the list and select Properties. The Component Properties dialog box appears.
4.
Under Referenced configuration, select Use named configuration.
5.
Select a bolt from the list. NOTE: If you do not see the configuration you want, you can add a new configuration to the Toolbox database using the procedure below.
6.
Click OK. The revised bolt appears.
To add a new fastener configuration to the Toolbox database:
1.
Click
to expand the Smart Fastener in the FeatureManager design tree.
2.
Right-click the fastener component and select Edit Toolbox Definition. The properties dialog box for the fastener appears.
3.
Select new parameters for the fastener. For example, choose a different length or drive type.
4.
Click OK. All fasteners in the series change to the new configuration. You can now change individual bolts in the bolt pattern to use either the old or the new configuration.
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Smart Fasteners Defaults You can configure default fasteners for different standards and hole types. You can also make the fastener's length change when the hardware stack changes, and make the stack hardware size change when the fastener size changes. To set Smart Fasteners defaults:
1.
Click Toolbox, Browser Configuration. The Configure Browser dialog box appears.
2.
Click the Smart Fasteners tab.
3.
Choose from the following options: •
•
•
4.
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Default Fasteners. •
Holes without standards. Choose a default Standard and a default fastener.
•
Holes with standards. Choose a default fastener for each Standard.
Fastener Update. Select the following check boxes to associate Smart Fasteners and hardware stack dimensions. •
Change fastener length when stack components are added or removed. Fastener length increases when you add additional stack hardware, and decreases when you remove stack hardware. Fastener length changes by standard increments and cannot be longer than the longest national standard.
•
Change stack components when fastener size is changed. Nut and washer sizes automatically change when the fastener size changes.
Stack Components. Select from options to limit the available washer types, depending on the size of your Smart Fastener.
Click OK.
•
Exact match. Limits the available types to washers that exactly match your fastener size.
•
Greater than tolerance. Limits the available types to hole diameters that match your fastener size within the tolerance you type.
•
Unrestricted. All washer types available.
10 Configurations
Configurations Overview Configurations allow you to create multiple variations of a part or assembly model within a single document. Configurations provide a convenient way to develop and manage families of models with different dimensions, components, or other parameters. To create a configuration, you specify a name and properties, then you modify the model to create the design variations you want. •
In part documents, configurations allow you to create families of parts with different dimensions, features, and properties, including custom properties.
•
In assembly documents, configurations allow you to create: o o
simplified versions of the design by suppressing or hiding components. families of assemblies with different configurations of the components, different parameters for assembly features, different dimensions, or configuration-specific custom properties.
You can create configurations manually, or you can use a design table to create multiple configurations simultaneously. Design tables provide a convenient way to create and manage configurations in an easy-to-use worksheet. You can use design tables in both part and assembly documents, and you can display design tables in drawings. Custom properties created in design tables are automatically added to the Configuration Specific tab in the Summary Information dialog box.
ConfigurationManager The ConfigurationManager on the left side of the SolidWorks window is a means to create, select, and view multiple configurations of parts and assemblies in a document. You can split the ConfigurationManager and either display two ConfigurationManager instances, or combine the ConfigurationManager with the FeatureManager design tree, PropertyManager, or third party applications that use the panel. The icons in the ConfigurationManager denote whether the configuration was created manually table .
or with a design
To activate the ConfigurationManager:
Click the ConfigurationManager tab
at the top of the left panel.
Each configuration is listed separately. To return to the FeatureManager design tree:
Click the FeatureManager design tree tab
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Show Preview You can display configuration previews of a part or assembly in the PropertyManager. You do not have to open a configuration to see it, which saves time in complex parts and assemblies. To display a configuration preview in the PropertyManager:
1.
In the ConfigurationManager, right-click the configuration you want to preview and select Show Preview. The FeatureManager design tree automatically splits, and the configuration preview appears in the PropertyManager. NOTE: If the preview does not appear, open each configuration, and save the document in each configuration. The next time you select Show Preview, the preview appears.
2.
While the preview is displayed, click any other configuration in the ConfigurationManager to update the preview.
3.
Click anywhere in the graphics area to hide the preview.
Configurations and In-context Components You can have more than one instance of an in-context component that is geometrically different in an assembly. To accomplish this, you must have the following: •
A driving part with two configurations.
•
An sub-assembly with two configurations.
•
In the sub-assembly, create a driven part with two configurations. The driven part is built in the context of the sub-assembly referencing the different geometry in the two configurations of the driving part. The configurations in the driving part, driven part, and sub-assembly do not need to have the same name. But, you must correctly organize the configuration names that represent each combination of geometrically different components.
Here is an example to show how to place components that are geometrically different into the same assembly: 1.
Create a cylindrical part called tube.
2.
Create two configurations of tube called large and small. Each configuration has a different diameter for the cylinder.
3.
Add tube to a sub-assembly called pipes and create two configurations of the sub-assembly called large and small. Each configuration of the sub-assembly, pipes, use tube in its large and small configurations.
4.
Create a part called plug in the context of the sub-assembly, referencing the different diameters of tube. Plug must have two configurations large and small that match the driving component, tube.
5.
Insert two instances of the sub-assembly, pipes, into a main assembly called plumbing. Set one instance of pipes to the large configuration and the other to the small configuration. You now have two instances of the driven part, plug, that are geometrically different in the same assembly. The important detail is matching the configurations of the driving part, driven part, and sub-assembly.
10-2
Configure Document When you open an assembly document, you can specify the configuration name to use for the parts contained in the assembly. You can also create a new configuration when you open an assembly, and either suppress or resolve all of the components at once. To use specific part configurations contained in an assembly:
1.
Click File, Open.
2.
In the Open dialog box: a.
Select an assembly document.
b.
Select the Advanced check box.
c.
Click Open.
The Configure Document dialog box appears. 3.
Select the Use specified configuration for part references when available check box, and type a part Configuration name. Any part that has a configuration with the specified name uses that configuration.
4.
Click OK. The document opens with the selected configuration.
To open a new configuration of an assembly:
1.
Click File, Open.
2.
In the Open dialog box:
3.
a.
Select an assembly document.
b.
Select the Advanced check box.
c. Click Open. In the Configure Document dialog box: •
To open the assembly with all the components resolved, click New configuration showing all referenced models.
•
To open the assembly with all the components suppressed, click New configuration showing assembly structure only.
4.
Type a name for the new configuration in the Configuration name box.
5.
Click OK. The assembly opens in the new configuration.
Configure Document for View / Configurations The Configure Document for View dialog box appears if you opened a drawing whose configuration no longer exists. The Configurations dialog box appears if you replaced a component in an assembly, and clicked the Manually select option. If either of these dialog boxes appears, select a configuration to use, then click OK.
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Manual Configurations Creating a Configuration Manually To create a configuration manually, you specify its properties, then modify the model to create variations in the new configuration. To create a configuration manually:
1.
In either a part or assembly document, click the ConfigurationManager tab FeatureManager design tree to change to the ConfigurationManager.
at the top of the
2.
In the ConfigurationManager, right-click the part or assembly name and select Add Configuration.
3.
In the Add Configuration dialog box, type a Configuration Name and specify properties for the new configuration. You can specify a configuration specific color.
4.
Click OK.
5.
Click the FeatureManager design tree tab
6.
Modify the model as needed to create the design variation.
7.
Save the model.
to return to the FeatureManager design tree.
Add Configuration/Configuration Properties This dialog box controls the following properties when you add a configuration or edit configuration properties: Configuration Name. Type a name for the configuration. The name must not include the forward slash (/) or at sign (@). A warning message appears when you close the dialog box if the name field contains either of these characters, if the field is blank, or if the name already exists. Description. Type a description that identifies the configuration. (Optional) Comment. Type additional descriptive information about the configuration. (Optional) Use configuration specific color. To specify a color for the configuration, select this check box, then click Color to choose a color from the color palette. •
If the color for wireframe and HLR modes is the same as the color for shaded mode, the configurationspecific color applies to all three modes. If the color is not the same for all three modes, then the configuration specific color applies to shaded mode only. To be sure the colors are the same for the three modes, select the Apply same color to wireframe, HLR and shaded check box in Tools, Options, Document Properties, Colors.
•
To apply a configuration-specific color to components in an assembly, right-click the selected components in the FeatureManager design tree, select Component Properties, and click Color. In the Assembly Instance Color dialog box, click Use Assembly and click OK.
Properties for newly inserted items. These check boxes control what happens when new items are added to another configuration, and then this configuration is activated again. For assemblies, the following check boxes are available:
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•
Suppress features and mates. When selected, new mates and features added to other configurations are suppressed in this configuration. Otherwise, new mates and features are unsuppressed in this configuration also.
•
Hide component models. When selected, new components added to other configurations are hidden in this configuration. Otherwise, new components are shown in this configuration also.
•
Suppress component models. When selected, new components added to other configurations are suppressed in this configuration. Otherwise, new components are resolved in this configuration also.
For parts, the following check box is available: •
Suppress features. By default, newly added features are unsuppressed in the active configuration. This option controls what happens when new features are added to another configuration, then this configuration is activated again. When selected, new features added to other configurations are suppressed in this configuration. Otherwise, new features are unsuppressed in this configuration also.
Part number displayed when used in a bill of materials. Click to specify how the assembly or part is listed in a Bill of Materials. •
Select one of the following: o
Document Name. The part number is the same as the document name.
o
Configuration Name. The part number is the same as the configuration name.
o
User Specified Name. The part number is a name that you type.
Don’t show child components in BOM when used as sub-assembly (assemblies only). When selected, the subassembly is always shown as a single item in the bill of materials. Otherwise, the child components may be listed individually in the BOM, when Show parts only or Show assemblies and parts in an indented list is selected. NOTE: After you create a configuration, if you right-click the configuration name in the ConfigurationManager and select Properties, the Configuration Properties dialog box appears. Click Custom to access Configuration Specific properties in the Summary Information dialog box.
Properties for Newly Inserted Items These options control what happens to this configuration when you add new items to another configuration. The options that are available depend on the type of document. Check box cleared
Check box selected
New features are included (not suppressed)
New features are suppressed
Suppress features and mates
New features* and mates are included (not suppressed)
New features* and mates are suppressed
Hide component models
New components are shown
New components are hidden
Suppress component models
New components are resolved (not suppressed)
New components are suppressed
Part documents Suppress features Assembly documents
* New features in assemblies include assembly feature cuts and holes, component patterns, reference geometry, and sketches that belong to the assembly (not to one of the assembly components).
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Derived Configurations Derived configurations allow you to create a parent-child relationship within a configuration. By default, all parameters in the child configuration are linked to the parent configuration. If you change a parameter in the parent configuration, the change automatically propagates to the child. You can override any configurable parameter in the derived configuration so that the parameter is no longer linked to the parent. Consider the following example. Part1 has three configurations: •
Configurations A and C are top-level configurations. Configuration B is a derived configuration of configuration A.
•
The following table shows the effect on configurations B and C when you change configuration A. Change configuration A and apply the change to:
Effect on configuration B
Effect on configuration C
This Configuration
Changes
Does not change
Specify Configurations (specify configuration A)
Changes
Does not change
All Configurations
Changes
Changes
Example of derived configurations. To create a derived configuration manually:
1.
In the ConfigurationManager, right-click a configuration and select Add Derived Configuration.
2.
In the dialog box, enter the appropriate configuration properties.
3.
Under Part number displayed when used in a bill of materials, select from:
4.
•
Document Name. The part number is the same as the document name.
•
Configuration Name. The part number is the same as the configuration name.
•
Link to Parent Configuration. The part number is the same as the parent configuration name.
•
User Specified Name. The part number is a name that you type.
•
Don't show child components in BOM when used as sub-assembly (assemblies only). When selected, the sub-assembly is always shown as a single item in the bill of materials. Otherwise, the child components can be listed individually in the BOM, when Show parts only or Show assemblies and parts in an indented list is selected.
Click OK. The derived configuration is added to the ConfigurationManager underneath its parent.
To create a derived configuration with a design table:
The column header in a design table for controlling derived configurations uses this syntax: $PARENT The column header is not case sensitive. In the table body cells, type the parent configuration names.
10-6
You cannot specify a parent configuration in a design table if its child configuration was created first, unless the parent configuration already existed in the model.
Valid: Parent created before derived configuration
Invalid: Parent created after derived configuration
This Configuration When you select This Configuration, the changes you make to the model are reflected in the current configuration only. Specify Configurations When you select Specify Configurations, the changes you make to the model are reflected in the configurations that you specify. All Configurations When you select All Configurations, the changes you make to the model are reflected in each of the model's configurations. Example of Derived Configurations This part contains three configurations: A, B, and C. Configuration A is the parent of configuration B, and configuration C is a top-level configuration, similar to configuration A.
Original configuration A (parent)
Modified configuration A
Configuration B (derived)
Configuration C
The extrude in configuration A is modified from 120mm to 60mm. In the Modify dialog box, when This Configuration is selected, the dimension changes in configurations A and B, but not C.
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Activating a Configuration To activate a different configuration:
1.
Click the Configuration Manager tab
to change to the ConfigurationManager.
2.
Right-click the name of the configuration you want to view and select Show Configuration. - or Double-click the configuration name. The named configuration becomes the active configuration, and the view of the model updates to reflect the newly selected configuration.
Configurable Items for Parts You can vary the design of part configurations as follows: •
Modify feature dimensions.
•
Suppress features, equations, and end conditions.
•
Use different sketch planes, sketch relations, and external sketch relations.
•
Set individual face colors.
•
Control the configuration of a base part.
•
Control the configuration of a split part.
•
Control the driving state of sketch dimensions.
•
Create derived configurations.
•
Define configuration-specific properties.
Sketch Dimensions in Configurations You can control the driving state of sketch dimensions in specified configurations to control the behavior of your model. To control the driving state of sketch dimensions:
1.
Right-click a dimension, and select Properties. The Dimension Properties dialog box appears.
2.
Select the Driven check box.
3.
Click Specify Configs. A dialog box appears.
4.
Select the configurations you want to apply the new settings to: This configuration, All configurations, or Specify configurations.
5.
Click OK.
6.
Click OK again to close the Dimension Properties dialog box. The sketch dimension is driven.
10-8
Sketch Planes in Configurations The plane on which a sketch lies is configurable through the Sketch Plane PropertyManager. You can place a single sketch on different planes in different configurations. To change a sketch plane in a configuration:
1.
In the FeatureManager design tree, right-click a sketch and select Edit Sketch Plane. The Sketch Plane PropertyManager appears.
2.
In the graphics area, click the face or plane on which you want the sketch to lie. - or Select a plane from the flyout FeatureManager design tree on which you want the sketch to lie.
3.
Under Configurations, select the configurations to which you want the new sketch plane to apply: This configuration, All configurations, or Specify configurations.
4.
Click OK
.
The sketch changes planes in the selected configurations. Sketch Relations in Configurations You can control the suppression state of sketch relations per configuration. To suppress or unsuppress sketch relations:
1.
Right-click a sketch in the FeatureManager design tree, and select Edit Sketch.
2.
Click Display/Delete Relations
3.
In the PropertyManager, under Configurations (at the bottom of the PropertyManager), select the configurations to which you want the sketch relations to apply: This configuration, All configurations, or Specify configurations (these options are only available if there is more than one configuration in the model).
on the Dimensions/Relations toolbar.
NOTES: •
You must select a configuration prior to changing sketch relations. When you change sketch relations, the change is immediately applied to the selected configuration.
•
If you selected Specify configurations, you cannot clear the active configuration.
4.
Under Relations, select the sketch relations to suppress or unsuppress.
5.
Select or clear Suppressed. When Suppressed is selected, the sketch relation's Information Status Driven.
6.
Click OK
changes from Satisfied to
, and exit the sketch.
The sketch relation is applied to the selected configurations. To suppress or unsuppress sketch relations in a design table:
The column header in a design table for controlling sketch relations uses this syntax: $STATE@<sketch_relation>@<sketch_name> For example, to control the suppression state of the first fixed relation in Sketch2, the column heading syntax is $STATE@Fixed1@Sketch2. The column header is not case sensitive.
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In the table body cells, type S for suppressed or U for unsuppressed. Sketch relations and sketch entities include an assigned number (such as Fixed1) in the Sketch Relations PropertyManager. Example of a design table that controls the suppression state of a sketch relation:
End Conditions in Configurations You can change the end condition of extruded features in specified configurations. To change the end condition of extruded features in specified configurations:
1.
In the FeatureManager design tree, right-click an extruded feature and select Edit Feature.
2.
In the PropertyManager, change the End Condition to the desired settings.
3.
Under Configurations, select the configurations to which you want the new end condition to apply: This configuration, All configurations, or Specify configurations.
4.
Click OK
.
The end condition is applied to the selected configurations.
Configurable Items for Assemblies You can vary the design of assembly configurations as follows:
10-10
•
Change the suppression state (Suppressed, Resolved) or visibility (Hide, Show) of components.
•
Change the referenced configuration of components.
•
Change the dimensions of distance or angle mates, or suppression state of mates.
•
Modify the dimensions or other parameters of features that belong to the assembly. This includes assembly feature cuts and holes, component patterns, reference geometry, and sketches that belong to the assembly (not to one of the assembly components).
•
Suppress features that belong to the assembly.
•
Define configuration-specific properties, such as end conditions and sketch relations.
•
Create derived configurations.
•
Change the suppression state of the Simulation folder in the FeatureManager design tree and its simulation elements. (Suppressing the folder also suppresses its elements.)
Modifying a Configuration Dimension To modify a dimension value for a selected configuration, do one of the following: •
Control the value in a design table.
•
Double-click the feature to display the dimension. Then double-click the dimension, change the value in the Modify box, and select one of the following (these options are only available if there is more than one configuration in the model): o
This Configuration
o
All Configurations
o
Specify Configuration(s)
This applies in part and assembly documents, to all types of feature dimensions, the values used in mates (distance or angle), the number of instances in patterns, and so on.
Editing a Configuration To edit a configuration:
1.
Activate the desired configuration.
2.
Change to the FeatureManager view, then: •
In a part document, change the suppression state of features, modify dimensions, and so on, as needed.
•
In an assembly document, change the suppression state or visibility of components, and so on, as needed.
To edit the configuration properties:
1.
Right-click the configuration name, and select Properties. The Configuration Properties dialog box appears.
2.
Edit the name, comments, or properties as desired.
3.
Click Custom to add or modify custom properties for the configuration.
4.
Click OK.
To suppress or hide features or components:
1.
Select the features or components to suppress or hide (or to unsuppress or show).
2.
Click Edit and choose from the following menu items: In parts: •
Suppress
•
Unsuppress
•
Unsuppress with Dependents
In assemblies:
3.
•
Hide
•
Show
•
Show with Dependents
•
Suppress
•
Unsuppress
•
Unsuppress with Dependents
Each menu item has the following choices: •
This Configuration
•
All Configurations
•
Specified Configurations
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4.
If you selected Specified Configurations, a dialog box appears with a list of configurations and buttons to Select All and Reset Selection. Select configurations in the list and click OK.
Special Assembly Configurations You can create new assembly configurations, by either suppressing or resolving all of the components at once. Open the assembly in a new configuration with one of these options: •
structure only shown (all components suppressed)
•
all referenced models shown (all components resolved)
To suppress or resolve all components in a new assembly configuration:
1.
Click File, Open.
2.
Browse to the desired assembly document, select the Advanced check box, and click Open.
3.
In the Configure Document dialog box, select either:
4.
•
New configuration showing all referenced models. Opens the complete assembly. The components are all resolved and shown, regardless of their suppression and visibility state when last saved. All components appear in the assembly model.
•
New configuration showing assembly structure only. Opens the assembly structure only. The components are suppressed, regardless of their state when last saved. No components appear in the assembly model until you change their suppression state to resolved.
Type a new Configuration name, and click OK. The assembly opens in the new configuration.
Component Configurations in an Assembly If a component (either an individual part or a sub-assembly) has more than one configuration, you can specify which configuration to use for each instance in the assembly. You can also specify certain configuration-specific properties for the component. To specify component configurations and configuration-specific properties:
1.
Right-click the component name in the FeatureManager design tree, or right-click a component face, and select Properties.
2.
In the dialog box, select from the following options: •
Visibility. Allows you to Hide Model and change component color.
•
Referenced configuration. Controls options for referenced configurations: o
Use component’s “in-use” or last saved configuration Any instances with this option use the active configuration (if the document is open), or the configuration that was active when it was saved. When you open an assembly, any active components that are not already open in their own windows are loaded into memory. If you change the configuration in the component’s own window, the newly selected configuration is placed in memory; any instances that use this option update when you return to the assembly. When you edit a part in the context of an assembly, the referenced configuration in the assembly becomes the active configuration in all open windows (for example, if the part is open in its own window, or in use in another open assembly, with this property selected). To change the active configuration for a component that is not already open, right-click the component name in the FeatureManager design tree, and select Open Part or Open Assembly. Then, in the model document, make the desired configuration active.
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You cannot change the referenced configuration of a suppressed component, because suppressed components are removed from memory. However, if you open the document of a suppressed component and change the configuration, the newly selected configuration is used if you restore the component to the resolved state. The words, "in-use" are displayed next to the component name in the FeatureManager design tree if a component is "in-use." o
Use named configuration To always use a specific configuration regardless of the configuration currently in memory, select this option and choose a configuration from the list. It is good design practice to use named configurations when components have multiple configurations, to prevent the in-use configuration from affecting the assembly in unexpected ways.
o
Use same configuration as pattern seed component If the selected component is an instance of a component pattern, this is the default setting. To specify a configuration that is different from the seed component, select Use named configuration, and choose a configuration from the list.
•
Change properties in. Allows you to set properties in This Configuration, All Configurations, or Specify Configuration(s). The Change properties in list is only available in assemblies with more than one configuration.
3.
•
Suppression state. Controls the suppression state of the component.
•
Solve as. Sets the component as Rigid or Flexible.
•
Exclude from bill of materials. Omits this component from the bill of materials.
Click OK. If you selected Specify Configuration(s) for Change properties in, a dialog box appears for you to select the desired configurations.
If the selected component is a component of a sub-assembly, you can do the following:
1.
2.
Under Visibility, choose which visibility properties to use: •
Use visibility properties specified in configuration of <subassembly_name>. The Visibility properties (Hide Model and Color) specified for this component in the selected configuration in the sub-assembly document are used.
•
Override visibility properties specified in configuration of <subassembly_name>. The Visibility properties specified for this component in this configuration of the assembly are used.
Under Solve as, select Rigid or Flexible.
Deleting a Configuration You can delete a configuration with either of the following methods: •
Manually
•
Within a design table
NOTE: Deleting a configuration does not delete any features or components. To delete a configuration manually:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
Right-click the name of the configuration you want to delete, and select Delete. You are asked to confirm the deletion of the configuration.
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3.
Click Yes. The selected configuration is deleted.
To delete a configuration within a design table:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
In the FeatureManager design tree, right-click Design Table and select Edit Table or Edit Table in New Window. The worksheet appears in the window. (If you select Edit Table in New Window, the worksheet opens in a separate Excel window.)
3.
Click the numbered cell beside the configuration name that you want to delete (this selects the whole row), then click Edit, Delete. You can also right-click the numbered cell, and select Delete. NOTE: Do not press the Delete key to delete the row. Pressing Delete clears the contents of the cells and leaves an empty row. Any rows below an empty row are ignored.
4.
When you click outside the table, the table is evaluated, and you are asked to confirm the deletion of the configuration.
5.
Click Yes. The selected configuration is deleted.
Design Table Configurations Creating a Design Table To create a design table, you define the names of the configurations you want to create, you specify the parameters you want to control, and you assign values for each parameter. There are several ways to create a design table: •
Insert a new, empty design table in the model, and enter the design table information directly in the worksheet. When you finish entering the design table information, the new configurations are automatically created in the model.
•
Have the SolidWorks software automatically create the design table. SolidWorks loads all configured parameters and their associated values from a part or assembly.
•
Create a design table worksheet as a separate operation in Microsoft Excel. Save the worksheet, then insert it in the model document to create the configurations.
You can insert a partially completed worksheet, then edit it later to add more configurations, to control additional parameters, or to update values. When you use design tables in the SolidWorks software, it is important to format the tables properly.
Creating a Design Table as a Separate Excel File You can create a design table as a separate Excel file, then use the Design Table PropertyManager to insert the file in your model. NOTES:
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•
When you use design tables in the SolidWorks software, it is important to format the tables properly.
•
If you copy and paste the contents of a design table to a new worksheet in Microsoft Excel, follow the instructions below.
To create a design table as a separate Excel file:
1.
Open Microsoft Excel and create a worksheet.
2.
In the first column (row header cells A2, A3, and so on), type the names of the configurations that you want to create. Leave cell A1 blank. The names can include numerics, but must not include the forward slash (/) or at (@) characters.
3.
In the first row, (column header cells B1, C1, and so on), type the parameters that you want to control. Column headers are not case sensitive.
4.
Type the parameter values in the spreadsheet cells.
5.
Save the worksheet.
6.
Open the model document where you want to insert the design table.
7.
Click Insert, Design Table.
8.
In the Design Table PropertyManager, under Source: a.
Click From file.
b.
Click Browse and open the Excel file. You can also select Link to file, which links the table to the model. A linked design table reads all of its information from an external Excel file. When a design table is linked, any changes you make to the table outside of SolidWorks are reflected in the table within the SolidWorks model, and vice versa. The path to the Excel file appears above the Browse button. If you update a linked design table in Microsoft Excel, then open the SolidWorks model, you can choose to update either: the model with the design table values
o
- or the design table with the model values
o
You can set the update options in Tools, Options, System Options, External References. Set Update out-of-date linked design tables to to Model or Excel File. 9.
Click OK
.
The worksheet appears in the model document, and the Excel menus and toolbars replace the SolidWorks menus and toolbars. 10. Edit the design table if necessary. When you finish editing, click anywhere outside the table to close it. A message indicates the names of any new configurations that were generated by the design table, and the SolidWorks menus and toolbars reappear. The Design Table icon
appears in the FeatureManager design tree.
To display the configurations added by the design table, click the Configuration tab at the bottom of the window. Double-click the configuration name, or right-click the configuration name and select Show Configuration.
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Inserting a Design Table A design table allows you to build multiple configurations of parts or assemblies by specifying parameters in an embedded Microsoft Excel worksheet. NOTES: •
When you use design tables in the SolidWorks software, it is important to format the tables properly.
•
To use design tables, it is strongly recommended that you have Microsoft Excel 97 or later installed on your computer.
There are several different ways to insert a design table. Click one of the following for instructions on how to insert a design table: To have the SolidWorks software insert a design table automatically:
1.
In a part or assembly document, click Design Table Table.
on the Tools toolbar, or click Insert, Design
2.
In the PropertyManager, under Source, select Auto-create.
3.
Set the Edit Control settings and Options, as desired.
4.
Click OK
.
Depending on the settings you selected, a dialog box may appear that asks which dimensions or parameters you want to add. An embedded worksheet appears in the window, and the SolidWorks toolbars are replaced with Excel toolbars. Cell A1 identifies the worksheet as Design Table for: <model_name>. 5.
Click anywhere outside of the worksheet (but in the graphics area) to close the design table.
To insert a blank design table:
1.
In a part or assembly document, click Design Table Table.
2.
In the PropertyManager, under Source, click Blank.
3.
Set the Edit Control settings and Options, as desired.
4.
Click OK
on the Tools toolbar, or click Insert, Design
.
Depending on the settings you selected, a dialog box may appear that asks which dimensions or parameters you want to add. An embedded worksheet appears in the window, and the SolidWorks toolbars are replaced with Excel toolbars. 5.
Cell A1 identifies the worksheet as Design Table for: <model_name>. Cell A3 contains the default name for the first new configuration, First Instance.
6.
In row 2, type the parameters that you want to control. Leave cell A2 blank. Notice that cell B2 is active. You can also enter parameters by double-clicking the feature or dimension in the graphics area or in the FeatureManager design tree. When you double-click a feature or dimension, its associated value appears in the First Instance row.
7.
In column A (cells A3, A4, and so on), type the names of the configurations that you want to create. The names can include numerics, but must not include the forward slash (/) or at (@) characters. You can change the configuration name in cell A3 (First Instance) if you want.
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8.
Type the parameter values in the worksheet cells.
9.
When you finish adding information to the worksheet, click outside the table to close it. A message lists the configurations that were created.
10. Click OK. The design table is inserted in the model, and Design Table
appears in the FeatureManager design tree.
To insert an external Microsoft Excel file as a design table:
1.
In a part or assembly document, click Design Table Table.
on the Tools toolbar, or click Insert, Design
The Design Table PropertyManager appears. 2.
Under Source: •
Click From file, then click Browse to locate the Excel file.
•
To link the design table to the model, select the Link to file check box. A linked design table reads all of its information from an external Excel file.
NOTE: If you update a linked design table in Microsoft Excel, then open the SolidWorks model, you can choose to update either: o
the model with the design table values - or -
o
the design table with the model values
You can set the update options in Tools, Options, System Options, External References. Set Update out-of-date linked design tables to to Model, Excel file, or Prompt. 3.
Set the Edit Control settings and Options, as desired.
4.
Click OK
.
An embedded worksheet appears in the window, and the SolidWorks toolbars are replaced with Excel toolbars. 5.
Click anywhere outside of the worksheet (but in the graphics area) to close the design table.
Design Table PropertyManager Use the Design Table PropertyManager to select design table settings when you insert a design table. Source •
Blank. Inserts a blank design table where you fill in the parameters.
•
Auto-create. Automatically creates a new design table, and loads all configured parameters and their associated values from a part or assembly.
•
From file. References a Microsoft Excel table. Click Browse to locate the table. You can also select the Link to file check box, which links the table to the model. When a design table is linked, any changes you make to the table outside of SolidWorks are reflected in the table within the SolidWorks model, and vice versa.
Edit Control •
Allow model edits to update the design table. If you change the model, the changes are updated in the design table.
•
Block model edits that would update the design table. You are not allowed to change the model, if these changes would update the design table.
NOTE: When you click a setting under Edit Control, you set the level of bi-directional control on the design table.
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Options Add new rows/columns in the design table for: •
New parameters. Adds new rows and columns to the design table if you add a new parameter to the model.
•
New configurations. Adds new rows and columns to the design table if you add a new configuration to the model. Warn when updating design table. Warns you that the design table will change based on the parameters you updated in the model.
•
Add Rows and Columns You made a change to the model, and the SolidWorks software wants to know if you want to add the new configurations or parameters to the design table. NOTE: The Add Rows and Columns dialog box appears because when you created the design table for this model, you selected New parameters or New configurations in the Design Table PropertyManager. To add rows and columns to the design table:
1.
In the Add Rows and Columns dialog box, select the configurations and parameters you want to add from the Configurations and Parameters boxes. NOTE: To select multiple features, hold down Ctrl as you select.
2.
If you do not select certain items in the Configurations and Parameters boxes, select the Show unselected items again check box to see these items next time this dialog box opens.
3.
Click OK. The selected items are added to the design table.
Creating Configurations with a Design Table A design table allows you to build multiple configurations of parts or assemblies by specifying parameters in an embedded Microsoft Excel worksheet. The design table is saved in the model document and is not linked to the original Excel file. Changes you make in the model are not reflected in the original Excel file. However, you can link the model document to the Excel file if you wish. To use design tables, it is strongly recommended that you have Microsoft Excel 97 or later installed on your computer. Parts. You can control the following items in a part design table: •
dimensions and suppression state of features
•
configuration properties, including part number in a bill of materials, derived configurations, equations, sketch relations, comments, and custom properties
Assemblies. You can control the following parameters in an assembly design table:
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•
components - suppression state, visibility, referenced configuration
•
assembly features - dimensions, suppression state
•
mates - dimensions of distance and angle mates, suppression state
•
configuration properties - part number and display in a bill of materials (when used as a sub-assembly), derived configurations, equations, sketch relations, comments, custom properties
Formatting a Design Table When you use design tables in the SolidWorks software, it is important to format the tables properly. This topic shows how to format a design table with: •
Automatically created design tables
•
Manually created design tables
•
Blank rows and columns
•
Invalid criteria
Automatically Created Design Tables When you select Auto-create or Blank in the Design Table PropertyManager, the SolidWorks software automatically creates the Excel file. Automatically created design tables include the Family cell. By default, cell A2 is reserved as the Family cell. This cell determines where the parameter and configuration data begins. The Family cell contains no text, however, in Excel, the Name Box displays Family.
When you edit a design table, you can create rows above and columns to the left of the Family cell. The example below is a valid design table as long as configuration names and SolidWorks parameters are kept below and to the left of the Family cell.
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Manually Created Design Tables When you select From file in the Design Table PropertyManager, you insert a design table by browsing to the location of the Excel file. When you manually create a design table, you type configuration names in the first column (row header cells A2, A3, and so on), and you type parameters in the first row (column header cells B1, B2, and so on). Cell A1 must be blank. The example below is a valid design table as long as cell A1 is blank.
Design Tables With Blank Rows and Columns When the SolidWorks software processes a design table, it processes each configuration in the column with configuration names (top to bottom), then processes each parameter in the parameter row (left to right). If the sofware encounters a: •
blank cell in the parameter row, it goes to the next configuration name and applies the associated parameters
•
blank cell in the configuration name column, it stops processing because it assumes the design table has ended
In the example below, only the Default configuration is processed by the software. Because row 4 is blank, configurations C1 and C2 are not processed.
Invalid Criteria The SolidWorks software stops processing a design table if it reaches invalid parameters in a cell. A summary of design table parameters is available. If you enter information to the left of the parameters row or below the configuration name column, the SolidWorks software warns of an invalid value, and stops processing the design table without completing the remaining rows and columns. If this happens, some configurations will not update properly.
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Manually Add Parameters in a Design Table When you use design tables in the SolidWorks software, it is important to format the tables properly. To manually add certain types of parameters in a design table, with the appropriate worksheet cell active: •
Dimensions. Double-click a dimension in the graphics area. (Make sure that the necessary dimensions are displayed before you insert the new design table.) The Dimension@Feature or Dimension@Sketch parameter is inserted in the cell.
•
Feature suppression. Double-click a face of the feature. The $STATE@Feature parameter is inserted in the cell.
•
Component suppression. Double-click a face of the component. The $STATE@component parameter is inserted in the cell.
As you continue to add parameters this way, the adjacent cell (C2, D2, and so on) is activated automatically. Each parameter is added to the header row, and the current value is displayed in row 3. Column headers are not case sensitive.
Numerical Configuration Name If a configuration name in a design table contains only numbers, Excel interprets the name as a numeric value, instead of text. This is not a problem, except in the following cases: •
If the value begins with zeroes, the leading zeroes are removed.
•
If the value is more than 12 characters long, it is displayed in scientific notation.
To correct the problem, right-click the header cell for column A (to select the whole column), and select Format Cells. On the Number tab, under Category, select Text.
Editing a Design Table When you use design tables in the SolidWorks software, it is important to format the tables properly. 1.
In the FeatureManager design tree, right-click Design Table and select Edit Table or Edit Table in New Window. The worksheet appears in the window. (If you select Edit Table in New Window, the worksheet opens in a separate Excel window.)
2.
Edit the table as needed. You can change the parameter values in the cells, add rows for additional configurations, or add columns to control additional parameters. Since design tables appear in drawings, you may wish to change their appearance while editing them in the model documents. You can edit the format of the cells, using the Excel functions to modify fonts, alignment, borders, and so on.
3.
Click outside of the table to close it. (If you are working with the design table in a separate window, click File, Close.)
4.
If you receive a confirmation message that the design table generated new configurations, click OK. The configurations update to reflect your changes.
Deleting a Design Table 1.
Right-click Design Table in the FeatureManager design tree and select Delete.
2.
Click Yes to confirm the deletion.
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Saving Design Tables You can save design tables directly in the SolidWorks software. To save a design table:
1.
In a document with a design table, select Design Table File, Save As.
in the FeatureManager design tree, then click
- or Right-click Design Table in the FeatureManager design tree and select Save Table. The Save Design Table dialog box appears. 2.
Type a File name, then click Save. The design table is saved as an Excel file (*.xls).
NOTE: Due to a Microsoft limitation, changes to linked design tables may not be saved if they contain values that are linked to other spreadsheets. To save the design table, you can: •
Remove the linked values from the design table
•
Clear Link to file in the Design Table PropertyManager to unlink the design table from the model
Deleting a Configuration You can delete a configuration with either of the following methods: •
Manually
•
Within a design table
NOTE: Deleting a configuration does not delete any features or components. To delete a configuration manually:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
Right-click the name of the configuration you want to delete, and select Delete. You are asked to confirm the deletion of the configuration.
3.
Click Yes. The selected configuration is deleted.
To delete a configuration within a design table:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
In the FeatureManager design tree, right-click Design Table and select Edit Table or Edit Table in New Window. The worksheet appears in the window. (If you select Edit Table in New Window, the worksheet opens in a separate Excel window.)
3.
Click the numbered cell beside the configuration name that you want to delete (this selects the whole row), then click Edit, Delete. You can also right-click the numbered cell, and select Delete. NOTE: Do not press the Delete key to delete the row. Pressing Delete clears the contents of the cells and leaves an empty row. Any rows below an empty row are ignored.
4.
When you click outside the table, the table is evaluated, and you are asked to confirm the deletion of the configuration.
5.
Click Yes. The selected configuration is deleted.
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Specifying Design Table Parameters Specifying Design Table Parameters When used in a design table, the names of dimensions, features, components, and configurations must match the name in the model. To ensure an exact match, you can copy and paste the name from the Properties dialog box for the selected item. You can use multiple languages in a design table. However, the language for the value in a table body cell must be in the same language as the parameter in the corresponding column header. For example, if the parameter in the column header is in English, then the corresponding value in the table body cell must also be in English. The next column header can be in another language, such as Japanese, but its corresponding value in the table body cell must also be in Japanese. NOTES: • When you use design tables in the SolidWorks software, it is important to format the tables properly. •
If the design table has been saved in English and then opened in Japanese, only English and Japanese will work. You cannot add another language, such as Polish, unless you use a Polish version of SolidWorks, or you have previously opened, closed, or saved the design table in a Polish version of SolidWorks.
•
Design tables used in versions prior to SolidWorks 2003 do not support multiple languages.
To copy and paste a dimension, feature, component, or configuration name:
1.
Right-click the item (dimension, feature, or configuration), and select Properties. For a component, select Component Properties from the shortcut menu.
2.
In the dialog box, copy (Ctrl+C) the item name (for dimensions and components, be sure to copy the Full name).
3.
Paste (Ctrl+V) the name into the appropriate column header cell.
Parameter specifications: •
Some parameter specifications that appear in the column header cells include a keyword, such as $CONFIGURATION, or $COMMENT. The parameter keywords are not case-sensitive.
•
Some parameters (suppression state, visibility, or referenced configuration of a component) also include a component name and instance number. These parameters use this syntax: $KEYWORD@component where component is the name of the component, and instance is the instance number (an integer), in angle brackets. For example, the column labeled $CONFIGURATION@gear<2> controls the referenced configuration of the second instance of the component named gear. Values that are not item names (Yes, Suppress, and so on) are not case-sensitive. The syntax and legal values for each parameter type are described in other topics.
Multiple instances: You can specify multiple instances of a component in a single column header cell. Use the following syntax for the instance numbers: •
<*> all instances
•
<1-4> range of instances
•
<1,3,6> non-consecutive instances, separated by commas
•
<1,3-6,8> combination, separated by commas
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Example: This is an example of a design table that creates three configurations, adds a comment for each one, suppresses a feature, and controls a dimension.
Do not include any rows or columns with blank headers in the middle of the design table. The SolidWorks software stops evaluating the data when it reaches a row or column that has an empty header cell. Data that appears in or after a row or column with an empty header is ignored. Summary of Design Table Parameters
NOTES: •
When you use design tables in the SolidWorks software, it is important to format the tables properly.
•
The parameter syntax (header cells) are not case sensitive. Parameter Syntax (header cell)
Legal Values (body cell)
Default if Value is Left Blank
$configuration@part_name
configuration name
not evaluated
$configuration@
configuration name
not evaluated
$comment
any text string
empty
$partnumber
any text string
configuration name
$state@feature_name
Suppressed, S Unsuppressed, U
Unsuppressed
dimension@feature
any legal decimal value for the dimension
not evaluated
$parent
parent configuration name
property is undefined
$prp@property
any text string
property is undefined
$state@equation_number@equations
Suppressed, S Unsuppressed, U
Unsuppressed
$state@lighting_name
Suppressed, S Unsuppressed, U
Unsuppressed
$state@sketch relation@sketch name
Suppressed, S Unsuppressed, U
Unsuppressed
$user_notes
any text string
not evaluated
$color
32-bit integer specifying RGB (red, green, blue) color
zero (black)
Yes, Y No, N
No
Parts only
Parts and Assemblies
Assemblies only $show@component
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$state@component
Resolved, R, Suppressed, S
Resolved
$configuration@component
configuration name
Component's "in-use" or last saved configuration NOTE: If the component uses a derived configuration, and the value is left blank, the configuration used is linked to its parent.
$never_expand_in_BOM
Yes (never expand) No (allow to expand)
No
Dimensions in Design Tables Design tables can control dimensions as follows: •
In a part document, you can use a design table to control the dimensions in sketches and in feature definitions.
•
In an assembly document, you can control dimensions that belong to assembly features. This includes mates (angle or distance), assembly feature cuts and holes, and component patterns (spacing or instance count). You cannot control the dimensions of a component contained in the assembly.
The column header in a design table for controlling dimensions uses this syntax: Dimension@Feature or Dimension@Sketch For example, the full name for the depth of an extrude feature is D1@Extrude1; the full name for the dimension of the first Distance mate is D1@Distance1. You can use the Properties command to assign meaningful names to dimensions. The column header is not case sensitive. In the table body cells, type the value for the dimension. If a cell is left blank, it inherits the current dimension at the time the configuration is created. NOTES: •
When you specify values, be sure to use the system of units specified for the model document (click Tools, Options, Document Properties, Units).
•
You can display dimensions that are driven by design tables in a different color. Click Tools, Options, System Options, Colors. Select Dimension, Controlled by Design Table in System colors and change the color.
Example of a design table that controls feature dimensions:
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Dimensions The Dimensions dialog box appears after you select the Auto-create option in the Design Table PropertyManager and click OK
. The SolidWorks software asks you which dimensions you want to add to the design table.
NOTE: The Dimensions dialog box appears if the model has only one configuration. To add dimensions to the design table:
In the Dimensions dialog box, select the dimensions you want to add to the design table (hold down Ctrl to select more than one dimension), then click OK. Component Configuration The column header in a design table to control component configuration uses this syntax: $CONFIGURATION@component The column header is not case sensitive. In the table body cells, enter the name of the desired configuration. If you leave this table body cell blank, SolidWorks uses the component's "in-use" or last saved configuration. If the assembly configuration is derived, and the table body cell is left blank, the value of the component configuration used is linked to the assembly configuration's parent. Below is an example of a design table that controls a component configuration. Because the table body cell of Derived_config is left blank, the component configuration used is linked to Parent_config, which is Default.
Component Visibility The column header in a design table for controlling component visibility uses this syntax: $SHOW@component The column header is not case sensitive. In the table body cells, to show the model, enter Yes (or Y). To hide the model, enter No (or N). If a cell is left blank, the default is No (do not show the model). If the component uses a derived configuration, and the table body cell is left blank, the value of the component visibility used is linked to its parent.
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Example of a design table that controls component visibility:
Component Suppression State The column header in a design table to control the suppression state of a component uses this syntax: $STATE@component The column header is not case sensitive. In the table body cells, type the value for the desired suppression state: Suppressed (or S), or Resolved (or R). You cannot set a component to the lightweight state. If a cell is left blank, the default suppression state is Resolved. If the component uses a derived configuration, and the table body cell is left blank, the value of the component suppression state used is linked to its parent. Example of a design table that controls the suppression state of a component:
Suppression of Features In a part document, you can suppress any feature. In an assembly document, you can suppress features that belong to the assembly. These include mates, assembly feature holes and cuts, and component patterns. Sketches and reference geometry may also belong to an assembly. You cannot control the suppression of a feature that belongs to an individual assembly component. In a design table, there are two ways to specify the suppression of features. •
Method 1 (recommended). The column header for controlling feature suppression uses this syntax: $STATE@feature where feature is the name of the feature. For example, the column labeled $STATE@Hole1 controls the suppression of the first hole. In the table body cells, type the value for the desired suppression: Suppressed (or S), Unsuppressed (or U). If a cell is left blank, the default is Unsuppressed.
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Chapter 10 Configurations
•
Method 2. Type only the feature name in the column header cell. To suppress the feature, leave the table body cell blank. To include the feature, type any string in the body cell. This is the syntax that was used in SolidWorks 98 and earlier versions, and is included for backward compatibility.
You can also suppress individual features with the shortcut menu. To suppress individual features with the shortcut menu:
1.
Right-click the feature you want to suppress in the FeatureManager design tree and select Properties.
2.
In the dialog box:
3.
•
Select Suppressed.
•
Select This Configuration, All Configurations, or Specify Configuration(s).
Click OK.
Base Parts You can control the configuration of a base part with a design table. This is available in part documents only. The column header in a design table for controlling base part configurations uses this syntax: $CONFIGURATION@<part name> where <part name> is the name of the base part. The column header is not case sensitive. In the table body cells, type the base part's configuration names. For example, to use the default configuration of a base part named washer.sldprt, the column heading syntax is $CONFIGURATION@washer. The table body cell value is Default. Example of a design table that controls a base part configuration:
Component Part Number When you create configurations with a design table, the software automatically sets options in the Configuration Properties dialog box. Under Part number displayed when used in a bill of materials, the Configuration Name is selected. A bill of materials for an assembly that contains the document lists the part configuration name in the PART NO. column. In a design table, the $PARTNUMBER parameter lets you specify a different value for the PART NO. column of the BOM. For an assembly document, this is the part number used when this configuration of the assembly appears in the BOM as a sub-assembly. The column header uses this syntax:
10-28
$PARTNUMBER The column header is not case sensitive. In the table body cells, type the part number for each configuration. The $PARTNUMBER parameter now includes the document name or the parent name (derived configurations only) in a bill of materials. The following table shows values that can be used with this parameter: Value
Property Used
$DOCUMENT
Document name
$PARENT
Parent configuration name
$CONFIGURATION
Configuration name
any text
Custom name
blank
Configuration name
If multiple configurations of the same document are used in an assembly, the BOM lists each configuration by name as a separate item number. If you do not want each configuration listed separately in the BOM, do one of the following: •
Assign the same value for the $PARTNUMBER parameter in all the configurations.
•
After the design table creates all of the configurations, edit the properties of each configuration, and select Document Name. To override the document name, you can use the Title specified under File, Properties for the component document.
Example of a design table that controls the value of a part number in a BOM with custom names:
Comment The Configuration Properties dialog box has a Comment box, where you can enter a description, or other additional information about the configuration. In a design table, the column header for entering information in this box for each configuration uses this syntax: $COMMENT The column header is not case sensitive. In the table body cells, enter the comments for the configuration. Comments are optional; if a cell is left blank, the Comment box is empty.
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Example of a design table with a comment parameter:
Equations in Configurations You can suppress or unsuppress equations in specified configurations. To suppress or unsuppress equations in specified configurations:
1.
Click Tools, Equations.
2.
In the dialog box, under the Active column, select or clear the check boxes next to the equations you want to unsuppress or suppress. When you clear a check box, you suppress the configuration.
3.
Click Configs.
4.
In the dialog box, select the configurations to which you want the equation to apply: This configuration, All configurations, or Specify configurations.
5.
Click OK.
6.
Click OK again to close the Equations dialog box.
7.
Click Rebuild
.
The equation is applied to the selected configurations. To suppress or unsuppress equations in a design table:
The column header in a design table for controlling equations uses this syntax: $STATE@equation_number@EQUATIONS The column header is not case sensitive. In the table body cells, type S for suppressed or U for unsuppressed. Example of a design table that controls the suppression state an equation:
10-30
Expand in BOM You can control how the assembly is listed in a BOM, when this configuration is used as a sub-assembly. The column header in the design table uses this syntax: $NEVER_EXPAND_IN_BOM This corresponds to the Don’t show child components in BOM when used as sub-assembly option in the Configuration Properties dialog box. The column header is not case sensitive. •
When turned off, the sub-assembly is expanded if you select either Parts only or Indented assemblies when you insert the BOM.
•
When turned on, the sub-assembly is never expanded, regardless of the option you select when you insert the BOM. The effect is the same as selecting Top level only.
In the table body cells, to turn on the option (never expand) type Yes (or Y). To turn off the option (allow to expand), type No (or N). If a cell is left blank, the default is No. Example of a design table that controls how the assembly is listed in a BOM:
Lighting in Design Tables Lights in the Lighting
folder can be suppressed in a design table.
The column header in a design table for controlling lights uses this syntax: $STATE@ For example, to control the suppression state of a directional light, the column heading syntax is $STATE@Directional1. The column header is not case sensitive. In the table body cells, type S for suppressed or U for unsuppressed. Example of a design table that controls lights:
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Chapter 10 Configurations
Split Parts You can control the configuration of a split part with a design table. This is available in part documents only. The column header in a design table for controlling split part configurations uses this syntax: $CONFIGURATION@ where is the name of the split feature. The column header is not case sensitive. In the table body cells, type the base part's configuration names. For example, to use the default configuration of the base part for a split feature named Stock-Part1-1.sldprt, the column heading syntax is $CONFIGURATION@Stock-Part1-1. The table body cell value is Default. Example of a design table that controls a split part configuration:
Custom Properties The column header in a design table to specify a custom property uses this syntax: $PRP@property where property is the name of a custom property. You can use one of the custom properties listed in the Summary Information dialog box (click File, Properties, Configuration Specific), or you can add a new custom property. NOTES: •
The column header is not case sensitive.
•
If you plan to use the custom properties as columns in the bill of materials, do not use property names that contain spaces.
For example, use the header $prp@Cost to control the custom property Cost for each configuration. In the table body cells, type the property value for each configuration. If a cell is blank, the property is undefined for the configuration. Properties that are associated with model parameters (dimensions and mass properties) update automatically when the model parameters change. To add a custom property to a design table:
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1.
Insert a design table into your model.
2.
In the design table spreadsheet: a.
For each column with a custom property, label the column in the form $prp@property; for example, $prp@length.
b.
In each column, type in the variable name of the property in the form "name@@configuration@model"; for example, "D2@Sketch1@@[email protected]".
Include the quotation marks and be sure the file name extension (.SLDPRT) is uppercase. c. 3.
In new columns, add the standard design table information, for example, D2@Sketch1 as the header, and dimension values in the column.
Click outside the design table to close it. Custom properties added in a design table appear automatically on the Configuration Specific tab of the Summary Information dialog box. You can use these properties in Notes and Bills of Materials. Example of a design table that specifies custom properties:
User Notes The design table can include additional columns or rows for information only (notes, intermediate calculations, and so on). Use the keyword $USER_NOTES in the header of any column or row that you do not want evaluated. You may use as many of these rows or columns as you need. However, you may not include rows or columns with empty headers in the middle of the table. The column header is not case sensitive. Example of a design table that uses notes:
Color Parameter The design table can include a column for configuration-specific colors. The value is a 32-bit integer that specifies RGB (red, green, blue). If no value is specified, zero (black) is used. If you know the 32-bit integer value of a color, you can type the number directly into the design table in a column with the $COLOR parameter as the header. If you do not know the 32-bit integer value, you can calculate it in the design table with the RGB component values. To determine the red, green, and blue components of a color:
1.
Click Edit Color on the Standard toolbar.
2.
In the PropertyManager, under Color Properties: a.
Click a color in Pick a Color palette.
b.
Select RGB.
c.
Select Numeric.
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Chapter 10 Configurations
d.
Note the component numbers next to Red Component of Color , and Blue Component of Color
3.
Click OK
, Green Component of Color
.
.
To calculate a color value in a design table:
1.
Click Insert, Design Table.
2.
In the Design Table PropertyManager, choose the design table settings, then click, choose the design table settings, then click OK
3.
.
In the design table: a.
Type $USER_NOTES in cells B2, C2, and D2, and type $COLOR in cell E2. The column header is not case sensitive. You may have to insert columns so that these parameters appear in cells B2 through E2.
b.
Type integers in cells B3, C3, and D3 for the red, green, and blue components of a color.
c.
Type the following formula in cell E3: = MAX(MIN(B3,255),0) + MAX(MIN(C3,255),0)*16*16 + MAX(MIN(D3,255),0) *16*16*16*16 The formula ensures that each component value is between zero and 255. Make sure there are no extra spaces before the = sign in the cell.
d.
Type other color components in the appropriate rows and copy the formula, adjusted for the row number, into the corresponding cells in column E.
The following table lists some typical colors, their components, and the equivalent integer values. Color
Red
Green
Blue
Integer
Black
0
0
0
0
Red
255
0
0
255
Orange
255
128
0
33023
Green
0
255
0
65280
Blue
0
0
255
16711680
Purple
255
128
255
16744703
Turquoise
0
255
255
16776960
White
255
255
255
16777215
If the color for wireframe and HLR modes is the same as the color for shaded mode, the configuration-specific color applies to all three modes. If the color is not the same for all three modes, then the configuration-specific color applies to shaded mode only. To set the color the same for wireframe, HLR, and shaded modes:
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1.
Click Tools, Options, Document Properties, Colors.
2.
Select Apply same color to wireframe, HLR and shaded.
3.
Click OK.
Design Tables in Drawings Design Tables in Drawings If a model document uses a design table to generate multiple configurations, you can display the table in a drawing of that model. This way, a single drawing can represent all the configurations. You can label the dimensions with letters or short, descriptive names, instead of using the full dimension names and the values. For example, instead of D1@BaseExtrude, you can use a label such as A or thickness as the column header in the table, and display the label instead of the value of the dimension in the drawing view. Displaying a Design Table in a Drawing 1.
2.
In the part or assembly document, edit the design table as needed. The design table is displayed in the drawing exactly as it appears in the model document. •
Drag the resize handles on the corners and sides of the table to adjust the boundaries of the table. Make sure that all the rows and columns that you want are displayed, and remove any empty rows or columns.
•
Hide any rows (or columns) in the middle of the table that you do not want to display in the drawing. Right-click the numbered cell at the left of the row (or the lettered cell at the top of the column) to select the whole row (or column), and select Hide.
•
Adjust the column width, row height, text alignment, borders, fonts, and so on, as needed to meet your company standards.
If you want to use labels (letters or names) for the dimensions: a.
Insert a new row between the header row (the row containing the full dimension names) and the row for the first configuration.
b.
In the new row, type a label for each dimension.
c.
Hide the header row as described in step 1.
3.
In a drawing of the part or assembly, select a drawing view.
4.
Click Insert, Tables, Design Table. The design table appears, and you can drag it into place on the sheet.
5.
If you need to change the size of the design table, right-click the table, and select Properties.
6.
In the dialog box, specify a value for Width or Height, or type a Scale value, then click OK. To restore the table to its original size, right-click the table, and select Reset Size.
7.
If you are using labels, modify the dimensions in the drawing view: a.
Right-click a dimension, and select Properties.
b.
In the dialog box, click Modify Text.
c.
Delete (the placeholder for displaying the dimension value) from the middle line, then type the corresponding label from the table.
d.
Click OK.
e.
Click OK again to close the Dimension Properties dialog box.
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Chapter 10 Configurations
Design Table in a Drawing The following illustrates how a design table and the dimensions it controls might appear in a drawing.
Editing a Design Table in a Drawing
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1.
Double-click the design table in the drawing. The model opens in its own window, and the design table opens for editing.
2.
Modify the table as needed. When you are done, click outside of the table to close it.
3.
Return to the drawing window, and click Rebuild
to see the updated table.
11 Drawings
Drawings Overview You can create 2D drawings of the 3D solid parts and assemblies you design. Parts, assemblies, and drawings are linked documents; any changes that you make to the part or assembly change the drawing document. One-way associativity can be set between drawings and models during the software installation. This prevents changes to model dimensions, thereby preventing changes to the model itself from within a drawing. This option can be reset only with a new installation of the software. Generally, a drawing consists of several views generated from the model. Views can also be created from existing views. For example, a section view is created from an existing drawing view. When you select a view on a drawing sheet, the view name appears in the PropertyManager title. You can open existing drawings from inside part and assembly documents. Right-click the top item in the FeatureManager design tree or anywhere on the model in the graphics area and select Open Drawing. SolidWorks looks for a drawing with the same name as the model, in the same folder as the model. If the drawing exists, it opens automatically. If such a drawing is not found, a browse window appears so you can locate a drawing manually. To replace components in assembly drawings, use File, Open and click References. Edit the references in the Edit Referenced File Locations dialog box. When you open a drawing of a large assembly, you are prompted with the option to open the drawing in Large Assembly Mode. When you save or close a drawing without all the sheets loaded into memory, you are prompted to update the drawing. If you choose to update, all drawing views on all sheets are updated. The prompt appears only once per drawing document per SolidWorks session. If you choose not to update, the views on sheets that were not loaded do not appear in the SolidWorks view-only mode or in the SolidWorks Viewer. Topics about drawings include: •
Setting options
•
Creating a Drawing
•
Customizing Sheet Formats
•
2D sketching in drawings
•
Drawing Documents
•
Creating standard views (model views and standard 3 views)
•
Creating derived views, such as detail, section, projected, broken, and so on
•
Aligning and displaying views
•
Printing and sending drawings
Dimensions, notes, datums, geometric tolerances, and other annotations are discussed in Detailing.
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Chapter 11 Drawings
Getting Started in Drawings Setting Options for Drawing Documents A variety of options customize drawings to your company’s standards and to the requirements of your printer or plotter. System drawing options Click Tools, Options, System Options, Drawings. Specify various display and update options for views. The settings on the System Options tab apply to all documents. Other system options for drawings are found under the following topics: •
Display Style. Drawing view display mode and tangent edge display.
•
Area Hatch/Fill. Hatch or solid fill, pattern, scale, and angle of area hatches.
•
Large Assembly Mode. Default settings for performance of drawings of large assemblies.
Document-specific detailing options Click Tools, Options. On the Document Properties tab, select Detailing. The settings on the Document Properties tab apply to the active document only. Other document properties for drawings are found under the following topics: •
Dimensions
•
Notes
•
Balloons
•
Arrows
•
Virtual Sharps
•
Annotations Display
•
Annotations Font
•
Tables
•
View Labels
Page Setup Set to meet your printer or plotter requirements. Click File, Page Setup to specify such properties as page margins and orientation, scale of printed drawing, and custom headers and footers. Drawing sheets You can customize the following properties of drawing sheets: •
Sheet Format. Customize information blocks and text.
•
Sheet Properties. Change the sheet size and orientation, sheet scale, and 1st or 3rd angle projection.
Templates Customize drawing templates to conform to the standards of your workplace. You can set drawing, detailing, and standards options in templates. You can also save drawing documents to be used as drawing templates. Tables (Bills of Materials, Hole Tables, Revision Tables, and Weldment Cut Lists) also use templates that you can customize and save.
11-2
Creating a Drawing Drawings consist of one or more views generated from a part or assembly. The part or assembly associated with the drawing must be saved before you can create the drawing. You can create a drawing from within a part or assembly document. Drawing files have the .slddrw extension. A new drawing takes the name of the first model inserted. The name appears in the title bar. When you save the drawing, the name of the model appears in the Save As dialog box as the default file name, with the default extension .slddrw. You can edit the name before saving the drawing. To create a drawing from within a part or assembly document:
1.
Click Make Drawing from Part/Assembly
on the Standard toolbar.
2.
Select a Sheet Format/Size, then click OK.
3.
Specify properties in the Model View PropertyManager, then place the view in the graphics area.
To create a new drawing:
1.
Click New
on the Standard toolbar, or click File, New.
2.
In the New SolidWorks Document dialog box, select Drawing
3.
Select a Sheet Format/Size, then click OK.
4.
In the Model View PropertyManager, select a model from Open documents or browse to a part or assembly file.
5.
Specify options in the PropertyManager, then place the view in the graphics area.
, then click OK.
Sheet Format/Size You select a sheet format when you open a new drawing. The standard sheet formats include links to system properties and custom properties. Sheet formats help create drawings with a uniform format. Drawing sheet formats are OLE documents in which you can embed objects such as bitmaps. To select a sheet format:
1.
Click New
2.
Select Drawing
3.
Select from the following, then click OK. •
•
on the Standard toolbar. , then click OK.
Standard sheet size. Select a standard sheet size, or click Browse and locate a custom sheet format file. o
Reload. If you make changes to the Sheet Format, click to return to the default format.
o
Display sheet format. Display border, title block, and so on.
Custom sheet size. Specify a Width and Height.
To select a different sheet format in an existing drawing document, right-click in the graphics area and select Properties. To save a sheet format, click File, Save Sheet Format.
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Chapter 11 Drawings
Sheet Properties You can set the sheet properties when you add a sheet to a drawing or modify existing sheet properties. To specify sheet properties:
1.
In the active drawing sheet, right-click the sheet icon in the FeatureManager design tree, or in any blank area of the drawing sheet, or on the sheet tab at the bottom of the drawing window, and select Properties. - or For a drawing sheet that is not active, right-click the sheet icon in the FeatureManager design tree, or on the sheet tab at the bottom of the drawing window, and select Properties. - or Right-click in any blank area of the drawing sheet, or on the sheet tab at the bottom of the drawing window, and select Add Sheet.
2.
Specify properties as described below and click OK.
Name. Enter a title in the box. Scale. Set a scale for the sheet. Type of projection. Select First angle or Third angle for Standard 3 View projection. Next view label. Specify the letter of the alphabet to be used for the next section and detail views. Next datum label. Specify the letter of the alphabet to be used for the next datum feature symbol. Sheet Format/Size •
•
Standard sheet size. Select a standard sheet size, or click Browse and locate a custom sheet format file. o
Reload. If you make changes to the Sheet Format, click to return to the default format.
o
Display sheet format. Display border, title block, and so on.
Custom sheet size. Specify a Width and Height.
Use custom property values from model shown in. If more than one model is shown on the sheet and the drawing contains notes that are linked to custom properties of a model, select the view thatcontains the model whose properties you want to use. If you do not specify otherwise, the properties of the model in the first view inserted into the sheet are used. See Linking Notes to Document Properties.
Multiple Drawing Sheets You can add sheets to the drawing at any time. To add a sheet:
1.
Click Insert, Sheet. You can also right-click any sheet tab or any sheet icon in the FeatureManager design tree, and select Add Sheet.
2.
The Sheet Properties dialog box appears, with the default name of the next new sheet in sequence, for example, Sheet2.
3.
Specify the sheet details as described in Sheet Properties, and click OK.
To view a different sheet:
•
Click the sheet tab of the desired sheet.
•
Right-click the sheet tab or the sheet icon in the FeatureManager design tree, and select Activate.
To delete a sheet:
1.
Right-click any sheet tab or any sheet icon in the FeatureManager design tree, and select Delete. You can also click anywhere in the graphics area and press Delete to delete the active sheet.
2.
11-4
Click Yes in the Confirm Delete dialog box.
Sheet Formats, Sheets, and Views Ownership of items in drawings is dependent on what is active when the item is created. Sketch entities, notes, and other items can belong to the drawing sheet, to an individual view, or to the drawing sheet format. In general, you must activate the owner of an item in order to edit the item. NOTE: Dimensions and annotations that are attached to model geometry are exceptions to this rule. They belong to the view where they are attached, regardless of whether the view is active when you create the item. For example, you can activate a view, and create a construction line that belongs to the view. If you move or delete the view, the construction line is moved or deleted also. To edit the construction line, you must activate the view again. You can create the same construction line on the sheet, when no view is active. However, if you move or delete the views on the sheet, the construction line is not affected. To edit the construction line, the sheet itself must be active. Similarly, you must activate the sheet format to edit any items that are owned by the sheet format. While the sheet format is active, the sheet is hidden, including all the items that belong to the sheet, and all the views.
Customizing Sheet Formats You can customize drawing sheet formats to match your company’s standard format. The sheet formats provided with the SolidWorks software do not conform to any standard. However, the following linked custom properties are automatically included in all the provided sheet formats and are populated if the information is in either the system properties or the custom properties of the drawing document. System properties are automatically available when you insert a note. You enter custom properties on the Summary Information - Custom tab for drawing, part, or assembly documents as appropriate. System properties linked to fields in the system sheet formats
SW-File Name (in DWG. NO. field) SW-Sheet Scale SW-Current Sheet SW-Total Sheets Custom properties of drawing documents linked to fields in the system sheet formats
CompanyName CheckedBy CheckedDate DrawnBy DrawnDate EngineeringApproval EngAppDate ManufacturingApproval MfgAppDate QAApproval QAAppDate Custom properties of parts or assemblies linked to fields in the system sheet formats
Description (in TITLE field) Weight Material Finish Revision To edit the drawing sheet format:
1.
Click Edit, Sheet Format, or right-click any blank area on the drawing sheet, or the sheet icon in the FeatureManager design tree, and select Edit Sheet Format. If the sheet does not already have a sheet format, you create one if you select Edit Sheet Format, then click Rebuild.
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Chapter 11 Drawings
2.
Edit the sheet format as described below.
3.
Click Edit, Sheet, or right-click any blank area on the drawing sheet, or the sheet icon in the FeatureManager design tree, and select Edit Sheet.
To edit existing text in the title blocks:
Double-click the text. You can edit the text in place, then click outside the text box to exit the edit mode. - or Right-click and select Properties. The Note PropertyManager appears. Change any items you wish, and click OK
.
To move, delete, or add lines or text:
•
To delete, click the line or text and press the Delete key.
•
To move, click the line or text and drag to a new location.
•
To add lines, click Line
•
To add text, click Note on the Annotations toolbar, or click Insert, Annotations, Note. Specify the text properties, then click to place the text in the desired location.
, or Tools, Sketch Entity, Line.
Table Anchor Points The standard sheet formats supplied with the software include anchor points for placing the tables in specific locations on the sheet. To set the anchor points, expand SheetFormats for the sheet in the FeatureManager design tree. Right-click one of the four anchors, select Set Anchor, then click where you want the anchor point on the sheet. When you set the anchor point from the FeatureManager design tree, you are automatically in Edit Sheet Format mode. When you are finished, right-click in the graphics area and select Edit Sheet. You can also right-click a sketch point in the sheet format, and select Set as Anchor, one of the four anchors. The anchor point is highlighted, and its visibility toggles when you click the icon. NOTE: You can add an anchor point to drawings that you created in versions earlier than SolidWorks 98Plus. Right-click the sheet, and select Edit Sheet Format. Then right-click a sketch point (add one if needed), and select Set as Anchor. If the sheet does not already have a sheet format, you create one when you perform this procedure. OLE Objects To add objects from other applications, such as bitmaps of your company logo, standard note text from a file, and so on, click Insert, Object. You can either create a new object or insert one from a file. Objects can be linked or embedded in drawing sheet files.
Saving Sheet Formats To save the sheet format:
1.
Click File, Save Sheet Format.
2.
Edit File name. You can overwrite standard formats or create custom formats. Sheet format files have extension .slddrt and are located in\data.
3.
Click Save. Custom properties in the document are saved with the sheet format and added to any new documents that use the format.
11-6
Linking Notes to Document Properties To automatically insert information in a drawing, you can link note text in the drawing sheet or drawing sheet format to document properties. For the procedure to add a link in a note, see Link to Property. All SolidWorks documents have the following system-defined properties: Property Name
Value
SW-Author
Author field in Summary Information dialog box
SW-Comments
Comments field in Summary Information dialog box
SW-Configuration Name
Configuration name in ConfigurationManager of part or assembly
SW-Created Date *
Created field in Summary Information dialog box *
SW-File Name
document name, no extension
SW-Folder Name
document folder with backslash at the end
SW-Keywords
Keywords field in Summary Information dialog box
SW-Last Saved By
Last Saved By field in Summary Information dialog box
SW-Last Saved Date *
Last Saved field in Summary Information dialog box *
SW-Long Date *
current date in long format *
SW-Short Date *
current date in short format *
SW-Subject
Subject field in Summary Information dialog box
SW-Title
Title field in Summary Information dialog box
*The formats of the dates are language and region dependent. For details, see Start/Settings/Control Panel/ Regional Settings/Date on your computer. Additionally, drawings have the following system-defined properties: Property Name
Value
SW-Current Sheet
sheet number of the active sheet
SW-Sheet Format Size
sheet size of the active sheet format
SW-Sheet Name
name of the active sheet
SW-Sheet Scale
scale of the active sheet
SW-Template Size
template size of the drawing template
SW-Total Sheets
total number of sheets in the active drawing document
You can link a note to the properties of the model shown in the drawing (the SW-File Name property, for example, or a user-defined custom property in the model document). While you are editing the sheet format, a variable for the property name is displayed (in the form $PRP: "<property name>"). When you return to editing the sheet, the value of the property, if found, is displayed. If the property value cannot be found, the note displays ERROR!. To show or hide the error message, click View, Show Annotation Link Errors. A linked note can include additional text, and it can include links to more than one property. For example, to display the current sheet number and the total number of sheets, you can add this note: SHEET $PRP:"SW-Current Sheet" OF $PRP:"SW-Total Sheets" On the sheet, the property values are displayed: SHEET 1 OF 2 (on the first sheet of a two-sheet drawing)
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Chapter 11 Drawings
The Drawing Window The drawing window includes a FeatureManager design tree that is similar to the design tree in the part and assembly windows. The FeatureManager design tree for drawings consists of a hierarchical list of items pertaining to the drawing. There is an icon for each sheet; under each sheet, there are icons for the sheet format and each view. You can reorder sheets of drawing documents in the FeatureManager design tree. Drag one sheet at a time to the desired location. The sheet tabs are updated automatically. A symbol beside an item’s icon indicates that it contains associated items. Click the display its contents.
to expand the item and
Standard views contain the feature list for the part or assembly shown in the view. Generated views, such as detail or section views, contain different, view-specific items (detail circles, section lines, and so on). You can zoom to a view by right-clicking the view and selecting View, Zoom to Selection or right-clicking the view name in the FeatureManager design tree and clicking Zoom to Selection. You can zoom to the sheet by right-clicking the sheet name in the FeatureManager design tree and clicking Zoom to Selection. The drawing window has rulers at the top and left side. The rulers (and the status line) show the position of the pointer on the sheet. To turn the ruler display on or off, click View, Rulers. To specify the major and minor ruler line graduations, click Tools, Options, Document Properties, Grid/Snap. Specify the Major grid spacing and Minor-lines per major settings. Some types of views are linked to their parent views: Detail, Section, Auxiliary, and Projected Views, for example. Right-click on the detail circle or section line and select Jump to Detail View (or Section View). Right-click the child view and select Jump to Parent View. Projected Views (including the side and top views of Standard 3 Views) and Auxiliary Views have jumps only from the child to the parent.
Views of Parts and Assemblies You can generate drawings of a part or assembly in a variety of view types: Standard 3 View, Model, and Relative views. The part or assembly document must be saved before you can create drawing views of it. •
From existing views on the active sheet, you can create Projected, Auxiliary, Detail, Crop, Section, Aligned Section, Broken-out Section, or Broken views.
•
Explode lines in exploded views of assemblies are displayed in drawings of the exploded configurations.
•
You can also create an Empty view for sketching or annotations. For more information, see 2D Sketching.
For some operations, you need to select a view; for others, you activate a view. •
Selecting a view allows you to create a projected view, to insert break lines for a broken view, to move the view on the sheet, and to resize the view boundary. A selected view has a green border (blue in Detached drawings) with drag handles. To select a view, click an empty area within the view boundary.
•
Activating a view allows you to sketch entities in that view. This is necessary for sketching section lines, and for defining profiles for detail views. To edit the sketch entity, the view to which it belongs must be active. The border of an active view is a shadowed box.
You can set an option that causes drawing views to activate automatically when the pointer passes over them. Click Tools, Options, System Options, Drawings. Select or clear the Dynamic drawing view activation check box. •
When Dynamic drawing view activation is selected, the view closest to the pointer position is activated automatically. To stop the dynamic activation temporarily, you can lock the focus on a view or on the sheet. Right-click the view or the sheet, and select Lock View Focus or Lock Sheet Focus.
•
Lock View Focus allows you to add sketch entities to a view, even when the pointer is close to another view. You can be sure that the items you are adding belong to the view you want.
•
Lock Sheet Focus allows you to add sketch entities to the sheet. Otherwise, the sketch entities belong to the view that is closest to where you begin sketching. To return to dynamic activation mode, right-click again, and select Unlock View Focus (or double-click a different view) or Unlock Sheet Focus (or double-click any view).
11-8
•
When Dynamic drawing view activation is cleared, double-click anywhere within a view’s boundary to activate the view, or right-click within the boundary and select Activate View. To de-activate a view, either double-click again, activate a different view, or right-click and select Activate Sheet.
View Boundaries When the pointer passes over the edge of a drawing view, the view boundary is highlighted. The size of the view boundary is calculated automatically, based on the size, shape, and orientation of the model shown in the view. You can adjust the size of the view boundary (enlarging the view boundary may make it easier to select or activate a view). You cannot make the view boundary smaller than the model displayed in the view. View boundaries, and the views they contain, can overlap. To change the size of the view boundary:
1.
Select the view.
2.
Point to a green drag handle at the corner or side of the boundary.
3.
When the pointer changes to resize
, drag the handle as needed to resize the boundary.
To turn the boundary display on/off:
Click Tools, Options, System Options, Drawings. Select the Display drawing view borders check box. When selected, the boundary of each view is displayed as a thin gray box. When cleared, the boundaries are hidden. This option applies to all the views in the drawing. Even if the boundaries are hidden, they still are highlighted when the pointer passes over them, and an active view still displays a shadowed box. If the model contained in the view is not in the active or last-saved configuration, the border is dashed.
Scales in Drawings Scales in drawings apply to sheets or views. The scale for the active drawing sheet appears in the status line at the bottom of the window, and the scale for the active view appears in the view PropertyManager. You can also scale a drawing when you print it. Setting Scales To set the scale of a drawing sheet:
•
For an existing drawing sheet, right-click the sheet and select Properties. In the Sheet Properties dialog box, edit the values of Scale.
•
For a new drawing sheet, right-click an existing sheet or the sheet tab and select Add Sheet, or click Insert, Sheet. In the Sheet Properties dialog box, edit the values of Scale for the new sheet. The scale of the drawing sheet applies to: o
New and existing drawing views that are not set to custom scales
o
New views that are not autoscaled
The default drawing sheet scale is 1:1. To set the scale of a drawing view:
•
For existing drawing views, select a view or views. In the view PropertyManager, select Use parent scale or Use sheet scale, or select Use custom scale and edit the values.
•
For new drawing views where the PropertyManager appears during view insertion (such as Model, Projected, Predefined, and so on), select Use custom scale under Scale in the PropertyManager and edit the values.
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Chapter 11 Drawings
Autoscaling •
Automatically scale new drawing views in the Drawings Options controls the scaling of new views as follows: o
o
When selected, the SolidWorks software automatically scales the views to best fit on the drawing sheet, and the scale of the drawing sheet becomes the same as the scale of the views. When cleared, the views are inserted at the scale of the drawing sheet. When you insert Projected Views, Auxiliary Views and Section Views, the scale is set to Use parent scale. If you change the scale of a parent view, the scale of all child views that use the parent scale is updated.
•
If a drawing sheet contains multiple Predefined Views, the views are scaled automatically when a model is inserted. If a drawing sheet contains only one Predefined View, the view uses the Custom Scale, if specified, or (if no scale is specified) the drawing sheet scale.
Dimension Type Dimensions in drawings are either: •
True. Accurate model values.
•
Projected. 2D dimensions.
The dimension type is set when you insert a drawing view. You can view and change the dimension type in drawing view PropertyManagers. The rules for dimension type are: •
SolidWorks specifies Projected type dimensions for standard and custom orthogonal views and True type dimensions for isometric, dimetric, and trimetric views.
•
If you create a projected or auxiliary view from another view, the new view uses Projected type dimensions, even if the original view used True type dimensions.
•
When inserting views in other orientations, such as custom views that are not orthogonal, you are prompted for the dimension type.
•
The dimension type does not change if you change the orientation of a named view.
Crosshatch in Drawings Crosshatch is added to drawings of section views, including section views of multibody parts and weldments. You can add a crosshatch pattern to a model face or a closed sketch profile in drawings with area hatch/fill. To set options for crosshatch patterns, in a part document click Tools, Options, Document Properties, Material Properties. Crosshatch patterns alternate between components in assemblies, or between bodies in multibody parts and weldments. Crosshatch identifiers are language-independent, so you can save a drawing in one language and open it in a different language, the crosshatch patterns are recognized.
2D Sketching in Drawings You can create drawing geometry using 2D sketched geometry only, without reference to existing models or assemblies. This sketched geometry can be controlled by relations (collinear, parallel, tangent, and so on), as well as parametric dimensions. To display a grid, right-click the active drawing sheet and select Display Grid.
11-10
Sketch tools and sketch relations work the same way in a drawing document as they do in a part or assembly document. The only difference is that instead of sketching on model planes or faces, you sketch on the drawing sheet or in an active view. For information about using sketch tools and sketch relations, see Sketching in SolidWorks and Geometric Relations. Empty View You can create an empty drawing view to contain your sketch geometry. When this view is activated, all sketch geometry added belongs to this view. The sketch geometry can then be scaled, moved, and deleted as a group while still retaining the editability of the individual sketch entities. To create an empty drawing view:
1.
Click Insert, Drawing View, Empty.
2.
Click to place the view in the graphics area.
3.
Resize as necessary.
Importing Sketch Geometry You can import DXF/DWG files into a SolidWorks drawing. Then you can insert that geometry into a sketch to create model features in a part. For more information, see DXF/DWG Files(*.dxf,*.dwg). 2D Emulator The SolidWorks software includes an add-in application that allows you to create sketch entities by entering commands in text form. For more information, see 2D Emulator.
Quality in Drawings Drawings take advantage of lightweight assemblies and optimized drawing files to improve performance in opening drawings and creating drawing views, especially for large assembly drawings. Drawings can be: •
High Quality. All model information is loaded into memory.
•
Draft Quality. Only minimum model information is loaded into memory. Used in Lightweight and Detached drawings. Some edges may appear to be missing, and print quality may be slightly degraded. You can annotate views in draft quality without resolving the model.
A drawing can contain views in both modes. The SolidWorks software sets the options so that most drawing views are created in High Quality, but views for assemblies in Large Assembly Mode are created in Draft Quality. To set the option for drawing view quality:
1.
Click Tools, Options, System Options, Display Style.
2.
Under Display quality for new views, select High Quality or Draft Quality, then click OK.
To set the option for views of assemblies in large assembly mode:
1.
Click Tools, Options, System Options, Large Assembly Mode.
2.
Under Drawings, Default display quality for new views, select High Quality or Draft Quality, then click OK.
If a drawing contains views in High Quality, and you set a component to lightweight, a message prompts you to convert the views to Draft Quality. You can set an option for SolidWorks to convert affected views automatically.
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Chapter 11 Drawings
To specify how to convert drawing views to draft quality:
1.
Click Tools, Options, System Options, Performance.
2.
Under Assemblies, Automatically convert drawing to draft quality when unloading components, select:
3.
•
Always - convert views to draft quality when components are set to lightweight.
•
Prompt - display a message with a choice to convert.
•
Never - do not convert any views.
Click OK.
To set assembly components to lightweight or resolved:
Right-click a component and select Set to Lightweight or Set to Resolved. When a component is lightweight, a feather appears on the part icon and when the pointer
in the FeatureManager design tree
hovers over the part in the graphics area.
Convert to Draft Quality When you insert a drawing view into a lightweight drawing, the view must be in Draft Quality for the drawing to remain lightweight. Click: •
Yes to convert the view to Draft Quality
•
No to continue in High Quality (the model is resolved)
To avoid this message: •
Select Always create Draft Quality views in the dialog box
•
Set the Display quality for new views to Draft Quality in Tools, Options, System Options, Display Style
Sending Drawing Documents Electronically You can send drawing documents by electronic mail. You can choose to send only the drawing itself, or you can send the drawing and all referenced documents. This function uses the electronic mail application installed on your system. To mail a drawing document to another computer:
1.
With a drawing document active, click File, Send To.
2.
In the Send Mail dialog box, select one of the following: •
Drawing_name.slddrw only
•
Drawing_name.slddrw and other documents it references A list of the referenced documents, the number of documents, and the combined size of the documents is displayed. NOTE: The size of the combined documents may be important to you because mailing large size documents may cause transmission problems. If you choose to send the drawing and referenced documents, you do not have to send all the documents. You can:
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•
Select a filename you do not want to send, and click Remove.
•
Select a removed filename and click Attach to replace the file.
•
Click Attach All to return all the removed files.
3.
Click OK to send the documents.
4.
Enter your mail password, the mailing address, and any other information requested by your mail application.
Types of Drawing Documents Drawing Documents Drawings are normally created with the model resolved; that is, all information about the model is available in the drawing document. You can improve performance in creating, opening, and working in drawing documents with the following: •
Detached Drawings. The model is not loaded into memory. Create when saving drawings. You can add detailing without the model. You are prompted when the model is required. When you load the model, it loads completely. You can save drawings as either resolved or detached, so you can save a detached drawing as a regular drawing and vice versa.
•
Lightweight Drawings. A subset of model data is loaded into memory; the remaining model data is loaded as needed. In a new drawing, create a lightweight drawing by specifying draft quality views. For existing drawings, select Lightweight when opening the drawing. Opening a lightweight drawing is faster than opening the same drawing with fully resolved models. You can toggle between resolved and lightweight mode while in a drawing. Lightweight is the default mode for Large Assembly Mode.
•
Reduced display data drawing files. Tessellated data for shaded and draft views is not saved with drawing documents when you clear the drawing option, reducing file size. The data is available in the model file. Resolved
Lightweight
Detached
yes
yes
no
normal
faster
somewhat slower (load required)
always resolved
resolve/lightweight
load completely, no unload
high
low
not as low as lightweight
not in all cases
yes
not in all cases
View creation
normal
faster
normal
Display quality
draft or high quality
draft only
draft or high quality
normal
feather on drawing view icon (for lightweight view) and on pointer (for lightweight part)
blue view border, axis and highlighting colors different, broken link on drawing icon and view icon
yes
no
yes
Model required Load, rebuild performance Resolve/load models Memory footprint Produce largest SolidWorks assembly drawings
Appearance
Line font per edge
Detached Drawings Detached drawings are designed so you can open and work in drawing files without the model files being loaded into memory or even being present. To create a detached drawing:
1.
Click Save on the Standard toolbar (for a new drawing) or File, Save As (for drawing that has been saved previously).
2.
In the Save As dialog box, select Detached Drawing (*.slddrw) for Save as type.
3.
Specify the file name, then click Save. You can save regular drawings as Detached drawings, and vice versa.
Detached drawings can be in Draft Quality, but they cannot be Lightweight drawings.
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Chapter 11 Drawings
View borders in Detached drawings are blue. When the referenced model is loaded into memory, the view borders change to the regular view border color. To see the view borders, select Display drawing view borders in Tools, Options, System Options, Drawings. In the FeatureManager design tree, the icons for Detached drawings display a broken link: Drawing icon for Detached drawing Drawing view icon for Detached drawing with model not loaded If the referenced model is needed for an operation within a Detached drawing, you are prompted to load the model file. You can load the model manually by right-clicking a view and selecting Load Model. When you create a drawing of a large assembly, a dialog box appears asking if you would like to use Detached format for the drawing because of improved performance. You can choose to use Detached format or continue with no change in format. When a Detached drawing is out of sync with its model, it prints with a watermark that states: SolidWorks Detached - Out-of-Sync Print Advantages of Detached Drawings You can send Detached drawings to other SolidWorks users without sending the model files. You also have more control over updating the drawing to the model. Members of the design team can work independently on the drawing, adding details and annotations, while other members edit the model. When the drawing and the model are synchronized, all the details and dimensions added to the drawing update to any geometric or topological changes in the model. Performance The time required to open a drawing in Detached format is significantly reduced because the model files are not loaded. Because the model data is not loaded into memory, more memory is available to process drawing data, which has significant performance implications for large assembly drawings. You have control over when to load the model, which takes time to load and update the drawing. File Size The Detached format requires storing more edge data and less surface data. Therefore, some files are larger when converted to Detached, while others are smaller. In general, if your drawings have section views, the file size should decrease. If the drawings do not have section views, the file size may increase. File size is directly related to the number of visible edges in the drawing. For example, if your parts have patterns of features with many instances, it is more likely that the file size will increase when converted to Detached format. Updating Views Some changes, such as changes to a section line, detail circle, scale, or projection angle, require a view update. When a drawing view requires an update, the view is displayed with a crosshatch pattern.
Working in Detached Drawings When opening a Detached drawing, the software checks all sheets in the drawing to be sure that they are synchronized with the model. If not, you are warned. If a Detached drawing is open, and you open a model document, either from File, Open or by right-clicking a view and selecting Open model name, the drawing does not synchronize with the model until you load the model.
11-14
To load the model:
1.
Right-click a view containing the model you want to load, and select Load Model. The Confirm Load Model dialog box appears.
2.
Select the Don't prompt me again in this or any future session check box if you want to prevent this message from appearing again.
3.
Click Yes to continue loading the model.
Operations Available in Detached Drawings Without the Model Following are some of the capabilities available when the model is not loaded: •
Save and Open drawings
•
Add o o
•
Annotations (Note, Surface Finish Symbol, Datum Feature Symbol, Datum Target, Geometric Tolerance, Weld Symbol, Center Mark)
o
New views (Empty, Detail, Crop)
o
New views of parts only (Auxiliary, Projected, Section, Broken-out Section)
o
Balloons (with asterisks, which are resolved to item numbers when the model is loaded)
o
Virtual sharps
Change o o
•
Dimensions
Scales of sheets or views Line Color, Line Style, and Line Thickness of model edges, silhouette edges, and sketch entities for both parts and assemblies
o
View alignments
o
Crop Views, and Auxiliary and Projected Views of parts
o
Bill of Materials, Balloons
Select o
Hidden Lines Removed (HLR), Hidden Lines Visible (HLV), Wireframe, and Tangent edge display. You can show views in Shaded mode if the views have previously been saved in Shaded mode. If any view is saved in Shaded mode, then all views of the same model can be shown in Shaded mode, and new views of the same model can be shown in Shaded mode.
o
Imported planes, sketches, origins, and axes
o
Section view edges
o
Cosmetic threads, including referencing and dimensioning
o
Model edges and vertices
o
Silhouette edges
o
Faces
o
Copy, Cut, and Paste views
•
Inference, reference, and dimension to model edges, vertices, and center points
•
Hide and show edges
•
Update the drawing with the Rebuild tool
•
Measure
•
True reference dimensions
•
View temporary axes
•
3D highlighting
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Chapter 11 Drawings
Operations Requiring the Model When the model is not loaded, the model entities do not appear in the FeatureManager design tree and the following operations are not available: •
•
Import o
Design Tables
o
Model items (dimensions, annotations, origins, planes, axes, or sketches)
o
Reference planes and axes into existing layers
Add o
•
o
Bills of Materials
o
Hole Callouts or Cosmetic Threads
Change o
o
•
New views (Standard 3 View, Named, Relative, Broken) and new views of assemblies (Auxiliary, Projected, Section, Broken-out Section)
Values or properties of feature dimensions (also origins and other reference geometry) imported from the model Hatch scales
Select o
Model faces
o
Surfaces
o
Component Line Font item from shortcut menu
•
Hide/Show Components or Hide Behind Plane
•
Export to non-SolidWorks file formats such as DXF/DWG
Lightweight Drawings Lightweight drawings are analogous to lightweight assemblies. When a drawing is lightweight, only a subset of its model data is loaded in memory. The remaining model data is loaded as needed. Performance of drawings of large assemblies is improved significantly with lightweight drawings. Loading a lightweight drawing is faster than loading the same drawing with fully resolved parts. Lightweight drawings are efficient because the full model data is loaded only as it is needed. Only parts that you select, and parts that are affected by changes that you make in the current editing session, become fully resolved. To load a drawing as lightweight:
When you open a drawing, select Lightweight in the Open dialog box. To set assembly components to lightweight or resolved:
Right-click a component and select Set to Lightweight or Set to Resolved. When a component is lightweight, a feather appears on the part icon and when the pointer
in the FeatureManager design tree
hovers over the part in the graphics area.
A feather in the FeatureManager design tree also indicates lightweight views
.
Lightweight drawings use Draft Quality views. You can specify new views to be Draft Quality in Tools, Options, System Options, Display Style. If you insert a view into a lightweight drawing as High Quality, you are prompted to convert the view to Draft Quality so that the drawing can remain lightweight. Detached drawings cannot be lightweight drawings.
11-16
With lightweight drawings, you can: •
Create all types of drawing views
•
Attach annotations to models in views
•
Specify edge properties
•
Highlight and dynamically select edges and vertices
•
Set drawings of sub-assemblies to lightweight or resolved
If you print a lightweight drawing when it is out of synchronization with its model, the drawing prints with a watermark: SolidWorks Lightweight - Out-of-Date Print
Standard Drawing Views Standard Drawing Views The standard views that generally begin a drawing are: Standard 3 View Model View Relative View Predefined View Empty View
Standard 3 View The Standard 3 View option under Insert, Drawing View creates three related default orthographic views of a part or assembly displayed at the same time. For information on the orientation of the Standard 3 View, see First Angle and Third Angle Projection. The alignment of the top and side views is fixed in relation to the front view. The top view can be moved vertically, and the side view can be moved horizontally. The top and side views are linked to the front view. Right-click a top or side view and select Jump to Parent View. The parent view can be on the same sheet or another sheet. For more information about arranging views on a sheet, see Moving Views and Rotating Views. There are several ways to create a Standard 3 View drawing. To create a Standard 3 View when starting a new drawing document:
1.
Open a new drawing.
2.
In the Model View PropertyManager, select a model from Open documents or browse to a model file, then click Next
.
3.
Under Orientation, select *Front, then place the view in the graphics area.
4.
With the Projected View PropertyManager open, place the two other views, then click OK
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Chapter 11 Drawings
Creating the Standard 3 View by the standard method:
1.
Open the part or assembly document, or a drawing document that contains a view of the model you want.
2.
Open a new drawing.
3.
Click Standard 3 View The pointer changes to
4.
on the Drawing toolbar, or click Insert, Drawing View, Standard 3 View. .
Select the model in one of these ways: •
To add the views of a part, in a part window, click a face, or anywhere in the graphics area, or click the part name in the FeatureManager design tree.
•
To add the views of an assembly, in an assembly window, click an empty region of the graphics area, or click the assembly name in the FeatureManager design tree.
•
To add the views of an assembly component, in an assembly window, click a face on the part, or click the name of either an individual part or a sub-assembly in the FeatureManager design tree.
•
In a drawing window, click a view that contains the desired part or assembly, either in the FeatureManager design tree or in the graphics area.
The drawing window returns to the front (if necessary) and the three views are placed in the drawing. Creating the Standard 3 View from a file:
If you prefer not to open the model document, you can still create a drawing of it. 1.
In a drawing, click Standard 3 View
.
2.
Right-click in the graphics area and select Insert From File.
3.
Browse to the desired model document, and click Open.
Creating the Standard 3 View by the drag-and-drop method:
The default view created when you drag and drop a part or assembly into a drawing is the Standard 3 View. 1.
Open a new drawing window.
2.
Drag a part or assembly document from Windows Explorer or from the Feature Palette window, and drop it into the drawing window, - or Drag the name from the top of the FeatureManager tree of an open part or assembly document, and drop it into the drawing window. The views are added to the drawing.
Creating the Standard 3 View from a hyperlink in Internet Explorer:
1.
In Internet Explorer (version 4.0 or later), navigate to a location that contains hyperlinks to SolidWorks part files. For example, on the SolidWorks web site, in the Support section, navigate to the Solid Modeling Library page. You may also be able to obtain SolidWorks parts from certain third-party vendors.
2.
Drag the hyperlink from the Internet Explorer window, and drop it in an open drawing window. The Save As dialog box appears.
3.
Navigate to the directory where you want to save the part, enter a new name if desired, and click Save. The part document is saved locally, and the views of the part are added to the drawing.
11-18
Standard 3 View PropertyManager Insert a part or assembly model into a drawing as a Standard 3 View. To insert a standard 3 view:
1.
In a drawing document, click Standard 3 View Standard 3 View.
on the Drawing toolbar or click Insert, Drawing View,
2.
Select a part or assembly document under Open documents - or Click Browse and browse to a file.
3.
Click OK
.
First Angle and Third Angle Projection Standard 3 Views are in either third angle or first angle projection. In third angle projection, the default front view from the part or assembly is displayed at the lower left. and the other two views are the top and right views. In first angle projection, the front view is displayed at the upper left and the other two views are the top and left views. For information about setting the default projection, see Sheet Properties.
3rd angle projection
1st angle projection
Model View The Model View PropertyManager appears when you create a new drawing, or when you insert a model view into a drawing document. You select an orientation for the view from the view names in the model document: •
Standard views (Front, Top, Isometric, and so on)
•
Current Model View (available only for open models and only until you place the view)
•
Custom views that you created by zooming and rotating the model, enabling Perspective if desired, then saving the view by name. The entire model is displayed, even if the selected view orientation displays a partial, zoomed-in view. You cannot activate a perspective view or add dimensions or annotations it.
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Chapter 11 Drawings
Example of Model View The drawing shows a Top View, an Isometric View, and a User-defined Model View.
To insert a model view into a drawing:
1.
Click Model View
on the Drawing toolbar, or click Insert, Drawing View, Model.
2.
In the Model View PropertyManager, select an Open document under Part/Assembly to insert, or browse to a part or assembly file. If you click Standard 3 View
, the PropertyManager changes to Standard 3 View, and the list of
open documents is available. Select a model and click OK 3.
Click Next
.
You can also click Standard 3 View of the selected model. 4.
to insert a Standard 3 View.
at this point, then click OK
to insert a Standard 3 View
Specify the view orientation, scale, and so on, then place the view. When you place the model view, if you selected an orthogonal view orientation, the Projected View PropertyManager appears. You can place any number of projected views for any orthogonal view in the drawing. To prevent the Projected View PropertyManager from appearing, clear Auto-start projected view under Options in the Model View PropertyManager.
5.
Click OK
.
To change the orientation of a model view:
11-20
1.
Select a model view.
2.
In the Model View PropertyManager, double-click a standard orientation or a custom orientation under Orientation.
Model/Predefined/Empty View PropertyManager This PropertyManager opens when you insert a Model View, a Predefined View, or an Empty View into a drawing, or when you select an existing Model, Predefined, or Empty View. The properties available depend on the type of view selected. Part/Assembly to insert Select a document from Open documents or click Browse and browse to a part or assembly file. The list of Open documents includes saved models (parts and assemblies) open in SolidWorks windows, plus models that already appear in drawing views, whether open in a window or not. Thumbnail Preview View a preview of the model selected in Open documents. Options Start command when creating new drawing. Available when inserting a model into a new drawing. The Model View PropertyManager appears whenever you create a new drawing. When you create a drawing with Make Drawing from Part/Assembly in a part or assembly document, the Model View PropertyManager appears even if you clear this check box. Auto-start projected views. Available when inserting an orthogonal view. The Projected View PropertyManager appears when you place an orthogonal model view. View Orientation View Orientation. Double-click a view orientation in the list to change the orientation of the selected view. Preview. Select to see a preview of the model while inserting a view. When cleared, only the outline of the view boundaries is shown. Insert Model For Predefined Views only. Select a model from the list under Part/Assembly of models open in the SolidWorks session, or click Browse and browse to a model file. Reference Configuration
For sheet metal flat patterns only. Select a model configuration name from the list. Flat Pattern Options
For sheet metal flat patterns only. Configuration name. You can edit the flat pattern configuration name (which appears underneath the model configuration name in the model ConfigurationManager) that appears in the box. Update Name. Click to update the configuration name in the Named View PropertyManager and in the model ConfigurationManager. View direction. Click Flip view to flip the view horizontally.
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Chapter 11 Drawings
Display Style Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Choose the scale for the view to be the same as the sheet scale or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). More Properties After you create a view or select an existing view, you can click More Properties to open the Drawing View Properties dialog box.
Relative to Model View A Relative to Model View is an orthographic view defined by two orthogonal faces or planes in the model and the specification of their respective orientations. Example of Relative to Model View A true view of an angled face perpendicular to the front face of a model is created as follows.
Specify the angled face as Front
11-22
Specify the front face as Left
Place the resulting view
To insert a relative view:
1.
Click Relative View
on the Drawing toolbar, or click Insert, Drawing View, Relative To Model. The
2.
pointer changes to . Select the model, using one of the methods described in Standard 3 View.
3.
Under Orientation, First orientation in the PropertyManager, select an orientation (Front, Top, Left, and so on), and select the face in the graphics area for that orientation in the drawing view.
4.
Under Second orientation, select another orientation, orthogonal to the first, and select another face in the graphics area for that orientation in the drawing view. A relative view can show one body or all the bodies in a model. To show one body, select both faces from the same body.
5.
Click OK
and return to the drawing document. The pointer changes to
.
6.
In the PropertyManager, select properties (Scale, Bodies, and so on), then click in the graphics area to place the view.
7.
Click OK
.
If the angle of the face in the model changes, the views update to maintain the orientation as originally specified. Relative View PropertyManager in Drawings The Relative View PropertyManager opens when you insert a Relative View into a drawing, or when you select an existing Relative View. When you go to a model document to select model faces, the PropertyManager displays different choices. Display Style Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality
•
Draft quality
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Use sheet scale. Use custom scale. Set a scale for the views.
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Bodies When placing a view of a model with multiple bodies, choose: •
Selected body. The body from which you have selected faces.
•
All bodies. All bodies in the model document.
Dimension Type Select either Projected or True. More Properties After you create the new view or select an existing view, you can click More Properties to open the Drawing View Properties dialog box. Relative View PropertyManager in Models When you create a Relative View in a drawing, you select planar faces in a model document as described below, then return to the drawing document to place the view. Orientation Select two faces in different orientations to define the orientation of the body in the relative view. To create a relative view of one body, select faces from the same body. •
First orientation. Select the orientation, then select a face in the graphics area.
•
Second orientation. Select the orientation, then select another face in the graphics area.
Drawing View Orientation Select the relative faces of a Relative to Model View in this dialog box. To create the relative view:
1.
Click on a face on the part.
2.
Select the direction you want the selected face to be orientated towards, then click OK.
3.
Click on a second face, then select its orientation and click OK.
4.
Activate the drawing window, and click where you want to place the Relative View.
Predefined Views You can define any orthogonal, projected, or named view in a drawing sheet and the populate the view. You can save a drawing document with predefined views as a document template. To insert a predefined view into a drawing:
1.
In a drawing document, click Predefined View
, or click Insert, Drawing View, Predefined.
2.
Click in the graphics area to place the view.
3.
In the Predefined View PropertyManager, select a View Orientation as Display Style, Scale, or Dimension Type.
4.
Click OK
.
You can populate the view as you insert it, or you can populate it later.
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and specify other options such
You can add Projected Views to a predefined view. For example, if you insert a front view, you can project top and right views to create a predefined Standard 3 View. Projected views are automatically oriented and aligned to the original view. You can copy and paste predefined views. To populate predefined views:
•
Drag. Drag a model from the FeatureManager design tree of an open part or assembly document into the drawing document. All available predefined views are populated.
•
Insert Model. Right-click in a predefined view and select Insert Model. In the Insert Model PropertyManager, select a model from the Open documents list, or click Browse and browse to a model file. The view and all its related views (such as projected views) are populated when you click OK
•
Select. Select a predefined view. In the Predefined View PropertyManager, under Insert Model, select a name from the Part/Assembly list of models open in the current session. The view and all its related views (such as projected views) are populated when you click OK
•
.
.
Browse. Select a predefined view. In the Predefined View PropertyManager, under Insert Model, click Browse and browse to a model file. The view and all its related views (such as projected views) are populated when you click OK
.
When you populate predefined views, the scale of the views is determined as follows: o o
If a drawing sheet contains more than one predefined view, the views are scaled automatically. If a drawing sheet contains only one predefined view, the view uses the Custom Scale, if specified, or (if no scale is specified) the drawing sheet scale.
Empty Views You can insert Empty Views into drawing documents. Empty views are often used to contain sketches in drawings. To insert an empty view:
1.
Click Empty View
, or click Insert, Drawing View, Empty.
2.
Click in the graphics area to place the view. The Empty View PropertyManager appears.
3.
Specify a Custom Scale if necessary and click OK
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Derived Drawing Views Derived Drawing Views The following types of drawing views are derived from other views, either from standard views or from other derived views. Projected View Auxiliary View Detail View Crop View Broken-out Section Broken View Section View Aligned Section View Alternate Position View
Projected View Projected views are created with the following tools: Standard 3 Views. The Front view is a model view and the other two views are projected views, using First angle or Third angle projection as specified in Sheet Properties. Model View. When inserting an orthographic model view, the Projected View PropertyManager appears so you can insert projected views from any orthographic views on the drawing sheet. Projected View. Insert projected views from any orthographic view. You can create a projected view of an exploded assembly view. To create a projection view:
1.
Click Projected View
on the Drawing toolbar, or click Insert, Drawing View, Projected.
The Projected View PropertyManager appears. 2.
Select a view from which to project. The pointer shape changes to
3.
.
To display an arrow indicating the direction of projection, select Display View Arrow. Type a label to be displayed with the parent view and the projected view. To select the direction of projection, move the pointer to the appropriate side of the selected view. A preview of the view is displayed, snapped to the nearest projection. To override the snapping behavior, hold Ctrl as you move the preview. To resume the snapping behavior while dragging, release Ctrl. You can project to the left, right, above, or below (in this example, the user moved the pointer to the right of the selected view).
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4.
To place more than one Projected View, click Keep Visible
.
5.
When the view is where you want it to be, click to place the view.
The projection view is placed on the sheet, aligned to the view from which it was created. By default, you can move a projection view only in the direction of the projection. For information about changing the alignment of views, see View Alignment and Display. Projection Views are linked from the child view to the parent. Right-click the Projection View and select Jump to Parent View.
Projected View PropertyManager The Projected View PropertyManager opens when you create a Projected View in a drawing, or when you select an existing Projected View. Arrow Arrow. Select to display a view arrow indicating the direction of the projection. Label
. Type text to be displayed with both the parent view and the projected view.
Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values.
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Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for projected views. More Properties For an existing Projected View, click More Properties to open the Drawing View Properties dialog box.
Auxiliary View An Auxiliary View is similar to a Projected View, but it is unfolded normal to a reference edge in an existing view. Example of Auxiliary View The angled edge on the front view is selected for the Auxiliary View, which is at the upper right, with a view arrow labeled C.
You can create an auxiliary view of an exploded assembly view. To create an auxiliary view:
1.
Click Auxiliary View
on the Drawing toolbar, or click Insert, Drawing View, Auxiliary.
The Auxiliary View PropertyManager appears. 2.
Select a reference edge (not a horizontal or vertical edge, which would create a standard Projection View). The reference edge can be an edge of a part, a silhouette edge, an axis, or a sketched line. If you sketch a line, activate the drawing view first. NOTE: Auxiliary views are not available from entities of section or detail views of parts in the FeatureManager design tree. As you move the pointer, a preview of the view is displayed. You can control the alignment and orientation of the view as follows: o
o
3.
Alignment. To override the default alignment as you place the auxiliary view, hold Ctrl as you move the preview. To resume the snapping behavior while dragging, release Ctrl. Orientation. You can toggle the view orientation (front or back) by dragging the view across the reference edge. An arrow shows the view orientation, which is useful when the Show contents while dragging view option is cleared. After you place the view, you can toggle the view orientation by double-clicking the arrow or by selecting Flip direction in the PropertyManager.
Move the pointer until the view is where you want, then click to place the view.
For information about changing the alignment of views, see View Alignment and Display. The view arrow (or set of arrows, if you use the ANSI dimensioning standard) indicates the orientation of the projection.
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To remove the arrow, select the Auxiliary View. In the PropertyManager, select or clear the Display view arrow check box and enter a label if desired (maximum of two characters). Auxiliary Views are linked to their parent views. Right-click the Auxiliary View and select Jump to Parent View. The parent can be on the same sheet or another sheet. Center Marks in Auxiliary Views are oriented to the viewing direction such that one of the lines of the Center Mark is parallel to the view direction. If you used a sketched line to create an Auxiliary View, the sketch is absorbed so you cannot delete it inadvertently. You can delete sketch entities while editing the sketch. To edit a sketched line used to create an auxiliary view:
1.
Select the Auxiliary View.
2.
In the Auxiliary View PropertyManager, select Display view arrow.
3.
Right-click the view arrow and select Edit Sketch.
4.
Edit the sketched line.
5.
Select the line and click Rebuild
to update the view.
Auxiliary View PropertyManager The Auxiliary View PropertyManager appears when you create a new Auxiliary View in a drawing, or when you select an existing Auxiliary View. Arrow Arrow. Select to display a view arrow indicating the direction of the auxiliary view. Label . Type text to be displayed with both the parent view and the auxiliary view. Specify the label display in Tools, Options, Document Properties, View Labels. Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style.
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Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for auxiliary views. More Properties For an existing Auxiliary View, click More Properties to open the Drawing View Properties dialog box.
Detail View You create a Detail View in a drawing to show a portion of a view, usually at an enlarged scale. This detail may be of an orthographic view, a 3D view, or a Section View. You cannot create a Detail View from the following: •
a named view that shows the model with perspective turned on
•
another Detail View
•
a Crop View
Detail views expand in the FeatureManager design tree so that all components and features are available. You can create a detail view of an exploded assembly view. To create a detail view:
1.
Activate an existing view.
2.
Click Detail View
on the Drawing toolbar, or click Insert, Drawing View, Detail.
The Detail View PropertyManager appears and the Circle 3.
tool is active.
Sketch a circle. NOTE: To create a profile other than a circle, sketch the profile before clicking the Detail View tool. Using a sketch entity tool, create a closed profile around the area to be detailed. You can add dimensions or relations to the sketch entities to position the profile precisely relative to the model. NOTE: If you plan to create a Broken View, you are advised to relate the sketch to the model. As you move the pointer, a preview of the view is displayed.
4.
When the view is where you want it to be, click to place the view.
The note on the detail view includes the letter label and view scale, if the scale is different from the sheet scale. Detail views are not aligned to other views by default, and may be moved freely to any location on the drawing sheet. If you wish to remove any sketches that are imported to the drawing, edit the model and hide any sketches that interfere with the Detail View. Detail Views are linked to their detail circles. Right-click the circle and select Jump to Detail View, which can be on the same sheet or another sheet. Right-click the Detail View and select Jump to Parent View.
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Example of Detail View The active view on the left shows the sketched profile (a circle) and the profile label (A). The Detail View on the right shows the Detail View note, which displays the label (A) and the scale (1:1).
Detail View PropertyManager The Detail View PropertyManager appears when you create a new Detail View in a drawing, or when you select an existing Detail View or detail circle. The PropertyManager controls the following properties: Circle Options •
Style
. Select either Circle or Profile. If you select Circle, various circle styles are available.
•
Label . Edit the letter associated with the detail circle and detail view. To specify the label format, click Tools, Options, Document Properties, View Labels.
•
Font. To choose a font for the detail circle label other than the document's font, clear the Document's font check box and click Font. If you change the detail circle label font, a message appears asking if you wish to also apply the new font to the detail view label.
View Options •
Full outline. Select to display the profile outline in the detail view.
•
Pin position. Select to prevent the detail view from moving if the parent view changes size.
•
Scale hatch pattern. Select to scale the hatch pattern based on the scale of the detail view.
Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style.
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Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for detail views. More Properties For an existing Detail View, click More Properties to open the Drawing View Properties dialog box. Modifying a Detail View To change the position or size of a profile:
1.
Select the profile.
2.
Drag the center point to change the position, or drag a side to change the size. The Detail View changes as the profile changes.
To change the profile by editing the sketch.
1.
Right-click the profile sketch and select Edit Sketch.
2.
Edit the profile as needed to change the shape or size. The pointer changes to
3.
Click Rebuild
when it is on the detail profile.
to update the detail view.
To select the profile display:
If you use a shape other than a circle as the profile, you can choose to display either the profile or its circle in the parent view. 1.
Select the Detail View or detail circle. The Detail View PropertyManager appears.
2.
Under Circle Options, Style, choose either Profile or Circle. •
If you select Circle as the display, you can choose the Style of the detail note, and you can drag the note anywhere except inside the circle.
•
If you select Profile as the display, you can drag the note anywhere except inside the profile.
You can choose whether the circle or profile is displayed by default in a new Detail View. Click Tools, Options, System Options, Drawings. Select or clear the Display new detail circles as circles check box. To change the scale of the Detail View:
1.
Select the Detail View or detail circle.
2.
In the Detail View PropertyManager, select Custom Scale, enter a new scale ratio, and click OK
.
The Detail View scale is displayed in the note if its scale is different from the sheet scale. To change the Detail View note text:
Double-click the note and edit the text in place. Click outside the note to exit. - or Right-click the text and select Properties. The Note PropertyManager appears. Modify the text and the text properties, such as font, justification, and so on and click OK. The label text on the detail profile also updates. Changes in font do not apply to the profile label.
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To change the text of the label on the detail profile:
Double-click the label and edit the text in place. Click outside the label to exit. - or Select the detail circle or label. The Detail View PropertyManager appears. Under Circle Options, modify the text and font. The Detail View note text also updates. A message appears asking if you want to apply the font change to the Detail View as well. To pin Detail Views:
You can pin Detail Views, to prevent them from moving if the parent view changes size. Select the Detail View. In the Detail View PropertyManager, under View Options, select Pin position. Detail Circle Styles Per Standard
ISO, JIS, DIN, BSI - No Leader ANSI - Broken Circle GOST -
Broken Circle
With Leader
No Leader
Connected
Crop View You can crop any drawing view except a Detail View, a view from which a Detail View has been created, or an exploded view. Crop View can save steps because you do not create a new view. For example, instead of creating a Section View and then a Detail View, then hiding the unnecessary Section View, you can crop the Section View directly. You cannot create a Detail View from a Crop View. To crop a view:
1.
Activate an existing view.
2.
Draw a closed profile with a sketch tool such as a circle.
3.
Click Crop View
on the Drawing toolbar, or click Tools, Crop View, Crop.
The view outside the profile disappears.
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A circle is drawn on this Section View
After cropping, only the view inside the circle is displayed.
To edit a Crop View:
1.
Right-click the view and select Crop View, Edit Crop, or select the view and click Tools, Crop View, Edit Crop.
2.
Edit the profile.
3.
Click Rebuild
to update the view.
To remove a Crop View:
Right-click the view and select Crop View, Remove Crop, or select the view and click Tools, Crop View, Remove Crop. The crop is removed and the view returns to its uncropped state.
Broken-out Section A broken-out section is part of an existing drawing view, not a separate view. A closed profile, usually a spline, defines the broken-out section. Material is removed to a specified depth to expose inner details. Specify the depth by setting a number or by selecting an edge in a related view. Use reference geometry to specify depth for precise section planes. You cannot create a broken-out section on an exploded detail, section, or alternate position view. Example of Broken-out Section This example shows (1) wall thickness and shaft and (2) how the shaft is welded to the cap.
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To create a broken-out section:
1.
Click Broken-out Section Section.
on the Drawing toolbar, or click Insert, Drawing View, Broken-out
The Broken-out Section PropertyManager appears with the pointer active. You are prompted to sketch a closed spline.
showing that the spline tool is
If you want a profile other than a spline, create and select a closed profile before clicking the Brokenout Section tool. 2.
Sketch a profile.
3.
In the PropertyManager, set the depth.
4.
Click OK
.
To delete or edit a broken-out section:
Right-click the broken-out section in the graphics area (the pointer changes to when it is over a broken-out section) or in the FeatureManager design tree and select one of the following. •
Delete.
•
Edit Definition. In the Broken-out Section PropertyManager, change the depth, then click
•
OK . Edit Sketch. Select the sketch entity and edit it. Select the sketch entity again and click Rebuild
.
Broken-out Section PropertyManager The PropertyManager for a broken-out section controls the following properties: Depth. Specify in one of the following ways: •
Depth Reference . Select geometry, such as an edge or an axis, in the same or a related view. The entity name appears in the Depth Reference selection box.
•
Depth
. Enter a number in the Depth box.
Use reference geometry to specify depth for precise section planes. Preview. When selected, the broken-out section is displayed as you change the depth. When cleared, the broken-out section is applied when you exit from the PropertyManager. Auto hatching. For assemblies only. If selected, the software adjusts automatically for neighboring components to alternate crosshatch patterns in 90 degree increments. If there are still adjacent section faces with the same pattern, the pattern spacing is adjusted.
Broken View You can use a broken (or interrupted) view on the drawing of a long part. Broken views make it possible to display the part in a larger scale on a smaller size drawing sheet. Reference dimensions and model dimensions associated with the broken area reflect the actual model values. You can specify the gap between the break lines and the extension of the lines beyond the part geometry in Tools, Options, Document Properties, Detailing. The gap between the break lines is the gap when the break lines are first inserted, and also the gap after the view has been broken. You can specify the line font for the break lines in Tools, Options, Document Properties, Line Font. You can apply the Break View and Un-Break View commands to multiple views.
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Example of Broken View
Insert break lines into the view geometry.
Drag the break lines into position.
Break the view.
To create a Broken View:
1.
Select the drawing view and click Insert, Vertical Break (or Horizontal Break). Two break lines appear in the view. You can add more than one set of break lines to a view; however, all breaks must be in the same direction. You can add breaks only to an unbroken view.
2.
Drag the break lines with the
pointer to the places on the part where you want the breaks to occur.
3.
Right-click inside the highlighted boundary and select Break View. The part is displayed with a gap in the part geometry. In addition to model geometry, broken views also support cosmetic threads and axes.
NOTE: When you break the view, any sketch entities that are between the break lines are deleted. Dimensions that are between the break lines become dangling. To restore a broken view to its unbroken state:
Right-click the broken view (or multiple broken views), and select Un-Break View. To modify a broken view:
•
To change the shape of the break lines, right-click a break line and select a style from the shortcut menu.
•
To change the position of the break, drag the break lines.
•
To change the width of the break gap, click Tools, Options, Document Properties, Detailing. Under Break line, enter a new value for Gap. To display the new gap, Un-Break and then Break the view again.
NOTE: You can select an Area Hatch in a broken view only in its unbroken state. You cannot select an area hatch that crosses a break.
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Broken View Break Line Styles Broken View break lines can be in one of four styles.
Straight
Curved
Zig Zag
Small Zig Zag
Section Views in Drawings You create a Section View in a drawing by cutting the parent view with a section line. The section view can be a straight cut section or an offset section defined by a stepped section line. The section line can also include concentric arcs. NOTE: You can also create section views in models. You can create section views of section views. A new section is calculated from the original solid model, and the view updates if the model changes. You can show hidden edges in section views when the view is in Hidden Lines Removed mode. Section views expand in the FeatureManager design tree so that all components and features are available. You can add dimensions to section lines without editing the section line sketch. You can dimension between two section lines, or between a section line and another line or edge. To create a section view:
1.
Activate an existing drawing view.
2.
Click Section View
on the Drawing toolbar, or click Insert, Drawing View, Section.
The Section View PropertyManager appears, and the Line tool 3.
is active.
Sketch a section line. NOTE: To create a multi-line section view, or to use a centerline as the section line, sketch the section line before clicking the Section View tool. If the section line does not completely cut through the bounding box of the model in the view, you are asked if you want this to be a partial section cut. If you click Yes, the Section View is created as a partial section view. As you move the pointer, a preview of the view is displayed. By default, the view is aligned in the direction of the arrows on the section line. To override the default alignment as you place the view, press Ctrl. To return to the default alignment while dragging, release Ctrl. The orientation of the section view toggles as you drag the pointer over the section line. If the section line has multiple segments, the view is aligned to the sketch segment that was selected when you clicked the Section View tool.
4.
Click to place the view.
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In its default alignment, a section view can only move in the direction of the section arrows. For information about changing the alignment of views, see View Alignment and Display. Multiple section lines can have the same label. A warning message appears if the drawing standard you are using does not allow it. Section Views are linked to their section lines. Right-click the section line and select Jump to Section View, which can be on the same sheet or another sheet. Right-click the Section View and select Jump to Parent View. Example of Section View A section line is drawn horizontally across the activated view.
The Section View shows crosshatching on sectioned areas. The parent view now shows the direction arrows and labels.
Section View PropertyManager The Section View PropertyManager opens when you create a Section View in a drawing, or when you select an existing Section View. The PropertyManager controls the following properties: Line Options
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•
Flip direction
. Select to flip the direction of the cut.
•
Scale with model. Select for the section line to scale parametrically with the model if the model changes size. This can result in a section cut that is not what you intend.
•
Label
•
Font. To choose a font for the section line label other than the document's font, clear the Document's font check box and click Font. If you change the section line label font, you can apply the new font to the section view label.
. Edit the letter associated with the section line and section view.
View Options •
Partial section. If the section line does not completely cross the view, a message states that the section line is smaller than the view geometry and asks if you want it to be a partial section cut. o o
•
Yes. The section view is a partial section view and the check box is selected. No. The section view appears but is not cut. You can select the check box later to create a partial section view.
Display only surface. Only the surfaces cut by the section line appear in the section view. Complete section
•
Partial section
Display only surface
Auto hatching. Crosshatch patterns alternate between components in assemblies, or between bodies in multibody parts and weldments.
Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for section views. More Properties For an existing Section View, click More Properties to open the Drawing View Properties dialog box.
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Modifying Section Views •
If a Section View in a Drawing needs to be updated (when a section line position or direction changes, for example), the view is marked with a crosshatch pattern. See Updating Views.
•
To change the length or location of the section line, the length of the leader, or the position of the label, select the line or label and drag it.
•
To edit the letter label on the section line, either: Double-click the letter label, edit in place, and click outside the label to exit. - or Select the section line and edit the label and its font in the Section View PropertyManager.
•
To edit the note text on the section view, double-click the text, edit in place, and click outside the label to exit. NOTE: To edit the properties of the section view note text, select the note and edit the properties in the Note PropertyManager.
•
To edit the sketch used to create the section line, right-click an entity of the sketch and select Edit Sketch.
•
Edit the sketch as needed. Then select one sketch entity and click Rebuild to update the section view. To change the cut direction as indicated by the arrows, double-click anywhere along the section line, or select the section line and select Flip Direction in the Section View PropertyManager.
•
To modify the crosshatch pattern, right-click a face, or hold Ctrl and select multiple faces, and select Properties. See Crosshatch Properties.
•
To modify the length of a centerline, drag the endpoints. Centerlines are automatically added where needed (holes, circular extruded bosses or cuts, and revolved features) in section views. You can specify the default distance for the centerline to extend beyond the model edge in Detailing Options. To remove centerlines, you can either delete them from the Section View, or you can turn the display of them on and off by clicking View, Axes.
Section Views of Assemblies When you create a Section (or Aligned Section) View of an assembly, you can exclude (leave uncut) selected components and set Auto hatching on the Section Scope tab of the Section View dialog box. To exclude components from a section view of an assembly:
1.
Activate a view, and create a section line as described in Section View or Aligned Section View.
2.
Click Section View or Aligned Section View View, Section or Aligned Section.
on the Drawing toolbar, or click Insert, Drawing
The Section Scope tab of the Section View dialog box appears. 3.
In the active drawing view, or in the same view in the FeatureManager design tree, click the components that you want to exclude from the section view. The selected components are listed in the Excluded components box. To remove a component from the list, select the component again, or select the component in the list and click Delete.
4.
If a selected component is used more than once in the assembly (for example, if it is a member of a pattern, or if it is used as a component of more than one sub-assembly):
5.
•
To exclude all the instances of the selected component, click the component name in the Excluded components list, and select the Don’t cut all instances check box. In the resulting view, all instances of the selected component will be left uncut.
•
To exclude only the selected instance, leave the Don’t cut all instances check box cleared. In the resulting view, only the selected instance will be uncut; all others will be cut.
Click OK. In the resulting section view, excluded components are not cut. They are shown in the view, or you can remove them from the view by setting the section line property Display only surface cut.
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To control auto hatching:
If you want the software to automatically adjust for neighboring components with the same crosshatch pattern, select the Auto hatching check box in the Section Scope dialog box. The angle used in the pattern automatically alternates in 90 degree increments. If there are still adjacent section faces with the same pattern, the pattern spacing is adjusted. If you do not use auto hatching, you can manually adjust the angle and spacing on adjacent components. See Crosshatch Properties. NOTE: A Detail View created from an assembly Section View inherits the crosshatch patterns of its parent view. Section Scope In a drawing, you can specify which components are to be left uncut in a section view of an assembly. The Section Scope dialog box appears when you create a section view in an assembly drawing. The Section Scope tab also appears in the Drawing View Properties dialog box for a section view. Section Scope controls the following items. Excluded components •
If you are creating a new section view, click the components to leave uncut in the parent drawing view on the sheet or in the FeatureManager design tree.
•
If you are editing an existing section view, click the components in the section view itself.
•
To remove a component from the list, click the component again, or click it in the Excluded components list and press Delete.
Don't cut all instances Specify what to do if the selected component is used more than once in the assembly (for example, if it is a member of a pattern, or if it is used as a component of more than one sub-assembly): •
Select. If you want to exclude all the instances of the selected component in the assembly, select the Don’t cut all instances check box. In the resulting view, all instances of the selected component are left uncut.
•
Clear. If you want to exclude only the selected instance, clear the Don't cut all instances check box. In the resulting view, only the selected instance are uncut; all others are cut.
Auto hatching •
Click Auto hatching if you want the software to automatically adjust for neighboring components with the same crosshatch pattern.
•
If you do not use Auto hatching, you can manually adjust the angle and spacing on adjacent components. See Area Hatch/Fill Properties.
Troubleshooting Section Views If a Section View is displayed with portions of the model uncut, and with the model in the dangling (brown) color, check for the following conditions: •
The section line may not extend completely across the model. Either extend the section line as needed, or use the Partial Section option. See Section Line Properties.
•
The cut may result in zero-thickness geometry that cannot be displayed correctly in the view. Modify the position of the section line to correct this problem.
•
There may be a problem with the model geometry. Use Tools, Check to identify the invalid geometry. For more information, see Check Entity.
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Chapter 11 Drawings
Modifying Section Line Properties You can make changes to a Section View or Aligned Section View in a drawing by editing the section line properties. You can set these properties before, during, or after creating the section view. To modify a section line before creating the view:
1.
Activate a drawing view and sketch a line.
2.
With the line selected, click Insert, Make Section Line.
3.
Select the section line. The Section View PropertyManager appears.
4.
Make any changes in the PropertyManager.
5.
Click Section View
or Aligned Section View
and place the view.
- or Click OK
to close the PropertyManager without creating a view.
NOTE: You can select the section line and create the view at any time. To modify a section line during creation of a section view:
Make any changes in the Section View PropertyManager, which appears when you click the Section View or Aligned Section View tool. To modify a section line after a section view is created:
1.
Select the section line or section view. The Section View ProprtyManager appears.
2.
Make any changes and click OK
.
Aligned Section View You can create an aligned section view in a drawing through a model, or portion of a model, that is aligned with a selected section line segment. The aligned section view is similar to a Section View, but the section line for an aligned section comprises two lines connected at an angle. Example of Aligned Section View The active view shows the section line, direction arrows, and labels. The resulting Aligned Section View is at the right.
To create an aligned section view:
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1.
Activate an existing drawing view.
2.
Click Centerline
3.
Sketch the section line. The section line should consist of two connected lines at an angle to each other.
4.
Select the segment of the sketched section line to which you want to align the view.
5.
Click Aligned Section View
or Line
or Tools, Sketch Entity, Centerline or Line.
on the Drawing toolbar, or click Insert, Drawing View, Aligned Section.
NOTE: If you are in an assembly, the Section View Section Scope dialog box appears. The Section View PropertyManager appears. You cannot change the angle of the line that you selected to align the view; however, you can change the position of the view. As you move the pointer, a preview of the view is displayed. By default, the view is aligned in the direction of the arrows on the selected segment of the section line. To override the default alignment as you place the view, press Ctrl. To return to the default alignment while dragging, release Ctrl. The orientation of the view flips as you drag the preview across the the section lline. You can also select Flip direction in the PropertyManager. The view is aligned to the sketch segment that was selected when you created the section line; the cut faces from the other segments are projected into the same plane. 6.
When the view is where you want it to be, click to place the view.
In its default alignment, an aligned section view can move only in the direction of arrows on the selected segment. For information about changing the alignment of views, see Drawing View Alignment and Display.
Alternate Position View You can superimpose one drawing view precisely on another with the Alternate Position View tool. The alternate position is shown with phantom lines. Alternate Position Views are often used to show the range of motion of an assembly. •
You can dimension between the primary view and the Alternate Position View.
•
The Alternate Position View is added to the FeatureManager design tree.
•
You can create more than one Alternate Position View in a drawing.
•
The Alternate Position View is not available in Broken, Section, Detail, or Crop views.
To insert an alternate position view:
1.
Click Alternate Position View Position.
on the Drawing toolbar, or click Insert, Drawing View, Alternate
The Alternate Position PropertyManager appears. You are prompted to select a drawing view in which to insert the alternate position. 2.
3.
Under Configuration, choose either: •
New configuration - to create a new Alternate Position configuration. Accept the default name or type a name of your choice.
•
Existing configuration - to choose an existing configuration in the assembly document. Select a configuration from the list.
Click OK
. The results are either:
•
New configuration - If the assembly document is not already open, it opens automatically. The assembly appears with the Move Component PropertyManager open and Free Drag activated. Continue to Step 4.
•
Existing configuration - The alternate position of the selected configuration appears in the drawing view, and the PropertyManager closes. The view is complete. No further steps are required.
4.
Use any of the Move Component tools to move the assembly components to the desired position.
5.
Click OK
to close the Move Component PropertyManager and return to the drawing.
The alternate position of the assembly configuration appears in the drawing view in phantom lines, and the Alternate Position PropertyManager closes.
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Example of an Alternate Position View
Alternate Position PropertyManager The Alternate Position PropertyManager opens when you insert an Alternate Position View into a drawing. You choose the Alternate Position configuration in the PropertyManager. Configuration •
New configuration - A default name appears in the box. You can accept the default name or type a name of your choice.
•
Existing configuration - Choose from existing assembly configurations that appear in the list.
Position Schematic PropertyManager The Position Schematic PropertyManager opens when you insert a schematic into a drawing document. You must have Microsoft Visio® Technical Edition installed on your system for this menu item to be available. To insert a Visio schematic into a drawing:
1.
Click Insert, Schematic. The Position Schematic PropertyManager opens.
2.
Drag-select a box in the graphics area to size and position the schematic.
3.
Under Schematic templates, select a template. NOTE: The PropertyManager lists the templates most commonly required in SolidWorks. To choose from the more extensive list in Visio, select Other from the SolidWorks list, or else make no selection.
4.
Click OK
to close the PropertyManager and activate Visio.
5.
Create a schematic in Visio.
Example of a Visio schematic in a SolidWorks drawing
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OLE Items in Drawings If any part of an active OLE item in a drawing is covered, the item does not redraw when it is uncovered. This behavior may occur, for example, when you move a stencil across an active Visio item. To redraw the OLE item and restore the drawing:
Deactivate the OLE item and reactivate it. - or Select one of the eight handles on the border of the OLE items.
Drawing View Update By default, all drawing views are updated automatically when the model changes. You can change this behavior to allow manual regeneration of drawing views. In manual view regeneration mode, you can update all the views at once when you are ready, or update them one by one. When the model changes, any drawing views that need to be updated are marked with a light gray crosshatch pattern. NOTE: You cannot activate or edit a view that needs to be updated. To manually update drawing views:
1.
Right-click the Drawing icon at the top of the FeatureManager design tree, and click Automatic view update. If there is no check mark, it indicates that manual view regeneration is enabled.
2.
To update all the views at once, either:
3.
•
Click Edit, Update All Views.
•
Click Edit, Rebuild or Rebuild
•
Right-click the Drawing icon in the FeatureManager design tree, and click Update All Views.
.
To update selected drawing views: •
Select the view, then click Edit, Update View, or click Update View on the Drawing toolbar. (Use Tools, Customize to add the Update View icon to your toolbar, if necessary.)
•
Right-click the view, and select Update View.
Press Ctrl to select more than one view at a time for updating.
Drawing View Alignment and Display Drawing View Alignment and Display Manipulating Views •
Drawing View Properties
•
Updating Views
•
Moving a Drawing
•
Moving Views
•
Aligning Views
•
Rotating Views
•
Copying and Pasting Views
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Chapter 11 Drawings
Hiding and Showing •
Hiding and Showing Views
•
Hiding and Showing Edges
•
Show Hidden Lines
•
Hide/Show Components
•
Hide Components Behind Plane
•
Hiding and Showing Sketches
Displaying •
Drawing View Display Modes
•
Component Line Font
•
Line Format
•
Layers
Manipulating Views Drawing View Properties The Drawing View Properties dialog box provides information about the drawing view and its associated model. To view and edit the Drawing View Properties:
1.
Right-click in a drawing view (but not on the model) and select Properties. - or From a view PropertyManager, click More Properties.
2.
Edit the following properties on the View Properties tab, or edit items on the Show Hidden Edges or Hide and Show Components tabs, and click OK.
View information. Displays the Name and Type of the view (read-only). Model information. The name of the model and the path of the referenced document are displayed (read-only). Model information is not available for Detached views when the model is not loaded. Configuration Information. Select one of the following: Use model’s "in-use" or last saved configuration. - or Use named configuration. To use a configuration that you previously created and named, select the configuration from the list. Show in exploded state. If the view contains an assembly with an exploded view defined, select this check box to display the exploded view. Bill of Materials (BOM). Linked to BOM. Selected automatically if the model in the view is linked to a Bill of Materials. The name of the BOM is displayed in the window. Align breaks with parent. If the view is a Broken View that was created from another broken view, select this check box to align the break gaps in the two views. Depending on the type of changes you have made, it may be necessary to click Update View Rebuild
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.
or
Multiple Views PropertyManager To set properties common to multiple drawing views:
1.
Select multiple drawing views in the graphics area.
2.
In the PropertyManager, set the properties described below and click OK
.
Display Style Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality
•
Draft quality
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Use parent scale. Available for related views (projected, auxiliary, section, detail, and so on) Use sheet scale. Use custom scale. Set a scale for the views. Dimension Type Select either Projected or True. Updating Views To control the update behavior of the views in an active drawing, specify the Automatic view update mode. If selected, drawing views update as you change the model. You can also set an option to specify whether views are updated when opening drawings. NOTE: You cannot activate or edit a drawing view that needs to be updated. To change the update mode in the current drawing:
Right-click the drawing icon at the top of the FeatureManager design tree, and select or clear Automatic view update. To update drawing views manually:
1.
Right-click the drawing icon at the top of the FeatureManager design tree and clear Automatic view update if it is checked.
2.
To update all the views at once, use one of these methods: •
Click Edit, Update All Views.
•
Click Rebuild
SolidWorks 2004 Reference Guide
or Edit, Rebuild to update any views that need to be updated.
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Chapter 11 Drawings
3.
To update selected drawing views, use one of these methods: •
Select the view, then click Update View on the Drawing toolbar, or click Edit, Update View. (Use Tools, Customize to add the Update View icon to the toolbar, if necessary.)
•
Right-click the view, and select Update View. You can select the view either in the FeatureManager design tree or on the drawing sheet for either method. You also can hold down Ctrl and select several views at once to update in this way.
To update automatically when opening drawings:
1.
Click Tools, Options, System Options, Drawings.
2.
Select Allow auto-update when opening drawings. NOTE: The automatic updating of views when opening drawings does not affect Automatic view update for the active drawing document.
Move Drawing You can move all of the entities of a drawing in relation to the drawing sheet. Entities that are on the drawing sheet (drawing views, annotations, and so on) or in the drawing sheet format are moved. To move drawing entities:
1.
Right-click the drawing name at the top of the FeatureManager design tree and select Move.
2.
Type a value in the X value or Y value box, and click Apply. All of the drawing entities move the specified distance in the X or Y direction.
3.
Click Close to exit the dialog box.
Moving Drawing Views To move a drawing view:
Press Alt, place the pointer anywhere in the view, and drag the view. - or Move the pointer over the boundary of a view to highlight the boundary, or select the view. When the move pointer
is displayed, drag the view to a new location.
Note the following restrictions: •
Standard 3 View. The alignment of the front view is fixed in relation to the other two views. When you move the front view, the other views also move. The other two views can move independently, but only horizontally or vertically, toward or away from the front view.
•
Auxiliary, Projected, Section, and Aligned Section views are aligned with the parent views from which they are created, and only move in the direction of the projection.
•
Broken views respect the alignment of the view before it was broken. Crop views and Alternation Position views retain the alignments of the original views.
Named, Detail, Relative to Model, and Empty views can be moved freely on the sheet and are not aligned to other views. Child views move relative to parent views. To retain exact positions between the views, press Shift while dragging.
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Aligning Views You can change the alignment of views that are not aligned by default, or views whose alignment you have broken. You can also break view alignments and return alignments to their defaults. To align one drawing view to another:
1.
Select a drawing view, and click Tools, Align Drawing View, Horizontal To Another View or Vertical To Another View. - or Right-click a drawing view, select Alignment, then select one of the following options: •
Align Horizontal by Origin
•
Align Vertical by Origin
•
Align Horizontal by Center
•
Align Vertical by Center The pointer changes to
2.
.
Select the view to which you want to align. The model origins or drawing view centers of the views are aligned along the chosen direction. The alignment is maintained if you move the reference view.
To align a drawing view to a model edge:
1.
Select a linear model edge in a drawing view.
2.
Click Tools, Align Drawing View, Horizontal Edge or Vertical Edge. The view rotates until the selected edge is oriented horizontally or vertically. If any views are projected from a view that you rotate this way, the projected views update to maintain their projection. For additional methods of rotating views, see Rotating Views.
To break a view’s alignment:
For views that are aligned, you can break the alignment and move the views independently. Right-click inside the view boundary (not on the model), and select Alignment, Break Alignment, or click Tools, Align Drawing View, Break Alignment. To return a view to its default alignment:
You can return a view whose alignment you have broken to its original alignment. Right-click inside the view boundary (not on the model), and select Alignment, Default Alignment or click Tools, Align Drawing View, Default Alignment. Rotating Views You can rotate a view to orient a selected edge either horizontally or vertically. You can also rotate a view around its center point to orient the view at any angle. To rotate a drawing view around a model edge:
1.
Select a linear model edge in a drawing view.
2.
Click Tools, Align Drawing View, Horizontal Edge or Vertical Edge. The view rotates until the selected edge is oriented horizontally or vertically. If there are any views projected from a view you change this way, they update to maintain their projection.
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To rotate a drawing view around its center point:
1.
Click Rotate View
on the View toolbar, or right-click the view and select View, Rotate View.
The Rotate Drawing View dialog box appears. 2.
Drag the view to the desired rotation. The view snaps to 45° increments, but you can drop the view at any angle. The angle appears in degrees in the dialog box. - or In the dialog box, type the angle in the Drawing view angle box, select or clear the Dependent views update to change in orientation check box, and click Apply to see the rotation.
3.
Click Close to close the dialog box.
To restore a view to its original rotation:
Right-click the view and select Alignment, Default Alignment. If the default alignment to another view was broken, this also restores the original alignment. Rotate Drawing View To rotate a drawing view:
1.
Select a drawing view (optional), and click Rotate View a view, and select View, Rotate View.
on the View toolbar. You can also right-click
The Rotate Drawing View dialog box appears. 2.
Rotate the view in one of these ways: •
Drag the view on the sheet. The view snaps to 45 degree increments, but you can drop the view at any angle.
•
Specify the Drawing view angle. (Select a view before entering an angle, if you did not pre-select a view.)
•
Use the left and right arrow keys. The increment value specified for the arrow keys (under Tools, Options, System Options, View Rotation) is used.
3.
Select Dependent views update to change in orientation if you also want to update any views that were created from the view you are rotating (projected views, for example).
4.
Select Rotate Center Marks with view if you want center marks to rotate with the view. You can rotate center marks in the Center Mark PropertyManager.
5.
Click Apply to update the views. You can rotate other views if needed, then click Close when you are finished.
6.
To restore the view to its original rotation, right-click the view and select Alignment, Default Rotation.
Copying and Pasting Views You can cut, copy, and paste drawing views from one sheet to another in the same drawing, and from one drawing document to another. You can also drag views from sheet to sheet within a drawing (but not to another drawing document). To perform these operations on multiple views at once, hold down the Ctrl key as you select the views. NOTE: To copy a Detail or Section View from one drawing to another, you must also copy the parent view. You can either copy the parent view first, or you can copy both the parent and the Detail or Section View at the same time. To cut/copy/paste a drawing view:
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1.
Select the view either on the sheet or in the FeatureManager design tree.
2.
Click Cut
or Copy
, or click Edit, Cut or Copy.
3.
Change to the target sheet or drawing document, click where you want to paste the view, and click Paste or Edit, Paste.
To move or copy views by dragging:
Select a view on the active drawing sheet, or select the view’s icon in the FeatureManager design tree. •
To move the view, hold down Shift, then drag the selected view or its icon, and drop it on the sheet icon for the target sheet.
•
To copy the view, hold down Ctrl as you drag and drop.
Hiding and Showing Hiding and Showing Views You can use Hide View to hide an entire view while working on a drawing. Once hidden, you use Show View to display that view again. When you hide a view that has dependent views (Detail, Section, or Auxiliary views), you are given the choice of hiding those views also. When you show either the parent view or a dependent view again, you are given the choice of showing the related view also. To hide/show views:
1.
Right-click the view on the sheet or in the FeatureManager design tree, and select Hide View. If the view has dependent views (Detail, Section, and so on), you are asked if you want to hide the dependent views as well. If the view was active when you hid it, the active view boundary (gray shadowed) is displayed. Otherwise, the view and boundary are invisible. To see where hidden views are placed on the sheet without displaying them, click View, Show Hidden Views. The boundaries of hidden views are displayed with an X.
The pointer changes to 2.
and the view boundary highlights when the pointer passes over a hidden view.
To show the view again, right-click the view, and select Show View. If the view has dependent views (Detail, Section, and so on), you are asked if you want to show the dependent views as well.
Hiding and Showing Edges To hide or show edges:
1.
Select an edge and click Hide Edge Edge.
on the Line Format toolbar, or right-click an edge and select Hide
The edge is removed from the display, but it still is highlighted when the pointer passes over it. 2.
To display the edge again, select the edge and click Show Edge Edge.
, or right-click the edge and select Show
If you cannot select the hidden edges, click Tools, Options, System Options, Drawings. Make sure that the Select hidden entities check box is selected. Showing or hiding an edge is a valid operation only if the edge would be shown in the view mode. For example, if the edge is hidden and the view mode is Hidden Lines Removed, you cannot show or hide the edge.
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Chapter 11 Drawings
Hiding and Showing Sketches You can show and hide model sketches in drawings. SolidWorks lists the sketches in the FeatureManager design tree but hides them in the graphics area by default. To show a sketch in a drawing:
Right-click the sketch in the FeatureManager design tree and select Show Sketch. NOTE: The sketch entities highlight in the graphics area when you point over the sketch name in the FeatureManager design tree. Drawing view with sketch hidden
Sketch shown
To hide a sketch in a drawing:
Right-click the sketch in the graphics area or in the FeatureManager design tree and select Hide Sketch. To show or hide dimensions of model sketches in drawings:
Right-click the sketch in the FeatureManager design tree (or in the graphics area if the sketch is shown) and select Show Dimensions or Hide Dimensions. When you insert model dimensions in a drawing, SolidWorks includes dimensions for all features and sketches. NOTE: SolidWorks does not insert dimensions for hidden, unabsorbed sketches. To insert dimensions for unabsorbed model sketches in a drawing:
1.
Right-click any unabsorbed sketches in the FeatureManager design tree and select Show Sketch.
2.
Click Model Items
3.
Hide the sketches or dimensions, or both, as necessary.
or Insert, Model Items, select Dimensions, and click OK.
Unabsorbed sketch with dimensions inserted
Show Hidden Edges You can show all the hidden lines of selected features and components in drawing documents. You can access this feature in two ways. To show or hide hidden edges from the shortcut menu:
Right-click a feature or component in the drawing view or in the FeatureManager design tree and select Show/Hide, Show Hidden Edges. If the hidden edges are visible, you can hide them again by right-clicking the feature or component and selecting Show/Hide, Hide Hidden Edges.
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To show or hide hidden edges in the Drawing View Properties dialog box:
1.
Right-click the drawing view and select Properties.
2.
Select the Show Hidden Edges tab.
3.
Select a feature or component from either the drawing view or the FeatureManager design tree to add it to the list of items to be shown with hidden lines.
4.
Click Apply to see the effect of your selection.
5.
To hide the hidden lines again, select an item from the list and press Delete. - or Select the feature or component in the drawing view or the FeatureManager design tree.
6.
Click OK to close the dialog box.
Hide/Show Components You can hide or show components in an assembly drawing. A quick selection method for hiding components is Hide Behind Plane. You can set an option in Tools, Options, System Options, Drawings to list hidden components automatically when you create a drawing view. New drawing views with the Automatic hiding of components on view creation check box selected display the list of hidden components on the Hide/Show Components tab in the Drawing View Properties dialog box. You can access Hide/Show Components in two ways. To show or hide a component from the shortcut menu:
Right-click a component in the drawing view or in the FeatureManager design tree and select Show/Hide, Hide Component. If the component is hidden, you can show it again by right-clicking the component in the FeatureManager design tree (not in the drawing view) and selecting Show/Hide, Show Component. To show or hide a component in the Drawing View Properties dialog box:
1.
Right-click the drawing view and select Properties.
2.
Select the Hide/Show Components tab.
3.
Select a component from either the drawing view or the FeatureManager design tree to add it to the list of items to be hidden.
4.
Click Apply to see the effect of your selection.
5.
To show the component again, select the component in the Hide/Show Components list and press Delete. - or Select the component in the FeatureManager design tree.
6.
Click OK to close the dialog box.
NOTE: You can hide or show surfaces in part and assembly documents without affecting their drawings. In a part or assembly document, right-click a surface and select Hide Surface Body. The surface remains visible in the associated drawing. To show the surface again, right-click the surface in the FeatureManager design tree and select Show Surface Body. Hide Behind Plane You can hide components of an assembly drawing behind a plane. This procedure is a quick selection method for Hide/Show Components. Only those components that are completely behind the plane are hidden. You can choose the direction to hide and the position of the plane. The X, Y, and Z coordinates of the plane distance are shown in the dialog box.
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Example of Hide Behind Plane The plane in the isometric view will hide components in the direction of the arrow. The plane and arrow are also displayed in the other views to aid in locating the components to be hidden.
The resulting isometric view.
To hide components behind a plane:
1.
In the FeatureManager design tree, right-click a plane under the view in which you want to hide components and select Hide Behind Plane. The Hide Behind Plane dialog box appears, and the plane and direction arrow are displayed in all views on the drawing sheet that contain the model.
2.
Change the distance of the plane in the Distance box to move the plane, if necessary. The X, Y, Z coordinates of the plane appear in the Plane point section, and the plane is displayed in the new location in all the views on the drawing sheet.
3.
Select the Reverse direction check box, if necessary.
4.
Click OK.
To show the components again:
1.
Right-click the view, and select Properties. The Drawing View Properties dialog box appears.
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2.
Select the Hide/Show Components tab.
3.
Select all the items in the list that are behind the plane and press Delete.
4.
Click OK.
Displaying Component Line Font The Component Line Font dialog box lets you change the line font style of edges on each of the components in an assembly drawing. To change the font style of component edges:
1.
Right-click a component in a drawing view and select Component Line Font. The Component Line Font dialog box appears.
2.
Choose from the following Component Display Properties and click OK.
Use document defaults - when selected, other choices in the dialog box are ignored. Type of edge - select one or more type of edge (Visible Edges, Hidden Edges, and so on) from the list. Line style - select a style (Solid, Dashed, and so on) from the list. Line weight - select a weight (Normal, Thin, and so on) from the list. The line you select is displayed in the Preview box. NOTE: Click Reset to return Line style and Line weight to the defaults you set in Tools, Options, Document Properties, Line Font. Drawing view - choose to apply the changes to the drawing view From selection or to All views. Layer - if the component is in a layer, the name of the layer appears in the box. You can change the layer for the component by selecting a named layer from the list. NOTE: Selections for line style and line weight in the Component Line Font dialog box take precedence over those set in Layers properties. Drawing View Display Modes You can display drawing views in the following modes, from either the View toolbar or in the view PropertyManager: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded When in Hidden Lines Visible or Hidden Lines Removed mode, you can select a style for Tangent Edge Display. Shaded mode is available for the following types of view: •
Model View
•
Standard 3 View
•
Projected View
•
Auxiliary View
•
Section View
•
Relative View
You can set the default display mode for drawings in Tools, Options, System Options, Display Style.
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Line Format You can specify the color, thickness, and style in drawings for: •
System settings for new sketch entities
•
Entities in layers
•
Properties of existing lines, edges, and sketch entities
You can specify the color for notes and other annotations in either layers or with the Line Color tool. The settings for the line formats are either: •
•
globally controlled - set in either: o
Layers
o
Tools, Options, System Options, Colors and Display Style
explicitly controlled - set by the Line Format tools
The following settings apply if the Default check box in a Line Format tool dialog box is: •
•
Selected o
Layer settings - if the entity is in a layer
o
System settings - if the entity is not in a layer
Cleared o
Line Format tool settings - set explicitly for the entity
When you add new sketch entities to a drawing, the line format follows the Layer settings. If no layer is active, the line format follows the system settings. For existing lines, edges, and sketch entities, the line format tool settings override layer specifications and system settings. Another method of setting line properties for assembly components in drawings is with Component Line Font. Format tools The tools on the Line Format toolbar change the following formats.
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•
Layer Properties. Set layer properties (Color, Thickness, and Style), move entities into layers, and select a layer for new entities.
•
Line Color. Choose a color from the palette, or select Default. You can toggle between the specified color and the system default colors with the Color Display Mode tool (below).
•
Line Thickness. Choose a thickness or Default from the menu. As you move the pointer over the menu, the thickness name (Thin, Normal, Thick, and so on) is displayed in the Status bar. Corresponding line weights for printing are defined in File, Print, Line weights.
•
Line Style. Choose a style or Default from the menu. As you move the pointer over the menu, the corresponding line style name (Solid, Dashed, Phantom, and so on) is displayed in the Status bar.
•
Color Display Mode. Click this tool to toggle between aesthetic colors (colors chosen in layers or with Line Color) and the system status colors (fully defined, under defined, and so on). Sketch endpoints and dangling dimensions are always in the system status color.
To specify the format for new sketch entities in the current and future drawings:
1.
Click outside the drawing sheet to activate the Line Format tools.
2.
Click a tool on the Line Format toolbar and select a format from the menu.
3.
Sketch entities of any type (lines, centerlines, circles, and so on) that you add to the drawing use the specified formats, until you select a different format.
To change the format of an existing line, edge, or sketch entity:
1.
Select the line, edge, or sketch entity you want to change. To select more than one entity at a time, hold Ctrl as you select.
2.
Click a tool on the Line Format toolbar and select a format from the menu. The new format is applied to the selected entities.
Tangent Edge Display Overview Tangent edges are transition edges between rounded or filleted faces in drawing views in Hidden Lines Removed or Hidden Lines Visible display modes. Tangent edges can be displayed as follows: •
Visible - a solid line
•
Use font - a line in the default font defined in Tools, Options, Document Properties, Line Font.
•
Removed - not displayed Visible
Use font
Removed
Tangent edges are always Visible in Isometric, Trimetric, and Dimetric oriented views. You can control tangent edge display in the following ways: •
Default - to set the display for all new drawing views, click Tools, Options, System Options, Display Style, and choose one of the options under Default display of tangent edges in new drawing views. In new installations, when you insert views into drawings, a dialog box appears so you can set the tangent edge display for the current view and future views.
•
Views - to set the display for an individual view in a drawing, right-click the view in either the graphics area or the FeatureManager design tree and select Tangent Edge, then choose one of the three tangent edge display modes.
Tangent Edge Display Select one of the display types as the default for tangent edges (transition edges between rounded or filleted faces in Hidden Lines Removed and Hidden Lines Visible display modes) for the current drawing view and for future views. •
Visible - a solid line
•
Use font - a line in the default font defined in Tools, Options, Document Properties, Line Font.
•
Removed - not displayed
As you select each button, the display is previewed in the drawing.
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Chapter 11 Drawings
The default in this dialog box is the default in the system options in Tools, Options, System Options, Display Style. Your choice in the dialog box becomes the new system option. You can control the default in either the dialog box or the system options. Don't ask me again. Select to prevent this dialog box from appearing each time you insert a drawing view. Layers You can create layers in a SolidWorks drawing document. You assign a line color, line thickness, and line style for new entities created on each layer. New entities are automatically added to the active layer. You can hide or show individual layers. You can move entities from one layer to another. •
Dimensions and annotations (including notes, area hatch, blocks, break lines, cosmetic threads, detail circles, section lines, and tables) can be moved onto layers; they use the color specified for the layer.
•
Sketch entities use all the properties of the layer.
•
Components, in either part or assembly drawings, can be moved onto layers. The Component Line Font dialog box includes a list for selecting a named layer for the component.
•
If you import a .dxf or .dwg file into a SolidWorks drawing, layers are created automatically. The layer information (names, properties, and entity locations) specified in the system where the .dxf or .dwg file originated is retained.
•
If you export a drawing with layers as a .dxf or .dwg file, the layer information is included in the file. When you open the file in the target system, the entities are on the same layers and have the same properties unless you use mapping to redirect the entities to new layers.
To create a drawing layer:
1.
In a drawing, click Layer Properties
on either the Layer toolbar or the Line Format toolbar.
The Layers dialog box appears. 2.
Click New, and enter the Name of a new layer. NOTE: If you save the drawing as a .dxf or .dwg file, the layer name may be changed in the .dxf or .dwg file as follows:
3.
•
All characters are converted to uppercase.
•
The name is truncated to 31 characters.
•
All spaces in the name are converted to underscores.
Specify the line format for entities on that layer as follows: •
To add a description, double-click in the Description column and type text.
•
To specify the line color, click the Color box, select a color, and click OK.
•
To specify the line style or thickness, click in the Style or Thickness column, and select the desired style or thickness from the list.
Active. An arrow
indicates which layer is active. To activate a layer, double-click beside the layer name.
Visible. A yellow lightbulb appears with any layer that is visible. To hide a layer, double-click its lightbulb. The lightbulb turns gray, and all the entities on the layer are hidden. To turn the layer back on, double-click the lightbulb again. Move. To move entities to the active layer, select the entities in the drawing and click Move. Delete. To delete a layer, select the layer name and click Delete.
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12 Detailing
Detailing Overview Detailing Overview You can add much of the necessary detailing of your models in part and assembly documents. This includes dimensions, notes, symbols, and so on. Then you can insert the dimensions and annotations from the model into a drawing. Once in the drawing, you can add reference dimensions, other annotations, and a bill of materials if required. Annotations and reference dimensions added in a drawing do not affect the part or assembly document. For drawings, sheet formats, and drawing views see Drawings.
Setting Detailing Options You can set options for various aspects of detailing. The options affect only the active document. To set detailing options:
1.
Click Tools, Options. On the Document Properties tab, select: •
Detailing - standards, trailing zeros, extension lines, and so on
•
Dimensions - text alignment, leaders, arrow styles and so on
•
Notes - text alignment, leaders, and borders
•
Balloons - balloon styles, sizes, and contents, and so on
•
Arrows - arrow sizes, styles, and attachments
•
Virtual Sharps - virtual sharp display styles
•
Annotations Display - display filter, text scale, and so on
•
Annotations Font - fonts for Note, Dimension, Detail, and so on
•
Tables - various controls for Hole Tables, Revision Tables, and Bills of Materials
•
View Labels - label content and format for Detail, Section, and Auxiliary view labels
2.
Change the options as necessary.
3.
Click OK to apply the changes and close the dialog box.
Inserting Model Items You can insert dimensions, annotations, and reference geometry from a model document (part or assembly) into a drawing. You can insert items into a selected feature, an assembly component, a drawing view, or all views. You can select a feature, component, or view in the graphics area or in the FeatureManager design tree. For directions, see Insert Model Items.
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Chapter 12 Detailing
Insert Model Items You can insert dimensions, annotations, and reference geometry from the model into the current drawing. You can insert items into a selected feature, an assembly component, a drawing view, or all views. When inserting into all views, dimensions and annotations appear in the most appropriate view. Features that appear in partial views, such as Detail or Section views, are dimensioned in those views first. To insert existing annotations or reference geometry into a drawing:
1.
Preselect views as follows: •
To annotate a single feature or assembly component, select the item.
•
To annotate a single drawing view, select the view.
•
To annotate all the views at once, do not select anything. NOTE: Dimensions are inserted for unabsorbed model sketches only if the sketch is visible in the drawing. To insert dimensions for an unabsorbed sketch, right-click the sketch in the FeatureManager design tree and select Show Sketch before inserting the dimensions. Dimensions belonging to an unabsorbed sketch are shown or hidden depending on the state of Show Sketch or Hide Sketch. You can also show or hide dimensions regardless of whether the sketch is shown or hidden. Right-click the sketch and select Show Dimensions or Hide Dimensions.
2.
Click Model Items
on the Annotation toolbar, or click Insert, Model Items.
The Insert Model Items dialog box appears. 3.
4.
Select the All types check box, or select individual types of items to insert: •
Annotations - Cosmetic thread (assemblies only), Datums, Datum targets, Dimensions, Geometric tolerances, Notes, Surface finish, Welds. If you select Dimensions, you have the option of also inserting Instance/Revolution counts if those dimensions exist in the part or assembly, Hole Wizard Profiles, and Hole Wizard Locations. Select Marked for drawing to insert only those dimensions that are marked in parts for drawings.
•
Reference Geometry - Axes, Curves, Planes, Surfaces, Routing points, Origins.
Choose other options as required: •
Layers - Select a layer from the Layers list (available if your drawing has layers) for the items to be inserted only in the specified layer.
•
Import from - If you have preselected a component or feature, you can select one of the following options: o o
o o
•
12-2
Entire model. Displays all of the selected item types that exist in the model. Selected component. If this drawing is of an assembly, displays the items that exist on the selected component only. Selected feature. Displays the annotations existing on the selected feature only. Only Assembly. When selected, annotations in the assembly are inserted. Annotations that were created in parts or subassemblies are not inserted. Reference dimensions created in the assembly, dimensions referring to mates, and dimensions referring to in-context features created in assemblies are inserted.
Include items from hidden features - To prevent the insertion of annotations that belong to hidden model items, clear the Include items from hidden features check box. Annotations on features that are completely hidden by other geometry are not inserted. The insertion operation is slower when the software filters out hidden features, but the resulting views do not contain inappropriate annotations.
•
Import items into all views - Change the selection of views if necessary. To insert dimensions into selected views, clear the Import items into all views check box, then click the desired views in the graphics area or FeatureManager design tree. The selected views are listed in the Import into views box. Click the views again to remove them from the list; right-click the drawing sheet, and select Clear selections to remove all the views from the list. NOTE: When Selected Feature or Selected Component is checked, annotations for the item are displayed only in the view where you selected the item. You cannot select a different view or all views.
•
5.
Eliminate duplicate model dimensions - When the Eliminate duplicate model dimensions check box is selected, duplicate dimensions are not inserted into drawings when model dimensions are inserted. The default for this check box follows the Eliminate duplicate model dimensions on insert option in Tools, Options, System Options, Drawings.
Click OK.
Attachment points of imported annotations can be dragged, but not re-attached to another edge, face, vertex, and so on. You can toggle the visibility of individual reference geometry items. Right-click the item, and select Hide or Show. Imported annotations display in the default Imported Annotations (Driving) or Imported Annotations (Driven) color; reference annotations (added in the drawing) are displayed in the default Imported Annotations (Driven) color. These colors are specified in Tools, Options, System Options, Colors.
Inserting Annotations into Drawings You can add all types of annotations to a drawing document. You can add most types in a part or assembly document, then insert them into a drawing document. However, there are some types, such as Center Marks, Area Hatch, and Blocks, that you can add only in a drawing document. Annotations behave like dimensions in all types of SolidWorks documents. You can add dimensions in a part or assembly document, then insert them into the drawing, or you can create dimensions in the drawing. When inserted into all views, annotations appear in the most appropriate view.
Inserting Dimensions into Drawings Dimensions in a SolidWorks drawing are associated with the model, and changes in the model are reflected in the drawing. Typically, you create dimensions as you create each part feature, then insert those dimensions into the various drawing views. Changing a dimension in the model updates the drawing, and changing an inserted dimension in a drawing changes the model. By default, inserted dimensions are black. This includes dimensions that are blue in the part or assembly document (such as the extrusion depth). Reference dimensions are gray and appear with parentheses. Dimensions are inserted only once for a part, even if the part shows in multiple instances in an assembly. Linear dimensions that have the same value and that could overlap or be parallel are not inserted. When you insert dimensions into all views, the dimensions appear in the most appropriate view. Features that appear in partial views, such as Detail or Section views, are dimensioned in those views first. When you insert dimensions into selected views, you can insert the dimensions for the entire model, or you can selectively insert the dimensions for one or more components (in an assembly drawing) or features (in a part or assembly drawing). Dimensions are placed only in the views where they are appropriate. Duplicate dimensions are not inserted automatically. Once a dimension has been inserted into one view, it is not inserted again into another view. You can delete a dimension from one view, then insert it into a different view, or you can move or copy it to another view.
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Chapter 12 Detailing
Inserting Reference Geometry into Drawings The reference geometry contained in a model is hidden by default in drawing views. When you insert reference geometry from the model, all entities of the selected types are shown. When you insert reference geometry into drawings, planes, axes, curves, and points are shown in gray. Surfaces are shown as visible lines (black). To toggle the display status of an individual reference geometry entity, right-click the entity in the FeatureManager design tree, and select Hide or Show.
Favorites You can define favorite styles, similar to paragraph styles in word processing documents, for dimensions and various annotations (Notes, Geometric Tolerance Symbols, Surface Finish Symbols, and Weld Symbols). With favorites, you can: •
Save any dimension or annotation property as part of a favorite.
•
Name favorites so that they can be referenced.
•
Apply favorite styles to multiple dimensions or annotations.
•
Add, update, and delete favorite styles.
•
Save and load favorite styles. You can also load styles saved from other documents and located in other folders.
The functionality of favorites includes: •
When adding a dimension or annotation, you can preselect an item that uses a favorite, and that favorite becomes the default for the new item. If you click a location first, no favorite is used for new items.
•
You cannot apply favorites to dimensions created by Hole Callouts.
•
When you insert dimensions from a part or assembly into a drawing with Insert Model Items, the dimensions' favorites belong to the original model. Therefore, you cannot assign drawing favorites to the inserted dimensions. You can load the part or assembly favorites into drawings. Changes to the favorites in the drawings change the favorites in the part or assembly document.
The extensions for favorites are: Dimensions
.sldfvt
Notes
.sldnotfvt
Geometric Tolerance Symbols
.sldgtolfvt
Surface Finish Symbols
.sldsffvt
Weld Symbols
.sldweldfvt
To add a favorite to a document:
1.
Select one or more dimensions or annotations.
2.
Edit the dimension or annotation properties in the PropertyManager or dialog box.
3.
Click Add or Update a Favorite
4.
In the dialog box, type a name under Enter a new name or choose an existing name and click OK.
.
To apply a favorite to a dimension or annotation:
12-4
1.
Select one or more dimensions or annotations.
2.
In the PropertyManager or dialog box, select a favorite in Set a current Favorite.
To save a favorite:
1.
With a favorite displayed in Set a current Favorite, click Save a Favorite
.
2.
In the Save As dialog box, browse to the folder where you want to save the file, edit the file name if necessary, and click Save.
To load a favorite:
1.
Click Load Favorites
.
2.
In the Open dialog box, browse to the appropriate folder and select one or more files. You can select multiple favorite files by using Shift or Ctrl.
3.
Click Open. The loaded favorites appear in the Set a current favorite list.
To update a favorite style:
1.
Select a dimension or annotation with the favorite style.
2.
Edit the dimension or annotation properties.
3.
Click Add or Update a Favorite
4.
Select the favorite name from the list, select Update all annotations linked to this favorite, and click OK.
.
To break association with a favorite:
1.
Click Add or Update a Favorite
.
2.
Select the favorite name, select Break all links to this favorite, and click OK. Dimensions and annotations retain the properties previously applied by the favorite unless the items are reset to the document default (see below).
To delete a favorite:
1.
Select a style from Set a current Favorite.
2.
Click Delete a Favorite
.
The current favorite is set to. Dimensions and annotations retain the properties previously applied by the favorite unless the items are reset to the document default (see below). To reset a dimension or annotation's properties to the document defaults:
1.
Select dimensions or annotations with favorite styles.
2.
Click Apply the default attributes to selected items
.
The style is reset to (the document default). Selecting a favorite of unlinks the dimension or annotation from the favorite, but the item retains the properties already applied. To reset the dimension or annotation properties, use Apply the default attributes to selected items. The designation indicates that the dimension is not linked to any favorite, so any future changes to favorites are not applied.
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Add or Update a Favorite Enter a new name or choose an existing name Type a name to add a new favorite to the current document. - or Choose a favorite from the list to apply one of the following actions. •
Update all annotations linked to this favorite. All annotations using the selected favorite style are updated with the changes to the selected annotation.
•
Break all links to this favorite. All links between the selected favorite and annotations are broken. The annotations retain the attributes previously applied by the favorite unless the annotations are subsequently reset to the document default.
Dimensions in Drawings Dimensions Overview Dimensions in a SolidWorks drawing are associated with the model, and changes in the model are reflected in the drawing. Model Dimensions. Typically, you create dimensions as you create each part feature, then insert those dimensions into the various drawing views. Changing a dimension in the model updates the drawing, and changing an inserted dimension in a drawing changes the model. Mark for Drawings. When creating dimensions in part sketches, you can specify whether the dimension should be included when inserting model dimensions into drawings. Right-click the dimension and select Mark for drawing. You can also specify that dimensions marked for drawings be inserted automatically into new drawing views. Click Tools, Options, Document Properties, Detailing and select Dimensions marked for drawings under Auto insert on view creation. Reference Dimensions. You can also add dimensions in the drawing document, but these are reference dimensions, and are driven; you cannot edit the value of reference dimensions to change the model. However, the values of reference dimensions change when the model dimensions change. Color. By default, model dimensions are black. This includes dimensions that are blue in the part or assembly document (such as the extrusion depth). Reference dimensions are gray and appear with parentheses by default. You can specify colors for various types of dimensions in Tools, Options, System Options, Colors and specify Add parentheses by default in Tools, Options, Document Properties, Dimensions. Arrows. Circular handles appear on dimension arrows when dimensions are selected. When you click on an arrowhead handle (on either handle if there are two for the dimension), the arrows flip outside or inside. When you right-click on a handle, a list of arrowhead styles appears. You can change the style of any dimension arrowhead individually by this method. Selection. You can select dimensions by clicking anywhere on the dimension, including dimension and extension lines and arrows. Hide and Show Dimensions. You can hide and show dimensions with Hide/Show Annotations on the Drawing toolbar or View menu. You can also right-click a dimension and select Hide to hide the dimension. Hide and Show Lines. To hide a dimension line or extension line, right-click the line and select Hide Dimensions Line or Hide Extension Line. To show hidden lines, right-click the dimension or a visible line and select Show Dimension Lines or Show Extension Lines. Angular Dimension Display. You can change a dimension from diameter to radius or linear display and vice versa in the Dimension Properties dialog box or on screen. On screen, right-click an angular dimension and select:
12-6
•
Display As Diameter
•
Display As Radius
•
Display As Linear
Slant. When you insert or select dimensions, handles appear so you can drag the dimension to slant the extension lines. See the section on Display Options for removing the slant. Display Options. Right-click a dimension and select Display Options. The choices available depend on the type of dimension and other factors and can include the following: •
Remove Slant
•
Center Dimension
•
Offset Text
•
Change Plane
•
Align Ordinate
•
Add to Ordinate
•
Jog
•
Re-Jog Ordinate
•
Show Parentheses
•
Show as Inspection
Link external dim text. You can right-click the top-level icon in a drawing FeatureManager design tree and select or clear Link external dim text to control whether text added to a dimension is displayed. Text added to a dimension in a drawing becomes an attribute of the dimension. The default is to have the option enabled.
Setting Dimensions Options You can set options for dimensions in the current document. You can also specify properties for specific dimensions in a document, either in the Dimension Properties dialog box or in the PropertyManager. To set options for the current document:
1.
Click Tools, Options, Document Properties, Detailing, Dimensions.
2.
Change selections, offset distances, arrows, and so on.
3.
Click OK.
To set properties in the Dimension Properties dialog box:
1.
Right-click a dimension and select Properties. The Dimension Properties dialog box appears. NOTE: You can select more than on dimension by holding Ctrl while clicking dimensions. Some properties are not available for multiple dimensions.
2.
Change units, precision, arrow style, and so on.
3.
Click OK.
To set dimension properties in the PropertyManager:
1.
In the drawing graphics area, select a dimension. - or Hold Ctrl to select multiple dimensions. The Dimension PropertyManager appears.
2.
Change the dimension tolerance, precision, arrow style, and so on. The changes appear in the graphics area.
3.
Click More Properties to open the Dimension Properties dialog box.
4.
Click OK
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or click in the graphics area to close the PropertyManager.
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Chapter 12 Detailing
Dimension PropertyManager In the Dimension PropertyManager, you can specify the display of dimensions. If you select multiple dimensions, only the properties that apply to all the selected dimensions are available. Dimension Favorite •
Apply the default attributes to selected dimensions the document defaults.
. Reset the selected dimension or dimensions to
•
Add or Update a Favorite
•
Delete a Favorite
•
Save a Favorite . Opens the Save As dialog box with favorite (.sldfvt) as the default file type to save an existing favorite.
•
Load Favorites . Opens the Open dialog box with favorite (.sldfvt) as the active file type. You can use Ctrl or Shift to select multiple files.
•
Set a current Favorite. Choose a favorite style from the list to apply to the selected dimension or dimensions, or to delete or save the favorite.
. Opens the Add or Update a Favorite dialog box.
. Deletes the selected favorite from the document.
Tolerance/Precision Tolerance Type . Select from the list (None, Basic, Bilateral, Fit, and so on). The list is dynamic. For example, types for chamfer dimensions are limited to None, Bilateral, and Symmetric. Maximum Variation
. Type in a value.
Minimum Variation
. Type in a value.
Primary Unit Precision value. Tolerance Precision
. Select the number of digits after the decimal point from the list for the dimension . Select the number of digits after the decimal point for tolerance values.
Classification . Available only for Fit, Fit with tolerance, or Fit (tolerance only) types. Classification can be User Defined, Clearance, Transitional, or Press. Select a classification from the list. When you select either Hole Fit or Shaft Fit (below), the list for the other category (Hole Fit or Shaft Fit) is filtered based on the classification. Hole Fit and Shaft Fit from the lists, or type any text.
. Available only for Fit, or Fit with tolerance, or Fit (tolerance only) types. Select
NOTE: Bilateral tolerances (Maximum Variation and Minimum Variation) and parentheses are available in the Fit with tolerance or Fit (tolerance only) type if you specify Hole Fit or Shaft Fit, but not both. Fit tolerance display. Available only for Fit or Fit with tolerance types. Choose from: Stacked with line display Stacked without line display Linear display Show parentheses. Parentheses are available for Bilateral, Symmetric, and Fit with tolerance tolerance types. When selected, parentheses bracket the tolerance values.
12-8
Second Tolerance/Precision A second Tolerance/Precision section is available for Chamfer Dimensions. Fit and Fit with tolerance types are not available for chamfer dimensions. Dimension Text Text. The dimension appears automatically in the center text box, represented by. Click to place the pointer in any of the text boxes and type text. The three boxes represent a line of text above the dimension, the middle line containing the dimension (plus prefixes, suffixes, and any other text), and a line or lines below the dimension. If you delete , you can reinsert the value by clicking Add Value If you delete or modify the dimension, a message warns that overriding the dimension value text disables tolerance display. You can continue with the modified value, but you cannot add tolerances to the dimension.
For some types of dimensions, additional text appears automatically. For example, a Hole Callout for a counterbore hole or a hole with blind depth displays the diameter and depth of the hole (represented by <MOD-DIAM>xx). Hole Callouts for holes created in the Hole Wizard display information from the Hole Wizard. You can edit the text and insert variables from the Variables dialog box. Justify. You can justify text horizontally and, for some standards such as ANSI, you can justify the leader vertically. •
Horizontal - Left Justify
•
Vertical - Top Justify
, Center Justify , Middle Justify
, Right Justify , Bottom Justify
Symbols. Click to place the pointer where you want a symbol. Click a symbol icon (for Diameter, Degrees, and so on) or click More to access the Symbol Library. The symbol is represented by its name in the text box, but the actual symbol appears in the graphics area. Chamfer Dimension Display. Choose from: Distance X Distance Distance
, or Chamfer
, Distance X Angle
, Angle X
(available only for chamfers with 45° angles, generally used in JIS standard).
Arrows Placement. Click Outside
, Inside
, or Smart
.
The type of arrows and leaders available depends on the type of dimension selected. For example, the following types are available for Chamfer Dimensions: Horizontal Text Horizontal, Underlined Text Angled Text Angled, Underlined Text Style. Select an arrow style from the list. The default style is the specified style for the dimensioning standard (ISO, ANSI, and so on). Layer In drawings with named layers, select a layer.
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Chapter 12 Detailing
Break Dimension Lines Break Dimension Lines. Select for the dimension extension lines to break when crossing other extension lines in drawings. You can choose for the extension lines to break only when crossing arrowheads. Click Tools, Options, Document Properties, Dimensions and select Break around arrow head only. For ANSI standard, the check box is selected by default. Use document's gap. Select to use the document default set in Tools, Options, Document Properties, Dimensions. Gap. Enter a value if you do not use the document's default. When the dimension lines are broken, they break around lines that are nearby. If a dimension is moved significantly, it may not break around the new nearby dimensions. To update the display, unbreak the dimension lines and then break them again. More Properties Click More Properties to open the Dimension Properties dialog box.
Symbol Inserts a symbol into a dimension, a note, a geometric tolerance symbol, and so on. The libraries include ANSI, GOST, ISO, JIS, hole, key, modifying, and flag symbols. Flag symbols contain: •
A letter or number
•
A period or no period
•
A border (a circle, a square, both a circle and a square, a triangle, or a rotated triangle)
To add a symbol to text:
1.
Select a library from the Symbol libraries list.
2.
Select a symbol name from the list, and click OK. The selected symbol appears in the preview box. The symbol is represented by its name in the Note text preview box, but the actual symbol appears in the drawing note.
To delete a symbol that currently appears in text:
In the Symbol dialog box, select No Symbol and click OK. For dimensions, you can delete symbols in the Dimension PropertyManager. For a Note, you can double-click the note and delete the symbol code in the on-screen editor.
Dimension Properties To modify the dimension properties, do one of the following:
12-10
•
Right-click a dimension and select Properties.
•
Select multiple dimensions while holding down Ctrl, then right-click one of the selected dimensions, and select Properties. You can view and make changes to any properties that the selected dimensions have in common.
•
Select a dimension, or multiple dimensions. The Dimension PropertyManager appears. Click More Properties to open the Dimension Properties dialog box.
The following options are available for all dimensions: Value
Display as inspection dimension
Name
Read only
Full Name Units Font Arrow Style Arrows Precision
Display
Modify Text
Tolerance
Depending on the type of dimension (linear, radius, reference, and so on) or the type of document, the following options may be available: Driven
Diameter dimension
Specify Configs Display with parentheses
Foreshortened radius
Display as dual dimension
Dimension to inside of arc
Display with solid leader
Display as linear dimension
Use document's second arrow
First arc condition, Second arc condition
Display second outside arrow Display as chain dimension
Layer
Value The current value of the dimension. To change the value, either type a new value or use the arrows to increment the value. (Not available if you select multiple dimensions.) Name The name of the dimension (used in equations and design tables). To change the name, type a new name. (Not available if you select multiple dimensions.) Full Name The dimension name plus the name of the feature or sketch the dimension is associated with. (Read only. Not available if you select multiple dimensions.) Units Either select Use document’s units, as defined in the Dimension Options, or clear this check box and click Units to specify the unit type for the selected dimension. The available options depend on the type of dimensions that you selected. For example, an Angular Unit can be Deg, Deg/Min, Deg/Min/Sec, or Radians. A Length Unit can be Angstroms, Nanometers, Microns, Millimeters, Centimeters, Meters, Microinches, Mils, Inches, Feet, or Feet & Inches. For feet and inch units, you can choose Decimal or Fraction; if Fraction, you can specify the Denominator.
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Chapter 12 Detailing
Font Either select Use document’s font, as defined in the Dimensions Options, or clear this check box and click Font to select a new font type, style, and size for the selected items. Arrow Style You can change an arrow style in either the Dimension PropertyManager or the Dimension Properties dialog box. •
In the Dimension PropertyManager, under Arrows, select a style from the list.
•
In the Dimension Properties dialog box, under Arrow style, select or clear Use document's style. o
Select to use the style in Arrows Options.
o
Clear to choose a new style from the lists.
Two lists of arrow styles appear in the Dimension Properties dialog box. You can choose separate styles for each arrow when there are two arrows for a dimension. This feature supports the JIS dimensioning standard. Two lists appear in the Dimension PropertyManager only when separate styles are specified by the dimensioning standard. Arrows You can specify placement of arrows with respect to the dimension extension lines: Inside, Outside, Smart, or Document (uses the document defaults, as defined in the Detailing Options). Smart specifies that arrows automatically appear outside of extension lines if the space is too small to accommodate the dimension text and the arrowheads. Circular arrowhead handles
appear on dimension arrows when you select dimensions. The pointer changes to
when it is over the arrowhead handles. When you click on arrowhead handle (either handle if there are two for the dimension), the arrows flip outside or inside. You can change arrow styles. Display as inspection dimension Specifies whether to display the dimension as an inspection dimension.
Read only Specifies that the dimension cannot be changed. Dimension Precision Enter the number of decimal places for the precision of the dimension: •
Value
•
Tolerance
for the type of units: •
Primary Units
•
Alternate Units (in dual dimension display)
•
Angular Units
In the Dimension Options dialog box, all unit types are available. In the Dimension Properties dialog box, only those unit types that are appropriate for the selected dimensions are visible. In the Dimension PropertyManager, only the primary dimension and tolerance are visible. You can choose Same as nominal for the tolerance precision, so that if the precision of the dimension value changes, the precision of the tolerance changes with it. In the Dimension Properties dialog box and Dimension PropertyManager, (Document) after the precision indicates that the precision is the same as the document option.
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Dimension Display The Dimension Display dialog box controls the display of extension lines and leader lines. To access this dialog box, click Display in the Dimension Properties dialog box. •
Extension Lines. Select to display the first or second extension lines, or both.
•
Dimension Lines. Select to display the first or second dimension lines, or both.
•
Smart display of extension lines. Clear to enable manual placement of extension lines.
•
Use document's bend length. Clear so you can specify the dimension bent leader length. Type a value in the box.
•
Center between extension lines. Select so that dimensions are automatically centered between extension lines.
•
Dimension display. Select Use document's dimension display, or select one of the display styles available.
Driven Specifies that the dimension is driven by other dimensions and conditions, and cannot be changed. Display with parentheses Specifies whether to display the dimension as a reference dimension (with parentheses). Display as dual dimension Specifies that the dimension is displayed in both the document's unit system and the dual dimension units. Both units are specified in Tools, Options, Document Properties, Units. Display with solid leader Specifies the display of a solid line across the circle when its radial dimension uses outside arrows. Not available with ANSI standard.
Use document's second arrow Specifies that a diameter dimension (displayed as radial, not linear) with outside arrows follows the document default setting for use of a second arrow. To specify the document's default setting, click Tools, Options, and on the Document Properties tab click Dimensions. In the Arrows section, select the Display 2nd outside arrow (Radial) checkbox. To override the document default, clear the Use document's second arrow check box, then use the Display second outside arrow check box to turn the arrow display on or off. NOTE: This option is not visible in the DimensionProperties dialog box unless the selected dimension is a radial dimension.
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Display second outside arrow Specifies the display of a second arrow for a diameter dimension (displayed as radial, not linear) with Outside arrows. This is available only when the Use document's second arrow check box is cleared.
Second arrow ON
Second arrow OFF
Display as chain dimension Displays ordinate dimensions with an arrow from the base point to the dimension position. The measurement of the dimensions is from the base ordinate (the 0.0 mark). When you change this option for one member of a group of ordinate dimensions, the change is applied to all the members.
Option selected
Option cleared
Diameter dimension Specifies that the dimension on an arc or circle displays the diameter, not the radius. To convert a diameter dimension to a radius dimension, clear this checkbox. Foreshortened radius Specifies that the radius dimension line is foreshortened (broken) when the centerpoint of a radius is outside of the drawing or interferes with another drawing view.
To change the length or angle of the segments, click the dimension and drag the handles.
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Dimension to inside of arc Specifies that the dimension arrow is inside the arc. Use this option in combination with the Arrows setting (either Inside or Outside) to meet your drawing standards.
Dimension to inside ON Arrows set to outside
Dimension to inside OFF Arrows set to outside
Display as linear dimension Specifies the display of a diameter dimension as a linear dimension (not radial).
Linear
Radial
First arc condition, Second arc condition When you are dimensioning distances to arcs or circles, the following options are available: •
First Arc Condition specifies where on the arc or circle the distance is measured.
•
Second Arc Condition specifies where on the second item the distance is measured, when both items are arcs or circles.
In these examples, the First arc condition is Center, and the Second arc condition is set as noted.
Center (default)
Min (closest point)
Max (farthest point)
Layer To move the dimension to a different layer, select the name of the layer in the Layer list.
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Dimension Units/Chamfer Dimension Units Specify the Length Unit or Angular Unit for the selected dimensions. For Chamfer Dimensions, both Length Unit and Angular Unit are available. The available options depend on the type of dimension that you select. For some length dimensions, you can choose Decimal or Fractions. For Fractions, you can specify the Denominator and whether to round to the nearest fraction.
Dimensioning to Midpoints To dimension to a midpoint of a linear edge in a drawing:
1.
Click Smart Dimension
.
2.
Right-click the edge whose midpoint you want to dimension, and click Select Midpoint.
3.
Select the second entity to dimension, then click to place the dimension.
You can also dimension to midpoints when you are adding baseline dimensions or ordinate dimensions. Select the baseline or zero ordinate. Then follow Step 2 to dimension to midpoints as needed.
Reference Dimensions Reference dimensions show measurements of the model, but they do not drive the model and you cannot change their values. However, when you change the model, the reference dimensions update accordingly. Reference dimensions of features are suppressed when the features are suppressed. Reference dimensions are enclosed in parentheses by default. To prevent parentheses around reference dimensions, clear the Add parentheses by default check box in Tools, Options, Document Properties, Dimensions. You can control the color of reference dimensions in Tools, Options, System Options, Colors. Select Imported Annotations (Driven) and click Edit. You can use the same methods to add parallel, horizontal, and vertical reference dimensions to a drawing as you use to dimension sketches. For more information, see Dimensioning in Sketches. Ordinate Dimensions and Baseline Dimensions are both types of reference dimensions in drawings. Ordinate dimensions in sketches are driving dimensions. Reference dimensions are automatically hidden when a feature is suppressed. The dimensions are shown again when the feature is unsuppressed. To add a reference dimension:
1.
Select the drawing view.
2.
Click Smart Dimension
3.
Click the items you want to dimension.
on the Dimensions/Relations toolbar.
You can dimension to a silhouette edge. Point to the silhouette edge, and when the appears, click to dimension. 4.
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Click to place the dimension.
pointer
Parentheses Reference dimensions are shown in parentheses by default. To specify the default use of parentheses for all reference dimensions in the current document, click Tools, Options, Document Properties, Dimensions. Select the Add parentheses by default check box. To specify the use of parentheses on a particular dimension:
Right-click the dimension and select Properties. In the Dimension Properties dialog box, select or clear the Display with parentheses check box. - or Right-click the dimension and select Display Options, Show Parentheses. A check mark appears beside the menu item when the parentheses are shown.
Baseline Dimensions Baseline dimensions are reference dimensions. You cannot change their values or use the values to drive the model. Baseline dimensions are automatically grouped, and they are spaced at the distances specified in Tools, Options, Document Properties, Dimensions under Offset distances. To create a baseline dimension:
1.
Click Baseline Dimension
on the Dimensions/Relations toolbar, or click Tools, Dimensions, Baseline.
2.
Click the edge or vertex you want to use as a baseline.
3.
Click each of the edges or vertices you want to dimension.
4.
Click to place the dimensions.
If you select an edge, dimensions are measured parallel to the selected edge. If you select a vertex, dimensions are measured point-to-point from the selected vertex. Edge as baseline
Vertex as baseline
Ordinate Dimensions Ordinate dimensions are a set of dimensions measured from a zero ordinate in a drawing or sketch. In drawings, they are reference dimensions and you cannot change their values or use the values to drive the model. Ordinate dimensions are measured from the axis you select first. The type of ordinate dimension (horizontal, vertical, or angular) is defined by the orientation of the points you select.
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Example of Ordinate Dimensions Dimensioned to arc, with chain
Chain removed
Zero ordinate moved
Ordinate dimensions in a sketch
You can dimension to edges, vertices, and arcs (centers and minimum and maximum points). Ordinate dimensions are automatically grouped to maintain alignment. When you drag any member of the group, all the members move together. To disconnect a dimension from the alignment group, right-click the dimension, and select Break Alignment. You can drag the zero dimension to a new position, and all the ordinate dimensions update to match the new zero position. If adjacent dimensions are very close together, the leaders are automatically jogged as needed to prevent overlapping text. Drag handles are displayed at the bends when you select an ordinate dimension with a bent leader. You can remove the bend, or add a bend to a different ordinate dimension. You can specify that the leaders not be automatically jogged by clearing Automatically jog ordinates in Tools, Options, Document Properties, Dimensions. To create ordinate dimensions:
1.
Click Ordinate Dimension Ordinate.
on the Dimensions/Relations toolbar, or click Tools, Dimensions,
You can select Horizontal Ordinate Dimension or specify the direction of the dimensions.
Vertical Ordinate Dimension to
2.
Click the first item (edge, vertex, and so on) from which all others will be measured to be the base (the 0.0 dimension), and click again to place the dimension outside the model.
3.
Click the edges, or vertices, or arcs you want to dimension using the same ordinate. As you click each item, the dimension is placed in the view, aligned to the zero ordinate.
4.
Select another mode or another tool or press Esc to exit from the ordinate mode. Newly placed ordinate dimensions automatically jog to avoid overlapping text. The size of the jog is determined by the size of the text and the potentially overlapping area of the text.
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To modify ordinate dimensions:
You can modify ordinate dimensions using commands on the shortcut menu. Right-click an ordinate dimension, select Display Options, then choose from these options: •
Align Ordinate. Aligns all the dimensions along the ordinate with the 0.0 ordinate.
•
Add to Ordinate. Adds more dimensions later, along the same ordinate.
•
Jog. Bends the leader line of a dimension and allows you to reposition the dimension.
•
Re-jog Ordinate. Applies the automatic jogging algorithm to the selected ordinate dimensions.
•
Show Parenthesis. Adds parentheses around the selected dimensions.
•
Show as Inspection. Shows the selected dimensions as inspection dimensions.
To display as chain dimensions:
1.
Right-click an ordinate dimension and select Properties.
2.
Select the Display as chain dimension check box. All the dimensions along the ordinate are affected when you select or clear this check box.
Horizontal Ordinate Dimensions Creates horizontal ordinate dimensions in a drawing or sketch, measured horizontally from the entity you select first. To create horizontal ordinate dimensions:
1.
With a drawing or sketch active, click Horizontal Ordinate Dimension toolbar, or click Tools, Dimensions, Horizontal Ordinate.
on the Dimensions/Relations
2.
Click the first item from which all others will be measured, and click again to place the dimension.
3.
Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.
Vertical Ordinate Dimensions Creates vertical ordinate dimensions in a drawing or sketch, measured vertically from the entity you select first. To create vertical ordinate dimensions:
1.
With a drawing or sketch active, click Vertical Ordinate Dimension toolbar, or click Tools, Dimensions, Vertical Ordinate.
on the Dimensions/Relations
2.
Click the first item from which all others will be measured, and click again to place the dimension.
3.
Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.
Parallel Dimensions To add parallel dimensions to a drawing:
1.
Click Smart Dimension
, or click Tools, Dimensions, Smart.
2.
Click the geometry to dimension. As you move the pointer around the model, a preview of the dimension is displayed. The position of the pointer relative to the attachment points causes the dimension to snap to the appropriate type (horizontal, vertical, linear, radial, and so on). When the preview shows the desired dimension type, you can lock the type by right-clicking.
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3.
Click to place the dimension. To override the snap behavior before selecting the points to dimension, select either Dimension or
Horizontal
Vertical Dimension (or click Tools, Dimensions, Horizontal or Vertical).
Chamfer Dimensions You can dimension chamfers in drawings. In addition to the usual dimension display properties, chamfer dimensions have their own options for leader display, text display, and X display. X display is the size of the X in a chamfer dimension with two numbers, such as 1 X 45° (Length X Angle), 45° X 1 (Angle X Length) or 1 X 1 (Length X Length). Example of Chamfer Dimensions Chamfer dimensions can be displayed with various types of text and leaders and sizes of X.
Tolerance types for chamfer dimensions are limited to None, Bilateral, and Symmetric. You can set document default for chamfer dimension leader display, text display, and X display in Tools, Options, Document Properties, Dimensions, Leaders. To insert chamfer dimensions into a drawing:
1.
Click Chamfer Dimension Chamfer. The pointer changes to
2.
on the Dimensions/Relations toolbar or click Tools, Dimensions,
.
Select the chamfered edge, select one of the lead-in edges, then click in the graphics area to place the dimension. You must select the chamfered edge first. However, the dimension does not appear until you subsequently select one of the lead-in edges. The Dimension PropertyManager appears, and the tool remains active for you to dimension other chamfers.
3.
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Click OK
to close the Dimension PropertyManager.
Dimension Leaders/Text By default, the display of dimension text with respect to the leaders follows the selected dimensioning standard. You can override the default display. To override the default alignment for dimension text:
1.
Select Override standard’s leader display.
2.
Choose display types in each column as described below, and click OK.
Linear, Radial, and Angular Dimensions •
Solid leader, text aligned with leader
•
Broken leader, horizontal text
•
Broken leader, text aligned with leader
Chamfer Dimensions •
•
•
Leader display: o
Horizontal Text
o
Horizontal, Underlined Text
o
Angled Text
o
Angled, Underlined Text
Text display: o
Distance X Distance
o
Distance X Angle
o
Angle X Distance
o
Chamfer (available only for angles of 45 degrees)
X display: o
Uppercase X
o
Lowercase x
Leader/Text Display for Chamfer Dimensions You can select chamfer dimension leader display, text display, and X display in this dialog box. To set the document's defaults, click Tools, Options, Document Properties, Dimensions, Leaders. Leader Display Use the display specified in the document properties options, or choose from: Horizontal Text Horizontal, Underlined Text Angled Text Angled, Underlined Text You can also select these display types in the Dimension PropertyManager.
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Text display Use the display specified in the document properties options, or choose from: •
1 X 1 (Distance X Distance)
•
1 X 45° (Distance X Angle)
•
45° X 1 (Angle X Distance)
•
C1 (Chamfer distance, available only for angles of 45°) You can also select these display types in the Dimension PropertyManager.
X Display Use the display specified in the document properties options, or choose from: •
X (Uppercase)
•
x (Lowercase)
Moving and Copying Dimensions Once dimensions are displayed in a drawing, you can move them within a view or to another view. When you drag a dimension from one place to another, the dimension reattaches to the model, as appropriate. You can only move or copy dimensions to a view where the orientation is appropriate for that dimension. •
To move a dimension within the view, drag the dimension to the new position.
•
To move a dimension from one view to another view, hold the Shift key as you drag the dimension into another view.
•
To copy a dimension from one view to another view, hold the Ctrl key as you drag the dimension into another view.
•
To move or copy several dimensions at once, hold the Ctrl key as you select
Aligning Dimensions To select a group of dimensions:
You can select a group of dimensions in a drawing view either by holding the left mouse button and dragging a box around the dimensions or by holding Ctrl while selecting them. The selected dimensions must be of the same type. You can align dimensions: •
Parallel/Concentric
•
Collinear/Radial See also Ordinate Dimensions.
To identify members of an aligned group:
Right-click the dimension you want to know about. •
If the selected dimension is a member of an aligned group, you can select Show Alignment to display a blue dot on each of the other members of the group.
•
If the selected dimension is not a member of an aligned group, the Show Alignment item does not appear in the shortcut menu.
To ungroup aligned dimensions:
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•
Right-click the dimension to ungroup, and select Break Alignment. The selected dimension is disconnected from the group, and may be moved freely; the other dimensions in the aligned group remain connected.
•
To break the entire group, select all the members of the group, then right-click one and select Break Alignment.
To center dimension text between extension lines:
•
Right-click a dimension (linear, radial, or angular), and select Display Options, Center Dimension.
•
If the text is inside the extension lines (or inside the circle, in the case of a radial or diameter dimension), it snaps to the center, and is locked in position between the extension lines. If the text is outside the extension lines, it remains outside.
•
To unlock the text position, right-click the dimension, and select Center Dimension again to toggle the option.
•
You can also drag the text toward the center of the extension lines to snap it to the center. When you center dimension text this way, its position is not locked between the extension lines, so you can move it freely.
To offset dimension text from its arrows:
•
Right-click a dimension (linear, linear radial, or angular), and select Display Options, Offset Text.
•
A leader is attached to the dimension text, and you can drag the text to a new location. When you select an offset dimension, a handle is displayed where the leader attaches to the arrows so you can move the arrows away from the model if needed.
•
To restore the dimension to its position between the arrows, right-click the dimension again, and select Offset Text again to toggle the option. Before Offset
Offset
Align Dimensions Parallel/Concentric In a drawing view, you can align selected linear, radial, or angular dimensions with uniform spacing. The selected dimensions must be of the same type. To align and group parallel dimensions:
1.
In a drawing view, hold Ctrl and select two or more dimensions that you want to align. You can also select the group of dimensions by holding the left mouse button and dragging a box around the dimensions.
2.
Click Align Parallel/Concentric
or Tools, Dimensions, Align Parallel/Concentric.
The dimensions are arranged with a uniform distance between the arrows. They also are grouped, and retain the parallel spacing when moved. Aligned Parallel
Aligned Concentric
To specify the distance between dimensions:
1.
Click Tools, Options, Document Properties, Dimensions.
2.
Under Offset distances, specify a value for From last dimension (B) (the distance between dimensions). The From model (A) value (the distance between the first dimension and the model) is not used with Align Dimensions Parallel/Concentric; it is used only with baseline dimensions.
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Align Collinear/Radial Dimensions In a drawing view, aligns and groups selected linear, radial, or angular drawing dimensions. The selected dimensions must be of the same type. To align and group dimensions to be collinear:
1.
In a drawing view, select a group of dimensions.
2.
Click
or Tools, Dimensions, Align Collinear/Radial.
The selected dimensions are arranged in a straight line. They also are grouped, and retain the linear arrangement when moved.
Aligned Collinearly
Aligned Radially
Dimension Extension Lines You can change the default attachment point of dimension extension lines, slant the extension lines, flip the direction of a leader, and drag extension lines between the center, minimum, and maximum attachment points of arcs and circles. You can specify in the Dimension PropertyManager that extension lines break when they cross other extension lines and specify in Tools, Options, Document Properties, Dimensions that the lines break only around dimension arrows. You can hide and show dimension lines and extension lines. Right-click a dimension line or extension line and select Hide Dimension Line or Hide Extension Line. To show hidden lines, right-click the dimension or a visible line and select Show Dimension Lines or Show Extension Lines. To change the attachment point of dimension extension lines:
1.
Select a dimension. Handles are displayed at the attachment end of the extension lines. The pointer changes to is over a handle.
2.
Drag a handle to the desired position or to a vertex (watch for the inferencing pointer
when it
).
If you choose a vertex, the default extension line gap is used. In sketches, the value of the dimension changes to reflect the new attachment point. In drawings, you can move attachment points only for reference dimensions, and the value is not updated. To return the extension line to its original position, right-click the dimension and select Display Options, Default Extension Snap.
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To slant dimension extension lines:
When you insert or select a dimension, handles appear so you can drag the dimension to slant the extension lines. Drag a handle at the end of the extension line nearest the arrow (the pointer changes to when it is over a handle that effects the slant). To return the dimension to its original position, right-click the dimension and select Display Options, Remove Slant. You can also drag the handle until the dimension snaps back to its original position.
To flip the direction of a dimension leader:
If a vertical dimension is displayed with horizontal text (in ANSI standard, for example), you can flip the direction of the leader. Select the dimension, then click the handle at the bend in the leader (the pointer changes to over the handle).
when it is
Example of Dimension Line Terminology
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Modify Text of Dimension You can modify the text of a dimension by adding prefix or suffix text and symbols. This functionality is also available in the Dimension PropertyManager. The dimension value is represented by in the middle box. To change the text of a dimension:
1.
Place the cursor in the Dimension Text box where you want to make changes. You can make the following changes: •
Add text before or after the dimension (in the middle box).
•
Add text or symbols above or below the dimension (in the upper or lower boxes).
•
Delete the dimension. If you delete or modify the dimension, a message warns that overriding the dimension value text disables tolerance display. You can continue with the modified value, but you cannot add tolerances to the dimension.
2.
To add a symbol, place the cursor in the text box where you want the symbol to appear. Click the symbol buttons on the left, - or Click Add Symbol. Select a library from the Symbol Libraries list. Select a symbol name from the list, and click OK. The symbol’s name is displayed in the Dimension Text box, but the actual symbol appears in the Preview box and in the drawing.
3.
To replace the dimension value if it was deleted, click Add Value.
4.
Click OK to return to the Dimension Properties dialog box. You can observe the resulting dimension text in the Preview box as you add text and symbols.
Modify Dimension You can change a dimension in a part, sketch, assembly, or drawing in the Modify dialog box. To change a dimension:
1.
Double-click a dimension. The Modify dialog box appears.
2.
Change the dimension value with the arrows or by typing in the dimension box. NOTE: You can use the dimension box as a calculator by entering values and arithmetic symbols directly.
3.
If the model has multiple configurations, you can apply the new value to This configuration only or to All configurations, or you can Specify configurations.
4.
Use the buttons as follows: Save the current value and exit the dialog. Restore the original value and exit the dialog. Rebuild the model with the current value. Rebuild is available in drawings if the model is not being edited in another document. Reset spin increment value. Mark dimension to be imported into drawing. Available only in part and assembly documents. When you Insert Model Items into a drawing, you can insert all dimensions or only those marked.
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Specify Configurations When you modify a dimension in a model with multiple configurations, you can specify the configurations to modify from the Modify or Dimension Properties dialog boxes. To modify a dimension in specified configurations from the Modify dialog box:
1.
Double-click the dimension to modify.
2.
In the Modify dialog box: a.
Change the dimension.
b.
Select Specify Configuration(s).
c.
Click Save
.
A dialog box appears. 3.
Select the configurations to modify. NOTE: Click Reset Selection to revert to the configuration that you modified.
4.
Click OK.
To modify a dimension in specified configurations from the Dimension Properties dialog box:
NOTE: This procedure applies only when you modify a sketch dimension. 1.
Right-click the dimension to modify and select Properties.
2.
In the Dimension Properties dialog box: a.
Change the dimension Value.
b.
Click Specify Configs. A dialog box appears.
3.
Click Specify configurations.
4.
Select the configurations to modify. NOTE: Click Reset Selection to revert to the configuration that you modified.
5.
Click OK.
6.
Click OK again to close the Dimension Properties dialog box.
Increment Linear Measure: Specifies the number of units added or subtracted when you click a spin box arrow to change a linear dimension value. Angular Measure: Specifies the number of degrees added or subtracted when you click a spin box arrow to change an angular dimension value. Select the Make Default check box to make your new specification the default for dimension increments.
Hide/Show Annotations Hide/Show Annotations allows you to toggle the visibility of individual annotations (dimensions and cosmetic threads) in a drawing. Hiding a dimension has a different effect than deleting it: •
If you hide a dimension, it is still present in the view. Therefore, it is not restored if you import dimensions again.
•
If you delete a dimension, it may be restored if you import dimensions again (if it does not already appear in another view).
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To hide or display dimensions:
1.
Click Hide/Show Annotations
on the Drawing toolbar, or click View, Hide/Show Annotations.
All dimensions and cosmetic threads are displayed; hidden dimensions and cosmetic threads are in gray.
2.
Click the dimensions and cosmetic threads that you want to show or hide. You can also right-click a dimension and select Hide. To show the dimension again, use the method described above.
Dimension Tolerance The Dimension Tolerance dialog box appears in both Dimensions Options and in the Dimension Properties dialog box. It controls the dimension tolerance values and the display of non-integer dimensions. The options available depend on the type of tolerance selected and whether you are setting options or applying the specifications to selected dimensions. A window previews the dimension and the tolerances. Tolerance type Select one of the following from the list: None, Basic, Bilateral, Limit, Symmetric, MIN, MAX, or Fit, Fit with tolerance, or Fit (tolerance only). Tolerance values Specify the Maximum Variation tolerance that you selected. Hole Fit
and/or Minimum Variation
values as appropriate for the type of
and Shaft Fit
Hole Fit and Shaft Fit are available only for Fit, Fit with tolerance, or Fit (tolerance only) types for Dimension Properties only. Specify a letter. NOTE: Tolerances and parentheses are available in the Fit with tolerance type if you specify Hole Fit or Shaft Fit, but not both. Font/Fit tolerance font Specify the font to use for the dimension tolerance text. For Fit and Fit with tolerance, Fit tolerance font is available for the Hole Fit and Shaft Fit text. •
Select Use dimension’s font if you do not want to change the font size for the dimension tolerance text.
•
To change the size of the dimension tolerance text, clear Use dimension's font and select either: o
Font Scale. Enter a number from 0 to 10.0 to scale the font.
o
Font Height. Enter a value to specify the font height.
Show parentheses Select for parentheses around the tolerances for Bilateral, Symmetric, or Fit with tolerance types. Linear tolerance or Angular tolerance Choose either Linear tolerance or Angular tolerance. The available options depend on the category you select.
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Fit tolerance display Choose either Stacked with line display
, Stacked without line display
, or Linear Display
.
Fit Tolerances Fit tolerances are available for dimensions in the Dimension PropertyManager. Fit tolerances are used typically for shafts in holes. Example of Fit Tolerances Hole dimension (top), Fit tolerance with Clearance and automatically calculated bilateral tolerance.
Shaft dimension (bottom), Fit tolerance with Clearance and automatically calculated bilateral tolerance.
Shaft dimension, both Hole and Shaft Fit tolerance type, Stacked with line display.
Hole dimension, Fit (tolerance only) type.
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Tolerance Types You can choose from the following types for showing Fit tolerances: •
Fit
•
Fit with tolerance
•
Fit (tolerance only)
Classification You can choose from the following classifications. The shaft and hole tolerances available are filtered to correspond to the classification. •
User Defined
•
Clearance
•
Transitional
•
Press
Hole Fit
and Shaft Fit
You can choose standard Fit tolerances from the hole and shaft lists. The software automatically checks whether the standard is appropriate for the dimension. When you select either a hole or a shaft Fit tolerance, the list for the other type is filtered to present only corresponding tolerances. The bilateral tolerances are also calculated automatically. NOTE: The Classification aid for selecting an appropriate Fit designation is either Hole Basis or Shaft Basis, depending on which Fit designation you choose first. As Hole Basis and Shaft Basis Fit classifications in the international standards are not fully bi-directional, you may get a different list of suggested Fit choices (or an empty list) depending upon the order in which you choose your designations. Hole Basis is preferred for most manufacturing processes Automatic Versus User Defined Tolerance The advantage of letting the SolidWorks software calculate the bilateral tolerance values for you is that if the dimension changes, the tolerances are updated automatically. To set tolerances manually, click the Hole Fit or Shaft Fit icon and type values in the Maximum Variation
and Minimum Variation
boxes.
Fit Tolerance Display For Fit or Fit with tolerance with both hole and shaft tolerances, you can select a display style. Stacked with line display Stacked without line display Linear display With Fit (tolerance only), the Fit standards are not displayed. Parentheses The Show parentheses check box is available for Fit with tolerance, but not for Fit or Fit (tolerance only).
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Annotations Annotations Overview Annotations behave like dimensions in each type of SolidWorks document. You can add annotations in a part or assembly document, then insert them to the drawing views, or you can create annotations in the drawing. For information on inserting annotations from models into drawings, see Inserting Model Items into Drawings. For information on setting options for annotations, see Annotations Options Overview. You can select annotations tools either from the Insert menu or from the Annotations toolbar.
The Align tools are available for aligning annotations. See Aligning Annotations.
You can change the arrowhead style on annotations by right-clicking the arrow to access a menu of styles. When you select an annotation, the geometry to which the annotation is attached is highlighted. You can select annotations by clicking any portion of them, including leaders and arrows. You can create multiple annotations without closing the dialog box or PropertyManager. This functionality applies to Notes, Surface Finish Symbols, Datum Feature Symbols, and Geometric Tolerancing. See Multiple Annotations. You can hide annotations and then show them again. For drawings, see Hide/Show Annotations. For parts and assemblies, click View, All Annotations to toggle the display.
Annotations Options Overview You can set options for annotations in various places. •
Annotations Display Options. Applies options to all annotations in the current document. Click Tools, Options, Document Properties, Annotations Display.
•
Annotation Properties. Contains the same options as Annotations Display. Right-click the Annotations folder
in the FeatureManager design tree and select Details.
•
Annotations Font Options. Sets separate fonts for various types of annotations (Note, Dimension, and so on). Click Tools, Options, Document Properties, Annotations Font.
•
Annotation Colors. Specifies colors for imported and non-imported annotations. Click Tools, Options, System Options, Colors.
The following types of annotations have their own options: •
Notes Options. Alignment, leaders, and borders for notes. Click Tools, Options, Document Properties, Notes.
•
Balloons Options. Style, size, text category, and leaders for balloons, and autoballoon layout. Click Tools, Options, Document Properties, Balloons.
•
Arrows. Size and style of arrows. Click Tools, Options, Document Properties, Arrows.
•
Virtual Sharps. Display of virtual sharps. Click Tools, Options, Document Properties, Virtual Sharps.
•
Tables Options. Various properties of hole, revision, and Bill of Materials tables. Click Tools, Options, Document Properties, Tables.
•
View Labels Options. Text and display of drawing view labels. Click Tools, Options, Document Properties, View Labels.
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Some annotations also have PropertyManagers or Properties dialog boxes for applying changes to individual annotations or a group of annotations. To access a PropertyManager, select the annotation. To access a Properties dialog box, right-click the annotation (or hold down Ctrl while selecting a group of annotations, then right-click one annotation) and select Properties.
Annotation Properties Lets you select the types of annotations that you want to display and set text scale and other annotations options. To select the types of annotations to display:
1.
In the FeatureManager design tree, right-click the Annotations folder,
, and select Details.
2.
In the Annotation Properties dialog box, specify a Display Filter by selecting the annotation types to display by default: Cosmetic threads
Geometric tolerances
Datums
Notes
Datum targets
Surface finish
Feature dimensions
Welds
Reference dimensions - or Select Display all types to show all kinds of annotations available for that part or view. 3.
Change the values in the Text scale edit box to change the scale of the text used in the annotations. NOTE: Always display text at the same size must be cleared, to specify a scale for the default size of annotation text.
4.
5.
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Select from the following options: •
Always display text at the same size. When checked, all annotations and dimensions are displayed at the same size regardless of zoom. Note that drawings have this option disabled and always zoom the text height.
•
Display items only in the view orientation in which they are created. When checked, any annotation is displayed only when the model is viewed in the same orientation as when the annotation was added. Rotating the part or selecting a different view orientation removes the annotation from the display.
•
Display annotations / Display assembly annotations. When checked, all annotation types that are selected in the Display filter are displayed. For assemblies, this includes not only the annotations that belong to the assembly, but also the annotations that are displayed in the individual part documents.
•
Use assembly’s setting for all components. When checked, the display of all annotations matches the setting for the assembly document, regardless of the setting in the individual part documents. Use this option along with Display assembly annotations to display different combinations of annotations.
•
If you use JIS dimensioning standards, specify the JIS surface finish size (1,2,3 characters) or Scale.
Click OK to accept your changes; click Cancel to exit the dialog without saving the changes.
Multiple Annotations The term multiple annotations refers to: •
Creating multiple instances of a type of annotation
•
Copying and pasting any combination of annotations and other entities
Multiple instances of an annotation You can create multiple instances of a type of annotation without closing the PropertyManager or dialog box. This functionality applies to: •
Notes
•
Surface Finish Symbols
•
Datum Feature Symbols
•
Geometric Tolerancing
To create multiple annotations:
1.
With nothing selected, click the appropriate tool from the Annotations toolbar, or click Insert, Annotations and select a tool from the menu. The PropertyManager or Properties dialog box for the tool appears.
2.
Type in text and select options as desired.
3.
With the PropertyManager or dialog box still open, click in the graphics area to place the annotation.
4.
•
Click as many times as necessary if you need to place multiple copies.
•
If the annotation has a leader, click once to place the leader, then click a second time to place the annotation.
•
To add a Multi-jog Leader to a Note, Geometric Tolerance Symbol, or Surface Finish Symbol, before placing the note or symbol, right-click and select Use Multi-jog Leader. Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point. To complete the leader and place the note or symbol, either double-click or right-click and select End Leader.
•
You can change text and other items in the dialog box for each instance of the annotation.
Click OK.
Combinations of annotations You can move or copy multiple annotations as follows: •
You can select any combination of annotations, dimensions, drawing views, and sketch entities. You can select items individually or by box selection.
•
You can cut and paste or drag multiple items in drawings, or you can use the Move or Copy tool. Any individual item can be moved, deleted, and so on at the new location.
•
When you paste multiple items, the paste point is the center of all the selected items. All pasted items retain their relative positions.
•
You can cut or copy items from one drawing sheet and paste them on another sheet.
•
You can cut or copy items that belong to different views. When pasted, the items are all attached to the active view.
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Aligning Annotations You can align annotations by inferencing or by using the Align tools. Inferencing You can control the snap behavior of detail items that you move. Click Tools, Options, System Options, Drawings. Under Detail Item Snapping, you have these options: •
Infer when dragging corner. When checked, you drag the selected item by the corner handles to infer to the corner of another detail item.
•
Infer when dragging center. When checked, you drag the center of the item to infer to the center of another detail item.
•
To ignore all inferences, and to prevent the display of inferencing lines, press the Alt key while dragging detail items.
To align an annotation with a neighboring annotation, drag the item (note, balloon, and so on) until inferencing lines appear. The item snaps to align with its neighbor. Align Tools You can access the Align tools in three ways: •
Click a tool button on the Align toolbar.
•
Click Tools, Align Annotation, and select a tool from the menu.
•
Select a group of annotations, right-click one of the annotations, select Align, and choose one of the options.
The Align tools are as follows:
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Leftmost
The left edges of all selected annotations line up at left edge of the leftmost one.
Rightmost
The right edges of all selected annotations line up at right edge of the rightmost one.
Uppermost
The top edges of all selected annotations line up at top edge of the uppermost one.
Lowermost
The bottom edges of all selected annotations line up at bottom edge of the lowermost one.
Space evenly across
The space is the largest space between selected annotations.
Space evenly down
The space is the largest space between selected annotations.
Center Horizontal
The centers of the annotations line up with the center of the leftmost annotation.
Center Vertical
The centers of the annotations line up with the center of the uppermost annotation.
Compact Horizontal
The edges of the annotations line up with each other in the horizontal direction. The leftmost annotation does not move.
Compact Vertical
The edges of the annotations line up with each other in the vertical direction. The uppermost annotation does not move.
Multi-jog Leaders You can use the Multi-jog Leader in drawings to create leaders with as many bends as required, or to create simple arrows or block diagrams. For example, a multi-jog leader can point a note to an entity in a drawing that is difficult to reach with a straight or bent leader. Some items to note about multi-jog leaders are as follows: •
You can attach multi-jog leaders to annotations, sketch entities, or model edges or faces, or you can insert a leader without attaching it to anything.
•
A preview of each segment of the leader appears as you move the pointer.
•
You can add jog points and branches to multi-jog leader segments.
•
You can start a multi-jog leader anywhere on a drawing sheet. You can end a leader anywhere on a drawing sheet by double-clicking. When a leader is not attached to an entity, the arrow at the endpoint follows the Unattached option in Tools, Options, Document Properties, Arrows. You can manually select a different arrow at the endpoint with a shortcut menu.
•
Multi-jog leaders inference to geometry. If you click a multi-jog leader point at an entity (for example, an edge or a face), the leader attaches to the entity with an smart arrow, and the leader is complete. To avoid inferencing and to prevent attaching to an entity, press Tab. The Tab key toggles between smart attachment and no attachment.
To add a multi-jog leader while creating an annotation:
1.
Click an annotation tool on the Annotation toolbar. NOTE: The annotations that currently support this method of inserting a multi-jog leader are Note, Surface Finish Symbol, and Geometric Tolerance Symbol.
2.
Edit properties in the annotation PropertyManager or dialog box.
3.
Before placing the annotation, right-click and select Use Multi-jog Leader.
4.
Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point.
5.
To complete the leader and place the annotation, either double-click or right-click and select End Leader.
Multi-jog leaders with other annotations •
You can attach a multi-jog leader to a dock point of an annotation (Note, Surface Finish Symbol, Geometric Tolerance Symbol, Weld Symbol, or Balloon).
•
Multi-jog leaders attached to annotations or sketch entities move with the annotations or entities.
•
When you specify a bent leader for an annotation, the length of the bent leader is set in Tools, Options, Document Properties, Dimensions. For documents in ANSI standard, bent leader is the default.
To create a multi-jog leader:
1.
Click Multi-jog Leader
on the Annotation toolbar, or click Insert, Annotations, Multi-jog Leader.
2.
Click the drawing sheet, at a dock point
3.
Move the pointer and click in the graphics area for each jog point.
4.
Complete the leader by clicking an entity such as an edge, or double-click the drawing sheet.
on an annotation, or at a point on a sketch entity.
To add a jog point:
Right-click a segment of the leader (the pointer changes to when it is over a segment) and select Add Jog Point. The jog point is added at the midpoint of the segment. You can drag the jog point. To delete a jog point:
Right-click the jog point (the pointer changes to Point.
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when it is over a jog point) and select Delete Jog
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To change the arrow at an endpoint:
Right-click the endpoint (the pointer changes to style from the menu.
when it is over an endpoint) and select an arrowhead
To add a branch:
Right-click a jog point and select Insert New Branch. Move the pointer and click to add segments to the branch. To delete a multi-jog leader:
Right-click anywhere along the leader and select Delete Leader, or select the leader and press Delete.
Notes A note can be free floating or placed with a leader pointing to an item (face, edge, or vertex) in the document. It can contain simple text, symbols, parametric text, and hyperlinks. The leader can be straight, bent, or multi-jog. To set Note options for the current document, click Tools, Options, Document Properties, Notes. To create notes:
1.
Click Note
on the Annotation toolbar, or click Insert, Annotations, Note.
The Note PropertyManager appears. 2.
Edit properties (arrows, leaders, font, border, and so on).
3.
Click in the graphics area to place the note. •
To add a Multi-jog Leader to the note, before placing the note, right-click and select Use Multijog Leader. Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point. To complete the leader and place the note, either double-click or right-click and select End Leader.
•
If the note has a leader, click first to place the leader, then again to place the note. A leader appears if you select Leader under Arrows/Leaders, or if you select Auto Leader and move the pointer near an object. See below for the procedure to add Multi-jog Leaders.
4.
Type the text.
5.
Click in the graphics area outside the note to complete the note.
6.
With the Note PropertyManager still open, repeat steps 2 through 5 to create as many notes as necessary.
7.
•
You can change text, properties, and formatting for each instance of the note.
•
To add multiple leaders, press Ctrl while dragging the note and before placing it. The note stops moving and a second leader appears. While still holding Ctrl, click to place the leader. Click as many times as necessary to place additional leaders. Release Ctrl and click to place the note.
Click OK
.
To create a note with a multi-jog leader:
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1.
Click Note
on the Annotation toolbar, or click Insert, Annotations, Note.
2.
Edit properties in the Note PropertyManager.
3.
Right-click in the graphics area and select Use Multi-jog Leader.
4.
Click in the graphics area to place the leader attachment point, then move the pointer and click in the graphics area for each jog point.
5.
To complete the leader and place the note, either double-click in the graphics area or right-click and select End Leader.
6.
Type the note text and click in the graphics area outside the note to complete the note.
To edit note text:
Double-click the note and edit the text in place. NOTE: During on-screen editing of notes, Pan, Zoom, and Rotate operations are not available. To edit note properties:
Select a note, or more than one note, and edit properties in the Note PropertyManager. NOTE: You can also right-click a note and select Properties to access the Note Properties dialog box. You can add more leaders to an existing note by holding down Ctrl and dragging a leader attachment point. Notes snap to a grid if the Display grid and Snap to points or Snap to angle options are selected. To set these options, click Tools, Options, Document Properties, Grid/Snap. Empty notes, which appear on screen as a box with an X
, do not appear in print previews or on printed pages.
Hyperlinks in Notes You can add an embedded hyperlink in a note, or you can add a floating hyperlink in any SolidWorks document. The hyperlink can be to a document on the Internet, on your local network, or on your own hard drive. If the link is to a web site, selecting the hyperlink launches a web browser, if one is not already running, and opens the associated URL (web site). If the link is to a SolidWorks document, clicking the link opens the document. If the link is to another type of document, such as a Word or Excel file, clicking the hyperlink launches the appropriate application, and opens the document. The actual path of a hyperlink embedded in a note does not appear in the note text. A hyperlinked note is displayed in blue; when the pointer moves over a note that contains a hyperlink, the pointer changes to a hand
, and the tooltip
indicates the path of the link. A floating hyperlink (one that is not attached to note text) displays the full path of the link (for example, HTTP://www.solidworks.com) in blue. NOTE: Because clicking a hyperlinked note activates the link, moving or editing a hyperlinked note can be difficult. Move the hyperlink pointer the note pointer
over the note until a box appears around the text. Point to a corner of the box. When
is displayed, drag the note to move it, or right-click the note to edit its properties.
To create an embedded hyperlink:
1.
Create a note, and click Insert Hyperlink while editing a note’s properties.
in the Note PropertyManager. You can also add a hyperlink
2.
Enter the path (or browse to the document) to which you want to link the note text. For a World Wide Web location, enter the website name in the format www.website.com. (You do not need to enter HTTP://)
3.
Click Use relative path for hyperlink if you want to the specify a directory path relative to the current location instead of the full pathname.
4.
Click OK to accept the path.
To create a floating hyperlink:
1.
Click Insert, Hyperlink.
2.
Enter the path (or browse to the document) and click OK. If you edit the properties of a floating hyperlink, you will see that it is a note, the text of which is $URL (a variable representing the path of the link).
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Note PropertyManager Use the Note PropertyManager to insert a Note, or to edit an existing note or balloon note. You can create a freefloating note or a note with a leader. •
You can place multiple notes without closing the Note PropertyManager. You can change the text and other properties for each note.
•
To edit text after creating a note, double-click the note and edit in place.
•
You can also edit note properties in the Note Properties dialog box.
Note Favorite In addition to the functionality described in Favorites, notes have two types of favorites: •
With text. If you type text in a note and save it as a favorite, the text is saved the with note properties. When you create a new note, select the favorite, and place the note in the graphics area, the note appears with the text. If you select text in the document and then select a favorite, the properties of the favorite are applied without changing the selected text.
•
Without text. If you create a note without text and save it as a favorite, only the note properties are saved.
Text Format Alignment. Choose Left Align Angle
, Center Align
, or Right Align
.
. Enter a value. A positive angle rotates the note counterclockwise.
Insert Hyperlink
. Click to include a Hyperlink in the note.
Link to Property
. Click to link a note to a document property.
Add Symbol . Place the pointer in the Note text box where you want the symbol to appear, then click Add Symbol. In the Symbol dialog box, select a library from the Symbol library list, then select a symbol name from the list, and click OK. The symbol’s name is displayed in the text box, and the actual symbol appears in the note. Use document's font. When selected, the text is in the font specified in Tools, Options, Document Properties, Notes. Font. When Use document's font is cleared, click Font to open the Choose Font dialog box and select a new font style, size, and effect. Block Settings The Block Settings section is available only when editing block definitions. Text appears in the Tag name box for notes with attributes imported from AutoCAD. You can also type tag names for notes created in the SolidWorks block definition editor. You can choose for a tag to be Read only, Invisible, or both. The Tag name and its attributes are shown in the Attributes editor, which you can access in the Block Instance PropertyManager. Border Style. Specifies the shape of the border (geometric shapes that enclose the text), or None. Size. Specifies either Tight Fit to the text, or a fixed number of characters.
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Leader Click Leader entity.
, No Leader
, or Auto Leader
Click Straight Leader , Bent Leader the shortcut menu as you create a note. Click a leader position of Leader Left
. Auto Leader inserts a leader if you attach the note to an
, or Underlined Leader
, Leader Right
, or Leader Nearest
Select an arrowhead style from Arrowhead Style. Smart Arrowhead (
to a face,
. You can add a Multi-jog Leader from
.
applies the appropriate arrowhead
to an edge, for example, depending on the detailing standard).
Select Apply to all to apply a change to all of the arrowheads of the selected note. If the selected note has multiple leaders, and Auto Leader is not selected, you can use a different arrowhead style for each individual leader. Layer In drawings with named layers, select a layer. Note Properties You can use the Note Properties dialog box to edit the properties of a Note or balloon note. After you have created a note and closed the Note PropertyManager, you can edit the text by double-clicking the note and editing in place, or by right-clicking the note and selecting Properties to open the Properties dialog box. You can also select a note and edit its properties in the Note PropertyManager. You can specify the following properties in the Note Properties dialog box. Note text/Balloon note text Type the text into the Note text box. For a parametric note, select a dimension on the drawing. If the note is a Balloon or Stacked Balloon, the title of the text section is Balloon note text. There are boxes for the type of text and the actual text for the Upper and Lower sections of the balloons. Add Symbol To add a symbol to the note text, place the pointer in the Note text box where you want the symbol to appear, then click Add Symbol. Select a library from the Symbol library list, then select a symbol name from the list, and click OK. The symbol’s name is displayed in the text box, and the actual symbol appears in the note. Layer To move the note to a different layer, select the name of the layer in the Layer list. Angle Type the text angle in the Angle box, or use the arrows to set the value. Text justification Text can be justified Left, Center, or Right. Text justification is not available for Balloons or Stacked Balloons. Stack Data For Stacked Balloons only. You can stack the balloons Up, Down, Left, or Right.
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Balloons per line For Stacked Balloons only. Set the number of balloons to stack in one line before starting the next line. Leader •
Choose one of the following: o o
o
Always show leaders. Automatic leaders. Adds a leader if you click an entity when you place the note; no leader if you click on the sheet or view. No leaders.
•
Style. If the selected note has a leader or if you select Always show leaders, you can choose the leader style to be Straight, Bent, or Underlined. NOTE: For balloons, the Underlined style is available under Border Style.
•
Display with bent leader. If the note is a balloon note and has a leader, you can choose the leader line to be bent.
•
Arrow style. When the Smart check box is selected, the arrow styles specified in Tools, Options, Document Properties, Detailing, Arrows are used. To choose a different arrow style, clear the check box and select a style from the list.
•
Leader anchor. Choose a default position: Closest, Left, or Right.
•
Apply to all arrowheads. If the selected note has multiple leaders, and Smart is not selected, you can use a different arrowhead style for each individual leader. To apply a change to all of the arrowheads of the selected note, select this check box.
Border •
Style. Specifies the shape of the border (various geometric shapes that enclose the text), or None.
•
Size. Specifies either Tight Fit to the text, or a fixed size to accommodate a specified number of characters.
Font •
If you want to use the font you selected in Tools, Options, Document Properties, Detailing, Notes for note text, leave the Use document’s font check box selected.
•
If you want to use a different font, clear the Use document’s font check box, and click Font to choose from various font styles and sizes.
Hyperlink Click Insert Hyperlink
if you want to include a Hyperlink in the note.
Link to Document Property Click Link to Property
if you want to link a note to a document property.
Tag For notes in Blocks only. Text appears in the Tag name box for notes with attributes imported from AutoCAD. You can also enter tag names for notes created in the SolidWorks block definition editor. You can choose for a tag to be Read Only, Invisible, or both. The Tag name and its attributes are shown in the Attributes editor, which you can access in the Block Instance PropertyManager.
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Multiple Leaders To create multiple leaders while generating a new annotation:
1.
After selecting the properties for the annotation, click in the graphics area to place the first leader.
2.
While dragging the annotation and before placing it, press Ctrl. The annotation stops moving and another leader is created.
3.
Click as many times as necessary to place additional leaders.
4.
Release Ctrl, drag the annotion into position, and click to place the annotation.
To add new leaders to an existing annotation:
1.
Select the annotation.
2.
Press Ctrl and drag a leader attachment point. A new leader is created.
Link to Property You can link the value of a document property, a custom property, or a configuration specific property to the text of a note. If the value of the property changes, the note text changes automatically. To link a note to a property:
1.
In the Note PropertyManager, click Link to Property - or In the Note Properties dialog box, click Link to Property
2.
3.
.
Select the place to link from: •
Current document
•
Model in view to which the annotation is attached (drawings only)
•
Model in view specified in sheet properties (drawings only)
•
Component to which the annotation is attached (assembly documents and part and assembly drawing documents)
View the list of available properties, which depends on your selection in step 2 and where the note is created. •
Part or assembly document. The list includes the properties of the model document, including any custom defined properties.
•
Drawing sheet or sheet format. The list includes the properties of the drawing document, including any custom defined properties.
•
Drawing view. The list includes the properties of the model document shown in the view. (If a view is selected when you insert the note, or if the note is attached to the model in a view, the note belongs to the view.)
NOTE: All documents have system-defined properties. Drawings have system-defined properties that you can use to customize a sheet format. For more information on document properties in notes, see Linking Notes to Document Properties 4.
To add a new custom property, or to edit an existing one, click File Properties, then edit the properties on the Summary Information – Custom and Configuration specific tabs.
5.
Select a system-defined or custom property from the list, and click OK.
The Note text shown in the dialog box is the name of the property in the form $PRP:"<property name>". In the document, the note text is the value assigned to the property.
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Prefixes for custom properties linked in notes are used as follows: Prefix
Evaluated from:
$PRP:
Current document
$PRPSHEET:
Model in the view specified in Sheet Properties. If the model specified in Sheet Properties for custom properties is Default, then for notes belonging to drawing views, the model in the drawing view to which the note belongs is used. For sheet and sheet format notes, the first view in the FeatureManager design tree is used. If a view is selected, the model for that view is used for all cases.
$PRPVIEW:
Model in the drawing view to which the note belongs
$PRPMODEL:
Component to which the annotation is attached
Links to dimensions are evaluated from the active document. If the appropriate document for custom properties cannot be located according to the designations above, the following rules apply: •
In edit sheet mode, all sheet format notes are blank. All sheet and drawing view notes show their property names.
•
In edit sheet format mode, all sheet format notes show their property names.
NOTE: When a note in a drawing is linked to a custom property or a dimension and then the property or dimension is deleted, the note displays ERROR!. The parametric text is retained, and you can double-click the note to see the text. As soon as the property or dimension is available, the note updates to the correct value. Other items in the note are not affected. You can choose whether to display the link error. Select or clear View, Show Annotation Link Errors. NOTE: If a missing property or dimension is detected when opening a drawing yet to be saved in SolidWorks 2001Plus SP01 or later, a message asks if you want to break the link. If you choose to break the link, SolidWorks replaces the parametric text with the last known value. If no value is available and the note contains no other text, the note is deleted. The message appears only once.
Balloons You can create balloons in a drawing document. The balloons label the parts in the assembly and relate them to item numbers on the bill of materials (BOM). However, you do not have to insert a BOM in order to add balloons. If the drawing has no BOM, the item numbers are the default values that the software would use if you did insert a BOM. If there is no BOM on the active sheet, but there is a BOM on another sheet, the numbers from that BOM are used. To set the default BOM balloon properties, click Tools, Options, Document Properties, Balloons. If the default BOM balloon Style is Circular Split Line, you can choose what type of text to display in both the Upper and Lower portions of the balloon. For other styles, only Upper is available. Type of text can be Item Number, Quantity, or Custom. Balloons are automatically suppressed when the components they reference are suppressed. You can also add balloons in assembly documents. To import balloons from an assembly document into a drawing view, select Notes in the Insert Models Items dialog box. You can attach balloons to sketch entities. This is useful when sketches (with no extrusions) are combined to form an assembly and then taken into a drawing.
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If you change the Item Number in a balloon, the item number in the bill of materials also changes. To change an Item Number in a table-based BOM, clear Do not change item numbers in the Bill of Materials PropertyManager. To return to assembly order after changing item numbers, click Follow assembly order
.
To change an Item Number in an Excel-based BOM, you must clear the Row numbers follow assembly ordering check box on the Control tab of the Bill of Materials Properties dialog box. If the check box is selected (default), a message appears stating that the item number cannot be changed. You can also create stacked balloons. See Stacked Balloons. To insert balloons:
1.
Click Balloon
on the Annotations toolbar, or click Insert, Annotations, Balloon.
The Balloon PropertyManager appears. 2.
Edit the properties in the PropertyManager as needed, then click a component in a drawing view of an assembly, or click a component in an assembly model, to place the leader, then click again to place the balloon. A balloon containing an item number attaches to the part. If you specified the text to be Item Number, the number in the balloon corresponds to the item number in the bill of materials.
3.
Continue inserting as many balloons as needed. Edit the properties for each balloon in the PropertyManager before inserting the balloon.
4.
Click OK
.
To move the balloon or leader arrow, select and drag the balloon, or drag the leader by the handle.
To change the balloon properties:
Select the balloon and edit the properties in the Balloon PropertyManager. - or Right-click the balloon and select Properties. Make changes in the Note PropertyManager and click OK. To edit balloon text:
Double-click the balloon text and edit in place. To add multiple leaders to a balloon:
You can add more leaders to an existing balloon by holding down Ctrl and dragging a leader attachment point.
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Balloon PropertyManager The Balloon PropertyManager opens when you insert Balloons into a drawing or assembly document, or when you select an existing balloon. You can insert multiple balloons without closing the PropertyManager. Change the settings in the PropertyManager as necessary and click in the graphics area to place the balloons. The PropertyManager controls the following properties: Style Select a style for the shape and border of the balloon from the list. The style None displays the balloon text with no border. Size Select a size from the list, either a specified number of characters or Tight fit, which adjusts automatically to the text. Balloon text Select the type of text for the balloon, or for the upper section of a split balloon, from the list. •
Item Number - The Item Number in the Bill of Materials
•
Quantity - The quantity of this item in the assembly
•
Custom - The Custom Text box opens for you to type text
Lower text If you select the Circular Split Line style, this box is available to specify the text for the lower section. You have the same options as in the Balloon text section. More Properties When you select an existing balloon, you can click More Properties to open the Note PropertyManager.
Stacked Balloons Stacked balloons have only one leader for a set. You can stack the balloons vertically or horizontally. You can insert stacked balloons in drawings of assemblies and in assembly documents. To import balloons from an assembly document into a drawing view, select Notes in the Insert Model Items dialog box. To set default stacked balloon properties, click Tools, Options, Document Properties, Balloons. Under Stacked balloons, set Style and Size. Under Balloon text, choose the type of text: Item Number, Quantity, or Custom. You can insert a stacked balloon without selecting a component, so you can annotate an item that is part of an assembly but not actually modeled, such as glue or a liquid. If you change the Item Number in a stacked balloon, the item number in the bill of materials also changes. To change an Item Number in a table-based BOM, clear Do not change item numbers in the Bill of Materials PropertyManager. To return to assembly order after changing item numbers, click Follow assembly order . To change an Item Number in an Excel-based BOM, you must clear the Row numbers follow assembly ordering check box on the Control tab of the Bill of Materials Properties dialog box. If the check box is selected (default), a message appears stating that the item number cannot be changed.
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To insert stacked balloons:
1.
Click Stacked Balloon
on the Annotation toolbar or click Insert, Annotations, Stacked Balloon.
The Stacked Balloon PropertyManager appears, and the pointer changes to 2.
.
Select the point on the component where you want the balloon leader attached, then click again to place the first balloon. The leader and the first balloon appear.
3.
Continue to select components. A balloon is added to the stack for each component selected. As you add the stacked balloons, you can rightclick any balloon in the stack, select Stack Direction, and choose a new stack direction, or you can select the stack direction in the PropertyManager (Up
, Down
, Left
, Right
).
Each balloon is a separate note that you can select to delete or edit. 4.
Click OK
to close the PropertyManager.
To add balloons to the stack later:
Right-click one of the stacked balloons and select Add to Stack. To edit balloon text, do one of the following:
•
Double-click the balloon text and edit in place.
•
Select the balloon and edit the text in the PropertyManager.
•
Right-click the balloon, select Properties, and edit the text in the Note Properties dialog box.
To change the properties of the stacked balloons, do one of the following:
•
Select a balloon or balloons in the stack and change properties in the PropertyManager. For additional properties, click More Properties. Many properties are available in both the PropertyManager and the Note Properties dialog box.
•
Select a balloon or balloons, right-click a selected balloon and select Properties, and change the properties in the Note PropertyManager. Changes to properties apply only to selected balloons. To change all balloons in the stack, select all of them. Balloons stacked Right
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Chapter 12 Detailing
Stacked Balloon PropertyManager The Stacked Balloon PropertyManager opens when you insert a Stacked Balloon into a drawing or assembly document, or when you select an existing stacked balloon. The properties apply to the selected balloons. Balloon Settings Style. Select a style for the shape and border of the balloons from the list. If you select Circular Split Line, the Lower Text window opens for the lower half of the balloons. Size. Select a size from the list, either a specified number of characters or Tight fit, which adjusts automatically to the text. Balloon text. Select the type of text for the balloons, or for the upper section of split balloons, from the list. •
Item Number. The Item Number in the Bill of Materials
•
Quantity. The quantity of this item in the assembly
•
Custom. The Custom Text box opens for you to type text
Lower text. If you select the Circular Split Line style, this box is available to specify the text for the lower section. You have the same options as in the Balloon text section. Balloons per line. Set the number of balloons to stack in one line before starting the next line. Stack Right , Stack Left respect to its leader.
, Stack Down
, Stack Up
. Click for the direction of the stack with
Layer In drawings with named layers, select a layer. More Properties For existing stacked balloons, click More Properties to open the Note PropertyManager.
AutoBalloons Insert a set of balloons into one or more drawing views. Balloons are inserted into the appropriate views without duplicates. You can specify that balloons be inserted when creating new drawing views. Example of AutoBalloon
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Square
Circular
Top
Bottom
Left
Right
To insert balloons into a drawing view:
1.
Click AutoBalloon
on the Annotation toolbar, or click Insert, Annotations, AutoBalloon.
2.
Set properties in the AutoBalloon PropertyManager, then click OK
.
The balloons are placed outside the view border, and the leaders do not intersect. Once you close the PropertyManager, you cannot open it again. You can delete the balloons or undo the autoballoon command, then reinsert the balloons. You can drag a group of balloons or a single balloon. To specify that balloons be inserted into new drawing views:
1.
Click Tools, Options, Document Properties, Detailing.
2.
Under Auto insert on view creation, select Balloons, then click OK.
To specify the default layout for autoballoons:
1.
Click Tools, Options, Document Properties, Balloons.
2.
Under AutoBalloon Layout, select one of the formats, then click OK.
AutoBalloon PropertyManager Set the properties when inserting autoballoons into a drawing. Balloon Layout Select: Square Circular Top Bottom Left Right Ignore multiple instances. Applies a balloon to only one instance for components with multiple instances.
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Balloon Settings Sets the properties to apply to all the balloons. Layer In drawings with named layers, select a layer.
Center Marks You can place center marks on circles or arcs in drawings. The center mark lines can be used as references for dimensioning. Example of Center Marks
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Single center mark
Single center mark with extended lines
Extended lines in centerline font
Single center mark rotated 45°
Linear pattern with default size marks
Linear pattern with specified mark size
Linear pattern with extended lines
Linear pattern with connection lines
Circular pattern with extended lines
Circular pattern with base center mark
Circular pattern with circular lines
Circular pattern with radial lines
Some items to note about center marks are as follows: •
The axis of the circle or arc must be normal to the drawing sheet.
•
Center marks are available as single marks, in linear patterns, or in circular patterns. Linear patterns can include connecting lines. Circular patterns can include circular lines, radial lines, and base center marks. Display attributes include mark size, extended lines, and specifying the centerline font for the center mark lines.
•
You can set an option so that center marks are inserted automatically in new drawing views.
•
You can insert a center mark manually into one circle or arc in a pattern and then propagate center marks to all entities in the pattern.
•
Center marks propagate or insert automatically into patterns if the pattern is created from a feature and not a face or body.
•
You can rotate center marks individually, specifying the rotation in degrees. In the Rotate Drawing View dialog box, you can choose to have center marks rotate automatically when the view is rotated.
•
Center marks in Auxiliary Views are oriented to the viewing direction such that one of the lines of the center mark is parallel to the view arrow direction.
To set options for center marks:
1.
Click Tools, Options, Document Properties, Detailing.
2.
Under Center marks, type a value for Size and select or clear the check boxes for Extended lines and Centerline font.
3.
Under Auto insert on view creation, select or clear the check box for Center marks. When selected, center marks are inserted automatically into all appropriate circles and arcs in new drawing views.
4.
Click OK.
To insert center marks manually:
1.
Click Center Mark
on the Annotation toolbar, or click Insert, Annotations, Center Mark.
The Center Mark PropertyManager appears and the pointer changes to 2.
Choose from the Options, Display Attributes, and Angle.
3.
Click the model edges or silhouettes of circles or arcs.
.
NOTE: You cannot apply a center mark to an ellipse or a torus. 4.
If you selected Linear Pattern to all entities in the pattern.
5.
Click OK
or Circular Pattern
, click Propagate
to apply center marks
.
To edit center marks:
1.
Select a center mark (the pointer changes to
when it is over a center mark).
2.
Edit the center mark properties in the Center Mark PropertyManager.
3.
Click OK
.
To dimension to center marks:
You can dimension to the horizontal lines, the vertical lines, or the circular edges to generate vertical, horizontal, or angular dimensions. You can dimension between two center marks, or between a center mark and another entity.
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Example of Center Mark Dimensions
Example of Center Mark Fonts The default center mark font is typical for ANSI standard.
The centerline font used for center mark lines is typical for ISO standard.
Center Mark PropertyManager You can control the following properties for center marks in the Center Mark PropertyManager. The properties available vary depending on the type of center mark selected. Options Single Center Mark. Insert a center mark into a single circle or arc. You can change the Display Attributes and rotation Angle of the center mark. Linear Center Mark. Insert center marks into a linear pattern of circles or arcs. You can select Connection lines and Display Attributes for linear patterns. Circular Center Mark. Insert center marks into a circular pattern of circles or arcs. You can select Circular lines, Radial lines, Base center mark, and Display Attributes for circular patterns. Example Display Attributes Clear Use document's defaults to change the following attributes:
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•
Mark size. Enter a value. Set the default in Tools, Options, Document Properties, Detailing.
•
Extended lines. Display extended axis lines, with a gap between the center mark and the extended lines.
•
Centerline font. Display the center mark lines in the centerline font.
Angle Displays the current angle of a single center mark. If the center mark is rotated because the view is rotated, the rotation angle appears here. Enter a new value if desired. Not available for linear or circular pattern center marks. Layer In drawings with named layers, select a layer.
Centerline Annotations You can insert centerlines into drawing views automatically or manually. The SolidWorks software avoids duplicate centerlines. Example of Centerline Annotations To insert centerlines throughout a feature, select one face.
To insert a centerline in one feature, select a face. To insert centerlines in selected features, press Ctrl and select multiple faces. To insert centerlines in all appropriate features, select the view in either the graphics area or the FeatureManager design tree. To insert a centerline from the middle of the left side to the middle of the right side, select the top and bottom edges.
To insert centerlines automatically into drawing views:
1.
In a drawing document, click Tools, Options, Document Properties, Detailing.
2.
Under Auto insert on view creation, select Centerlines.
3.
Click OK.
4.
Insert a drawing view. Centerlines appear automatically in all appropriate features.
To insert centerlines manually:
1.
In a drawing document, click Centerline Centerline.
on the Annotations toolbar, or click Insert, Annotations,
The Centerline PropertyManager appears. NOTE: You can select either the tool or an entity first.
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2.
Select one of the following: •
Two edges (parallel or non-parallel)
•
Two sketch segments (except splines)
•
A face (cylindrical, conical, toroidal, or swept)
•
A drawing view in the graphics area (except isometric orientation)
•
A feature, component, or drawing view in the FeatureManager design tree
•
Insert Component Centerline in the component shortcut menu in the graphics area (assembly drawings only) Centerlines appear in all appropriate segments of the selected entities.
3.
Click OK
.
Hole Callouts Hole callouts are available in drawings. If you change a hole dimension in the model, the callout updates automatically. Hole callouts use Hole Wizard information when a hole has been created by the Hole Wizard. The default formats for the Hole Wizard types are stored in installation directory\lang\\calloutformat.txt. A second file, calloutformat_2.txt, is a simplified version. You can edit either file. If you want to use the second file, you must rename the file to calloutformat.txt, which is the file name the SolidWorks software references. You can set the location of the default folder for Hole Callout Format File in Tools, Options, System Options, File Locations. The number of instances is included in the hole callout if multiple holes with the same format are created in the Hole Wizard. Example of Hole Callouts A hole callout using information from the Hole Wizard.
The same hole callout, but defined by geometry.
The axis of the hole must be normal to the drawing sheet. To add hole callouts in a drawing:
1.
Click Hole Callout The pointer changes to
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on the Annotation toolbar, or click Insert, Annotations, Hole Callout. .
2.
Click the edge of a hole. A Hole Callout is inserted and the Dimension PropertyManager appears. The callout contains a diameter symbol and the dimension of the hole diameter. If the depth of the hole is known, the callout also contains a depth symbol and the dimension of the depth. If the hole is created in the Hole Wizard, the callout contains additional information (the dimensions of a countersink or number of hole instances, for example).
3. 4.
Click in the graphics area to place the hole callout. Edit the callout in the Dimension PropertyManager. You can specify precision, select an arrow style, or add text (for example, the number of places where the hole occurs). However, you should retain the dimensions and symbols for the size and type of hole. If the hole has been created by the Hole Wizard, you can also click Variables in the Dimension PropertyManager to access a list of Hole Wizard variables to insert into the hole callout. If you attach a hole callout to a tapped hole in ANSI inch standard and the current drawing units are millimeters, the drill diameter and hole depths are reported in mm but the thread description retains the ANSI inch size designation. You might want to replace the thread description with other variables from the Hole Callout Variable dialog box.
5.
Repeat steps 2 through 4 to insert additional hole callouts, then click OK
.
To edit the properties of a hole callout:
Select the callout and make the changes in the Dimension PropertyManager. If you manually change a portion of the callout text, you might break that portion's link with the model. SolidWorks displays a warning message if you are about to break a link. To toggle between Hole Wizard and geometry definitions:
1.
Right-click the hole callout and select Display Options, Define by Geometry.
2.
To return to the Hole Wizard definition, right-click the hole callout and select Display Options, Define by Hole Wizard. These menu items are available only when holes have been created using the Hole Wizard.
Hole Callout Variables You can choose a hole callout variable from the list of Hole Wizard variables. The variable is inserted in the hole callout text where the pointer is located in the Dimension Text section of the Dimension PropertyManager. The variable name (for example, for Fastener Size) appears in the Dimension PropertyManager. The value in the variable (5/16, for example) appears in the hole callout in the graphics area.
If you select a variable from the list that is not appropriate for the hole for which you are editing the hole callout, a value of zero is displayed in the hole callout.
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Cosmetic Threads A cosmetic thread represents the inner diameter of a thread on a boss or the outer diameter of a thread on a hole and can include a hole callout.
The properties and functionality of cosmetic threads include:
•
You can represent threads on a part, assembly, or drawing, and you can attach a thread callout note. You can add cosmetic threads to conical holes. If the conical thread does not end at a flat face, it is trimmed by the curved face.
•
A cosmetic thread differs from other annotations in that it is an absorbed feature of the item to which it is attached. For example, the cosmetic thread on a hole is in the FeatureManager design tree under the Hole feature, along with the sketches used to create the hole.
•
When the pointer is over a cosmetic thread, the pointer changes to
•
Cosmetic threads in part documents are inserted automatically into drawing views if the drawing document is in ANSI standard. A copy of any present thread callout is also inserted. Thread callouts are not used in ISO, JIS, or other standards, but you can show them with Insert Callout on the shortcut menu (see the next paragraph). To insert cosmetic threads from assembly documents into drawings, click Insert, Model Items and select Cosmetic Threads. In ANSI drawings, one copy of a cosmetic thread callout is also imported into a sheet.
•
In drawings, Insert Callout appears in the shortcut menu. If a cosmetic thread callout is defined in the part but is not displayed in the drawing, you can display the callout by selecting this menu item. A leader attaches to the thread by default. The callout is a note. You can edit the callout as you would edit any note.
•
If you add a cosmetic thread while working in a drawing view, the part or assembly is updated to include a Cosmetic Thread feature.
•
You can attach notes to both the circular faces and silhouette edges of cosmetic threads. You can dimension both the circular cosmetic thread and the linear dimension of the sides in drawings. You can dimension the silhouette edge of a cosmetic thread to a sketch entity. You cannot dimension cosmetic threads in part or assembly documents.
•
A cosmetic thread that is created in a part cannot be deleted from a drawing, but it can be hidden and shown. To hide or show a cosmetic thread, right-click the cosmetic thread and select Hide or Show.
•
The visibility of cosmetic threads follows the visibility of the owner feature. When you change display mode, add features to the Show Hidden Edges list, or hide a component, the visibility of cosmetic threads changes automatically.
•
You can reference patterned cosmetic threads.
•
You can display cosmetic threads on assembly feature holes. The cosmetic thread appears only on the last component cut by the hole.
•
For tap and pipe tap holes, you can add cosmetic threads in the Hole Wizard.
.
NOTE: For tapped holes with cosmetic threads created in the Hole Wizard, the hole diameter is the diameter of the tap drill. For tapped holes without cosmetic threads, the hole diameter is the outer diameter of the thread. •
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For shaded display of cosmetic threads, click Tools, Options, Document Properties, Annotations Display. Under Display filter, select Shaded cosmetic threads.
To insert cosmetic threads:
1.
On a cylindrical feature (a boss, a cut, or a hole), select the circular edge where the thread begins. If the feature is a conical hole, select the major diameter. If the feature is a conical boss, select the minor diameter. You can also select the feature after you click the tool.
2.
Click Cosmetic Thread
on the Annotations toolbar, or click Insert, Annotations, Cosmetic Thread.
3.
Set the properties in the Cosmetic Thread PropertyManager.
4.
Click OK
.
To edit a cosmetic thread:
1.
In a part or assembly document, right-click the Cosmetic Thread feature and select Edit Definition.
2.
Make the necessary changes in the Cosmetic Thread PropertyManager, and click OK
.
To specify the line style and weight for cosmetic threads in the active drawing document:
1.
Click Tools, Options. On the Document Properties tab, select Line Font.
2.
In the Type of edge section, select Cosmetic Thread.
3.
Choose a Style and Thickness from the lists. The Preview box shows the results.
Cosmetic Thread PropertyManager Specify the following properties when inserting a cosmetic thread in a part or drawing. Thread Settings Circular Edges
. Select a circular edge in the graphics area.
End Condition. The cosmetic thread extends from the edge selected above to the end condition: •
Blind. A specified depth. Specify the depth below.
•
Through. Completely through the existing geometry.
•
Up to Next. To the next entity that intercepts the thread.
Depth
. Enter a value when the End Condition is Blind.
Minor Diameter, Major Diameter, or Conical Offset entity type with the cosmetic thread.
. Sets the diameter for the dimension corresponding to the
Thread Callout. Type text to appear in the thread callout. Layer In drawings with named layers, select a layer.
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Surface Finish Symbols You can specify the surface texture of a part face by using a surface finish symbol. You can select the face in a part, assembly, or drawing document. For ISO and related drafting standards, you can specify Display symbols per 2002 in Tools, Options, Document Properties, Detailing to display surface finish symbols per 2002 standards. To insert a surface finish symbol:
1.
Click Surface Finish
2.
Set the properties in the PropertyManager.
3.
Click in the graphics area to place the symbol.
4.
on the Annotations toolbar, or click Insert, Annotations, Surface Finish Symbol.
•
Multi-jog Leader. Before placing the symbol, right-click and select Use Multi-jog Leader to add a multi-jog leader. Click in the graphics area to place the arrow end of the leader, then move the pointer and click to add each jog point. To complete the leader and place the symbol, either doubleclick or right-click and select End Leader.
•
Multiple instances. Click as many times as necessary to place multiple copies.
•
Editing each instance. You can change text and other items in the dialog box for each instance of the symbol.
•
Leaders. If the symbol has a leader, click once to place the leader, then click a second time to place the symbol.
•
Multiple leaders. While dragging the symbol and before placing it, press Ctrl. The note stops moving and a second leader is added. While still holding Ctrl, click to place the leader. Click as many times as necessary to place additional leaders. Release Ctrl and click to place the symbol.
Click OK
.
Drag You can drag a surface finish symbol with a leader to any location. If you attach a leaderless symbol to an edge, then drag it off the model edge, an extension line is created.
Edit To edit a surface finish symbol, select the symbol. Rotate You can rotate surface finished symbols attached to sketch entities by 180°. Right-click the symbol and select Rotate by 180. Rotate by 180 is not available for model edges or faces, it is not available in ANSI standard, and the symbol must not have a leader. Multiple Leaders You can add more leaders to an existing symbol by holding down Ctrl and dragging a leader attachment point.
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Surface Finish PropertyManager Edit properties of surface finish symbols. Surface Finish Favorite Symbol Select a symbol style. The symbols available vary depending on the drafting standard specified. For ISO and related standards, the symbols available also vary depending on whether you select display of surface finish symbols using 2002 standards. Specify both options in Tools, Options, Document Properties, Detailing. Basic Machining Required Machining Prohibited Local All Around JIS Basic JIS Grind JIS No Machining If you select JIS Basic or JIS Grind, several surface textures are available. Symbol Layout For ANSI symbols and symbols using ISO and related standards prior to 2002, specify: •
Maximum Roughness
•
Minimum Roughness
•
Material Removal Allowance
•
Production Method/Treatment
•
Sampling Length
•
Other Roughness Values
•
Roughness Spacing
•
Lay Direction
For symbols using ISO and related standards from 2002, specify: •
Manufacturing Method
•
Texture Requirement 1
•
Texture Requirement 2
•
Texture Requirement 3
•
Machining Allowance
•
Surface Lay and Orientation
For JIS symbols, specify: •
Roughness/Ra
•
Roughness Rz/Rmax
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Format Use document font. To specify a different font for the symbol and text, clear and click Font. Select: Upright Rotated/Perpendicular Leader Select a leader style: Leader No Leader Auto Leader Straight Leader Bent Leader Select an Arrow Style. Layer In drawings with named layers, select a layer.
Datum Feature Symbols You can attach a datum feature symbol to the following items: •
In a part or assembly, on a planar model surface or on a reference plane
•
In a drawing view, on a surface that appears as an edge (not a silhouette) or on a section view surface
•
A geometric tolerance symbol frame
To insert datum feature symbols:
1.
Click Datum Feature Symbol Symbol.
on the Annotations toolbar, or Insert, Annotations, Datum Feature
2.
Edit the options in the Datum Feature PropertyManager.
3.
Click in the graphics area to place the attachment and then the symbol.
4.
Continue inserting as many symbols as needed.
5.
Click OK
.
If you drag a datum feature symbol off the model edge, an extension line is added. To edit a datum feature symbol, select the symbol. NOTE: If you use ANSI dimensioning standards, you can display datum feature symbols in the 1982 style. To select this option for the active document, click Tools, Options, Document Properties, Detailing. In the Dimensioning standard section, select ANSI from the list, then select the Display datums per 1982 check box.
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Datum Feature PropertyManager The PropertyManager controls properties of datum feature symbols. Settings Label
. The text appears in the datum feature box.
Use document style. The document style follows the standard (ANSI, ISO, and so on) specified in Tools, Options, Document Properties, Detailing. Clear to select a different style of box and attachment. Each style of box has a different set of attachment styles.
Square
Round (GB)
Filled Triangle
Perpendicular
Filled Triangle With Shoulder
Vertical
Empty Triangle
Horizontal
Empty Triangle With Shoulder Layer In drawings with named layers, select a layer.
Datum Targets You can attach a datum target and symbol to a model face or edge in any document. To create a datum target and symbol:
1.
Click Datum Target
on the Annotations toolbar, or click Insert, Annotations, Datum Target.
2.
Set the properties in the PropertyManager.
3.
Click in the graphics area to place the target and then the symbol. You can insert multiple symbols.
4.
Click OK
.
To move the datum target symbol (the balloon, the crosshatch area, or the point), select the symbol and drag the item. To edit the datum target symbol, select the symbol. In a drawing, you can dimension to the center of a datum target area. Activate the view, then click either the symbol or the area to add the dimension.
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Datum Target PropertyManager Attach a datum target and associated symbol to a model face or edge. Settings Target symbol. Select the target symbol style: Target symbol Target symbol with area size outside No target symbol Target area. Select the target area display: X target area Circular target area Rectangular target area Do not display target area Target area size Datum references
. Specify Width and Height (for rectangles) or Diameter (for X's and circles). . Specify up to three references.
Leader Select a leader style: Bent, solid leader Bent, dashed leader Straight, solid leader Straight, dashed leader Select an Arrow style. Layer In drawings with named layers, select a layer.
Geometric Tolerancing The SolidWorks software supports the ANSI Y14.5 Geometric and True Position Tolerancing guidelines.
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•
You can place geometric tolerancing symbols, with or without leaders, anywhere in a drawing, part, assembly, or sketch, and you can attach a symbol anywhere on a dimension line.
•
A geometric tolerance symbol can have any number of frames.
•
The pointer changes to dimension.
•
You can add multiple symbols without closing the dialog box.
•
You can display multiple leaders. The leaders can be straight, bent, or perpendicular.
•
When you drag the leader of a geometric tolerance symbol off a model edge, an automatic witness line is created.
when it is near the handle of an arrow of a geometric tolerancing symbol on a
Example of Geometric Tolerance Symbols Multiple frames
Perpendicular leaders
Automatic witness line
To create geometric tolerancing symbols:
1.
Click Geometric Tolerance
, or click Insert, Annotations, Geometric Tolerance.
2.
Type in values and select symbols. As you add items, a preview is displayed. For more information on the options available (Geometric Characteristic Symbols, Material Condition Symbols, Projected tolerance zone, and so on), see Geometric Tolerance Properties. For information on leader, arrow, anchor, and font options, see Geometric Tolerance Options.
3.
4.
Click to place the symbol. •
To add a Multi-jog Leader to the symbol, before placing the symbol, right-click and select Use Multi-jog Leader. Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point. To complete the leader and place the symbol, either doubleclick or right-click and select End Leader.
•
Click as many times as necessary to place multiple copies.
•
If the symbol has a leader, click once to place the leader, then click a second time to place the symbol.
•
You can change text and other items in the dialog box for each instance of the symbol.
•
While dragging the symbol and before placing it, hold down Ctrl. The note stops moving, but the leader continues, lengthening the leader. While still holding Ctrl, click to place the leader. Click as many times as necessary to place additional leaders. Release Ctrl and click to place the symbol.
Click OK to close the dialog box.
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You can drag the symbol any place in the document. To edit an existing symbol, double-click the symbol, or right-click the symbol and select Properties. You can add more leaders to an existing symbol by holding down Ctrl and dragging a leader attachment point. Geometric Tolerance Properties You can specify the properties and insert Geometric Tolerance symbols. Feature control frames 1.
In the first Feature Control Frame, click GCS (Geometric Characteristic Symbol). In the Symbols dialog box, choose a Symbol library, select a symbol, and click OK. As you make each selection, a preview is displayed.
2.
Enter a tolerance value in the Tolerance 1 box, and click
to include a Diameter symbol.
3.
Click MC to choose the material condition symbol for Tolerance 1, and click OK.
4.
Repeat steps 2 and 3 for Tolerance 2.
5.
Enter datum names and material condition symbols for the Primary, Secondary, and Tertiary datums.
6.
For additional frames, increment the number in Frames and repeat steps 1 through 5 for each frame.
Composite frame. To create a composite frame, select Composite Frame and enter values and material condition symbols. Between two points. Select if the tolerance value applies to a measurement between two points or entities, and type the labels of the points in the boxes. Projected tolerance zone To enter a Projected Tolerance Zone (PTZ) height, select Show PTZ and enter a value in the Height box. The value appears in the first frame’s tolerance box. GTol Favorite Layer In drawings with named layers, select a layer. Additional Properties To specify styles for leaders, arrows, anchors, and fonts, click Options. Geometric Tolerance Options You can specify properties for leaders, arrows, and fonts of the selected geometric tolerance symbol. Attached leader •
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Choose one of the following: o
Always show leaders.
o
Automatic leaders. Adds a leader if you click an entity; no leader if you click on the sheet or view.
o
No leaders.
•
Display with bent leader. With this selected, you can also select an All Around leader.
•
Perpendicular leaders.
•
All Around. Indicates that the profile tolerance extends all the way around the feature to which the tolerance applies.
Arrow Select Smart to use the default arrow style (specified in Tools, Options, Document Properties, Detailing) for the type of item the symbol is attached to. To select a different arrow style, clear this check box and select an arrow style from the Arrow list. Anchor Choose the location of the leader anchor from Closest, Left, or Right sides. Font Select Use document’s font to use the default font, or clear the check box and click the Font button to choose from various font styles and sizes. Click OK to return to the Geometric Tolerance Properties dialog box.
Dowel Pin Symbols You can add dowel pin symbols to holes (circular edges or sketched circles) in drawings. The symbol conforms to the size of the selected hole. Example of Dowel Pin Symbols Dowel pin symbols are added to holes of various sizes. The symbol in green is flipped 90°.
Following are some restrictions on dowel pin symbols: •
The face containing the hole must be normal to the plane of the currently active view.
•
You cannot move dowel pin symbols with Copy or Cut and Paste operations.
To insert dowel pin symbols into a drawing:
1.
Click Dowel Pin Symbol edge.
, or click Insert, Annotations, Dowel Pin Symbol, and select a circular
- or Select one or more circular edges and click Dowel Pin Symbol Pin Symbol.
or click Insert, Annotations, Dowel
Dowel pin symbols appear in the selected holes, and the Dowel Pin Symbol PropertyManager appears. You can continue to select circular edges to insert additional dowel pin symbols. 2.
Under Display Attributes, select Flip symbol if desired. The dowel pin symbols currently selected rotate 90°. NOTE: To flip a dowel pin symbol after it has been inserted, right-click the symbol (the pointer changes to when it is over the symbol) and select Flip Symbol.
3.
Click OK
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Weld Symbols When you create a weld bead in an assembly, a weld symbol is created automatically on the weld bead component, representing the parameters you specify. You can also construct weld symbols independently in a part, assembly, or drawing document. When creating or editing a weld symbol, you can: •
Add secondary weld fillet information to the weld symbol for certain types of weld (Square or Bevel, for example).
•
Choose a Leader anchor of None and add a Multi-jog Leader later.
•
Choose the text font for each weld symbol.
To insert a weld symbol:
1.
Click a face or edge where you want to indicate a welded joint.
2.
Click Weld Symbol
on the Annotations toolbar, or click Insert, Annotations, Weld Symbol.
The Weld Symbol Properties dialog box appears for ISO, BIS, DIN, JIS, and GB standards. Different dialog boxes appear for ANSI and GOST standards. 3.
Type in values and select symbols and options. A preview is displayed. Click OK to close the dialog box and place the symbol.
To edit a weld symbol:
Double-click the symbol - or Right-click the symbol and select Properties. Weld Symbol Properties You can create weld symbols in part, assembly, and drawing documents. The Dimensioning standard in Tools, Options, Document Properties, Detailing must be set to ISO, BSI, DIN, JIS, or GB for this dialog box, or ANSI or GOST to access dialog boxes for weld symbols in those standards. Many of the properties are available both above and below the weld symbol line and are described in order from the line. A preview of the symbol is displayed in the graphics area.
Peripheral. Adds Field/Site. Adds
to indicate that the weld is applied all around the contour. to indicate that the weld is applied in the field or on-site.
Weld symbol. Click and select a symbol from a symbol library. Other options become available, depending on the symbol chosen. Type dimensions to the left and right of the Weld symbol button. Specification process. Type text in the large box at the right, in any number of lines, to appear in the tail of the symbol. Contour. Applies a contour shape above the symbol. 2nd fillet. The 2nd fillet is available for only certain weld symbols (Square or Bevel, for example). Type dimensions in the fields to the left and right of the check box. Symmetric. Properties on one side of the symbol line also appear on the other side.
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Stagger. Fillet weld symbols above and below the line are staggered. Identification line on top. Moves the dashed identification line above the symbol line. Font. To specify a font for text and size of symbols, clear Use document's font and click Font. Leader anchor. Anchor the leader to the specified location on the weld symbol. Layer. In a drawing with named layers, choose a layer from the list. Weld Symbol Favorite. ANSI Weld Symbol Properties You can create ANSI weld symbols in part, assembly, and drawing documents. The Dimensioning standard in Tools, Options, Document Properties, Detailing must be set to ANSI. Many of the properties are available both above and below the weld symbol line and are described in order from the line. A preview of the symbol is displayed in the graphics area.
Around. Adds Field/Site. Adds
to indicate that the weld is applied all around the contour. to indicate that the weld is applied in the field or on-site.
Weld Symbol. Click and select a symbol from a symbol library. Other options become available, depending on the symbol chosen. Type dimensions to the left and right of the symbol. Specification process. Type text in the box, in any number of lines, to appear in the tail of the symbol. Contour. Select None, Flat, Convex, or Concave. Finishing method. Select None, Chipping, Grinding, Hammering, Machining, Rolling, or Unspecified.
Stagger weld. Fillet weld symbols above and below the line are staggered. 2nd fillet. Type dimensions. Root opening. Type a dimension. Arrow. Offset text. Groove angle. Type an angle in degrees. Inside. Text placed inside the weld symbol. Joint with spacer. Choose None or one of the types (Double V Groove Spacer and so on). Font. To specify a font for text and size of symbols, clear Use document's font and click Font. Leader anchor. Anchor the leader to the specified location on the weld symbol. Layer. In a drawing with named layers, select a layer from the list. Weld Symbol Favorite.
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GOST Weld Symbol Properties You can create GOST weld symbols in part, assembly, and drawing documents. The Dimensioning standard in Tools, Options, Document Properties, Detailing must be set to GOST. Field. Adds Around. Adds
to indicate that the weld is applied in the field. to indicate that the weld is applied all around the contour.
Other Side. Move the arrow from the upper
to the lower
side of the leader.
Leader anchor. Anchor the leader to the specified location on the weld symbol. Layer. In a drawing with named layers, choose a layer from the list. Solder. Adds Glue. Adds
to the symbol leader. to the symbol leader.
Weld Text. Type the weld dimensions and specifications. •
The box on the left contains the text that appears on the bent leader; the other two boxes contain the text that appears above and below the horizontal leader.
•
Place the cursor in the text box where you want one of the following symbols and click the symbol button. Fillet
Stagger Check
Heat
Not all around
Smooth
Diameter
Stagger Chain
Number
Surface Finish Symbol. To add surface finish information to the symbol, under SF Symbol, select Top or Bottom to place the symbol above or below the horizontal leader. Enter the information in the Surface Finish Symbol dialog box, and click OK. To modify the surface finish information, click Details for the side you want to modify. Font. To specify a font for text and size of symbols, clear Use document's font and click Font. Weld Symbol Favorite.
Area Hatch/Fill You can apply a crosshatch pattern or solid fill to a model face or to a closed sketch profile. Area hatch can be applied only in drawings. Some characteristics of area hatch include the following: •
If you choose the area hatch to be solid fill, the default color of the fill is black. You can change the color with the Line Color
tool on the Line Format toolbar.
•
You can include area hatch in blocks.
•
You can move area hatch into layers.
•
You can select an area hatch in a Broken View only in its unbroken state; you cannot select an area hatch that crosses a break.
•
When the pointer is over an area hatch or fill, the pointer changes to
.
To set options for Area Hatch/Fill, click Tools, Options, System Options, Area Hatch/Fill.
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Example of Area Hatch/Fill and Crosshatch Area hatch on model face and in sketched profile.
Solid fill on model face.
Crosshatch in section view.
Solid fill in section view.
To add area hatch or solid fill to a model face or sketched profile:
1.
In a drawing document, select a model face, or select a segment of a closed sketch profile.
2.
Click Area Hatch/Fill
on the Drawing toolbar, or click Insert, Area Hatch/Fill.
The Area Hatch/Fill dialog box appears. 3.
Choose from the selections in Properties, Layer, Pattern, Scale, and Angle. You can clear Always show dialog on creation to prevent the dialog box from appearing whenever you insert area hatch.
4.
Click OK. The area hatch or solid fill appears in the model face or sketched profile. You can change the shape and size of a sketch profile and the area updates to fill the modified profile. To delete an area hatch, select it in the graphics area and press Delete. Sketched profiles are not deleted when the area hatch is deleted.
To edit an area hatch or solid fill:
1.
Right-click the area hatch and select Properties. The Area Hatch/Fill dialog box appears.
2.
Edit the properties and click OK.
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Area Hatch/Fill Properties You can change the properties of crosshatch, area hatch, and solid fill in drawings with this dialog box. The pattern is displayed in the Preview window. The properties available vary depending on the type of hatch or fill selected. To open the dialog box:
Right-click a crosshatch, area hatch, or solid fill and select Crosshatch Properties. - or Select a face or closed sketch profile and click Area Hatch/Fill Insert, Area Hatch/Fill.
on the Drawings toolbar, or click
To set default options:
•
To set default options for area hatch or solid fill, click Tools, Options, System Options, Area Hatch/Fill.
•
To set default options for crosshatch, click Tools, Options, Document Properties, Material Properties. You can set the Material Properties options only in part documents.
Properties. Select None, Solid, or Hatch. •
Pattern, Scale, and Angle are available only for Hatch.
•
The default color of the solid fill is black. You can change the color of the fill by selecting the fill in the graphics area and clicking Line Color
•
on the Line format toolbar.
To remove crosshatch, select None.
Pattern. Select a material from the list. Layer. Select an existing layer from the list. Scale. Set a value for the scale of the pattern. Angle. Set a value for the angle of the pattern. Material crosshatch. Uses the pattern, scale, and angle for the material specified in the part document. Apply To. If the crosshatch is on a section face, select one of the following levels: •
View. All instances in the currently active section view (lowest priority, overrides only the document default).
•
Component. All section faces on the currently selected component in an assembly.
•
Region. The currently selected surface only (highest priority, overrides all other specifications).
Always show dialog on creation. Clear to prevent the dialog box from appearing whenever you insert area hatch or solid fill.
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Blocks You can make, save, edit, and insert blocks for drawing items that you use often, such as standard notes, title blocks, label positions, and so on. Blocks can include text, any type of sketch entity (except points), balloons (except stacked balloons), imported entities and text, and area hatch. You can attach blocks to geometry or to drawing views, and you can insert them into sheet formats. Blocks can be used only in drawing documents. Example of Blocks
Title block
First angle and third angle projection
Routing schematic symbols
Blocks have the following forms: •
Definition. named in the FeatureManager design tree. If the block definition is edited, the new version appears in subsequent instances. If you link to an external file while editing the block definition, the changes are automatically applied to any instances of the block in the current document.
•
Instance. inserted into the graphics area based on a definition. Changes in properties of a block instance apply only to the selected instance.
Saving blocks is optional. You can make, edit, copy, and move blocks within a drawing document without saving the blocks to file. Pointers When the pointer is over block entities, the pointer changes to
. When the pointer is over blank spaces in a
block, the pointer changes to . • When you right-click an entity in the block instance, you access the shortcut menu for the block. •
When you right-click a space within the block instance, you access the shortcut menu for the drawing sheet.
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Base Points Blocks have a base point. When you insert or paste a block, the block instance is located so that its base point is at the insertion or paste point. Block instances are scaled and rotated about their base points. When you select a block instance, the base point is displayed in blue . You can change the position of a block base point in the block definition editor. Leaders Block leaders have an anchor point (the end anchored to the block) and an attachment point (the end attached to a model or the drawing sheet). You can add a leader to a block instance, and you can drag the leader anchor point anywhere within the block.
Note leaders that are attached to a model are frozen when included in a block. Leaders on notes within blocks do not adjust to attach to any model or sketch entity. Layers You can move sketch entities and annotations onto layers before making blocks. You can also move them onto layers in the block editor. If you change properties of layers while in the block editor, the changes apply to all entities in the layers, not just the entities in the block. Selecting a layer in the Insert Block PropertyManager or Block Instance PropertyManager applies to the block leader and arrow. To specify a default path for locating blocks:
1.
Click Tools, Options, System Options, File Locations.
2.
Under Show folders for, select Blocks from the list, then click Add.
3.
In the Browse For Folder dialog box, browse to the desired folder, then click OK. The list can include more than one directory; the first path in the list is displayed by default in the Open dialog box when you insert a block.
To create a new block in the block definition editor:
1.
In a drawing document, click Tools, Block, New. The block definition editor opens, with a temporary drawing sheet in the graphics area and the Block Definition PropertyManager in the left panel.
2.
Create the block definition with sketch tools and the Note tool. You can apply and edit Block Settings (Tag name, Read only, and Invisible) to notes as you create or edit them in the block definition editor. When editing the properties of a block instance, you can change the Value (text) of a note that has not been specified to be Read only.
3.
Close any sketches or PropertyManagers and click OK block to the FeatureManager design tree.
to close the block definition editor and add the
The block name appears under the Blocks folder in the FeatureManager design tree. You can edit the block name in the FeatureManager design tree. The block name appears in the list of available blocks when you insert a block instance (see below). You can also save the block to file (see below).
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To create a new block from entities in a drawing:
1.
In a drawing, sketch the entities that make up the block. To add text, use the Note tool.
2.
Box-select all the entities.
3.
Click Tools, Block, Make. If you select entities for the block that belong to one view, the block belongs to the view. If you select entities for the block that belong to more than one view, the block then belongs to the sheet. If you link a note to a system or custom property, the block stores the system variable ($PRPMODEL, for example) that identifies the entity to which the note is attached and resolves the link when block instances are attached to the model, view, sheet, or document. It also stores and later resolves the system or custom variable name ("SW-Created Date", for example). The block name appears under the Blocks folder in the FeatureManager design tree. You can edit the block name in the FeatureManager design tree. The block name appears in the list of available blocks when you insert a block instance (see below). You can also save the block to file (see below).
4.
Click OK
.
To move or copy a block:
To move a block, select the block and drag it. To copy a block, press Ctrl while dragging the block. To save a block:
Right-click the block and select Save to File. - or Select the block and click Tools, Block, Save to File. The Save As dialog box appears. The default extension for block files is .sldblk. The SolidWorks software still supports .sldsym for inserting blocks and editing blocks, but all new blocks saved to external files use the .sldblk extension. NOTE: Properties of the block (scale and rotation angle) are saved in the file. To insert a block into a drawing:
1.
Click Insert Block
, or click Insert, Block.
The Insert Block PropertyManager appears. NOTE: You can also drag a block from the Blocks folder in the FeatureManager design tree into the graphics area. 2.
Under Source, do one of the following: Select a block Name from the list of blocks in the drawing document. - or Click Browse and browse to an external file that contains a block definition. You can insert files with extensions .sldblk, .sldsym, .dwg, and .dxf. If desired, select Create external reference to file to link the definition in the document to the file definition.
3.
Click in the graphics area as many times as necessary to place as many copies of the block as you want. The block is positioned so that the block base point is at the point in the graphics area where you click. The block base point snaps to grid points if Snap to points is enabled in Tools, Options, Document Properties, Grid/Snap, and to sketch entities and annotations. If you press Esc while inserting blocks, all instances created in the current operation are lost.
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4.
Click OK
.
You can edit block notes either for all instances or for each instance individually. Edit the text in the Block Definition PropertyManager to apply the change to all instances. To enable editing of each instance, give the note a tag name in the definition and then edit the note attribute in the Block Instance PropertyManager. You cannot doubleclick a block note to edit it on screen. To edit the properties of a block instance:
1.
Select a block instance in the graphics area.
2.
The Block Instance PropertyManager appears.
3.
Specify a leader, scale, rotation angle, and text display. Click Attributes to edit the values of notes.
4.
Click OK
.
To edit a block definition:
1.
Select the block definition in the FeatureManager design tree and click Tools, Block, Edit Definition. - or Right-click the block definition in the FeatureManager design tree, or right-click a block instance in the graphics area, and select Edit Definition. The block appears on a temporary sheet and the Block Definition PropertyManager opens.
2.
You can add, delete, and edit entities in the graphics area. In the Block Definition PropertyManager, you can edit the name of the block, change the base point position, and link the block definition to a file.
3.
Click OK
to save changes and remake the block.
To explode a block:
1.
Right-click the block in the graphics area and select Explode. - or Select the block and click Tools, Block, Explode.
2.
To remake the block, select the entities to include and click Tools, Block, Make. The name of the new block appears in the FeatureManager design tree with the next sequence number. If you explode a block that is on a layer, the entities retain their old colors when you move them to a new layer. To reset the colors so that the entities inherit the color of the new layer, first select the entities, click Line Color
on the Line Format toolbar, select Default, and click OK.
To change the position of the block base point:
1.
Edit the block definition (see above). The base point of the block is identified in the graphics area of the block definition editor by
2.
. The
pointer changes to . Drag the base point to any position in the editor's graphics area. - or Under Base Point in the Block Definition PropertyManager, enter relative values in the X Coordinate and Y Coordinate
boxes.
The original base point position is identified by 3.
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Click OK
.
.
To change the position of the leader attachment point and leader anchor point:
1.
Select a block instance.
2.
In the Block Instance PropertyManager, under Arrow/Leader, select Display leader. NOTE: The block must have a leader in order for you to change the position of the leader attachment point and anchor point. The leader attachment point appears by default at the lower left corner of the block, on top of the anchor point.
3.
In the graphics area, select the leader attachment point (the pointer changes to point) and drag it anywhere on the drawing sheet.
when it is over the
The leader anchor point is now visible. 4.
Select the leader anchor point (the pointer changes to another position within the block.
when it is over the point) and drag the point to
Insert Block PropertyManager The Insert Block PropertyManager appears when you insert a block instance into a drawing. To insert a block:
1.
Click Insert Block
on the Annotation toolbar, or click Insert, Block.
2.
Select a block under Source, or browse to a block file.
3.
Specify the properties described below, then click in the graphics area to place the block.
4.
Repeat steps 2 and 3 as many times as necessary, then click OK
.
Source Select the block to insert by one of the following methods: •
Name. Select a block name from the list of blocks in the document.
•
Browse. Browse to a block file (.sldblk, .sldsym, .dwg, .dxf).
Location As you move the pointer, the coordinates of the block base point appear in the X Coordinate
and Y Coordinate
boxes. Click in the graphics area to place the block. You can enter values for X Coordinate and Y Coordinate for the last block inserted.
Blocks snap to grid if snap is enabled in Tools, Options, Document Properties, Grid/Snap, and to sketch entities and annotations. If the block has a leader, place the leader first, then the block. Block Display Block Scale . Enter a positive non-zero number. If you enter an invalid number (zero or negative), the scale is reset to the previous valid number. Block Rotation
. Enter a value in degrees. A positive value rotates the block counterclockwise.
Leader Display leader. Select to attach a leader to the block. Bent leader. Select to add a horizontal segment at the block end of the leader. Arrowhead Style. Select a style from the list.
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Layer In drawings with named layers, select a layer that applies to the block leader and arrow. Block Instance PropertyManager You can control block leaders, arrows, scale, rotation angle, and text display while you insert a block instance or for an existing block instance. Block Display Block Scale . Enter a positive non-zero number. If you enter an invalid number (zero or negative), the scale is reset to the previous valid number. Block Rotation
. Enter a value in degrees. A positive value rotates the block counterclockwise.
Text Display Select one of the following for display of note text: •
Normal. Notes are displayed based on their visibility settings.
•
All. All text is displayed, regardless of visibility settings.
•
None. No text is displayed.
Attributes. Click to edit values of note attributes. Leader Display leader. Select to attach a leader to the block. Bent leader. Select to add a horizontal segment at the block end of the leader. Arrowhead Style. Select a style from the list. Layer In drawings with named layers, select a layer that applies to the block leader and arrow. Move sketch entities and annotations onto layers in the block definition, or before making the block. Attributes You can edit the values of Block attributes in this editor. Changes apply to the current instance of the block. Attributes can be created automatically when you import blocks from AutoCAD files, or manually when you assign a Tag name (and specify Invisible or Read Only, or both) when you insert a note into a block definition. NOTE: Attributes in SolidWorks drawings can have multi-line values (note text). However, if you plan to export blocks to AutoCAD, you should use only single-line values. To access the editor, select a block instance in a drawing document and click Attributes in the Block Instance PropertyManager. The following columns appear in the editor: •
Name. The name of the attribute (Tag name in the Note PropertyManager).
•
Value. The value, or text, of the attribute. You can edit the value if the attribute is not Read Only.
•
Invisible. This column contains an X if the attribute is invisible (information only).
•
Read Only. This column contains an X if the attribute is read only (information only). NOTE: Values that are linked to file properties or custom properties display the link path and variable name ($PRP:"SW-File Name", for example) during editing but show the values of the properties (WIDGET, for example) when block instances are inserted into drawings.
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Block Definition PropertyManager Edit the block definition and specify the properties described below. To access the block editor:
•
Right-click the name of the block in the FeatureManager design tree and select Edit Definition.
•
Right-click a block instance in the graphics area and select Edit Definition.
•
Select the name of the block in the FeatureManager design tree and click Tools, Block, Edit Definition.
•
Select a block instance in the graphics area and click Tools, Block, Edit Definition. The block is displayed on a temporary sheet in the graphics area and the Block Definition PropertyManager opens.
The block is in exploded form in the definition editor. When you click OK definition is automatically remade.
to exit from the editor, the block
You can move sketch entities and annotations onto layers. Changes you make to layer properties while in the block editor apply to all entities in the layer, not just the block entities. Block Name Type to edit the block name. The name appears in the FeatureManager design tree. Base Point Drag the base point (designated by
, initially at the lower left corner of the block) to a new relative position or
enter values for its relative X Coordinate was opened is identified by
and Y Coordinate
. The position of the base point when the editor
.
When you insert a block in a drawing graphics area, the block instance is located so that its base point is at the insertion point. External Reference If you selected the Create external reference to file check box in the Open dialog box when you inserted the block into the drawing document from a file, Link to file is selected automatically and the file name appears in the box. If you select Link to file after you open the block definition editor, the local definition updates to reflect any changes in the selected file definition. When you exit from the definition editor, the local definition is still linked to the specified file and reflects any subsequent changes to the file definition. When Link to file is selected, you cannot edit the block definition. To edit the file definition, select the file name in the FeatureManager design tree and click Tools, Block, Edit File.
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Tables Annotation Tables Tables are available on the Annotation toolbar for: •
Bills of Materials
•
Hole Tables
•
Revision Tables
•
Weldment Cut Lists
All tables have the following functionality: •
Drag with the pointer
•
Snap to an anchor point that you can set
•
Snap to lines, points, and vertices in the sheet format
•
Use standard or custom templates
•
Add columns and rows and adjust their dimensions
•
Select and delete tables, columns, and rows
•
Split or merge tables
•
Merge or split cells
•
Sort the contents of columns
•
Zoom to selection
•
Control color in layers
Selecting the title bar selects the whole table for such operations as dragging, formatting, and adjusting column width or row height. To drag a table:
1.
In the table PropertyManager, clear Attach to anchor.
2.
Hold Alt and drag the table from anywhere inside the table - or Drag the table title bar.
To snap a table to sheet format entities:
1.
Drag the table toward a vertical or horizontal line, a point, or a vertex in the sheet format.
2.
As the edge of the table snaps to the line or point, release the pointer.
To add a column or row to a table:
In the column or row where you want to add the new column or row, right-click and select Insert: •
Column Right
•
Column Left
•
Row Above
•
Row Below
To adjust column width or row height:
Drag a border - or Select one or more columns or rows (or select the whole table by the title bar), right-click and select Formatting, Column Width or Row Height, then type a number in the dialog box.
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To select or delete a table, column, or row:
Right-click in the table and choose Select or Delete, then Table, Column, or Row. To split a table:
Right-click in the table and select Split: •
Horizontally Above
•
Horizontally Below
•
Vertically Left
•
Vertically Right
To merge a table that has been split, right-click in a section of the table and select Merge. To merge or split cells:
1.
Select the cells.
2.
Right-click and select Merge or Split.
To sort columns in a Bill of Materials:
1.
Right-click in the Bill of Materials and select Sort.
2.
Select options in the Sort dialog box, then click OK.
To sort a column in a hole table or weldment cut list:
Right-click in a column and select Sort, Ascending or Descending. Editing Tables •
If you edit items in a table, automatic controls do not change them. To edit text, double-click the text and edit on screen. The Note PropertyManager appears, allowing you to format the text in addition to editing it.
•
If the cell value is parametrically linked to a part or assembly document, a message warns you that editing the value will sever the link. To restore the link in the future, delete the user-defined text from the cell.
PropertyManagers Each table has PropertyManagers for: •
Table Properties
•
Table Format
•
Column Properties
•
Cell Properties
Buttons for the other PropertyManagers appear at the bottom of each PropertyManager, as appropriate.
Table Anchors Each type of annotation table has its own anchor point in a drawing sheet format. To set a table anchor point:
1.
In the FeatureManager design tree, expand
Sheet Format for the active drawing sheet.
2.
Right-click the anchor you want to set and select Set Anchor. Choose from: Bill of Materials Anchor Hole Table Anchor Weldment Cut List Anchor Revision Table Anchor
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3.
Click in the graphics area to specify the anchor point. You are in Edit Sheet Format mode.
4.
Right-click in the graphics area and select Edit Sheet.
In the table PropertyManagers, select the corner of the table to attach to the anchor point.
Table Templates Standard templates for Bills of Materials, Hole Tables, Revision Tables, and Weldment Cut Lists are available in\lang\. You can specify a different folder, and you can save and use custom templates. Table
File Name Extension
Bill of Materials Hole Table Revision Table Weldment Cut List
.sldbomtbt .sldholtbt .sldrevtbt .sldwldtbt
Custom templates contain headings and formatting, but not table contents. The table PropertyManagers remember the last used template. To change the location of table templates:
1.
Click Tools, Options, System Options, File Locations.
2.
Under Show folders for, select: •
BOM Templates
•
Hole Table Templates
•
Revision Table Templates
•
Weldment Cut List Templates
3.
Click Add, browse to a folder, and click OK.
4.
Repeat steps 2 and 3 as necessary, then click OK.
To save a custom template:
1.
Insert a table into a drawing.
2.
Customize the table.
3.
Right-click in the table and select Save as template.
4.
In the Save As dialog box, type in the template name, browse to a folder, and click Save.
To use a custom template:
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1.
When inserting a table, under Table Template in the PropertyManager, click Browse for template.
2.
In the Select Template dialog box, browse to a template, then click Open.
Custom Table Templates You can customize standard table templates to save for future use. To customize a table template:
1.
2.
3.
Open a model that contains the characteristics needed for the template: •
Components
•
Custom properties
Insert a table. In the table PropertyManager, specify one of the standard templates shipped with the SolidWorks software; for example: •
bom-standard.sldbomtbt for a Bill of Materials
•
standard hole table--letters.sldholtbt for hole table
•
standard revision block.sldrevtbt for a revision table
•
cut list.sldwldtbt for a weldment cut list
Edit the table as described below, then save the table as a template.
To add a column:
1.
Right-click in a table column and select Insert, Column Right or Column Left.
2.
In the Column PropertyManager, select from the list of Column Properties. To select a custom property, the property must be available in the model documents. For properties in the various types of tables, see the Column PropertyManager topic for Bill of Materials, hole tables, revision tables, or weldment cut lists.
3.
Edit the column Title.
To add a row:
Right-click in a table row and select Insert, Row Above or Row Below. See Annotation Tables for procedures to adjust column width or row height, split or merge a table or cells, sort columns, and so on.
Table Format PropertyManager Specify formatting for a Bill of Materials, Hole Table, Revision Table, or Weldment Cut List. To specify formatting for a table:
1.
In one of the table PropertyManagers (Table, Column, or Cell), click Table Format.
2.
Specify the formatting described below, then click OK
.
Header Title. Edit the table header title if Display title is selected. Display title. Displays the text in Title in a header row across the width of the table. Position. The header can be at the Top
or the Bottom
of the table.
Border Click Box Border
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, Grid Border
, or All Borders
, then select a corresponding thickness.
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Text Format Table text format for the document is set in Tools, Options, Document Properties, Annotations Font. You specify formatting for individual tables in this PropertyManager and override formatting for individual cells in the Table Cell PropertyManager. •
Click Left Justify
, Center Justify
, or Right Justify
to justify text horizontally.
•
Click Top Justify
, Middle Justify
, or Bottom Justify
•
Use document's font. When selected, the text is in the font specified for Tables in Tools, Options, Document Properties, Annotations Font.
•
Font. When Use document's font is cleared, click Font to open the Choose Font dialog box and select a new font style, size, and effect to apply to the table. You can specify a different font for cells.
to justify text vertically.
Layer In drawings with named layers, select a layer. Table Properties Click to access the table properties. Cell Properties Click to access the Table Cell PropertyManager. Column Properties Click to access the table column properties. BOM Contents In a Bill of Materials, click to access the Bill of Materials Contents dialog box.
Table Cell PropertyManager Specify formatting for one or more cells in a Bill of Materials, Hole Table, Revision Table, or Weldment Cut List. Table text format is set in the Table Format PropertyManager. You override formatting for individual cells in this PropertyManager. To specify formatting for cells:
1.
Select one or more cells in a table - or Click Cell Properties in another table PropertyManager.
2.
Specify the formatting described below, then click OK
.
Text Format
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•
Click Left Justify
, Center Justify
, or Right Justify
to justify text horizontally.
•
Click Top Justify
, Middle Justify
, or Bottom Justify
•
Click Rotate
•
Use table's font. When selected, the text is in the font specified in the Table Format PropertyManager.
•
Font. When Use table's font is cleared, click Font to open the Choose Font dialog box and select a new font style, size, and effect for the selected cells.
to justify text vertically.
to rotate the text in 90° increments counterclockwise.
Column Properties Click to access the table column properties. Table Properties Click to access the table properties. Table Format Click to access the Table Format PropertyManager.
Bill of Materials You can insert Bills of Materials into assembly drawings. A drawing can contain a table-based Bill of Materials or an Excel-based Bill of Materials, but not both. The table-based Bill of Materials is based on SolidWorks tables and includes: •
Templates
•
Anchors
•
Quantities for configurations
•
Whether to keep items that have been deleted from the assembly
•
Zero quantity display
•
Excluding assembly components
•
Following assembly order
•
Item number control
Example of Bill of Materials
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You can specify a starting Item Number, but the increment is always a single integer (1, 2, 3 ..., or 100, 101, 102 ..., for example). You can change the text in any cell by double-clicking and editing on screen, but if you edit data generated by SolidWorks (Item Number, Quantity, and so on), you break the link between the data and the Bill of Materials. To set options for a Bill of Materials in the active document:
1.
Click Tools, Options, Document Properties, Tables.
2.
Set options under Bill of Materials Table, then click OK.
To insert a Bill of Materials into a drawing document:
1.
Click Bill of Materials
on the Annotation toolbar, or click Insert, Tables, Bill of Materials.
2.
Select a drawing view to specify the model.
3.
Set the properties in the Bill of Materials PropertyManager, then click OK
4.
If you did not select Attach to anchor, click in the graphics area to place the table.
.
To exclude assembly components from Bills of Materials:
1.
In the assembly document, right-click the component and select Properties.
2.
In the Component Properties dialog box, select Exclude from bill of materials, then click OK.
To sort columns in a Bill of Materials:
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1.
Right-click anywhere in the Bill of Materials and select Sort.
2.
In the Sort dialog box, choose up to three columns to sort by, select other options, then click OK.
Bill of Materials PropertyManager Specify properties for Bills of Materials. To specify properties for Bills of Materials:
1.
Click Bill of Materials
on the Annotation toolbar, or click Insert, Tables, Bill of Materials.
2.
Specify the properties described below, then click OK
.
Table Template Click Browse for template insertion.
to choose a standard or custom template. This option is available only during table
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. BOM Type Select: •
Top level only. List parts and sub-assemblies, but not sub-assembly components.
•
Parts only. Does not list sub-assemblies. Lists sub-assembly components as individual items.
•
Indented assemblies. Lists sub-assemblies. Indents sub-assembly components below their sub-assemblies without item numbers.
Configurations Lists quantities in the Bill of Materials for all selected configurations. Select configurations manually, or click Select all configurations
or Unselect all configurations
.
Part Configuration Grouping Display as one item number. If a component has multiple configurations, all the configurations appear with the same item number. Use this option with BOM Type set to Top level only. To see the configuration name in the PART NUMBER column, go to the part document. On the Configuration tab, right-click each configuration, and select Properties. Under Part number displayed when used in a bill of materials, select Configuration Name. Keep Missing Item If components have been deleted from the assembly since the Bill of Materials was created, you can keep the components listed in the table. If missing components are still listed, the text for the items can appear with strikethrough display.
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Zero Quantity Display If an assembly component does not appear in a configuration, displays the zero quantity with a dash (-), a zero (0), or a blank cell. Item Numbers Start at. Type a value for the beginning of the item number sequence. The sequence increases by single digits. Click Follow assembly order for the item numbers to follow the order in which the assembly appears in the FeatureManager design tree. For components with multiple instances, the first instance appears in the order of the FeatureManager design tree, and subsequent instances increment the quantity. Click Do not change item numbers to keep the item numbers with their components when reordering rows (manually in BOM Contents, by sorting, or when you click Follow assembly order, for example). BOM Contents Click to access the Bill of Materials Contents dialog box. Table Format Click to access the Table Format PropertyManager. Cell Properties Click to access the Table Cell PropertyManager. Column Properties Click to access the Bill of Materials Column PropertyManager. Bill of Materials Contents In this display of the Bill of Materials contents, you can move rows up or down, and you can group and ungroup rows. To edit Bill of Materials Contents:
1.
In the Bill of Materials, Column Properties, Cell Properties, or Table Format PropertyManager, click BOM Contents.
2.
Edit properties as described below, then click Apply.
3.
Click OK.
Show balloon state Toggle row visibility Row up
. The icon shows whether the component has a balloon . Click the icon to hide
or Row down
or show
or not
.
the row.
. Select a row and click to move the row up or down.
To keep the item number with its component when reordering rows, click numbers in the Bill of Materials PropertyManager.
Do not change item
Group and Ungroup . Select two or more rows to group the components under one item number. To dissolve the group, select a member and click Ungroup.
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Bill of Materials Column PropertyManager Specify the columns to be included in a Bill of Materials and their position in the table. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To edit Bill of Materials column properties:
1.
2.
Access the PropertyManager by one of the following methods: •
Add a new column to the Bill of Materials
•
Click at the head of a column when the pointer changes to
•
Click Column Properties in another Bill of Materials PropertyManager (Cell, Table Properties, Table Format)
Specify the properties described below, then click OK
.
Column Properties For the selected column, choose one of the following column types, listed with its header title. You can edit the header in the Title box below. •
Item Number. ITEM NO.
•
Part Number. PART NUMBER
•
Quantity. QUANTITY
•
User Defined. Select a document property under Custom Property.
Custom Property. Document's custom properties, available when you specify User Defined under Column Properties. Use Title Summary. In Part Number, use the data in the Title field of File, Properties, Summary Information in part documents. Title. Edit the text of the column header. Column position. Click Move Column Left
or Move Column Right
to move the selected column.
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Bill of Materials PropertyManager. Table Format Click to access the Table Format PropertyManager. BOM Contents Click to access the Bill of Materials Contents dialog box. Bill of Materials Sort To sort the columns of a Bill of Materials:
1.
Right-click anywhere in the Bill of Materials table and select Sort.
2.
Edit the options as described below, then click OK.
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Sort by Select the name of a column and either Ascending or Descending for the primary sort. Then by Select the name of a column and either Ascending or Descending for a secondary sort. Then by Select the name of a column and either Ascending or Descending for a tertiary sort. Group items Assemblies, Parts, Other. Select one or more category to sort rows within the category. If you select more than one category, order them by selecting one and clicking Up or Down. Other is user-defined data (oil or grease, for example). Item numbers Do not change item numbers. Select to keep the item numbers with the configuration row.
Hole Tables Hole tables in drawing documents measure the positions of selected holes from a specified origin datum. The software labels each hole with a tag that corresponds to a row in the table. Non-circular holes such as rectangles and slots are recognized as holes. The table lists the X and Y coordinates of the entities, but you must enter the size. In addition to the functionality for all tables, you can specify in options and in the Hole Table PropertyManager: •
Tags to be alphabetic or numeric
•
Tag leaders to be visible
•
Cells with the same tags to be combined
•
Cells for holes of the same size to be combined
•
Precision of hole locations
Example of Hole Tables
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To set options for hole tables in the active document:
1.
Click Tools, Options, Document Properties, Tables.
2.
Set the options under Hole Table, then click OK.
To create a hole table:
1.
Click Hole Table
on the Annotation toolbar, or click Insert, Tables, Hole Table.
2.
In the graphics area, select a vertex to specify the origin datum. You can select an X axis and Y axis to define a vertex for the datum. You can also drag the origin datum into position after you place the table.
3.
Select hole edges, or select a model face to include all the holes on the face.
4.
In the PropertyManager, select a template or anchor, then click OK
5.
If you did not select Attach to anchor, click in the graphics area to place the table.
.
To edit the origin datum:
Select the datum in the graphics area - or Right-click the hole table in the FeatureManager design tree and select Edit datum definition. To add holes to a table:
Right-click the hole table in the FeatureManager design tree and select Add holes.
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To format hole tags:
1.
Select one or more tags.
2.
In the Note PropertyManager: •
Under Text Format, specify justification, angle, and font.
•
Under Border, select a border style and size.
•
Under Leader, select a leader and arrow. Apply to all applies to all the arrows on the selected tags. To see a preview leader without adding a visible leader, hold the pointer over the tag for a few seconds. The leader and arrow appear in red.
• 3.
Under Layer, in drawings with named layers, select a layer.
Click OK
.
Hole Table Add Holes To add holes to an existing hole table:
1.
Right-click the table in the FeatureManager design tree and select Add Holes.
2.
Select edges of holes or faces containing holes, then click OK
.
Hole Table PropertyManager Specify properties for existing hole tables. For new hole tables, see Hole Table Insert PropertyManager. To specify properties for hole tables:
1.
2.
Access the PropertyManager by one of the following methods: •
Right-click anywhere in the table and select Properties.
•
Right-click the table in the FeatureManager design tree and select Properties.
•
In another PropertyManager (Cell, Column, or Table Format), click Table Properties.
Specify the properties described below, then click OK
.
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. Alpha/Numeric Control Specify the tags identifying the holes to be letters or numbers. Scheme Combine same tags. Combines rows with holes in the same pattern, which also combines holes with the same sizes. The columns of location values are removed. Combine same sizes. Available only if Combine same tags is cleared. Merges cells for holes of the same size. The columns of location values remain.
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Hole Location Precision Specify the number of significant digits for the hole location values. Visibility Select to hide any or all of the following: •
Hide origin indicator
•
Hide hole centers
•
Hide hole tags
Table Format Click to access the Table Format PropertyManager. Hole Table Axis PropertyManager To edit the hole table origin datum:
1.
Select the hole table origin datum in the graphics area. The pointer changes to
when it is over the origin datum.
2.
Edit the axis labels, font, and layer.
3.
To edit the position of the datum, click Edit datum definition.
4.
Click OK
.
You can drag the origin datum to a new location in the graphics area. The location values in the table update. Hole Table Insert PropertyManager Specify properties for new hole tables. For existing hole tables, see Hole Table PropertyManager. To specify properties for new hole tables:
1.
Click Hole Table
on the Annotation toolbar, or click Insert, Tables, Hole Table.
2.
Specify the properties described below, then click OK
.
Table Template Click Browse for template insertion.
to choose a standard or custom template. This option is available only during table
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor.
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Datum During insertion, Origin is ready for you to select a vertex. To define the origin with an X axis and Y axis, click X Axis Direction Reference and select a horizontal model edge in the graphics area, then click Y Axis Direction Reference and select a vertical model edge. After the table has been created, you can drag the datum origin to another position. The location values in the table update. To edit the origin datum, select it in the graphics area, or right-click in the FeatureManager design tree and select Edit datum definition. Holes Select individual hole edges, or select a model face to include all the holes in the face. After the table has been created, right-click the hole table in the FeatureManager design tree and select Add Holes. Hole Table Column PropertyManager Specify the columns to be included in a hole table and their position in the table. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To edit hole table column properties:
1.
2.
Access the PropertyManager by one of the following methods: • •
Add a new column to a hole table. Click at the head of a column when the pointer changes to
•
Click Column Properties in another hole table PropertyManager.
Specify the properties described below, then click OK
.
.
Column Properties For the selected column, choose one of the column types, listed with its header title. You can edit the header in the Title box below. •
X. XLOC
•
Y. YLOC
•
Hole. TAG
•
Quantity. QUANTITY
•
Size. SIZE
•
Custom. Type a header under Title.
Title. Edit the text for the column header. Column position. Click Move Column Left
or Move Column Right
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Hole Table PropertyManager. Table Format Click to access the Table Format PropertyManager.
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to move the selected column.
Revision Tables Insert a revision table into a drawing to track document revisions, including revision symbols. In addition to the functionality for all tables, you can select: •
Revision symbol shapes
•
Alphabetic or numeric sequence The latest revision also appears under REV in the lower-right corner of a sheet format.
To set options for revision tables in the active document:
1.
Click Tools, Options, Document Properties, Tables.
2.
Set the options under Revision Table, then click OK.
To insert a revision table:
1.
Click Revision Table
on the Annotation toolbar, or click Insert, Tables, Revision Table.
2.
Set the properties in the Revision Table PropertyManager, then click OK
.
To add a revision to the table:
Right-click in the revision table and select Revisions, Add Revision.
Revision Symbols You can add revision symbols (the revision letter or number enclosed in a circle, triangle, square or hexagon) to the drawing. •
If you select Enable symbol when adding new revision under Options in the Revision Table PropertyManager, you can click in the graphics area to place symbols when you add a revision to the table.
•
If you clear Enable symbol when adding new revision or to add a symbol later, right-click in a row of the revision table and select Revisions, Add Symbol, then click in the graphics area to place symbols.
•
If you edit revision text, the symbols update.
Alphabetic or Numeric Control You can choose either letters or numbers for revisions in Tools, Options, Document Properties, Tables. If you switch from one to the other, you can change the revisions already in the table, or you can leave them unchanged and continue with future revisions in the new format. Any revision text you edit remains unchanged by automatic operations.
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Note Linked to Revision Level You can link a note (generally at the lower left in the Sheet Format) to the revision letter so that it is synchronized. To synchronize the revision in a note:
1.
With no revision table in the drawing, right-click in the graphics area and select Edit Sheet Format.
2.
Click Note
3.
In the PropertyManager, click Link to Property
4.
In the dialog box, click File Properties.
5.
In the Summary Information dialog box, select the Custom tab and do the following:
on the Annotation toolbar and click in the graphics area to place the note. .
a.
Under Name, select Revision (type Revision if it does not appear in the list).
b.
Place the pointer in the Value field and press the space bar.
c.
Click Add.
d.
Click OK.
6.
In the Link to Property dialog box, under Use custom property from, select Revision from the list, then click OK.
7.
Right-click in the graphics area and select Edit Sheet.
8.
Insert a revision table. The note displays the latest revision level.
Revision Table PropertyManager Specify properties for revision tables. Table Template Click Browse for template insertion.
to choose a standard or custom template. This option is available only during table
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. Revision Symbol Shapes Select a border shape for revision symbols: Circle Triangle Square Hexagon
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Options Enable symbol when adding new revision. Allows you to click in the graphics area to place revision symbols when you add a revision to the table. Table Format Click to access the Table Format PropertyManager. Revision Table Column PropertyManager Specify the columns to be included in a revision table and their position in the table. The columns are populated with data from the document's properties. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To edit revision table column properties:
1.
2.
Access the PropertyManager by one of the following methods: •
Add a new column to a revision table
•
Click at the head of a column when the pointer changes to
•
Click Column Properties in another revision table PropertyManager.
Specify the properties described below, then click OK
.
Column Properties For the selected column, choose one of the column types, listed with its header title. You can edit the header in the Title box below. •
Zone. ZONE
•
Revision. REV.
•
Description. DESCRIPTION
•
Date. DATE
•
Approved. APPROVED
•
Custom Properties. Select a document property under Properties.
Properties. Document's custom properties, available when you specify Custom Properties under Column Properties. Title. Edit the text for the column header. Column position. Click Move Column Left
or Move Column Right
to move the selected column.
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Revision Table PropertyManager. Table Format Click to access the Table Format PropertyManager.
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Excel-based Bill of Materials Bill of Materials Overview Applies to Excel-based Bills of Materials. A drawing can contain an Excel-based Bill of Materials or a tablebased Bill of Materials, but not both. You can insert a bill of materials (BOM) into the drawing of an assembly. If you add or delete components in the assembly, the bill of materials automatically updates to reflect the changes if you select the Automatic update of BOM option under Tools, Options, Document Properties, Detailing. Such changes include adding, deleting, or replacing components, changing component names or custom properties, and so on. •
If you do not select Automatic update of BOM, you must delete and re-insert the BOM to update it NOTE: To insert a bill of materials in a drawing, you must have Microsoft Excel 97 or later installed on your computer.
•
Rows in bills of materials are combined when all fields (except for Item Number) are the same. However, bills of materials in drawings created in releases prior to SolidWorks 2000 are not automatically updated to combine rows.
•
You can insert balloons or stacked balloons that label the parts in an assembly and relate them to item numbers in the bill of materials.
•
If you change the Item Number in a balloon, the item number in the bill of materials also changes.
•
SolidWorks includes several BOM templates in the following directory: \install_directory\lang\english.
•
You can embed dimensions and mass property parameters into values of custom properties in part documents. You can then include the custom properties in a bill of materials. The values in the BOM update automatically if the part dimensions or mass properties change.
To hide a bill of materials:
Right-click the bill of materials in the graphics area or in the FeatureManager design tree and select Hide Bill of Materials. NOTE: To show the bill of materials again, right-click the bill of materials in the FeatureManager design tree (expand the drawing view if necessary) and select Show Bill of Materials.
Bill of Materials Templates Applies to Excel-based Bills of Materials. The default template, Bomtemp.xls, contains columns for ITEM NO., QTY., PART NO., and DESCRIPTION. The SolidWorks software populates the columns in the default template automatically. Other templates supplied with the software add the following columns to the default format. BOM template file name
Columns added to default format
Bomtemp-Material.xls
MATERIAL
Bomtemp-StockSize.xls
STOCK SIZE
Bomtemp-Vendor.xls
VENDOR NO
Bomtemp-Weight.xls
WEIGHT
Bomtemp-All.xls
VENDOR NO, WEIGHT, STOCK SIZE, MATERIAL
You must add the custom properties into the parts of your assembly in order to take advantage of the additional columns in these templates.
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Bill of Materials - Inserting Applies to Excel-based Bills of Materials. You can insert a bill of materials into the drawing of an assembly. If you add or delete components in the assembly, the bill of materials automatically updates if you have selected the Automatic update of BOM option under Tools, Options, Document Properties, Detailing. NOTE:To insert a bill of materials into a drawing, you must have Microsoft Excel 97 or later installed on your computer. To insert a bill of materials:
1.
With a drawing view selected, click Insert, Bill of Materials.
2.
In the Select a BOM Template dialog box, select an Excel template for the BOM and click Open. NOTE: The default BOM template is in install_folder\lang\english\bomtemp.xls.Several other BOM templates are available in the same directory. You can customize the templates by adding columns or changing the text formatting. You can also create new templates to meet your company’s standards.
3.
In the Bill of Materials Properties dialog box, select properties from the Configuration, Contents, and Control tabs.
4.
Click OK.
A bill of materials is displayed that lists the components of the assembly.
Bill of Materials - Configuration Applies to Excel-based Bills of Materials. The Configuration tab in the Bill of Materials Properties dialog box specifies basic display properties of a bill of materials. The other tabs available in the dialog box are Contents and Control. The software remembers your selections from session to session. The Configuration tab controls the following properties. •
Use summary info title as part number. If you assigned a part identifier number in the title box of the Summary Info for the part, you can use that identifier in the bill of materials.
•
Use the document’s note font when creating the table. When selected, the BOM uses the text font specified for notes, under Tools, Options, Document Properties, Detailing, Notes, Font. Otherwise, the font specified in the BOM template is used.
•
Choose one of the following to specify the way to list sub-assemblies and their components in the bill of materials: o
o
o
Show parts only. Select this option to list only parts in the bill of materials. Subassemblies are not listed; their components are listed as individual items. Show top level subassemblies and parts only. Select this option to list parts and subassemblies in the bill of materials. Each subassembly type is an item; the individual subassembly components are not listed. Show assemblies and parts in an indented list. Subassemblies are listed as items; subassembly components are shown below the subassembly to which they belong, but without item numbers.
•
Anchor point. Select or clear Use table anchor point. The standard templates supplied with the software include an anchor point for placing the BOM in a specific location on the sheet. To use the point, select this option, then select which corner of the BOM table to make coincident with the point (top left, bottom right, and so on). If you do not use the anchor point, the BOM is placed on the sheet near the selected view.
•
Add new items by extending top border of table. New components are always added at the bottom of the table, and the rest of the table shifts upward. The last row of the table remains in the same position on the drawing sheet. This option applies only when you do not use an anchor point.
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Bill of Materials - Contents Applies to Excel-based Bills of Materials. The Contents tab in the Bill of Materials Properties dialog box specifies which items appear in the bill of materials, and allows you to reverse the order of the list. The other tabs available in the dialog box are Configuration and Control. The Contents tab controls the following properties: •
Select which items to include in the table. A green check mark in the ITEM NO. column means that the item is displayed in the table. Clear the check mark to hide the item. This has the same effect as hiding the row in the Excel worksheet.
•
To move the header row to the bottom of the table, and to list the items in order from bottom to top, clear the Display labels at top check box.
•
To sort the items alphanumerically by a column (for example, to sort by part number), hold down the Ctrl key, and click the box at the top of the column. The item numbers are re-assigned so that the first line is still Item 1, and the remaining item numbers are in order. NOTE: If you do not hold down the Ctrl key, the item number for each line stays with the original item, resulting in a list with item numbers out of order.
Bill of Materials - Control Applies to Excel-based Bills of Materials. The Control tab in the Bill of Materials Properties dialog box specifies how row numbers are assigned, what happens when a component is deleted, and how to split long BOM tables. The other tabs available in the dialog box are Configuration and Contents. The Control tab controls the following properties: Row numbers •
Row numbers follow assembly ordering. Select to use the item numbers assigned by the software. Clear to assign the item numbers in Excel, and override the system-defined item numbers. NOTE: When you select this check box: o o
•
Any sorting other than by Item No. is not preserved in the Bill of Materials. If you try to change an item number in a balloon, a message appears stating that you cannot change the item number.
Reserve row numbers for missing components. Specify what happens if a component is removed from the assembly. o o
No. The rows for the removed components are deleted from the table. Yes. Specify how the row is displayed: Display with zero quantity, Hide, or Display with strike through text.
Split Tables •
Split tables into multiple sections. Select to allow the table to split.
•
Table height before splitting. Specify a value for the height.
•
Split direction for new sections. Select Left or Right from the list. If the BOM exceeds the height you specify, the table splits and continues in another column to the Left or Right.
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Bill of Materials - Edit Text Applies to Excel-based Bills of Materials. To edit text in a bill of materials (BOM):
1.
Double-click the BOM, or right-click the BOM and select Edit Bill of Materials. While the bill of materials is active, it is displayed with shaded borders, and row and column headers. Excel toolbars replace the SolidWorks toolbars.
2.
Edit the worksheet as needed, using Excel functions. You can perform these kinds of edits: •
Edit the cells in the Item No. column or the Description column. Before you edit the Item No. column, you must clear the Row numbers follow assembly ordering check box on the Control tab of the Bill of Materials Properties dialog box. See the previous section for more information.
•
If you edit text in the Qty. or Part No. columns, these changes will be lost the next time that the BOM updates for any reason.
•
To edit linked properties, Automatic Update of BOM in Tools, Options, Document Properties, Detailing must not be selected. If this option is selected, the linked properties are reset to the values in the Summary Info dialog box when you rebuild the drawing.
•
Rename the column headers. Type the new text in the header cell or in the Formula Bar. Do not edit the text in the Name box.
•
Add columns, before the cell marked $$END, and rows (but not above the header row). You can include rows for bulk items, such as oil or adhesive.
•
Change the order of the columns. Insert a new column, cut and paste the existing columns until they are arranged as needed, then delete the empty column.
•
Hide columns. Right-click the lettered cell at the top of the column, and select Hide. If the BOM includes a column that you do not want to display, do not delete it; hide it instead.
•
Hide rows. Right-click the numbered cell at the left of the row, and select Hide. This has the same effect as clearing the check mark beside the item on the Contents tab of the Bill of Materials Properties dialog box.
•
Do not delete rows to remove them from the table. If you delete a row in Excel, the row is replaced the next time the BOM is updated.
•
You cannot delete or hide the header row.
•
Change the text alignment (left, right, center) by column.
•
Adjust the column width or row height.
•
Change the text font.
•
Some editing operations apply to an entire row or column in the table. To select an entire row, click the numbered cell at the left of the row. To select an entire column, click the lettered cell above the column. NOTE: The following types of cell formatting are not supported in a bill of materials: cell shading (colors and patterns), borders, text orientation (text at an angle), wrap text, merge cells.
3.
Click outside the worksheet to return to the drawing.
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Chapter 12 Detailing
Bill of Materials - Part No. Column Applies to Excel-based Bills of Materials. You can display a name other than the document name in the part number column of the BOM. For example, you can use a stock number specified by your company, or the configuration name for a part or sub-assembly that has more than one configuration. To do so, it may be necessary to edit the Advanced properties of the configuration. To specify the name to use in the Part No. column:
1.
In the part or sub-assembly document, click the Configuration tab change to the ConfigurationManager view.
2.
Right-click the configuration you want to edit, and select Properties.
3.
In the Configuration Properties dialog box, under Part number displayed when used in a bill of materials, select one of the following:
4.
•
Document name.
•
Configuration name.
•
User-specified name. Type a name in the box.
at the lower left of the window to
If you always want a sub-assembly to be listed as a single component in the bill of materials, select the Don’t show child components in BOM when used as sub-assembly check box. When cleared, child components are listed individually in the BOM, when Show parts only or Show assemblies and parts in an indented list is selected in the Bill of Materials Properties dialog box.
5.
Click OK.
Bill of Materials - Multiple Configurations Applies to Excel-based Bills of Materials. You can specify how to list component configurations in a BOM. When multiple configurations of the same component are used in an assembly, there are some additional considerations. •
In the Item No. column, you can list the configurations as a separate entries with individual item numbers, or you can group all the configurations as a single entry with one item number.
•
In the Part No. column, you can display a user-defined name, the configuration name, or the document name for each item.
In the component document, you need to perform certain steps to achieve the desired results. The steps vary, depending on how you create the configurations If you use a design table to create configurations:
Item No.
Part No.
Procedure
each configuration as a separate item
use-defined names
Use $PARTNUMBER in the table, with a different value for each configuration
configuration names
This is the default. Design tables automatically set the Advanced Configuration Properties to use the configuration name.
a user-defined name
Use $PARTNUMBER in the table, with the same value for each configuration
the document name
Use $PARTNUMBER in the table, with the document name for all configurations
all configurations as a single item
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If you create configurations manually:
Item No.
Part No.
Procedure
each configuration as a separate item
use-defined names
Under Advanced Configuration Properties, click Use name below, and specify a different value for each configuration.
configuration names
Under Advanced Configuration Properties, click Use name below. The configuration name is the default.
a user-defined name
1 Use the default Advanced Configuration Properties (Use document name selected). 2 Click File, Properties, and enter a Title in the Summary Information dialog box. 3 When you create the BOM, select Use summary information title as part number.
the document name
This is the default for the Advanced Properties (Use document name selected).
all configurations as a single item
To edit the Add Configuration/Configuration Properties, right-click the configuration name, and select Properties. When the Configuration Properties are not defined in the same way for all the configurations of the components, the following order of precedence applies: •
User-defined name or configuration name (if Use name below is selected)
•
Summary Information Title (if the option is selected, and if Title is defined for the component)
•
Document name
Bill of Materials - Save as Excel File Applies to Excel-based Bills of Materials. To save a bill of materials as an Excel file:
1.
Click the bill of materials on the drawing sheet.
2.
Click File, Save As. The Save as type is set to Excel Files (*.xls) by default.
3.
Enter a file name, and click Save.
You can use the saved bill of materials in Excel, or as an OLE object in other applications. The saved file is not linked to the bill of materials in the drawing; edits to one do not affect the other.
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Chapter 12 Detailing
Bill of Materials - Custom Properties Applies to Excel-based Bills of Materials. You can add more information such as Material, Vendor_Number, Cost, and so on to the open part or sub-assembly document by clicking File, Properties, and selecting the Custom tab or the Configurations specific tab. (See Summary Info - Custom and Configuration Specific for information about specifying properties.) SolidWorks provides several templates for bills of materials in the directory \install_directory\lang\english. Columns in the templates are populated automatically as follows: Property
Automatically populates
ITEM NO. QTY. PART No.
In all templates supplied
DESCRIPTION MATERIAL STOCK SIZE VENDOR WEIGHT
1) When the column appears in the selected template, and 2) you add the property to the Custom or Configuration Specific information in the part or assembly document
custom properties
1) When you add a custom column to a BOM or template, and 2) you add the property to the Custom or Configuration Specific information in the part or assembly document
Custom properties can include model dimensions and mass properties, which update automatically in the BOM if they are changed in the model. To add custom columns to the bill of materials:
1.
Open the BOM template file. To add the columns to the default BOM template, open install_directory\lang\english\Bomtemp.xls. To create a new BOM template, it is a good idea to make a copy of the default template, then open the copy.
2.
Insert a new column where you want the information to appear. The new column must be to the left of the column marked $$END.
3.
Enter the column heading for the property you want to display in that column, and press Enter. The name appears in the Formula Bar in the Excel toolbar. This column heading does not need to match the custom property name.
4.
Click the cell to select it, then click Insert, Name, Define and type in the name of the property that you want to appear in this column. This cell name replaces the default alphanumeric cell name that appears in the Name Box in the Excel toolbar whenever you click a cell. The cell name is listed in the Names in workbook list for the selected cell. This name must match the name of the property from the part or sub-assembly document, and must not contain any spaces.
5.
Click Add, then click OK. When you add a bill of materials to a drawing, it now includes the added column. The cells are populated with the values of the custom properties of the document, or the values of the configuration specific properties for the item. NOTE: Do not change the cell names in the Name Box for the default columns in the BOM template. You can change the text in the column heading, but not the cell name.
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13 Import/Export
Importing and Exporting Files This section describes these SolidWorks file import and export topics: •
ACIS®
•
Parasolid® text and binary
•
Autodesk Inventor®
•
PDF
•
CADKEY®
•
Pro/ENGINEER®
•
CATIA®Graphics
•
Solid Edge®
•
DXF 3D
•
STEP
•
DXF™/DWG
•
STL
•
eDrawings
•
TIFF™
•
Highly Compressed Graphics
•
Unigraphics®
•
HOOPS®
•
VDAFS
•
IGES
•
Viewpoint®
•
JPEG
•
VRML
•
Mechanical Desktop®
•
ZGL Files
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Chapter 13 Import/Export
Importing/Exporting SolidWorks Documents You can import files to the SolidWorks software from other applications. You can export SolidWorks documents to a number of formats for use with other applications. The following table displays the data translation methods available for SolidWorks documents: Parts Application
Assemblies
Import
Export
Import
Export
ACIS
X
X
X
X
Autodesk Inventor
X
CADKEY
X
CATIA Graphics
X
DXF/DWG
X
DXF 3D
X
X
X
Highly Compressed Graphics
X
X
HOOPS
X
X
X
X
X
Mechanical Desktop
X
Parasolid
X
PDF
X
X
X
X
Solid Edge
X
STEP
X
X
X
X
STL
X
X
X
X
TIFF
X
X
X
X
Unigraphics
X
VDAFS
X
ZGL
X
X
X
X
X X X X X
X X
X X
NOTE: X = This option is available. A blank box = This option is not available.
13-2
X
X
X
X
X
X
Pro/ENGINEER
VRML
X
X X
X
Viewpoint
X X X
JPEG
Export
X
X
X
Import
X
eDrawings
IGES
Drawings
X
Importing Documents Before you import a document to the SolidWorks software, make sure that you have the import options set for your purposes. To import a file from another application:
1.
Click Open
or File, Open.
The Open dialog box appears. 2.
In the Files of type list, click the desired format.
3.
Browse to the desired file, and click Open. The selected file is opened. If there are surfaces in the file, they are read as follows: •
If there are blanked surfaces, they are imported and added to the FeatureManager design tree as surface features.
•
If the attempt to knit the surfaces into a solid succeeds, the solid appears as the base feature (named Imported1) in a new part file. You can add features (bosses, cuts, and so on) to this base feature, but you cannot edit the base feature itself.
•
If the surfaces represent multiple closed volumes, then one part is made for each closed volume. An assembly file also is made that includes the imported parts positioned relative to the assembly origin, according to how the surfaces are defined in the imported file. For ACIS files, if the imported ACIS file consists of surfaces only, then only surfaces are created even though they represent multiple closed volumes, regardless of the import options you choose. If the ACIS file consists of data about multiple solid bodies, parts or surfaces are created, depending on the import options you choose.
•
If the attempt to knit the surfaces fails, the surfaces are grouped into one or more surface features (named Surface-Imported1, 2, ...) in a new part file.
•
If you import a .dxf or .dwg file, the DXF/DWG import wizard appears.
Importing Geometry You can import surfaces, solids, sketches, curves, and graphics models (CATIA CGR, STL, or VRML files only) from ACIS, CATIA CGR, IGES, Parasolid, STEP, STL, VDAFS, or VRML files as reference geometry into part documents. To import the geometry from another application:
1.
In a part document, click Imported Geometry Imported.
on the Features toolbar, or click Insert, Features,
The Open dialog box appears. 2.
Browse to the desired file, and click Open. NOTE: For ACIS, IGES, STEP, STL, VDAFS, or VRML files, you can click Options to set the import options One or more features are imported, and the Imported features are added to the part. The features are positioned relative to the origin, using the coordinates in the imported file. NOTE: Wireframe geometry and curves are ignored when importing surfaces as reference geometry.
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Chapter 13 Import/Export
Editing Imported Features You can replace an imported feature with geometry from a new file. To edit a feature created from an imported document:
1.
In the FeatureManager design tree, right-click the feature created from the imported document, and select Edit Feature. The Open dialog box appears.
2.
In the Files of type list, select the desired format.
3.
Browse to select the desired file to import. The file name appears in the File name box.
4.
5.
Select the Match faces and edges check box, if desired. This does the following: •
Propagates the dependencies of the old faces and edges in the old body, such as sketches or features, to the new faces and edges in the new body.
•
Ensures you get the correct results when you open a file that has imported features.
Click Open. An imported solid is replaced only if the data in the new document can be successfully knitted into a body. A surface feature is replaced with the first surface in the new document, and subsequent surfaces in the new file are added to the model. NOTE: You can edit only features that were created from an IGES, STEP, ACIS, VRML, Parasolid, or VDAFS file.
If you had added features to the imported body before selecting Edit Feature, SolidWorks attempts to rebuild these features whenever possible. For example, this STEP file contains an imported feature. You need to add a feature to the imported body. 1. Select the bottom face of the imported body. 2.
Click Chamfer
.
The Chamfer PropertyManager appears. 3.
Under Chamfer Parameters, make the desired settings and click OK . The imported body now shows the additional chamfer feature on the bottom face.
4.
Right-click Imported1 in the FeatureManager design tree and select Edit Feature. A message box appears warning that this feature has a parent/child relation or is being referenced.
5.
Click OK. The Open dialog box appears.
6.
Select the STEP file and click Open. The STEP file opens with the imported body. The chamfer feature that you added to the imported body is rebuilt. You did not have to rebuild this feature that you had added to the imported body before selecting Edit Feature.
13-4
Open - Match Faces and Edges of Imported Features The Match faces and edges check box appears in the Open dialog box when you edit the definition of an imported feature. To edit the definition of an imported feature:
1.
Open a file containing an imported feature.
2.
In the FeatureManager design tree, right-click the imported feature, and select Edit Feature. The Open dialog box appears.
3.
Browse to select the edited file to import. The file name appears in the File name box.
4.
5.
Select the Match faces and edges check box. This does the following: •
Propagates the dependencies of the old faces and edges in the old body, such as sketches or features, to the new faces and edges in the new body.
•
Ensures you get the correct results when you open a file that has imported features.
Click Open. The file opens and the imported features are correctly displayed.
Import Diagnosis Use the Diagnosis tool to diagnose and repair gaps and bad faces on imported features. Use the Diagnosis tool when you have: •
An imported solid or surface body that has rebuild errors.
•
An imported surface that was not able to knit into a solid body. If you try to fix gaps but all the gaps cannot be healed, try fixing the faces to fix the gaps.
To view and fix gaps:
1.
Right-click the Imported feature in the FeatureManager design tree and select Diagnosis. The Import Diagnosis PropertyManager appears.
2.
In the PropertyManager, under Gaps, click Diagnose. The PropertyManager reports the number of gaps found.
3.
View and fix the gaps using the View/Close Gaps tools.
4.
Click OK
.
To diagnose and fix or simplify faces:
1.
Right-click the Imported feature in the FeatureManager design tree and select Diagnosis.
2.
In the PropertyManager, under Faces, click Diagnose.
3.
Faces that are faulty or require simplification highlight in the graphics area and appear in the Faces to be
4.
fixed/removed . Move the pointer over a face in the list to display a tooltip that reports the problem with that face.
5.
Click Fix to simplify that face. The diagnosis automatically finds faulty faces and spline curves/surfaces that can be simplified to analytical ones for operations such as sheet metal creation and assembly mating.
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Chapter 13 Import/Export
To simplify entities with a tolerance greater than 1.0e-8 meters and less than 1.0e-5 meters, you must manually select the relevant faces, then click Fix. The example has some plane-like and cylinder-like faces, but they are not in analytical forms. 1.
Select the two faces in the graphics area.
2.
Click Fix. If two faces are meant to be one (for example, the two halves of a cylindrical face), the two faces merge.
The diagnosis performs an in-depth check on all the entities in a model. The number of faults or faulty faces may differ from those found by the more generic Tools, Check command. This detailed check is required to heal the faulty entities. 3.
Click OK
.
If the imported body still shows rebuild error markers even though a body check and the Import Diagnosis PropertyManager report no surface problems, the body is probably valid. Click Rebuild clear the rebuild error markers.
to
Import Diagnosis PropertyManager The Import Diagnosis PropertyManager appears when you import a file, right-click the imported body, and select Diagnosis. The PropertyManager controls the following properties: Gaps •
Diagnose. Checks the imported body for gaps and reports the number of gaps found.
View/Close Gaps •
Next. Views the next gap. An arrow
points to the gap or gap edge in the graphics area.
•
Previous. Views the previously viewed gap.
•
Healing Preview. Zooms in to the next or previous gap and displays a preview of the proposed fix.
•
Accept (Available only when Healing Preview is selected). Accepts the fix for the currently viewed gap. The number of gaps found updates.
•
Close All. Fixes all gaps and updates the number of gaps found.
Faces
13-6
•
Diagnose. Checks the imported body for bad faces. Diagnosis reports the problem and faces under Faces to be fixed/removed.
•
Faces to be fixed/removed . Reports the bad faces found when you click Diagnosis. Hover over the face name for a tooltip that describes the problem with the face. You can manually select faces in the graphics area to add to this list. You can also select multiple faces to merge.
Click the selected face in Faces to be fixed/removed to view normal to that face. Click the selected face in the list again to flip the face 180 degrees and view it from the opposite direction. This is useful when manually fixing faces. •
Fix. Fixes the bad faces.
•
Remove. Removes the bad faces. You can use surface creation functionality to try to create new surfaces to fill gap, then try to knit again.
•
All selected. Fixes all faces listed in Faces to be fixed/removed individually or manually.
. Clear this option to fix faces
General Import Options You can set the general import options when you import IGES, STEP, SAT (ACIS), VDAFS, or Inventor Part files. To set the general import options:
1.
Click Open
or File, Open.
The Open dialog box appears. 2.
Set Files of type to IGES (*.igs,*.iges), STEP AP203/214 (*.step,*.stp), ACIS (*.sat), VDAFS (*.vda), or Inventor Part (*.ipt) , then click Options. The Import Options dialog box appears with General selected on the File Format tab. If you move the pointer over General, a tooltip displays the file formats that the General item controls.
3.
Select from the following options: •
Surface/solid entities. Imports surface and solid entities. You must also select one of the following options: Try forming solid(s). Tries to form solids. Additionally, you can select the following option: • B-REP mapping. Attempts to import the model by directly mapping topologies using boundary representation (BREP) data. In general, this mode is faster than knitting, especially for complex models. If you select the Try forming solid(s) option, but do not select the B-REP mapping option, the SolidWorks application attempts to knit the surfaces into solid(s). o Knit surface(s). Imports as surfaces and attempt to knit the imported surfaces. o Do not knit. Imports as surfaces and prevent surfaces from knitting. Free point/curve entities. Imports free points and free curve entities. You must also select one of the following options: o
•
Import as sketch(es). Imports data as 2D and 3D sketch data. If you want to import free curves, SolidWorks strongly recommends you select this option, for performance reasons. Free points and 2D sketches import as 2D sketches. 2D curves, 3D curves, and 3D sketches import as 3D sketches. o Import as 3D curves. Imports data as 3D curves data. 2D and 3D curves import as curves. Free points and 2D sketches import as 2D sketches. Import multiple bodies as parts (STEP and ACIS files only). Imports a multibody part as an assembly document. The multiple bodies are imported as part documents contained in the assembly. With this option cleared, the multibody part imports as a part document that contains multiple imported bodies. o
•
•
Perform full entity check and repair errors. Checks and repairs errors (default is selected). With this option selected, import performance is slower because the software spends more time checking and repairing the model entities wherever possible. If the quality of the imported data is good, you may not have to select this option.
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Chapter 13 Import/Export
•
Customize curve tolerance. Customizes the tolerance when you import models with very small entities (smallest values on the order of 1.0e-6 to 1.0e-7 meters). With this option cleared, SolidWorks uses internal tolerance settings which are too large to properly import and display these small models. Enter the desired tolerance in the box.
•
Unit. Set the units of measure for the imported file. You must select one of the following options: File specified unit. Use the units of measure from the imported file. Document template specified unit. Use the units specified in the SolidWorks template files under Tools, Options, System Options, Default Templates. IGES - Show IGES levels. Displays the IGES-In Surfaces, Curves, and Levels dialog box if there are curves or different levels (or layers) in the IGES file. o o
• •
STEP - Map configuration data. Applies to STEP files only. Imports STEP file configuration data plus geometric data. Leave this option cleared to import only geometric data.
4.
Click OK to return to the Open dialog box.
5.
Select the file to open, then click Open to import the file as a SolidWorks document.
STL and VRML Import Options You can set the import options when you import STL or VRML files as SolidWorks documents. The VRML translator supports explicit normals, crease angle smooth shading, and color per vertex, which results in smooth blending of colors. To set the STL and VRML import options:
1.
Click Open
or File, Open.
The Open dialog box appears. 2.
Set Files of type to STL (*.stl) or VRML (*.wrl) and click Options. The Import Options dialog box appears with STL/VRML selected on the File Format tab.
3.
Select from the following options: •
Import as o
Graphics Body. Imports data as graphical data only. The translator does not attempt to create any features. The graphics icon
appears in the FeatureManager design tree with the file
type, for example, STL Graphics1. Solid Body. Attempts to import data as solid bodies. In many cases (especially complex models) some of the data does not knit into a usable solid, in which case the translators import that data as surface bodies. Therefore, in the FeatureManager design tree, you can potentially see a Solid Bodies folder, a Surface Bodies folder, imported solid body features, and imported surface body features. o Surface Body. Imports data as surfaces. The Surface Bodies folder and the imported surface body features appear in the FeatureManager design tree. Unit. Select the unit of measure for the SolidWorks document. The available units are Millimeters, Centimeters, Meters, Inches, and Feet. The translator does not convert units during import. For example, if the unit of measure of the original document is meters and you import the document with the unit Millimeters, an edge that measures 1 meter in the original document will measure 1 millimeter in the imported document, not 1000 millimeters. o
•
•
13-8
Import texture information (applies only when you select import as Graphics Body). Imports texture information, which if contained in the file, results in a high-quality, realistic-looking image. Choosing to not import texture information may improve performance.
4.
Click OK to return to the Open dialog box.
5.
Select the file to open, then click Open to import the file as a SolidWorks document.
Exporting Documents and Setting Options When you export a document from the SolidWorks application, you can set the options for the new file you create. The options vary, depending on the type of file. To export a SolidWorks document as another file type:
1.
Select one of the following: •
The face or surface of a part in the graphics area
•
A solid body or surface body from the Solid Bodies FeatureManager design tree
•
The components of an assembly
or Surface Bodies
folder in the
NOTE: If you do not select any entities, the entire part or assembly is exported. 2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to the desired file type, then click Options. The Export Options dialog box appears with the desired file type selected on the File Format tab.
4.
Set the appropriate options for the target file type. See the target file type below for the available options: •
ACIS (*.sat)
•
DXF/DWG (*.dxf, *.dwg)
•
eDrawing (*.eprt, *.easm, or *.edrw)
•
IGES (*.igs)
•
Parasolid (*.x_t, *.x_b)
•
STEP (*.step)
•
STL (*.stl)
•
Tif (*.tif)
•
VDAFS (*.vda)
•
VRML (*.wrl)
5.
In the File name box, type a name. The extension for the selected format is added automatically when you save the document.
6.
Click Save. NOTES: •
If you export an assembly that contains lightweight parts, the Resolve Lightweight Parts dialog box appears. You must resolve any lightweight parts before you can export an assembly.
•
If you export an assembly that contains hidden or suppressed parts, a message box appears asking if you want to resolve these parts. To export these parts, you must resolve them.
•
If you select any faces, surfaces, solid bodies or surface bodies of a part, the Export dialog box appears verifying if you want to export only the selected objects. Click Selected face(s) to export only the selected faces, Selected bodies to export only the selected bodies, or All bodies to export all solid bodies.
ACIS Export Options You can set the export options when you export SolidWorks part or assembly documents as ACIS files. To set the ACIS export options:
1.
Open the SolidWorks document that you want to export as an ACIS file.
2.
Click File, Save As. The Save As dialog box appears.
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Chapter 13 Import/Export
3.
Set Save as type to ACIS (*.sat), then click Options. The Export Options dialog box appears with ACIS selected on the File Format tab.
4.
5.
Select from the following options: •
Solid/Surface geometry. Exports the geometry as all solids and surface bodies.
•
3D curves. Exports the solid and surface bodies as wireframe entities. All 3D curves (composite curves, 3D wires, imported curves, and so on) are also saved.
•
Export sketch entities (available only when you select 3D curves). The Export sketch entities item is available as an option for 3D curves. Select this check box to export all the items in 3D curves, plus all 2D and 3D sketches in the document.
•
Version. Select the type supported by the target system.
•
Units. Select the default units of length to use for ACIS files.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
DXF/DWG Export Options You can set the export options when you export SolidWorks drawing documents as DXF or DWG files. To set the DXF or DWG export options:
1.
Open the SolidWorks drawing document that you want to export as a DXF or DWG file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Dxf (*.dxf) or Dwg (*.dwg), then click Options. The Export Options dialog box appears with DXF/DWG selected on the File Format tab.
4.
5.
Select from the following options: •
Version. Select the type supported by the target system. The SolidWorks DXF and DWG translators support all AutoCAD® versions up to and including AutoCAD 2002.
•
Fonts. Select either TrueType or AutoCAD STANDARD only. If you select AutoCAD STANDARD only, the drawFontMap.txt mapping file is used. See AutoCAD Font Support for details.
•
Line styles. Select AutoCAD Standard Styles to map SolidWorks line fonts to the original AutoCAD stock line types. Line font weight is mapped to the closest AutoCAD line weight value. AutoCAD line weight value mapping is only supported for AutoCAD Version setting R2000 and higher. Select SolidWorks Custom Styles to use the SolidWorks line styles.
•
Custom Map SolidWorks to DXF. Implements mapping. See DXF/DWG Mapping.
•
Don't show mapping on each save. Prevents the SolidWorks To DXF/DWG Mapping dialog box from appearing every time you save a drawing with Custom Map SolidWorks to DXF selected. The map file specified in the Map file box is used.
•
Map file. Select a previously saved map file, or browse to the desired file.
•
1:1 Scale output. Exports the drawing using a model geometry scale of 1:1 and enable the Base scale list. The paper or sheet scale is not normally used when you enable this option.
•
Base scale. Refers to the basis used for the 1:1 scale output of the geometry, based on the various drawing view scales on the sheet. If you have a view selected, the view scale and count values for this selected view appear in the Base scale list. If no view is selected, the view scale with the highest count is displayed by default. Count indicates the number of occurrences of this scale in the drawing document.
Click OK, then click Save to export the document. If you selected the 1:1 Scale output check box, the drawing document is saved with a model geometry scale of 1:1 for the chosen views, with the remainder of the sheet scaled accordingly.
13-10
eDrawings Export Options You can set the export options when you export SolidWorks documents as eDrawing files. To set the eDrawings export options:
1.
Open the SolidWorks document that you want to export as an eDrawing file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to eDrawing (<eDrawing file type>), then click Options. NOTE: The eDrawings translator automatically displays the appropriate eDrawing file type based on the open document: eDrawing (*.edrw) for drawings, eDrawing (*.eprt) for parts, or eDrawing (*.easm) for assemblies. The Export Options dialog box appears with EDRW/EPRT/EASM selected on the File Format tab.
4.
5.
Select from the following options: •
Okay to measure this eDrawing. Select this check box to enable measurement of the geometry in this eDrawing file. Recipients of this eDrawing file can measure the geometry in the eDrawings Viewer.
•
Compress this eDrawing. Select this check box to compress the eDrawing file size. File compression may decrease the quality of some shaded images.
•
Allow export to STL for parts and assemblies. Select this check box to allow recipients of the eDrawing file to save it as an STL file from the eDrawings Viewer.
•
Save shaded data in drawings. For SolidWorks drawings only. Select this check box to save the shaded data from the SolidWorks drawing document in the published eDrawing file.
Click OK, then click Save to export the document.
IGES Export Options You can set the export options when you export SolidWorks part or assembly documents as IGES files. To set the IGES export options:
1.
Open the SolidWorks document that you want to export as an IGES file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to IGES (*.igs), then click Options. The Export Options dialog box appears with IGES 5.3 selected on the File Format tab.
4.
Select from the following options: •
Output as o
o
IGES solid/surface entities. Exports the data as solid or surface entities. Select Trimmed Surface (type 144) to convert the faces of the part, assembly, or the selected surfaces to trimmed surfaces in the IGES file. Select Manifold Solid B-rep Object (type 186) to export boundary representation (BREP) data to the IGES file. IGES Wireframe (3D curves). Converts the solid body to a 3D wireframe representation in the IGES file. Unlike surfaces or faces, you cannot export individually selected model edges to an IGES file. Select either B-Splines (Entity type 126) or Parametric Splines (Entity type 112) depending on the entity types required by the target system. For more information, see the IGES 3D Curves table.
NOTE: If you select both of the above options, the model is exported as both trimmed surfaces and 3D curves.
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Chapter 13 Import/Export
•
Surface representation/System preference. The IGES entity types that compose the trimmed surfaces depend on the export format chosen. The Surface representation table shows the IGES entity types that compose the trimmed surfaces.
•
Export 3D Curve features. Includes 3D curve features in the exported file.
•
Export sketch entities. Includes sketch entities in the exported file. All 2D and 3D sketch entities are included.
•
Use high trim curve accuracy. Exports using high trim curve accuracy; the file size is larger than if the check box is cleared. This setting affects files exported both with Trimmed surfaces and with 3D curves. High trim curve accuracy can sometimes help if the target system has trouble importing the IGES file, or cannot knit the surfaces into a useful solid.
•
IGES assembly structure o
o
• 5.
Save all components of an assembly in one file (assemblies only). Saves all assembly components, sub-assemblies, and sub-assembly components in one file. Otherwise, the assembly components and the sub-assembly components are saved as individual IGES files in the same directory. Flatten assembly hierarchy (assemblies only). Flattens the assembly to one level of only part bodies. A flattened file contains a top-level assembly and a series of parts that contain imported features.
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
Surface Representation Surface Representation
Exported IGES Entity Types
STANDARD
144, 142, 128, 126, 122, 120, 110, 102, 100
NURBS
144, 142, 128, 126, 110, 102, 100
ALIAS
144, 142, 128, 126, 122, 120, 110, 102, 100
ANSYS
144, 142, 128, 126, 110, 102, 100
COSMOS
144, 142, 128, 126, 110, 102, 100
MASTERCAM
144, 142, 128, 126, 110, 102, 100
SURFCAM
144, 142, 128, 126, 110, 102, 100
SMARTCAM
144, 142, 128, 126, 110, 102, 100
TEKSOFT
144, 142, 128, 126, 110, 102, 100
ALPHACAM
144, 142, 128, 126, 110, 102, 100
MULTICAD
144, 142, 128, 126, 110, 102, 100
NOTE: If the system you are exporting to is not listed, refer to the documentation for that system to see which entities are supported, and choose an appropriate setting.
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Parasolid Export Options You can set the export options when you export SolidWorks part or assembly documents as Parasolid files. To set the Parasolid export options:
1.
Open the SolidWorks document that you want to export as a Parasolid file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Parasolid (*.x_t) or Parasolid Binary (*.x_b), then click Options. The Export Options dialog box appears with Parasolid selected on the File Format tab.
4.
5.
Select from the following options: •
Version. Select the type supported by the target system.
•
Flatten assembly hierarchy (assemblies only). Flattens the assembly to one level of only part bodies. A flattened file contains a top-level assembly and a series of parts that contain imported features.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
STEP Export Options You can set the export options when you export SolidWorks part or assembly documents as STEP files. To set the STEP export options:
1.
Open the SolidWorks document that you want to export as a STEP file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to STEP AP203 (*.step) or STEP AP214 (*.step), then click Options. The Export Options dialog box appears with STEP selected on the File Format tab.
4.
Select from the following options: •
Output as o o
o
•
Solid/Surface geometry. Exports the geometry as solids and surface bodies. 3D curves. Exports the solid and surface bodies as wireframe entities. All 3D curves (composite curves, 3D wires, imported curves, and so on) are also saved. Export sketch entities (available only with 3D curves selected). Exports all the items in 3D curves, plus all 2D and 3D sketches in the document.
Set STEP configuration data (available only when exporting to STEP AP203 (*.step) file types). Displays the STEP Configuration Data for Export dialog box. NOTE: If you select 3D curves or Export sketch entities, you can only open the exported STEP files in SolidWorks 2001Plus or later.
• 5.
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document. If you selected Set STEP configuration data, the STEP Configuration Data for Export dialog box appears, as described in step 4. NOTE: Because you cannot group the sketch elements together in a STEP file, when you open the exported STEP file in SolidWorks: •
All lines and splines are imported into a single 3D sketch.
•
Circles, ellipses, and parabolas are imported into individual 2D sketches.
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Chapter 13 Import/Export
STL Export Options You can set the export options when you export SolidWorks part or assembly documents as STL files. To set the STL export options:
1.
Open the SolidWorks document that you want to export as an STL file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to STL (*.stl), then click Options. The Export Options dialog box appears with STL selected on the File Format tab.
4.
Select from the following options: •
Output as o Select either Binary or ASCII as the file format. Binary files are smaller than ASCII files, but they are not supported in some other systems. Select the type supported by the target system. o Unit. Select the unit of measure.
•
Resolution. Controls the tessellation of non-planar surfaces for Stereolithography (STL) output. A lower deviation setting produces a more finely tessellated STL file. Files generated with higher accuracy settings (increased tessellation) are larger in size and slower to generate. o o
Coarse or Fine. Select one of these preset resolutions. Custom. Move the Deviation and Angle slider controls to adjust the resolution or type values for deviation Tolerance and angle Tolerance. If you click Custom: •
Move the Deviation slider to adjust the deviation Tolerance, which controls whole-part tessellation. Lower numbers generate files with greater whole-part accuracy.
•
Move the Angle slider to adjust the angle Tolerance, which controls smaller detail tessellation. Lower numbers generate files with greater small-detail accuracy, but those files take longer to generate. As you move the two sliders, the corresponding concentric circles adjust accordingly. The circles show, approximately, how the tessellation will vary as a result of the settings. (See the Preview option below.)
o
o
5.
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Show STL info before file saving. Displays a SolidWorks dialog box (when you click Save in the Save As dialog box) that contains the following information: Triangles (number), File Size, File Format, and the directory path and file name. Preview. Displays a faceted model preview in the graphics area and display the Triangles (number) and File size information in the Export Options dialog box.
•
Do not translate STL output data to positive space. Makes exported parts maintain their original position in global space, relative to the origin.
•
Save all components of an assembly in a single file (assemblies only). Saves the assembly and each of its components in a single .stl file.
•
Check for interferences (assemblies only). Performs an interference check on an assembly document prior to saving. Export of an assembly with coincident or interfering bodies to a single .stl file produces a file that may be unsuitable for some rapid prototyping systems. It is recommended that you check for interference between the components prior to saving the assembly document. For more information, see Interference Detection.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
TIFF Export Options You can set the export options when you export SolidWorks documents as TIFF files. To set the TIFF export options:
1.
Open the SolidWorks document that you want to export as a TIFF file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Tif (*.tif), then click Options. The Export Options dialog box appears with TIF selected on the File Format tab.
4.
Select from the following options: •
Image type. Select either RGB full color, or Black & white (bilevel) image.
•
Compression scheme. Select the type supported by the target system: o
Uncompressed.
o
Packbits. Results in the smallest color image.
o
•
Capture type. Select either Screen capture or Print capture. o o
5.
Group 4 Fax. Results in the smallest file size of the three formats, but can only be used for a black and white image. Screen capture. Captures the image at the resolution of the screen display. Print capture (drawings only). Enables the options under For drawings. Capture the image at a user-defined DPI (dots per inch) and Paper size. The drawing Width and Height information update automatically. Select the Scale to fit check box to scale the drawing automatically, or set the scale manually in the Scale box.
Click OK, then click Save to export the document.
VRML Export Options You can set the export options when you export SolidWorks part or assembly documents as VRML files. To set the VRML export options:
1.
Open the SolidWorks document that you want to export as a VRML file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to VRML (*.wrl), then click Options. The Export Options dialog box appears with VRML selected on the File Format tab.
4.
Select from the following items: •
Output as o
o
5.
Version. Select the type supported by the target system. VRML 97 is also called VRML version 2.0. Unit. Select the unit of measure.
•
Quality. Advises you that the resolution of the exported VRML file depends on the current display resolution. To change the current display resolution, click Tools, Options, Document Properties, Image Quality and adjust the options.
•
Save all components of the assembly in a single file (assemblies only). Includes each assembly and sub-assembly component in one file.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
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Chapter 13 Import/Export
Exporting Multibody Documents When you export a multibody part document as another file type, you have the option to export selected solid bodies or all solid bodies. To export a multibody part document:
1.
With a multibody part document open, select at least one face or solid body in the graphics area, or one solid body from the Solid Bodies
folder in the FeatureManager design tree, and click Save As.
The Save As dialog box appears. 2.
Set the Save as type to the desired file type and click Save. The Export dialog box appears. NOTE: If you select a solid body, the Selected face(s) option in the Export dialog box is unavailable.
3.
4.
Click one of the following: •
Selected face(s). Exports only the selected faces.
•
Selected bodies. Exports only the selected bodies.
•
All bodies. Exports all solid bodies.
Click OK to export the multibody part document.
Print3D Print3D is a web portal linked to the SolidWorks software. You can contact rapid part and prototype vendors to request price quotes and place orders for the current part document through the Print3D web portal. Print3D automates the prototype request process, eliminating the need to save parts as STL files, FTP parts to vendors, or perform other operations. To access the Print3D web portal:
1.
Open a part document for which you want to get a price quote or place an order.
2.
Click File, Print3D. The Print3D web portal opens in your browser. A list of rapid part and prototype vendors is displayed in the web portal. You can also access the Print3D web portal from the Save As dialog box. Select STL (*.stl) in Save as type and click Try Print3D.
3.
13-16
Click any of the following: •
What is Print3D? Explains the Print3D process and contains basic technical definitions of rapid prototyping processes and materials.
•
Print3D button. Leads you to a web-based quote and order process controlled by the vendor, which may involve a web form or wizard. Follow the on-screen instructions to complete the process.
•
Tell me more. Displays more information about a vendor and its offerings.
File Types ACIS Files (*.sat) The ACIS™ translator supports import and export of body and face colors, curves, and wireframe geometry. You can export the entity attribute information of faces and edges to ACIS files, and this information is retained in the ACIS file. If you import that same ACIS file back into SolidWorks, for entity attribute information of faces, you can select any import options and the faces retain the entity attribute information. However, if you import edges, you must select the B-Rep mapping check box in the Import Options dialog box to retain the entity attribute information for the edges. Import The ACIS translator imports ACIS part or assembly files as SolidWorks part or assembly documents. If the units of length are not explicitly specified in the ACIS file, a dialog box gives you the opportunity to specify the units. Files created with early versions of the ACIS modeler do not contain information about the units of length. The default import mode is knitting. SolidWorks supports import of generic named attributes (integer, position, real, string, and vector) associated with bodies and faces from ACIS (.sat) files. These attributes are displayed as features in the FeatureManager design tree. Their values are accessible only through the SolidWorks Application Programming Interface (API). Export The ACIS translator exports SolidWorks part or assembly documents as ACIS files. When you export parts, you can export faces or bodies as separate ACIS files. You can select to export individual parts or subassemblies from an assembly tree, limiting export to only those parts or subassemblies. If you select a subassembly, all of its components are automatically selected. The ACIS translator does not support assembly hierarchy. Version Information The ACIS translator supports all SAT versions up to and including version 8.0.
Autodesk Inventor Files The Inventor Part translator imports Autodesk Inventor® part files as SolidWorks part documents. The imported part files contain only geometry; features are not imported. The Inventor Part translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box. To open an Autodesk Inventor part:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to Inventor Part (*.ipt) and click Options. The Import Options dialog box appears with General selected on the File Format tab.
3.
Set the import options, then browse to the desired file and click Open.
Version Information The Inventor translator supports all Autodesk Inventor versions up to and including Autodesk Inventor 5.3.
CADKEY Files The CADKEY® translator imports CADKEY part and assembly files as SolidWorks part or assembly documents. All CADKEY files have the same .prt file extension. The CADKEY translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box.
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Chapter 13 Import/Export
To open a CADKEY file:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to CADKEY (*.prt).
3.
Browse to the desired file, and click Open.
Version Information The CADKEY translator supports import of surface or solid entities from CADKEY version 19 part or assembly files.
CATIA Graphics Files The CATIA® Graphics (CGR) translator is integrated into the SolidWorks software and is always available as a file type in the Open and Save As dialog boxes. Import The CATIA Graphics translator imports CGR files as SolidWorks part documents. CGR files contain only graphical information and are for viewing only. System Requirements: Windows NT® or Windows 2000 or above. To open a CGR file in SolidWorks:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to Catia Graphics (*.cgr).
3.
Browse to the desired file and click Open.
Export The CATIA Graphics translator exports SolidWorks part or assembly documents as CATIA graphics files that users can view in CATIA, CATweb, and DMU Navigator. To export a SolidWorks document as a CGR file:
1.
With a SolidWorks part or assembly document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to Catia Graphics (*.cgr).
3.
Type the file name in the File name box, and click Save.
Version Information The CATIA Graphics translator supports CATIA version 5, release 1 through release 9.
DXF 3D Files The DXF 3D translator extracts ACIS information from a DXF file, if that information exists in the file, and imports it into a SolidWorks part document. If a DXF file contains multiple bodies or an assembly, SolidWorks creates an assembly document. Note the following translator limitations: •
It is not a 2D to 3D converter.
•
It does not import 2D or wireframe data from DXF files.
The DXF 3D translator is integrated into the DXF/DWG translator in the SolidWorks software and is always available when you select DXF (*.dxf) under Files of type in the Open dialog box.
13-18
To open a DXF 3D part:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to DXF (*.dxf).
3.
Browse to the desired file, and click Open. The Conversion Unit dialog box appears.
4.
Select the unit in which the original model was created, or click Other and type the scale in the Unit Scale box.
5.
Click OK.
Version Information The DXF 3D translator supports DXF 3D files including, but not limited to, versions AutoCAD® R14 and above.
DXF/DWG Files (*.dxf, *.dwg) Bitmaps stored in DXF/DWG files in AutoCAD®'s native bitmap format are not supported. You can copy and paste entities from an AutoCAD DXF or DWG file into SolidWorks part, assembly, and drawing documents. You can insert DXF or DWG files directly into the current SolidWorks part or drawing document with the Insert, DXF/DWG tool. The menu item activates the DXF/DWG Import Wizard at the appropriate dialog box, with simplified options to help you insert these files. The DXF/DWG translator supports the import and export of hole tables. Import The DXF/DWG translator imports DXF or DWG files, including Mechanical Desktop files, as SolidWorks part or drawing documents, according to the option settings in the DXF/DWG Import Wizard. This translator also imports DXF 3D files without the wizard. In a drawing document, you can import the geometry to the drawing sheet or the drawing sheet format. Entities in either paper space or model space are imported. When you import drawings, the most popular AutoCAD SHX or True Type fonts are supported, even though you may not have the fonts installed. See AutoCAD Font Support. If you import a DXF or DWG file that contains a large number of blocks (more than 200), you are prompted to enable the Explode Blocks option. Explode the blocks to improve import performance. The DXF/DWG translator imports: •
AutoCAD Mechanical annotations, known as proxy entities, (such as surface finish symbols or GTOL frames) and automatically drawn objects (such as cams and springs) when you import DXF or DWG files as SolidWorks drawing documents. The translator converts these imported items to equivalent SolidWorks objects, or creates them as blocks of primitive geometry, as appropriate.
•
Associative and non-associative crosshatches as area hatches.
•
XREFs in AutoCAD DWG files.
•
DWG files with multiple sheets.
When you import DWG files, you can now see a thumbnail image of the file in the Preview panel of the Open dialog box. Previews appear for DWG files created by both SolidWorks and AutoCAD. In AutoCAD, the bitmap preview option must be enabled when the file is last saved. The Open dialog box remembers the Preview check box state from the last time you opened a DWG file. The SolidWorks software fully supports the import of AutoCAD block definitions and instances with properties and attributes. When you import AutoCAD DWG files saved in paper space (layout mode) as SolidWorks drawing documents, the DXF/DWG Import Wizard converts each AutoCAD viewport into a separate SolidWorks drawing view. Drawing view data is selectable if you activate the drawing view.
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Chapter 13 Import/Export
Data that does not belong to a viewport is imported to the drawing sheet. Drawing sheet data is selectable if you activate the drawing sheet. If Dynamic drawing view activation is enabled, you must lock sheet focus to select drawing sheet data. The DXF/DWG translator alerts you to problems encountered when importing a DXF or DWG file. To import an AutoCAD 2004 DXF or DWG file, you must save the file in AutoCAD 2004 as "AutoCAD 2000/ LT2000." SolidWorks warns you if you try to import AutoCAD 2004 DXF or DWG files that are not saved in this format. You can import entire DWG sheets as view only SolidWorks drawing sheets, which allows the direct display of the original DWG entities inside SolidWorks drawing documents. You can view, pan, zoom, and print these sheets. Select View only in the DWG Import - Drawing Layer Mapping dialog box to import DWG sheets as view only sheets. Export The DXF/DWG translator exports only drawing documents as .dxf or .dwg files. When you export a drawing as a .dxf or .dwg file, the drawing's sheet scale is used for the new file. All entities (such as edges, annotations, and assembly components) on layers are exported to the assigned layer. SolidWorks crosshatch patterns are translated into AutoCAD hatch patterns when you export SolidWorks documents as DXF or DWG files. The SolidWorks software translates the SolidWorks crosshatch patterns as non-associative hatch definitions, and preserves the layer and color of the original crosshatch. The SolidWorks application also supports crosshatch export when you map layers with a mapping file. You have the option to map only those items whose layers are not otherwise defined when you export SolidWorks drawing documents as DXF or DWG files. All entity types that you can assign to AutoCAD layers through the mapping file support layering in the SolidWorks drawing format. The DXF/DWG translator supports line thickness, hidden sketches, and auto-centerlines. Version Information The DXF/DWG translator supports importing and exporting of OLE objects through DXF/DWG files of version 13 and higher. DXF/DWG View Only You can import entire DWG sheets as view only SolidWorks drawing sheets, which allows the direct display and printing of the original DWG entities inside SolidWorks drawing documents. You can view, pan, zoom, and print these sheets. Only view-related controls are available. The View only functionality improves import and viewing performance. If you have a large schematic drawing to include as a reference in a SolidWorks drawing document, View only eliminates the need to convert the schematic drawing document entities. When you print the SolidWorks drawing, the printed document contains all the items from the view only sheet. When you open a SolidWorks drawing document that contains view only DWG data, the DXF/DWG View Only PropertyManager appears and (VIEW ONLY) appears in the SolidWorks title bar. To import a DWG file as view only:
1.
Open a DWG file. The DXF/DWG Import Wizard appears.
2.
3.
In the DXF/DWG Import - Drawing Layer Mapping dialog box: a.
Select Import to drawing.
b.
Select View only to import the current sheet only, or View only all to import all sheets in the DWG file.
Click Next to set options in the DXF/DWG Import - Document Settings dialog box, or click Finish to accept all settings and import the DWG file. The DWG file opens and the DXF/DWG View Only PropertyManager appears.
13-20
4.
Set the values in the PropertyManager to manage link references. Use the PropertyManager to enable and manage the external reference between the view only sheet and its source DWG file.
5.
Click OK
.
DXF/DWG View Only PropertyManager The DXF/DWG View Only PropertyManager appears when you import a DWG file as a drawing and select View only or View only all in the DWG Import - Drawings Layer Mapping dialog box. The PropertyManager controls the following properties: Link to. Enables linking of the view only sheet in the SolidWorks drawing document (*.slddrw) to its source DWG file. When you select this option, if the DWG source file has been modified since the *.slddrw file was created, the view only sheet appearance updates accordingly. Folder. Displays the path to the linked source DWG file. . Click to browse to a new DWG file to display as view only. The path is displayed in the Folder box. Update. Click to manually update the link and the view only display after you browse to the source DWG file in the Folder box. Inserting DXF/DWG Files You can insert DXF or DWG files directly into the current SolidWorks drawing or part document with the Insert, DXF/DWG tool. The menu item activates the DXF/DWG Import Wizard at the appropriate dialog box, with simplified options to help you insert these files. When you insert DXF or DWG files into SolidWorks drawing documents, the SolidWorks software inserts a new sketch on the current sheet. When you insert DXF or DWG files into SolidWorks part documents, the SolidWorks software inserts a new sketch, and the software prompts you to select a plane or face for the sketch if you have not selected one. For example, you can insert a DXF file as a sketch into a SolidWorks part document, then use the inserted sketch to modify the part. To insert a DXF file into a SolidWorks part document:
1.
Open the SolidWorks part document into which you want to insert a DXF file.
2.
Select a face on the part. NOTE: The file is inserted as a sketch onto the face or plane you select.
3.
Click Insert, DXF/DWG. The Open dialog box appears.
4.
Open the DXF file you want to insert. The DXF/DWG Import Wizard opens to the Part Document Options dialog box, with the appropriate options selected.
5.
Click Finish to accept the default settings.
The DXF file entities are inserted into the SolidWorks part document as a sketch on the selected face. Now you can use the inserted sketch to modify the part. 6.
Click Extruded Cut
SolidWorks 2004 Reference Guide
on the Features toolbar, or Insert, Cut, Extrude.
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Chapter 13 Import/Export
7.
8.
Under Direction1, do the following: •
Set End Condition to Through All.
•
Select the Flip side to cut check box, if necessary, to make sure you create the desired part.
Click OK
.
The imported DXF sketch creates the cut on the SolidWorks part, resulting in the finished part document. Copying and Pasting from AutoCAD to SolidWorks You can copy and paste entities from an AutoCAD DXF or DWG file into SolidWorks part, assembly, and drawing documents. In the SolidWorks drawing document, the lines, arcs, notes, annotations, and so forth that you paste are attached to either a drawing view or the sheet, whichever is active. The pasted entities inherit scaling, grouping, visibility, and other properties from the drawing view or sheet. In SolidWorks part and assembly files, you must select a planar face onto which you paste the entities as a sketch. To copy and paste entities from AutoCAD to a SolidWorks drawing document:
1.
In AutoCAD, open a DXF or DWG file. This example shows a DWG file. Select the entities inside the box, then click Edit, Copy.
2.
In SolidWorks, open the SolidWorks drawing document into which you want to paste the entities. Click inside the sheet in the graphics area where you want to paste the entities.
3.
Click Edit, Paste to paste the entities onto the active sheet.
AutoCAD file entities
AutoCAD file entities pasted into SolidWorks document
Imported DXF/DWG Entities Entities that are imported from a .dxf or .dwg file can appear to be dimensioned and to be related to one another. To actually add the dimensions and relations, you must attach the dimensions and constrain all of the entities. You can then create a sketch in a part or assembly from the imported entities. Attach Dimensions You can attach the dimensions to the nearest reasonable sketch entities all at once. To attach dimensions:
With an imported .dxf or .dwg drawing document active, click Tools, Dimensions, Attach Dimensions.
13-22
Constrain All You can set relations on the sketch entities of an unconstrained imported .dxf or .dwg file. To solve relations in an imported drawing:
Click Tools, Relations, Constrain All. The SolidWorks software adds all the apparent relations and reports the number of relations that are added. Sketch from Drawing You can transfer entities from a drawing to an open sketch in a part or assembly. To insert sketch entities from a drawing:
1.
Open a sketch in a part or assembly.
2.
Click Insert, Customize Menu, and select Sketch from Drawing to activate this menu item.
3.
Click Insert, Sketch from Drawing.
4.
Make your drawing the active window and drag-select the sketch entities. The sketch entities must lie entirely within the drawing view border.
5.
Make your part or assembly the active window, and notice the sketch entities have been inserted into the open sketch.
DXF/DWG Mapping You can map selected SolidWorks entities or colors to different layers or colors in a .dxf or .dwg file. You create map files in the SolidWorks software to assign selected items to designated layers or colors in the .dxf or .dwg file. To create a map file:
1.
Open the SolidWorks drawing document for which you want to create a map file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Dxf (*.dxf) or Dwg (*.dwg), then click Options. The Export Options dialog box appears with DXF/DWG selected on the File Format tab.
4.
5.
Do the following: a.
Select the Custom Map SolidWorks to DXF check box.
b.
Click to clear the Don’t show mapping on each save check box.
c.
Click OK to close the Export Options dialog box.
Type a name for the drawing file in the File name box, then click Save. The SolidWorks To DXF/DWG Mapping dialog box appears.
6.
Define the layers then map the entities, or map the colors you want to map in the .dxf or .dwg file. Select the Keep existing SolidWorks drawing layers for entities check box to apply the mapping file settings only to those entities whose layers are not defined and to preserve existing SolidWorks drawing file layers in the exported file. If you do not select this option, the mapping file definitions overwrite all of the current SolidWorks drawing file layers.
7.
Click OK to save the SolidWorks drawing with mapping applied to the document.
See also Define Layers, Map Entities, or Color Mapping. To save a map file:
1.
Click Map File Settings in the SolidWorks To DXF/DWG Mapping dialog box. The Map File Settings dialog box appears.
2.
Select the Save map file check box, and clear the Load map file check box.
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Chapter 13 Import/Export
3.
Type a path and name for a new map file in the box, or browse to an existing file.
4.
Click OK.
To use a previously saved map file:
1.
Click Map File Settings in the SolidWorks To DXF/DWG Mapping dialog box. The Map File Settings dialog box appears.
2.
Select the Load map file check box, and clear the Save map file check box.
3.
Browse to an existing file, and click OK. NOTE: Previously saved map files can contain information for each of the mapping tabs. Review all tabs prior to saving the SolidWorks drawing document.
eDrawings eDrawings lets you animate and view models and drawings. It also allows you to create a document convenient for sending to others. Two tools are available on the eDrawings 2004 toolbar: •
Animate an eDrawing 2004 . Also available by clicking View, Modify, Animate. Begins continuous animation of the model in shaded mode. To stop the animation, click the Animate an eDrawing 2004 tool again, or click View, Modify, Animate again.
•
Publish an eDrawing 2004 . Also available by clicking File, Publish eDrawing 2004. Opens the eDrawings Viewer, which has tools for viewing, shading, animating, hyperlinking, and arranging drawing views. NOTE: If the eDrawings 2004 toolbar is not visible, click View, Toolbars, eDrawings 2004.
You can: •
Create eDrawing files from SolidWorks part, assembly, and drawing documents.
•
Open SolidWorks documents in the eDrawings Viewer.
•
Save eDrawing data to SolidWorks documents in the eDrawings Viewer.
You can view any SolidWorks document from SolidWorks 97Plus and later. If the document does not contain eDrawings data, in the SolidWorks application: •
Select Save eDrawings data in SolidWorks document in Tools, Options, System Options, General before you save the document -or-
•
Select Save eDrawing data in the Save As dialog box
Saving the eDrawings data in the SolidWorks document enables functionality in the eDrawings Viewer, such as: •
13-24
Configurations o
Component names in the Component tree
o
Multiple configurations (only the last saved configuration is visible)
•
Explode in assembly documents
•
Hole information for Measure
•
Hyperlinks in drawing views
•
Mass properties
•
OLE objects
•
Shaded information and animation in drawing documents
To save a SolidWorks document as an eDrawing file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
In the Save as type list, select one of the following: •
eDrawing (*.eprt). Part documents.
•
eDrawing (*.easm). Assembly documents.
•
eDrawing (*.edrw). Drawing documents. NOTE: SolidWorks displays the correct eDrawing file type based on the SolidWorks document type.
3.
Click Save to create the eDrawing file.
eDrawings Professional With the optional eDrawings Professional tools, you can: •
Mark up files
•
View cross sections
•
Measure dimensions
•
Move assembly components
•
View exploded views
•
Display mass properties
For more information, click Help, eDrawings Help Topics in the eDrawings Viewer, or visit the web site at www.solidworks.com/edrawings.
Saving Drawing Sheets in eDrawing Files If a SolidWorks drawing document has multiple sheets, when you publish an eDrawing file, you can select which sheets to save to the eDrawing file. If you publish multiple sheets, the file size and the time required to save the eDrawing file may increase. NOTES: •
You must have eDrawings Professional installed to choose the sheets to save. If you have the free eDrawings Viewer, all the sheets are published with the eDrawing file.
•
You must select the eDrawings2004 check box under Tools, Add-Ins to display the eDrawings toolbar and to publish eDrawing files.
To save sheets when you publish eDrawing files:
1.
Open the SolidWorks document containing multiple sheets that you want to publish as an eDrawing file.
2.
Click Publish an eDrawing 2004
on the eDrawings toolbar, or click File, Publish eDrawing 2004.
The Sheets to Save to eDrawing dialog box appears. 3.
4.
Select one of the following: • Current sheet. Save the current sheet only. •
All sheets. Save all sheets.
•
Selected sheets. Select the sheets to save from the list displayed below.
Click OK to publish the eDrawing file. A progress bar reports the publication process. The eDrawings Viewer opens and lists the selected sheets on the Sheets tab in the eDrawing Manager
5.
To display a different sheet in the graphics area, double-click the sheet on the Sheets tab, or click the tab with the sheet name below the graphics area.
6.
In the eDrawings Viewer, click Save
SolidWorks 2004 Reference Guide
to save the eDrawing file with the sheets.
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Chapter 13 Import/Export
Saving Configurations in eDrawing Files If a SolidWorks part or assembly document has multiple configurations, when you publish an eDrawing file, you can select which configurations to save to the eDrawing file. If you publish multiple configurations, the file size and the time required to save the eDrawing file may increase. NOTES: •
You must have eDrawings Professional installed to choose the configurations to save. If you have the free eDrawings Viewer, only the active configuration is published with the eDrawing file.
•
You must select the eDrawings2004 check box under Tools, Add-Ins to display the eDrawings toolbar and to publish eDrawing files.
To save configurations when you publish eDrawing files:
1.
Open the SolidWorks document containing multiple configurations that you want to publish as an eDrawing file.
2.
Click Publish an eDrawing 2004
on the eDrawings toolbar, or File, Publish eDrawing 2004.
The Configurations to Save to eDrawing dialog box appears. 3.
4.
Select one of the following: •
Current configuration (default). Save the current configuration only.
•
All configurations. Save all configurations.
•
Selected configurations. Select the configurations to save from the list displayed below.
Click OK to publish the eDrawing file. A progress bar reports the publication process. The eDrawings Viewer opens with images of the saved configurations displayed on the Configurations tab. You can click the images to display the different configurations.
5.
In the eDrawings Viewer, click Save
to save the eDrawing file with the configurations.
Highly Compressed Graphics Files The Highly Compressed Graphics (HCG) translator exports SolidWorks documents as Highly Compressed Graphics files. HCG files, used by CATIA® in CATweb, are optimized for transmission over the Web. You can export only parts and assemblies with the HCG translator. The exported files contain graphical information only; you cannot edit these files. The HCG translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as an HCG file:
1.
With a SolidWorks part or assembly document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to HCG (*.hcg).
3.
Type the file name in the File name box, and click Save.
Version Information The HCG translator exports SolidWorks documents as CATIA version 5, release 9 files.
13-26
HOOPS Files The HOOPS translator exports SolidWorks part or assembly documents as HOOPS (.hsf) files. HOOPS files are streaming graphics files that download details piece by piece to a web page, which is helpful when you display large files. You can view HOOPS files over the Internet using the HOOPS viewer. See www.hoops3d.com for information about the HOOPS viewer. NOTE: The exported files contain graphical information only; you cannot edit these files. The HOOPS translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as a HOOPS file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to HOOPS HSF (*.hsf).
3.
Type the file name in the File name box, and click Save.
Version Information The HOOPS translator exports SolidWorks documents as HOOPS version 8.0 files.
IGES Files (*.igs, *.iges) The following IGES entity types are supported for import and export, except where noted. The IGES translator can import and export IGES surfaces and BREP solids. The IGES error file information is merged into the IGES report file (.rpt). Import If there is wireframe geometry in an imported file, the software reads the IGES data and forms curves for the IGES wireframe entities. The 2D geometry is imported into a sketch rather than imported as reference curves. If you want the software to try to form a solid from imported IGES data, export the solid or surfaces from the source system as trimmed surfaces (Entity type 144) or as untrimmed surfaces (Entity types 128, 122, 120, 118, 114). Also, set the number of significant digits (precision) as high as possible to ensure accurate translation. You can import 3D curves in an IGES file as 3D sketch entities. In the Import Options dialog box, select the Free point/curve entities check box and click Import as sketch(es). The IGES translator supports colors when you import curves. You can select the levels to import for IGES files that contain multiple levels. Select the Show IGES levels option in the Import Options dialog box to display the IGES-In Surfaces, Curves, and Levels dialog box. Export The IGES translator exports SolidWorks part and assembly documents as IGES files. Parts and surfaces exported to IGES format retain their part or surface color, and are displayed in color when in Shaded mode. You can export both surfaces and solids in the same IGES file. If you export a SolidWorks assembly document that has hidden or suppressed components to IGES format, a dialog box appears asking if you want to resolve these components. •
Click Yes, and all the components, including the hidden or suppressed ones, are exported.
•
Click No, and the hidden or suppressed components are not exported.
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Chapter 13 Import/Export
IGES Entity Types
13-28
IGES Entity Type
Entity Name
514
Shell Entity
510
Face Entity
508
Loop Entity
504
Edge Entity
502
Vertex Entity
416
External reference entity
408
Singular subfigure instance entity
406 Form 12
External reference file
402 Form 7
Group entity
314
Color definition entity
308
Subfigure definition entity
198
Toroidal Surface
196
Spherical Surface
194
Right Circular Conical Surface
192
Right Circular Cylindrical Surface
190
Plane Surface
186
Manifold Solid B-Rep Object Entity
144
Trimmed (parametric) surface
143 Import only
Bounded Surface
142
Curve on a parametric surface
140 Import only
Offset surface
128
Rational B-spline surface
126
Rational B-spline curve
124
Transformation matrix entity
123
Direction entity
122
Tabulated cylinder
120
Surface of revolution
118 Import only
Ruled surface
116
Point
114 Import only
Parametric spline surface
112
Parametric spline curve
110
Line
108
Plane
106 form 12 Import only
Copious Data—3D Piecewise linear curve
106 form 11 Import only
Copious Data—2D Piecewise linear curve
104 Import only
Conic arc
102
Composite curve
100
Circular arc
IGES Levels If there are curves in the IGES file or if there are different levels (or layers) in the IGES file, the IGES-In Surfaces, Curves, and Levels dialog box appears. Levels are sometimes used by other systems to separate assembly components or to separate IGES entity types. To select the desired entities and levels:
1.
Select Include surfaces to import any surfaces in the file, if applicable.
2.
Select Include curves to import any curves in the file, if applicable.
3.
Select the levels to include:
4.
•
Include all levels. All levels are imported to level zero.
•
Include levels. Only the specified levels are imported to level zero.
Click OK to exit the IGES-In Surfaces, Curves, and Levels dialog box or click Cancel to abort the import process.
IGES 3D Curves Type of 3D Curve
Exported IGES Entity Types
B-splines (entity 126)
126, 110, 102*, 100
Parametric splines (entity 112)
112, 110, 102*, 100
JPEG Files The JPEG translator takes a snapshot of anything displayed in the graphics window of a SolidWorks part, assembly, or drawing document, and exports it as a .jpg file. A .jpg file is an image file that you can open in most image viewers. The .jpg file displays only the information from the graphics window; toolbars and other areas of the SolidWorks window do not appear. The JPEG translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as a JPEG file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to JPEG (*.jpg).
3.
Type the file name in the File name box, and click Save.
Mechanical Desktop Files The MDT translator imports part and assembly information from Mechanical Desktop® (MDT) files as SolidWorks part or assembly documents. You must have MDT installed on your desktop, but it does not have to be running, to use the MDT translator. NOTE: If you import large assemblies from MDT, SolidWorks recommends you do the following: •
Start Mechanical Desktop and open the MDT file inside the MDT application before you import the file into the SolidWorks application.
•
Set the MDT temporary files path to a drive where you have sufficient space (1GB minimum).
•
Increase the paging file size to appropriate limits. This is relevant mainly for low configuration systems.
MDT files can contain a combination of part, assembly, and drawing files. The MDT translator provides different conversion options, depending upon the contents of the MDT file. The MDT translator supports import of MDT assembly relations.
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Chapter 13 Import/Export
The MDT translator supports the following items during import: •
Large MDT assembly files, in excess of 130MB in size, depending on the complexity of the data.
•
All types of mates, including point-to-point and line-to-line mates
•
MDT combined features, which are sometimes referred to as toolbodies
•
MDT tapped hole features (cosmetic thread annotation)
•
MDT design tables (Design Variable Tables - Global Variable Sheets)
•
MDT Work Features (Work Planes, Work Axes, and Work Points)
•
MDT pattern features, which creates multiple disjoint bodies
The MDT translator is integrated into the DXF/DWG translator in the SolidWorks software, and is always available when you select DXF (*.dxf) or DWG (*.dwg) under Files of type in the Open dialog box. Version Information The MDT translator supports the following MDT versions: •
MDT4.0 or higher (MDT4.0 with Windows 2000 or Windows® XP is not supported)
•
MDT5.0 only with Windows 98, Windows 2000, or Windows NT (Windows 98 must have MDT5.0 Service Pack 1 or later)
•
MDT 6.0 only with Windows® 98, Windows® 2000, Windows® Me, Windows NT® 4.0 (with Service Pack 5 or later), or Windows® XP Professional.
To open an MDT file:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to DXF (*.dxf) or DWG (*.dwg).
3.
Browse to the desired file, and click Open. The MDT File Import dialog box appears. NOTE: If you do not have Mechanical Desktop installed, the DXF/DWG Import Wizard appears instead of the MDT File Import dialog box.
4.
Do one of the following: •
To import the MDT file as a part document using the MDT translator: 1.
Click Import as a part with MDT translator, then click OK. The DXF/DWG Import - Document Settings dialog box appears with the most appropriate options automatically selected. You can change the options if desired.
2.
Select from the following options: •
Units of imported data. Select the unit in which the imported model was created.
•
MDT Options, Component Import Options. Click one of the following options: o o
•
Use Geometry Import. Imports one solid part that you cannot directly edit.
MDT Options, If file with the same name exists. Click one of the following options: o
13-30
Use Feature Import. Imports individual features that you can edit.
Use existing. Uses the existing SolidWorks file and does not import the new part or assembly file.
o
Overwrite. Overwrites the existing SolidWorks file.
o
Save with new name. Prompts you to save the file with a new name.
3.
Adjust the following Preview box options to change the preview displayed as desired: •
4.
Select from the following viewing options: o
Previous view
o
Zoom to Fit
o
Rotate
o
Select a view from the pulldown menu
, Zoom to Area
, Zoom In/Out
, Pan
•
White background. Select this check box to display the model with a white background color.
•
Import this sheet. Select this check box to import drawing views.
•
Model tab. Select this tab to display the part data of the imported model. This tab is selected by default when you import MDT files as parts.
Click Finish to import the MDT file as a part document. The Mechanical Desktop to SolidWorks Converter dialog box reports on the conversion process. The MDT translator imports the MDT file as a SolidWorks document.
•
To import the MDT file as a drawing document using the DXF/DWG translator (MDT does not need to be installed in this case): 1.
Click Import as a drawing with the DXF/DWG translator, then click OK. The DXF/DWG Import - Drawing Layer Mapping dialog box appears with the most appropriate options automatically selected. You can change the options if desired.
2.
Select from the following options: •
Import to drawing. Imports the MDT file as a drawing and creates two sheets, one with the model outline and another with the drawing data. This option is selected by default when you import MDT files as drawings.
•
Import to part. Imports the MDT file as a part, creating one part with 3D solid data and a sheet.
•
Show Layers. Select one of the following options: o
o
o
All selected layers. Shows all the layers being imported to either the drawing sheet or the sheet format. If a layer is not selected, the entities on that layer are ignored for import and not included in the drawing, as shown in the preview image. Layers selected for drawing sheet. Shows the subset of layers whose entities are imported to the drawing sheet. Layers selected for sheet format. Shows the subset of layers whose entities are imported to the sheet format. Drawing sheet layers and sheet format layers are mutually exclusive; entities cannot be directed to both the drawing sheet and the sheet format at the same time.
NOTES:
3.
•
The layers themselves are always present in the resulting drawing. Depending on the option you selected, the layer entities may be ignored, and the initial status of the layer may be off.
•
These options allow you to direct or redirect entities by layer to either the drawing sheet or the sheet format, or to completely block out the entities of a specific layer.
Adjust the following Preview box options to change the preview displayed as desired: •
SolidWorks 2004 Reference Guide
Select from the following viewing options:
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Chapter 13 Import/Export
4.
o
Previous view
o
Zoom to Fit
o
Rotate
o
Select a standard view from the pulldown menu
, Zoom to Area
, Zoom In/Out
, Pan
•
White background. Select this check box to display the model with a white background color.
•
Import this sheet as. This check box is selected by default when you import MDT files as drawings. The name of the selected sheet appears in the box to the right. You can rename the sheets you import and the new names appear in the new SolidWorks document.
•
Model tab. Select this tab to display a preview of the model space from the imported model. This tab is selected by default when you import MDT files as drawings.
•
Layout tab. Select this tab to display a preview of the drawing layout and to display the tab name in the box next to Import this sheet as. The tabs match the tabs shown when you have the DXF or DWG file open inside the AutoCAD application.
Do one of the following: •
Click Finish to accept the remaining default options and import the MDT file as a part document.
•
Click Next to set the document settings. The DXF/DWG Import - Document Settings dialog box appears.
5.
Set the following options: •
Input file properties. Set the Data units. You can set the units to Angstroms (1.0e-10 meters), Nanometers (1.0e-9 meters), Microns (1.0e-6 meters), Microinches (1.0e-6 inches), or Mils (1.0e-3 inches), in addition to the standard Feet, Inches, and Meters units.
•
Output file properties. Set the following options: o
o
Width. Sets the width of the drawing sheet.
o
Height. Sets the height of the drawing sheet.
o
Geometry scaling. Sets the scale for the imported drawing. The default is 1:1.
•
Geometry positioning. Sets the position of the geometry on the sheet. Click one of the following:
o o
13-32
Document template. Sets a document template for the imported entities. If Paper size, Width, and Height are specified in the sheet format of the template, these settings update accordingly. This template information is saved in the registry for DXF files, and used in future DXF file imports, unless you change the template.
•
o
6.
Paper size. Sets the drawing sheet size. Select User Defined to specify the Width and Height.
Move entities onto the sheet. Moves the lower left corner of the imported drawing to the origin of the SolidWorks drawing sheet. Center in sheet. Centers the imported drawing in the drawing sheet. Position (default). Specifies where to place the origin position of the imported drawing on the SolidWorks drawing sheet. Input X and Y coordinates to place the origin of the imported drawing.
Click Finish to import the MDT file as a drawing document.
Parasolid Files (*.x_t, *.x_b) •
Data exported to or imported from Parasolid format retains its color when displayed in Shaded mode.
•
Component names in assemblies are retained for both import and export.
•
The Parasolid translator does not support the import or export of point data.
•
The Parasolid translator supports import and export of curves and wireframes.
Import •
The Parasolid translator imports Parasolid text files or binary files as SolidWorks documents.
•
The Parasolid translator imports files with the extension .x_t, .x_b, .xmt_txt, or .xmt_bin.
Export The Parasolid translator exports SolidWorks part or assembly documents as Parasolid text files or binary files. Binary files are smaller than text files, but binary files are not supported in some target applications. Select the type supported by the target application. If you export a SolidWorks assembly document that has hidden or suppressed components to a Parasolid text or binary file, a dialog box appears asking if you want to resolve these components. •
Click Yes, and all the components, including the hidden or suppressed ones, are exported.
•
Click No, and the hidden or suppressed components are not exported.
Version Information The Parasolid translator supports all Parasolid versions up to and including version 15.0.
PDF Files This add-in module exports SolidWorks part, assembly, and drawing documents as Portable Document Format (PDF) files. Save as PDF is not available on Windows® Me. To deactivate or reactivate the PDF translator:
1.
Click Tools, Add-Ins.
2.
Select or clear Save As PDF.
To export a SolidWorks document as a PDF file:
1.
With a SolidWorks document open, click File, Save As.
2.
In the dialog box, select PDF (*.pdf) in Save as type.
3.
Type the file name File name, and click Save.
Pro/ENGINEER Files The Pro/ENGINEER translator imports Pro/ENGINEER® files into SolidWorks and exports SolidWorks documents as Pro/ENGINEER files. The Pro/ENGINEER translator is integrated into the SolidWorks software and is always available as a file type in the Open and Save As dialog boxes. NOTE: Pro/ENGINEER accepts only ASCII characters in its file names. When you save a SolidWorks document as a Pro/ENGINEER file, any non-ASCII characters are replaced by an underscore (_).
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Chapter 13 Import/Export
Importing Pro/ENGINEER Files into SolidWorks The Pro/ENGINEER translator imports Pro/ENGINEER part or assembly files as SolidWorks part or assembly documents. The attributes, features, sketches, and dimensions of the Pro/ENGINEER part are imported. If all of the features in the file are not supported, you can choose to import the file as either a solid body or a surface model. The Pro/ENGINEER translator supports import of free curves, wireframes, and surface data. When importing an assembly, you can control how to import individual components. Sub-assemblies are supported as well. You can import Pro/ENGINEER surface-trim and surface-extend features into SolidWorks. These features are read in from the Pro/ENGINEER file and mapped to SolidWorks. Some known limitations are as follows: •
Version Information - Versions 17 through 2001 of Pro/ENGINEER are supported. Pro/ENGINEER Wildfire™ files are not supported.
•
Assembly features are not supported.
Exporting SolidWorks Documents as Pro/ENGINEER Files The Pro/ENGINEER translator exports part or assembly documents as Pro/ENGINEER part or assembly files. Version Information - The exported files are saved as Pro/ENGINEER version 20 files. More Information Click the links below for details about these topics: •
Importing Pro/ENGINEER assembly files into SolidWorks
•
Exporting SolidWorks part or assembly documents as Pro/ENGINEER files
Importing Pro/ENGINEER Part Files Into SolidWorks To import a Pro/ENGINEER part file into SolidWorks:
1.
Click File, Open.
2.
In the Open dialog box, set Files of type to ProE Part (*.prt;*.prt.*;*.xpr).
3.
Browse to the desired file, and click Open. The Pro/ENGINEER To SolidWorks Converter dialog box appears.
4.
Set these options: •
Import geometry directly. Imports a model without features, either as a solid or surfaces. o
o
5.
BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid. Knitting. Attempts to knit surfaces during import. Select the Try forming solid model(s) check box to try to form solids using Knitting mode. Otherwise, the models are imported as surface bodies.
•
Analyze the model completely. Determines the number of features that SolidWorks can recognize and import.
•
Import material properties
•
Import sketch/curve entities
Click OK. If you select Import geometry directly, SolidWorks imports the model. If you select Analyze the model completely, SolidWorks parses the imported file and redisplays the Pro/Engineer to SolidWorks Converter dialog box with the following options:
13-34
6.
•
Features. Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.
•
Body. Attempts to import the model as a solid using Knitting. The Attempt to correct invalid feature check box has no effect if you click Body.
•
Generate translation report. If you select Features, generates a report that includes the features plus the recognition and import status.
Select Feature or Body to import the part. If you selected Generate translation report, the Translation Report dialog box appears.
7.
8.
Click one of the following: •
Print
•
Copy. Copies the translation report to the clipboard so you can paste it into another file.
Close the dialog box to import the part.
Importing Pro/ENGINEER Assembly Files Into SolidWorks To import a Pro/ENGINEER assembly file into SolidWorks:
1.
Click File, Open.
2.
In the Open dialog box, set Files of type to ProE Assembly (*.asm;*.asm.*;*.xas).
3.
Browse to the desired file, and click Open. The Pro/ENGINEER To SolidWorks Converter dialog box appears.
4.
Set these options: •
Component Import Options section. Select one of the following: o
Use feature import for all parts. Imports all component parts as features.
o
Use body import for all parts. Imports all component parts as bodies.
o
•
5.
•
BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid.
•
Knitting. Attempts to knit surfaces during import.
Prompt for each part. Prompts you to import each component part individually as a feature or a body.
If same name SolidWorks file is found section. Select one of the following: o
Use Existing. Uses the existing SolidWorks file and does not import the new file.
o
Overwrite. Overwrites the existing SolidWorks file.
o
Save with new name. Saves the file with a new name automatically.
•
Import material properties
•
Import sketch/curve entities
Click Import. SolidWorks converts and imports the file. If you selected Prompt for each part in the Component Import Options section, SolidWorks redisplays the Pro/ENGINEER To SolidWorks Converter dialog box.
6.
Set these options: •
Import geometry directly. Imports a model without features, either as a solid or surfaces. o
SolidWorks 2004 Reference Guide
BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid.
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Chapter 13 Import/Export
o
7.
Knitting. Attempts to knit surfaces during import. Select Try forming solid model(s) to try to form solids using Knitting mode. Otherwise, the models are imported as surface bodies.
•
Analyze the model completely. Determines the number of features that SolidWorks can recognize and import.
•
Import material properties
•
Import sketch/curve entities
Click OK. If you select Import geometry directly, SolidWorks imports the model. If you select Analyze the model completely, SolidWorks parses the imported file and redisplays the Pro/Engineer to SolidWorks Converter dialog box with the following options:
8.
•
Features. Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.
•
Body. Attempts to import the model as a solid using Knitting. The Attempt to correct invalid feature check box has no effect if you click Body.
•
Generate translation report. If you select Features, generates a report that includes the features plus the recognition and import status.
Select Feature or Body to import the model component. If you selected Generate translation report, the Translation Report dialog box appears.
9.
Click one of the following: •
Print
•
Copy. Copies the translation report to the clipboard so you can paste it into another file.
10. Close the dialog box. SolidWorks imports the component. The Pro/ENGINEER to SolidWorks Converter dialog box prompts you to import the next component. 11. Continue importing components until you have imported the entire assembly.
Exporting SolidWorks Documents as Pro/ENGINEER Files To export a SolidWorks document as a Pro/ENGINEER file:
1.
Click File, Save As. The Save As dialog box appears.
2.
3.
Set the Save as type box to one of the following: •
ProE Part (*.prt)
•
ProE Assembly (*.asm)
Click Save. The SolidWorks to Pro/ENGINEER Converter dialog box informs you of the progress, and the file is saved. If you export an assembly document that is referenced by other open documents, a message appears directing you how to proceed. Click OK to save the file. See Saving an Assembly and its Components for more information.
Solid Edge Files The Solid Edge translator imports the Parasolid information of Solid Edge® parts or assemblies into SolidWorks part or assembly documents. Only the Parasolid information is extracted, not the proprietary feature information. The Solid Edge translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box.
13-36
To open a Solid Edge part or assembly:
1.
Click File, Open. The Open dialog box appears.
2.
3.
Set Files of type to one of the following: •
Solid Edge Part (*.par)
•
Solid Edge Assembly (*.asm)
Browse to the desired file, and click Open.
Version Information The Parasolid translator imports Parasolid information from Solid Edge parts up to and including the most current version of Solid Edge.
STEP Files (*.step) The STEP translator supports import and export of body, face and curve colors of STEP AP214 files. The STEP AP203 standard does not have any color implementation. Import The STEP translator imports: •
STEP files as SolidWorks part or assembly documents.
•
Body geometry, body, face, and curve colors, and topology information from an AP214 STEP file.
•
Wireframe geometry from STEP AP203 and AP214 files.
•
STEP configuration data. You have the option to import this data by selecting the Map configuration data check box under STEP in the Import Options dialog box.
Export •
The STEP translator exports SolidWorks part or assembly documents to STEP files.
•
You can select to export individual parts or subassemblies from an assembly tree, limiting export to only those parts or subassemblies. If you select a subassembly, all of its components are automatically selected. If you select a component, its ascendants are partially selected, preserving the assembly structure.
•
SolidWorks supports exporting the unit of length of a part or assembly document to a STEP AP203 or AP214 file.
•
You can set export options in the STEP Export Options dialog box.
Version Information •
•
STEP Application Protocol AP203 is supported for both import and export. o
For import, Conformance Classes 1, 2 (surface data only), 4, 5, and 6 of AP203 are supported.
o
For export, Conformance Classes 1, 4, and 6 are supported.
STEP Application Protocol AP214 is supported for both import and export.
STL Files (*.stl) You can assign a unit of measure to a model for both import and export. Import The STL translator imports STL files as SolidWorks part documents. SolidWorks assembly files that you export as STL files import into SolidWorks as part documents. You have the option to import STL files as graphical data, solids, or surfaces. When you import STL files as graphical data, you can select the Import texture information check box to import texture information if this data exists.
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Chapter 13 Import/Export
Export The STL translator exports SolidWorks part and assembly documents as STL files. Click Try Print3D to open the Print3D web portal linked to the SolidWorks software. Print3D automates the prototype request process, eliminating the need to save parts as STL files. You can contact rapid part and prototype vendors to request price quotes and place orders for the current part document through the Print3D web portal.
TIFF Files (*.tif) Import You can insert a TIFF image as a background into part or assembly documents. See Inserting TIFF Files for more information. NOTE: The SolidWorks application does not support LZW format compression for TIFF files. Export The TIFF translator exports any SolidWorks document as a TIFF image. You can capture the image as it appears on a normal view (screen), or you can capture the image as it appears on a print preview. For drawing documents, you can select the sheet size and scale factor.
Inserting TIFF Files You can import a TIFF image and use it as a background of a part or assembly. The SolidWorks application does not support LZW format compression for TIFF files. To import a TIFF file:
1.
In a part or assembly document, click Insert, Customize Menu, and select Picture to activate this menu item.
2.
Click Insert, Picture.
3.
In the Open dialog box, browse to the desired file, and click Open. The selected file opens as a background image of your part or assembly. You can import RGB Full Color and Black & White (Bilevel) images, and you can also import Grayscale and Palette images from other systems.
To turn the display of the TIFF image on or off:
1.
Click View, Display, Customize Menu, and select Picture to activate this menu item.
2.
Click View, Display, Picture. When the Picture option is selected, the image is displayed; when the Picture option is cleared, the image is hidden.
To delete a TIFF image from a document:
1.
Click View, Modify, Customize Menu, and select Picture to activate this menu item.
2.
Click View, Modify, Picture, Delete.
To replace one TIFF image with another:
13-38
1.
Click View, Modify, Customize Menu, and select Picture to activate this menu item.
2.
Click View, Modify, Picture, Replace.
3.
In the Open dialog box, browse to the TIFF file that you want to use as a replacement, and click Open.
Unigraphics II Files The Unigraphics translator imports the Parasolid information of a Unigraphics® II part or assembly into a SolidWorks part or assembly document. Only the Parasolid information is extracted, not the proprietary feature information of a Unigraphics II part. You can import Unigraphics II compressed files. The Unigraphics translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box. To open a Unigraphics part or assembly:
1.
Click File, Open.
2.
In the Open dialog box, set Files of type to UGII (*.prt).
3.
Browse to the desired file, and click Open. If the file contains multiple bodies, the Unigraphics to SolidWorks Converter dialog box appears.
4.
5.
Select an import option: •
Multibody as separate parts. Imports the multiple bodies as parts contained in an assembly document.
•
Multibody in the same part. Imports the multiple bodies as imported bodies contained in a part document.
Click OK.
Version Information You can import parts and assemblies from Unigraphics II version 10 and higher.
VDAFS Files (*.vda) VDAFS is a neutral file format for the exchange of surface geometry. Import Options The VDA translator imports VDAFS part files as SolidWorks part documents. Export Options The VDA translator exports SolidWorks part documents as VDAFS files. You can set the following option: •
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Viewpoint Files This add-in module exports SolidWorks part or assembly documents to Viewpoint (.mts) files. You can view Viewpoint files over the Internet using the Viewpoint viewer. The Viewpoint files contain the compressed geometry of the model. The Viewpoint (MTS) translator also creates an .mtx file, which is in XML. This is the animation and attribute file of the model. The exported files contain graphical information only; you cannot edit these files. To deactivate or reactivate the Viewpoint translator:
1.
Click Tools, Add-Ins.
2.
Select or clear the SolidWorks MTS check box from the list of installed compatible software products.
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Chapter 13 Import/Export
To export a SolidWorks document as a Viewpoint file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to Viewpoint MTX/MTS (*.mts).
3.
Type the file name in the File name box, and click Save.
Version Information The Viewpoint translator exports SolidWorks documents as Viewpoint version 3.0.11 files.
VRML Files (*.wrl) VRML files can display 3D graphics over the Internet. Import The VRML translator imports all VRML files as SolidWorks part documents. SolidWorks assembly files that you export as VRML files import into SolidWorks as part documents. The VRML translator attempts to knit the VRML polygons into a solid. There are no contoured surfaces in the imported file; all surfaces are planar. This import option is intended as a last resort for importing data into SolidWorks. In many cases (especially complex models) the data does not knit into a usable solid, and is useful for viewing purposes only. You have the option to import VRML files as graphical data, solids, or surfaces. When you import VRML files as graphical data, you can select the Import texture information check box to import texture information if this data exists. Export The VRML translator exports SolidWorks part or assembly documents as VRML files. When you export as a VRML file, the SolidWorks software takes the View, Display, Section View option into account. If Section View is on, only the visible geometry is exported to the VRML file. This is different from the way the software behaves when you save documents as IGES, STEP, Parasolid, or ACIS files. When you export SolidWorks documents as VRML files, you can choose the version to export, VRML 1.0 or VRML 2.0 (VRML 97). Version Information The VRML translator supports all versions of VRML files up to and including VRML version 2.0 (VRML 97).
ZGL Files The ZGL translator exports SolidWorks part or assembly documents as RealityWave's ZGL file format. After you export the document, you must save the ZGL file into a RealityWave® database (VizStream Server). This converts the ZGL file into RealityWave’s streaming format that you can view over the Internet with the RealityWave viewer. The exported files contain graphical information only; you cannot edit these files. The ZGL translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as a ZGL file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to RealityWave ZGL (*.zgl).
3.
Type the file name in the File name box, and click Save.
Version Information The ZGL translator exports SolidWorks documents as RealityWave version 2.0 files.
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14 Library Features and the Feature Palette Window
Library Features and the Feature Palette Window A library feature is a frequently used feature, or combination of features, that you create once and then save in a library for future use. You can create commonly used features, such as holes or slots, in common sizes, and save them as library features to use whenever you need them. You can use several library features as building blocks to construct a single part. This can save time, and it can help ensure consistency in your models. The Feature Palette™ window helps you organize and use library features, sheet metal forming tools, piping components, and other commonly used parts. The Feature Palette window gives you quick access to the items you use most, by simply dragging them into the SolidWorks window. This topic describes: •
Creating and editing library features
•
Adding library features to parts
•
Organizing library features, forming tools, piping components, and other parts in the Feature Palette window
•
Inserting palette items in parts and assemblies
•
Palette Features and Library Features - Similarities and Differences
Palette Features and Library Features - Similarities and Differences Similarities between palette features and library features: •
You create a palette feature in the same way as a library feature.
•
The palette feature is displayed as a library feature in the FeatureManager design tree of the target part.
•
You can dissolve a palette feature the same way as a library feature.
Differences between palette features and library features: •
When you add a palette feature to a part, you can simply drag the feature roughly where you want it to be, then place it precisely by re-attaching and modifying any locating dimensions saved in the feature.
•
You can edit the dimensions of the palette feature as you insert it into the part.
•
Not all library features are suitable for use in the Feature Palette window. A palette feature is limited to one mandatory reference (one face, plane, edge, or vertex) on the target part. See Mandatory References.
•
Library features that have multiple mandatory references (such as draft features that depend on the selection of several faces) cannot be added through the Feature Palette window.
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Chapter 14 Library Features and the Feature Palette Window
You can also use the Feature Palette window to add parts to an assembly. You can organize parts in logical groups, and you can see a miniature graphical view of each palette part. You can add fittings to piping assemblies by dragging them from the Feature Palette window. For more information, see SolidWorks Piping Help Topics. The Feature Palette window is also used to apply forming tools to sheet metal parts. Forming tools are special parts that punch, stretch, or shape the sheet metal part, to create embossments, lances, flanges, louvers, ribs, and so on. Limitations In library features, you cannot have relations to silhouette edges or axes.
Mandatory References A palette feature is limited to one mandatory reference on the target part. The limitation of a single mandatory reference does not mean that a palette feature can consist of only one feature. As long as the parent feature uses a single reference, the palette feature can include multiple child features. To examine the parent/child relationships, right-click the feature, and select Parent/Child. To determine if a library feature is suitable for use in the Feature Palette, insert it as a library feature in a target part (see Adding a Library Feature to a Part). If there is only one mandatory reference listed, you can use the library feature as a palette feature. Feature Limitations Because of the limitation of a single reference, lofts, sweeps, and shape features are allowed only in certain cases: •
For lofts, the single mandatory reference is the sketch plane of one of the profiles. This must be the face or plane where you drop the feature. Additional sketch planes must be offset from this plane, or from each other. The library feature must include the planes.
•
For sweeps, the sweep path is the single mandatory reference. This must be a model edge. The sketch plane for the sweep section must be a Normal to Curve plane, with the model edge as the curve (when you select the edge, click near the vertex where the plane should be placed). Include this plane in the library feature. Then, when you drop the palette feature in the target part, drop it on the edge that is the sweep path, near the appropriate vertex.
•
For shape features, the shape must not be constrained to any entities. The definition can include only variations in Pressure, Bend, and Stretch (on the Controls tab of the Shape Feature dialog box).
Library Features Library Features A library feature can contain one or more features. Most feature types are supported, some with certain limitations. You can edit a library feature once it has been inserted into a part. After a library feature is added to a part, there is no associativity between the target part and the library feature part. If you edit a library feature part, the change is not propagated to parts that contain the library feature. Usually, library features consist of features added to a base feature, but not the base feature itself. Because you cannot have two base features in a single part, you cannot insert a library feature that includes a base feature into a part that already has a base feature. However, you can create a library feature that includes the base feature and insert it in an empty part. NOTE: A base feature is either the first solid feature or a solid feature not attached to another feature. You can only add a library feature to a part, or while editing a part in the context of an assembly. You cannot add a library feature to an assembly itself.
14-2
This section describes: •
Creating a Library Feature
•
Adding a Library Feature to a Part
•
Editing a Library Feature
•
Adding Color to a Library Feature
•
Dissolving a Library Feature
Creating a Library Feature To create a library feature, you first create a base feature, then create the features that you want included in the library feature on the base. Library features have the .sldlfp extension. NOTES: •
A base feature is either the first solid feature or a solid feature not attached to another feature.
•
You cannot create a library feature part (*.sldlfp file) from a multibody part document.
To create a library feature:
1.
Open a new part, sketch a profile, and create a base feature.
2.
Create the features you want to have in the library feature. Dimension the features to the base if you want to use the dimensions to locate the library feature when you place it on the target part.
3.
In the FeatureManager design tree, select the features you want to save as the library feature. This library feature has three features: a boss, a hole, and a fillet.
To select more than one feature, hold down the Ctrl key while you select. To select several features in a row, click the first feature, hold down the Shift key, then click the last feature.
Do not select the Base feature unless you plan to insert the library feature into an empty part. 4.
Base
Click File, Save As. The Save As dialog box appears.
5.
From the Save as type list, select Lib Feat Part (*.sldlfp). Enter a name and click Save. The part icon beside the part name in the FeatureManager design tree changes to the library feature icon and each feature that is included is marked with a letter L.
,
NOTE: To create a library feature from an existing part, open the part, select those features that you want to use in your library feature, and save them as a library feature part (*.sldlfp). You can create a library feature part that excludes some of the features of the source part, or one that contains all the features in the source part (with the exception of the base feature). It is important to note that excluding some features may cause rebuild errors in the library feature part because of unresolved dependencies.
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Chapter 14 Library Features and the Feature Palette Window
Adding a Library Feature to a Part There are two ways to add a library feature to a part: •
Place the library feature in the Feature Palette (available for most, but not all types of features), then drag and drop the feature into the part. See Feature Palette Window.
•
Use Insert, Features, Library Feature (for those types of features that are not supported in the Feature Palette).
To add a library feature to a part:
1.
With the target part open, click Insert, Features, Library Feature. The Open dialog box appears.
2.
Browse to the directory where the library feature is located, and select the library feature file (.sldlfp).
3.
Click Open. Two windows and a dialog box appear, and tile automatically: •
the library feature window
•
the target part window
•
the Insert Library Feature dialog box
In the Insert Library Feature dialog, there is at least one Mandatory reference, and there may be Optional references also.
4.
•
A Mandatory reference is preceded by an exclamation point ;
•
An Optional reference is preceded by a question mark references.
. Dimensional references are optional
To locate the library feature on the target part, click a Reference entity (Plane, Edge, Face, or Vertex) that is listed as Mandatory on the target part. The ex,clamation point in the Reference list changes to a check mark
5.
.
Select any optional references. As you click each item in the Reference list, notice that the corresponding entity is highlighted in the library feature window. Select the corresponding entity in the target part window. To deselect an entity, either double-click the check mark or click Deselect All.
6.
Click OK.
The library feature is added to the target part.
14-4
Insert Library Feature Wizard 1.
Select the entity on the target part that corresponds to the Reference item listed as Mandatory.
2.
If you are placing a library feature that includes a Base feature in an empty part, select the plane where you want to place the library feature. (You cannot add a library feature that includes a Base feature to a part that already has a Base feature.) NOTE: A base feature is either the first solid feature or a solid feature not attached to another feature.
3.
As you click each item in the Reference list, the entity is highlighted in the library feature window. Select the corresponding entity in the target part window.
4.
Select entities for Reference items listed as Optional, if desired. If you select the wrong entity, double-click the item in the Reference list to deselect it, or click Deselect All.
5.
When you are satisfied, click OK.
Editing a Library Feature You can change which features are included as part of a library feature in the library feature part document (.sldlfp): •
To add another feature, right-click the feature to add, and select Add To Library.
•
To remove a feature, right-click the feature, and select Remove From Library.
•
You can edit an existing library feature and save it with a new name (and .sldlfp extension) to create additional, similar library features.
After the library feature is inserted into a part, you can edit a library feature in the following ways: •
Use the same techniques that you would use to edit any SolidWorks feature, such as Edit Sketch or Edit Feature.
•
Move the library feature to a different location on the target part, by modifying the locating dimensions. Double-click the library feature icon in the FeatureManager design tree to display the dimensions.
Change Dimensions After inserting a feature from the Feature Palette, you can modify its dimensions. To modify the inserted feature's dimensions:
1.
In the Change Dimensions dialog box, click a Name or Value. The dimension appears on the model.
2.
Double-click the Value, and enter a new value.
3.
Click Apply to see the changes.
4.
When you are satisfied with the dimension values, click Finish.
Adding Color You can apply color to a library feature either in its own document or in a target part. To change the color of library features:
1.
Click Tools, Options, and on the Document Properties tab, select Colors.
2.
In the Model\Features colors box, select Library Feature.
3.
Click the Edit button and select a color from the color palette (or create a custom color), and click OK.
4.
Click OK. •
In a library feature document (.sldlfp), all the features that are included in the library feature use the new color.
•
In a target part, all inserted library features use the new color.
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Chapter 14 Library Features and the Feature Palette Window
Dissolving a Library Feature After the library feature is inserted into a part, you can dissolve (break down) a library feature into the individual features it contains. To break down a library feature into the features it contains:
In the FeatureManager design tree, right-click the library feature icon, and select Dissolve Library Feature from the shortcut menu. The library feature icon is removed, and each of the features it contains is listed individually in the FeatureManager design tree.
Feature Palette Window Feature Palette Window The Feature Palette window gives you quick access to the features and parts you use most often. It helps you organize features and parts in a way that suits your specific needs. This section describes: •
Displaying the Feature Palette Window
•
Organizing Feature Palette Items
•
Creating a Palette Item
•
Thumbnail Graphics
•
Working with Palette Items and Folders
•
Palette Parts as Derived Parts
•
Adding Palette Items to Documents: Parts and Assemblies
•
Applying a Palette Forming Tool to a Sheet Metal Part
Feature Palette Window Overview The Feature Palette window gives you quick access to the parts, assemblies, and library features you use most often. The Feature Palette window has several default folders. Each folder contains a group of palette items, displayed as thumbnail graphics. Palette items can include parts (.sldprt files), assemblies (.sldasm files), sheet metal forming tools (.sldprt files), and library features (.sldlfp files). To display the Feature Palette window:
Click Tools, Feature Palette. The palette stays open, and on top of the SolidWorks window, while you work. If the palette is displayed when you exit the SolidWorks software, it will be displayed when you start the SolidWorks software the next time. You can display the folder icons and the thumbnail graphics of palette items in two sizes. To change the size, right-click a blank area of the Feature Palette window, and select View, Large Icons or Small Icons. To dismiss the palette, click the X in the upper right corner of the Feature Palette window, or click Tools, Feature Palette again to remove the check mark from the item in the menu. To navigate in the Feature Palette window:
When you display the Feature Palette window, it opens at the top level, or Palette Home. To specify the folders that appear at Palette Home, see Organizing Feature Palette Items and File Locations. To open a folder, double-click it. The window controls include a dropdown history list of the last folders opened (up to 16), and these buttons (similar to the controls in Internet Explorer):
14-6
Go Backward
Back up through the list of folders
Go Forward
Go ahead through the list of folders
Reload
Refresh the palette window after changing the contents
Home
Return to Palette Home
Displaying the Feature Palette Window The Feature Palette window has several default folders. Each folder represents a directory; each palette item contained in that directory is displayed as a thumbnail graphic. Palette items can include parts, assemblies, sheet metal forming tools (.sldprt files), and library features (.sldlfp files). •
To display the Feature Palette window, click Tools, Feature Palette. The Feature Palette window stays open, and on top of the SolidWorks window, while you work. If the Feature Palette window is displayed when you exit SolidWorks, it will be displayed when you start SolidWorks the next time. See Organizing Feature Palette Items and File Locations for information on how to specify the folders displayed in the Feature Palette window.
•
To dismiss the Feature Palette window, either click in the upper-right corner of the window, or click Tools, Feature Palette again to remove the check mark from the item in the menu.
•
You can display the folder icons and the thumbnail graphics of palette items in two sizes. To change the size, right-click a blank area of the window, and select View, Large Icons or View, Small Icons.
Navigating in Feature Palette Window When you display the Feature Palette window, it opens at the top level, or Palette Home. To open a folder, doubleclick it. These toolbar controls are similar to the controls in Internet Explorer. •
Back
•
Forward
•
Reload
•
Home (to Palette Home)
•
The history list, with the names of the last folders opened (up to 16).
Organizing Feature Palette Items The Feature Palette window has several default folders. You can create and name new folders to suit your specific needs, and you can place items in each folder according to the way you want to organize the contents. The SolidWorks software includes some palette items to get you started. They are stored in these folders by default: •
install_directory\data\Palette Assemblies\folder_name
•
install_directory\data\Palette Features\folder_name
•
install_directory\data\Palette Parts\folder_name
•
install_directory\data\Palette Forming Tools\folder_name
If you chose a different path for the data directories when you installed SolidWorks, these folders are placed in the path you specified instead.
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Chapter 14 Library Features and the Feature Palette Window
Folders •
You add individual items to a folder by placing parts, assemblies, forming tools (.sldprt) or library feature parts (.sldlfp) in the appropriate folder.
•
A folder can contain individual palette items, and other folders. You can have as many folders, and as many levels of folders, as you want.
•
You can store palette items anywhere you want; the folders do not have to be located in the default path. You can have folders on different disk drives on your system, or on different computers on a network.
To specify which folders appear at the Palette Home level:
1.
Click Tools, Options, and on the System Options tab, select File Locations.
2.
From the Show folders for list, select the type of file for which you are defining a folder list: Palette parts, Palette assemblies, Palette features, or Palette forming tools. The first time you edit the Folders list, the default paths for the palette folders are already listed. These folder lists are always used, whether the Search file locations for external references check box under Tools, Options, System Options, External References is selected or not (this check box applies only to the Documents folder list). You can have more than one folder in the Palette Home for each type of item.
3.
•
To add a new path to the list, click the Add button. In the Browse for Folder dialog box, locate the path, and click OK.
•
To delete a path from the list, select the path in the Folders list, and click the Delete button.
•
To change the order of the list, select a path in the Folders list and use the Move Up or Move Down buttons to rearrange the list. Folders appear in the Palette Home in the order of the list.
Click OK. If you change the paths while the Feature Palette window is open, click Reload the paths.
to update
The icons in the Feature Palette window identify the type of item that the folder contains (with large icons only).
Creating a Palette Item There are several ways to add items to the Feature Palette window. Move or copy existing parts, assemblies, forming tools (.sldprt) or library feature parts (.sldlfp) into the appropriate folder, using Windows Explorer utilities. •
Drag the item from an open part or assembly document.
•
Drag a document from Windows Explorer.
•
Drag a hyperlink to a palette item from the Internet Explorer (version 4.0 or later).
To add a palette item from an open document:
1.
Create and save a new part, assembly, forming tool, or library feature part, or open an existing document (.sldprt or .sldlfp).
2.
Display the Feature Palette window, and navigate to the folder where you want to store the palette item.
3.
Drag the part from the graphics area, or the part icon from the top of the FeatureManager design tree of the active document, and drop it on the Feature Palette window. The Save As dialog box appears.
4.
Either accept the current name, or enter a new name, and click Save.
To add a palette item from Windows Explorer:
14-8
1.
Display the Feature Palette window, and navigate to the folder where you want to store the palette item.
2.
In Windows Explorer, navigate to the folder that contains the palette item.
3.
Drag the file from the Explorer window and drop it in the Feature Palette window.
To add a palette item from a hyperlink in Internet Explorer:
1.
Display the Feature Palette window, and navigate to the folder where you want to store the palette item.
2.
In Internet Explorer (version 4.0 or later), navigate to a location that contains hyperlinks to SolidWorks palette items. For example, on the SolidWorks web site, in the Gallery, Model Library section, navigate to the Solid Modeling Library page. You may also be able to obtain SolidWorks palette items from third-party vendors.
3.
Drag a hyperlink from the Internet Explorer window, and drop it in the Feature Palette window. The document is saved in the specified folder. NOTE:You can also just open a hyperlinked item, without adding it to the palette. To open the document, drag it to an empty area of the SolidWorks window. Then you can decide if you want to add the item to the palette, save it to a different folder, or close it without saving.
See also Forming Tools when using the Feature Palette window with sheet metal parts.
Thumbnail Graphics When you save a palette item, the thumbnail graphic reflects the view when the document is saved. Be sure to orient the part or assembly so that the thumbnail graphic looks the way you want it to look. To make it clear which features are included in a palette feature, consider changing the color in the library feature part. Thumbnail graphics use a palette of 16 colors; if the color you choose for the feature is not available, the software replaces it with a similar color in the thumbnail graphic. See Adding Color. NOTE: In the target part, palette features that consist of more than one feature use the color specified for Library Features under Tools, Options, on the Document Properties tab, select Colors. Palette features that consist of a single feature are automatically dissolved when you add them. Therefore they use the color specified for the individual feature type. Another way to emphasize the features is to select them, then click Zoom to Selection before you save the library feature part. That way, the thumbnail graphic provides a close-up view of the included features.
Working with Palette Items and Folders To copy a palette item:
Hold down the Ctrl key, then drag a palette item within the Feature Palette window. You can only copy an item this way in the same folder. The new item is named Copy of- . To rename a palette item:
You can rename the palette items and the folders, except the folders at the Palette Home level. Click-pauseclick the name in the Feature Palette window, and enter a new name. To edit a palette item:
1.
Right-click the item in the palette window, and select Edit Palette Item. – or – Drag the item from the Feature Palette window and drop it in an empty area of the SolidWorks window (not an empty area of a document window). The part (.sldprt) or library feature (.sldlfp) document is opened in a new window.
2.
Edit the document as needed, then Save. The palette updates automatically to reflect the changes. NOTE: The thumbnail graphic reflects the newly saved view. Be sure to orient the part or assembly so that the graphic looks the way you want it to look.
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Chapter 14 Library Features and the Feature Palette Window
To change the contents of a palette folder:
1.
In Windows Explorer, navigate to the directory you want to modify.
2.
Add, move, or delete the files as needed, using Windows file management commands.
3.
Click Reload
on the toolbar in the Feature Palette window to update the folders.
To delete a palette item:
Click the item in the Feature Palette window, and press Delete. The item is removed from the window, and the file is deleted from the corresponding folder. To delete a palette folder:
1.
Exit SolidWorks.
2.
Navigate to the directory to delete, move the contents to a new location, if necessary, then delete the directory.
Palette Parts as Derived Parts You can use the Feature Palette window to create a derived part, based on the selected palette part. 1.
With an empty part document open, click Tools, Feature Palette, then navigate to the folder that contains the desired part.
2.
Drag the part from the Feature Palette window and drop it into the part window.
3.
When you are asked if you want to create a derived part: •
Click Yes if you want to create a derived part (a part that has another part as its first feature). See Derived Parts for more information.
•
Click No if you want to edit the palette part itself. The palette part is opened in the current window.
Adding Palette Items to Documents Adding a Palette Feature to a Part Try using either Hidden Lines Removed or Hidden Lines Visible view mode, in order to see the preview and dimensions easily. To add a palette feature to a part:
1.
With a part open, click Tools, Feature Palette, and navigate to the folder that contains the feature.
2.
Drag the feature from the Feature Palette window, observing the preview as you drag. Drop the feature in the general area of the face where you want the feature to be placed. NOTE: You can also drag a hyperlink to a library feature part (.sldlfp) from Internet Explorer (4.0 or later) and drop it on the face of the part. If you want to save the hyperlinked palette feature for future use, be sure to also drag a copy into the palette, or into an empty area of the SolidWorks window, then save it. Otherwise, no local copy of the document is saved. Hyperlinked library feature parts have the same limitations and behaviors as library feature parts in the Feature Palette window. The Edit This Sketch dialog box appears, and remains open while you position the sketch.
3.
14-10
Click Zoom to Selection
to get a closer view of the feature.
4.
Click Modify Sketch on the Sketch toolbar, and move or rotate the sketch as needed. See Modify Sketch for more information. If the feature has locating dimensions, they are left dangling, and are displayed in brown.
5.
Re-attach the dangling dimensions. Select a dimension, then drag the red handle on the dimension line. The pointer has the shape until it is over a suitable entity for re-attachment. When you release the handle over an edge or vertex, the dimension re-attaches and the handle turns green. You can also add geometric relations to control the position of the sketch.
6.
Adjust the values of the locating dimensions. (Double-click the dimension, change the value, and press Enter.) You can also adjust the locating dimensions in the next step, or later, by editing the appropriate sketch.
7.
Click Next in the Edit This Sketch dialog box. The Change Dimensions dialog box appears. The Name and Value of each available dimension is displayed. If the dimensions are named in the part where you created the library feature, those names are used. Otherwise, the default dimension names D1 through Dn are used. Some dimensions of the feature may be unavailable, because they are specified as Internal Dimensions. See Dimension Access.
8. To display a feature dimension on the model, click either the Name or Value. To modify a dimension, double-click the Value, and enter a new value. Click Apply to see the changes.
9.
When you are satisfied with the dimension values, click Finish. If the palette item consists of more than one feature, a library feature icon appears in the FeatureManager design tree. If the palette item consists of a single feature, the item is automatically dissolved, and the appropriate icon for the feature type appears in the FeatureManager design tree. In either case, the name of the feature is the name of the item in the Feature Palette window.
Edit This Sketch 1.
Click Modify Sketch
2.
Re-attach any dangling dimensions (displayed in brown). Select a dimension, drag the red handle on the dimension line, and drop it on a suitable entity for re-attachment (edge or vertex).
3.
Adjust the values of the locating dimensions. You can either do this now (by double-clicking and editing the dimensions), or later.
on the Sketch toolbar, and move or rotate the sketch as needed.
NOTE: If the palette feature does not include dimensions that locate the feature on the face, you can use the
4.
Dimension tool Click Next.
SolidWorks 2004 Reference Guide
now to position the feature.
14-11
Chapter 14 Library Features and the Feature Palette Window
Edit Dimension Access For some types of features, such as sheet metal forming tools and library features, you may want to prevent other users from changing certain dimensions. You can also edit dimension access to reduce the clutter of unnecessary dimensions in the display. When you drag one of these features into a part document (from the Feature Palette window, or from Windows Explorer, or from a hyperlink in Internet Explorer), the dimensions are displayed, and they are available for editing. You can control the access to each dimension, to prevent other users from making unwanted changes when they use these features. To control dimension access:
1.
Right-click the part icon at the top of the FeatureManager design tree, and select Edit Dimension Access. In the Dimension Access dialog box, there are two lists: User dimensions (those that may be edited) and Internal dimensions (those that may not).
2.
Specify which dimensions are visible and available: •
To move a dimension from one list to the other, click the name, then click the left
or right
arrow button. As you click each name, the dimension is displayed in the model. • 3.
To move all the dimensions, use the double arrow button
.
Click Finish. When you insert an item that has restricted dimension access, only the User dimensions are visible and available for editing. The Internal dimensions are not displayed, and they are not available for editing. To make them visible and available again, repeat this procedure in the target part, after adding the library feature.
Internal Dimensions For some types of parts, such as sheet metal forming tools and library feature parts, you may want to prevent other users from changing certain dimensions. When you drag one of these items into a part document (from the Feature Palette window, or from Windows Explorer, or from a hyperlink in Internet Explorer), the dimensions are displayed, and available for editing. To prevent other users from making unwanted changes when they use these items, you can control the access to each dimension. Adding a Palette Part to an Assembly To add a palette part to an assembly:
1.
With the assembly open, click Tools, Feature Palette, and navigate to the folder that contains the desired part.
2.
Drag the part from the Feature Palette window and drop it into the assembly window.
3.
If the part has multiple configurations, the Select a configuration dialog box appears, with a list of the configurations in the part. Select the configuration you want, and click OK.
If you defined a mate reference in the part, you can create some types of mates automatically when you drop the part in the assembly. For more information, see Mate Reference. If you are editing a piping sub-assembly, you can drag fittings (T-junctions, flanges, and so on) from the Feature Palette window and drop them on vertices in the sketch. For more information, see SolidWorks Piping Help Topics.
14-12
15 Sheet Metal
Sheet Metal Sheet metal parts are generally used as enclosures for components or to provide support to other components. You can design a sheet metal part on its own without any references to the parts it will enclose, or you can design the part in the context of an assembly that contains the enclosed components. This chapter introduces the SolidWorks sheet metal functionality and describes: •
Designing Sheet Metal with Sheet Metal-Specific Features
•
Designing a Solid Body, Then Converting it to a Sheet Metal Part
•
Comparing Sheet Metal Design Methods
•
Other Sheet Metal Topics: o
Adding and Editing Bends
o
Bend Allowance and Bend Deduction
o
Flattening Bends in a Sheet Metal Part
o
Adding and Editing Auto Reliefs
o
Inserting Rips
o
Making Lofted Bends
o
Creating Sketched Bends
o
Adding Hems
o
Creating Jogs
o
Breaking Corners
o
Mirroring a Sheet Metal Part
o
Creating Flat Pattern Configurations
o
Using Forming Tools with Sheet Metal
o
Creating Drawings of Sheet Metal Parts
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Chapter 15 Sheet Metal
Designing Sheet Metal with Sheet Metal Features Base Flange A base flange is the first feature in a new sheet metal part. When you add a base flange feature to a SolidWorks part, the part is marked as a sheet metal part. Bends are added wherever appropriate, and sheet metal specific features are added to the FeatureManager design tree. Some additional items to note about a base flange feature: •
The Base-Flange feature is created from a sketch. The sketch can be a single open, a single closed, or multiple-enclosed profiles.
•
There can be only one base flange feature in a SolidWorks part.
•
The thickness and bend radius of the Base-Flange feature become the default values for the other sheet metal features.
To create a Base-Flange feature:
1.
Create a sketch that meets the requirements above. Alternatively, you can select the Base-Flange feature before you create a sketch (but after you select a plane). When you select the Base-Flange feature, a sketch opens on the plane.
2.
Click Base-Flange/Tab
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Base Flange.
The controls on the Base Flange PropertyManager update according to your sketch. For example, the Direction 1 and Direction 2 boxes do not appear for a sketch with a single closed profile. 3.
If necessary, under Direction 1 and Direction 2, set the parameters for the End Condition and Depth
4.
Under Sheet Metal Parameters:
5.
6.
•
Set a value for Thickness
•
Select Reverse direction to thicken the sketch in the opposite direction.
•
Set a value for Bend Radius
.
to specify the sheet metal thickness.
.
Under Bend Allowance, select a bend allowance type. •
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
•
If you selected Bend Table, select a bend table from the list, or click Browse to browse to a bend table file.
Under Auto Relief, select a relief type. If you selected Rectangular or Obround: •
Select Use relief ratio and set a value for Ratio. - or -
• 7.
Clear Use relief ratio and set a value for Relief Width
Click OK
and Relief Depth
.
.
Examining the FeatureManager Design Tree A Base Flange feature creates three new features in the FeatureManager design tree: Sheet-Metal1. Contains the default bend parameters. To edit the default bend radius, bend allowance, bend deduction, or default relief type, right-click Sheet-Metal1 and select Edit Feature. Base-Flange1. Represents the first solid feature of the sheet metal part. Flat-Pattern1. Flattens the sheet metal part. It is suppressed by default as the part is in its bent state. Unsuppress the feature to flatten the sheet metal part.
15-2
When Flat-Pattern1 is: •
suppressed, all new features are inserted above it in the FeatureManager design tree
•
unsuppressed, all new features are inserted below in the FeatureManager design tree and are not shown in the folded part
Edge Flange The Edge Flange feature adds a flange to your sheet metal part at an edge that you select. Here are some items to note about an edge flange feature: •
The selected edge must be linear.
•
The thickness is automatically linked to the thickness of the sheet metal part.
•
One sketch line of the profile must lie on the selected edge.
To create an edge flange feature:
1.
In an open sheet metal part, click Edge Flange Metal, Edge Flange.
on the Sheet Metal toolbar, or click Insert, Sheet
The Edge-Flange PropertyManager appears. 2.
In the graphics area, select the edge where you want to place the feature. The selected edge appears in the Edge
3.
box.
In the Edge-Flange PropertyManager, do the following: •
Under Flange Parameters, click Edit Flange Profile to edit the sketch of the profile.
•
To use something other than the default bend radius, clear the Use default radius check box and set Bend Radius
to the desired bend radius.
4.
Under Angle, set the Flange Angle
.
5.
Under Flange Length, set the Length End Condition and its corresponding parameters. For example, if you select Blind, you must set the Length Virtual Sharp
and Outer Virtual Sharp
or Inner
to determine where the length is measured from. You can also click Reverse Direction
to change the direction of the edge flange. 6.
Under Flange Position, do the following: •
Set the bend position to Material Inside
•
Bend from Virtual Sharp . See Bend Positions for a description of each of these selections. To remove extra material in neighboring bends, select the Trim side bends check box.
•
, Material Outside
, Bend Outside
, or
To offset the flange from the sheet metal body, select the Offset check box. Then, set the Offset End Condition and its corresponding parameters.
7.
To use something other than the default bend allowance, select the Custom Bend Allowance check box, and set a bend allowance type and value.
8.
If you want relief cuts added automatically, select the Custom Relief Type check box, then select the type of relief cut. If you select Rectangular or Obround, then you must specify a Relief Ratio.
9.
Click OK
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.
15-3
Chapter 15 Sheet Metal
Profile Sketch You can edit the profile sketch of an edge flange. The profile sketch has the following requirements: •
One sketch line of the profile must lie on the edge you selected when creating the Edge Flange. This sketched line does not have to be the same length as the selected edge.
•
The profile can be a single open, a single closed, or multiple-enclosed profiles.
To edit the profile sketch:
1.
When editing an edge flange feature, click Edit Flange Profile under Flange Parameters. The Profile Sketch dialog box appears.
2.
In the graphics area, drag one of the sketch entities of the Edge Flange preview to modify the sketch. Additionally, you can use the tools on the Sketch Tools toolbar to modify the sketch. For example, you can add a circle to the sketch to place a hole in the Edge Flange.
3.
Click Back to accept the changes to the profile sketch and to continue editing the Edge Flange feature. - or Click Finish to accept the changes to the profile sketch and to create the Edge Flange feature. - or Click Cancel to cancel the change to the profile sketch and close the Edge Flange PropertyManager.
Miter Flange A miter flange feature adds a series of flanges to one or more edges of a sheet metal part. Some items to note about a miter flange feature: •
The sketch for a miter flange must adhere to the following requirements: o
The sketch can contain lines or arcs. If you use an arc to create a miter flange, the arc cannot be tangent to the thickness edge. The arc can be tangent to the long edges, or by putting a small sketch line between the arc and the thickness edge. Click here for an example of creating a sketch for a miter flange with arcs.
o
o
The Miter Flange profile can contain more than one continuous line. For example, it can be an L-shaped profile. The sketch plane must be normal to the first edge where the Miter Flange is created. Click here for instructions to create a sketch for a miter flange.
•
The thickness is automatically linked to the thickness of the sheet metal part.
•
You can create a miter flange feature on a series of tangent or non-tangent edges. Click here for an illustration of each.
•
Instead of creating a miter flange across the entire edge of a sheet metal part, you can specify an offset of the flange.
To create a miter flange feature:
1.
15-4
Create a sketch that meets the requirements above. Alternatively, you can select the Miter Flange feature before you create a sketch (but after you select a plane). When you select the Miter Flange feature, a sketch opens on the plane.
2.
Click Miter Flange on the Sheet Metal toolbar, or click Insert, Sheet Metal, Miter Flange. The first edge for the Miter Flange feature is selected and a preview of the Miter Flange appears in the graphics area.
3.
In the graphics area, select the edges to miter for Along Edges
.
To select all of the edges tangent to the selected edge, click Propagate midpoint of the selected edge. 4.
Under Miter Parameters: •
To use something other than the default bend radius, clear Use default radius and set a value for Bend Radius
5.
that appears at the
.
•
Set the Flange position to Material Inside , Material Outside See Bend Positions for a description of each of these selections.
, or Bend Outside
•
Select Trim side bends to remove extra material in neighboring bends.
•
Set Gap distance
.
to use something other than the default gap.
If necessary, specify the offset distances for a partial miter flange: •
Under Start/End Offset set a value for Start Offset Distance
and End Offset Distance
•
. (If you want the miter flange to span the entire edge of the model, set these values to zero.) Select Custom Relief Type, and select a Relief type of: Rectangular, Tear, or Obround. If you selected Rectangular or Obround: Select Use relief ratio and set a value for Ratio.
o
- or Clear Use relief ratio and set a value for Relief Width
o
•
6.
and Relief Depth
.
To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value.
Click OK
.
The miter flange is added to the sheet metal part.
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Chapter 15 Sheet Metal
Miter Flange - Arc Sketches
Valid sketch: Arc is tangent to long edge
Valid sketch: Line is coincident to thickness edge, and arc is tangent to line
Invalid sketch: Arc is tangent to thickness edge
Miter Flange - Sketch Creation The sketch for a Miter Flange must adhere to the following: •
The sketch can contain only lines or arcs.
•
The Miter Flange profile can contain more than one continuous line. For example, it can be an L-shaped profile.
•
The sketch plane must be normal to the first edge where the Miter Flange is created.
To create a sketch for a Miter Flange feature:
1.
Select the first edge in the series of edges where you want to create a Miter Flange feature. Make sure to click the edge near the endpoint at the start of the series of edges.
2.
Click Line on the Sketch toolbar, or click Tools, Sketch Entities, Line. A sketch opens normal to the selected edge. The origin of the sketch is at the endpoint of the edge that is closest to where you clicked in step 1.
3.
Sketch the profile of the Miter Flange. Make sure that one line starts at the endpoint of the edge where the sketch origin is located. Back to Miter Flange.
15-6
Miter Flange - Edge Selection Before Miter Flange
After Miter Flange
Tangent Edges
Non-tangent Edges
Bend Positions In a Miter Flange, Edge Flange, Sketched Bend, Hem, or Jog, you have to select a bend position. The following table explains your choices. Bend Position
Preview
Material Inside . The top of the shaded preview of the flange coincides with the top of the fixed sheet metal entity.
Material Outside . The bottom of the shaded preview of the flange coincides with the top of the fixed sheet metal entity.
Bend Outside . The bottom of the shaded preview of the flange is offset by the bend radius.
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Chapter 15 Sheet Metal
Bend from Virtual Sharp . This preserves the dimension to the original edge and will vary the bend material condition to automatically match with the flange's end condition.
No preview available. Bend Centerline . The bend line is placed such that it equally splits the bend region in the flattened part. This is available only for Sketched-Bend features.
Trim Side Bends To remove extra material in neighboring bends, select the Trim side bends check box. Extra material appears when one of the bends of a Miter Flange touches an existing bend. The cut that trims the neighboring bends is automatically sized, and cannot be edited. Here is an example, using an Edge Flange feature: This is the preview of an Edge Flange feature. Notice the bend region of the blue preview touches the bend of the L-shaped base flange.
This is the end result without the Trim side bends check box.
This is the end result with the Trim side bends check box.
15-8
Sheet Metal Tab A Tab feature adds a tab to the sheet metal part. The depth of a Tab feature is automatically set to the thickness of the sheet metal part. The direction of the depth automatically coincides with the sheet metal part to prevent a disjoint body. Here are some additional items to note about a Tab: •
The sketch can be a single closed, multiple closed, or multiple-enclosed profile. The illustration shows a single tab feature that adds two tabs to the sheet metal part. The sketch must be on a plane or planar face that is perpendicular to the direction of thickness of the sheet metal part. You can edit the sketch, but you cannot edit the definition. This is because the depth, direction, and other parameters are set to match the parameters of the sheet metal part.
•
•
To create a Tab feature in a sheet metal part:
1.
Create a sketch on a plane or planar face that meets the above requirements.
2.
Click Base-Flange/Tab on the Sheet Metal toolbar, or click Insert, Sheet Metal, Tab. The tab is added to the sheet metal part. The tab's depth and direction are automatically set to match the parameters of the Base Flange feature.
Sketched Bend You can add bend lines to the sheet metal part while the part is in its folded state with a sketched bend feature. This allows you to dimension the bend line to other folded-up geometry. Some items to note about a sketched bend feature: •
Only lines are allowed in the sketch. You can add more than one line per sketch.
•
The bend line does not have to be the exact length of the faces you are bending. A Sketched Bend feature is commonly used with a Tab feature to bend the tab.
SolidWorks 2004 Reference Guide
15-9
Chapter 15 Sheet Metal
To create a Sketched Bend feature:
1.
Sketch a line on a planar face of the sheet metal part. Alternatively, you can select the Sketched Bend feature before you create a sketch (but after you select a plane). When you select the Sketched Bend feature, a sketch opens on the plane.
2.
Click Sketched Bend on the Sheet Metal toolbar, or click Insert, Sheet Metal, Sketched Bend.
3.
In the graphics area, select a face that does not move as a result of the bend for Fixed Face
4.
.
Click a Bend position of Bend Centerline Inside
, Material Outside
, Material
, or Bend Outside
5.
Set a value for Bend Angle, and click Reverse Direction
6.
if necessary. To use something other than the default bend radius, clear
7.
8.
.
Use default radius and set Bend Radius . To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value. Click OK
.
Hem The Hem tool adds a hem to your sheet metal part at a selected edge. Here are some additional items to note about the Hem tool: •
The selected edge must be linear.
•
Mitered corners are automatically added to intersecting hems.
•
If you select multiple edges to add a hem, the edges must lie on the same face.
To create a hem feature:
1.
In an open sheet metal part, click Hem
2.
In the graphics area, select the edges where you want to add a hem. The selected edges appear in Edges
3.
15-10
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Hem.
.
In the PropertyManager, under Edges: •
Select Material Inside
•
Click Reverse Direction
or Bend Outside
to specify where to add the material.
to create the hem on the opposite side of the part.
4.
Under Type and Size: a.
b.
Click a hem type:
o
Closed
o
Open
o
Tear Drop
o
Rolled
o
Length
o
Gap Distance
o
Angle
o
Radius
Set: (closed and open hems only) (open hem only)
(tear drop and rolled hems only) (tear drop and rolled hems only)
5.
Under Miter Gap, set Rip Gap if you have intersecting hems. Mitered corners are automatically added to intersecting hems, and you can set the gap between these hems.
6.
To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value.
7.
Click OK
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Chapter 15 Sheet Metal
Closed Corner You can create a Closed Corner feature to extend one face of a Butt rip so it overlaps the other face of the Butt rip. This is shown as follows:
Corner with Butt rip
Corner with Closed Corner feature
Here are some additional items to note about a Closed Corner feature: •
You can close more than one corner at a time. Select the faces for all of the rips that you want to close.
•
You can select only planar faces to close. The planar faces must be perpendicular to each other.
•
A closed corner cannot be applied in some cases where flange angles are not 90°.
To close a corner:
1.
Create a sheet metal part with a Base-Flange and a Miter-Flange, so that one corner looks like the illustration at right.
2.
Click Closed Corner on the Sheet Metal toolbar, or click Insert, Sheet Metal, Closed Corner. The Closed Corner PropertyManager appears.
3.
Select one of the planar faces on the corner, like the one that is highlighted, as the Faces to Extend
4.
Select a Corner type of Butt or Underlap
5.
Click OK
, Overlap
. .
The face is extended to close the corner.
15-12
. ,
Designing a Solid Body, then Converting it to Sheet Metal Bend Types Three types of bends are available when converting a solid body to a sheet metal part. These bends are: sharp bends, round bends, and flat bends. Sharp Bends A sharp bend is created by adding bends to a model that has sharp corners and a uniform thickness.
Round Bends A round bend can be created by adding bends to a model that has filleted or rounded corners and a uniform thickness. Round bends can also be created from cylindrical and conical faces.
Flat Bends A flat bend is created from a bend line sketched in the flattened sheet metal part. These lines are sketched in Flat-Sketch1 under Process-Bends1 in the FeatureManager design tree. The lines across the model in the illustration below on the left are sketched bend lines.
Creating a Sheet Metal Part Using Sharp Bends When bending sheet metal, you may want to create sharp bends instead of round bends. To create a sheet metal part with sharp bends:
1.
Create a part by sketching the part profile, then extruding a thin-feature part.
2.
Click Insert Bends
or Insert, Sheet Metal, Bends.
The Bends PropertyManager appears.
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15-13
Chapter 15 Sheet Metal
3.
Under Bend Parameters: •
Select the fixed face on the model. The fixed face remains in place when the part is flattened. The name of the face is displayed in the Fixed Face or Edge
•
Type the Bend Radius
box.
.
4.
Under Bend Allowance, select from the following options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
5.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
6.
If you want relief cuts added automatically, select the Auto Relief check box, then choose the type of relief cut. If you choose Rectangular or Obround, then you must specify a Relief Ratio. NOTE: The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
7.
Click OK
.
A bent sheet metal part is created whose dimensions in the flattened state reflect the specified bend allowance and radius values.
Creating a Sheet Metal Part Using Round Bends When bending sheet metal, you can create round bends instead of sharp bends. To create a sheet metal part with round bends:
1.
Create a thin feature part. In the Extrude PropertyManager, under Thin Feature: a.
Select Auto-fillet corners.
b.
Set a value for Bend Radius
to determine the inner bend radius.
2.
Click OK
.
3.
Click Insert Bends
4.
In the PropertyManager, under Bend Parameters, set the following:
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Bends.
a.
Fixed Face or Edge . In the graphics area, click a fixed face on the model. The fixed face remains in place when the part is flattened.
b.
Bend Radius . Set the value to zero, because the radius is propagated from the Bend Radius under Thin Feature.
5.
Under Bend Allowance, select from: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
6.
If you selected K-Factor, Bend Allowance, or Bend Deduction, set a value.
7.
If you want relief cuts added automatically, select Auto Relief, then choose the type of relief cut. If you choose Rectangular or Obround, set a Relief Ratio. The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
8.
Click OK
.
A bent sheet metal part is created whose dimensions in the flattened state reflect the specified bend allowance and radius values.
15-14
Creating Sheet Metal Parts with Conical Faces Parts with conical faces can also be made of sheet metal. To create a sheet metal part with conical faces:
1.
2.
Create a thin feature part with one or more conical faces: •
Any adjacent planar and conical faces must be tangent.
•
At least one end face of any conical face must have at least one linear edge.
Click Insert Bends
or Insert, Sheet Metal, Bends.
The Bends PropertyManager appears. 3.
Under Bend Parameters: •
Select a linear edge on an end face of a conical face as the fixed edge. - or Select a planar face tangent to the conical face as the fixed face. The fixed edge remains in place when the part is flattened. The name of the edge is displayed in the
• 4.
Fixed Face or Edge
box.
Set the Bend Radius
.
Under Bend Allowance, select from the following bend allowance options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction. NOTE: If creating a sheet metal part with one or more conical faces, you must select K-Factor as the type of bend allowance.
5.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
6.
If you want relief cuts added automatically, select the Auto Relief check box, then choose the type of relief cut. If you choose Rectangular or Obround, then you must specify a Relief Ratio. NOTE: The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
7.
Click OK
.
NOTE: Only parts with exact analytic conical faces can be unfolded. Oblong or non-right angle cones are not supported. As a test, try to insert an axis on the conical face. If you can insert an axis, the model is an exact cone. If you cannot insert an axis, then the model is not an exact cone and cannot be unfolded. However, sheet metal parts created with the Lofted Bends feature avoid this limitation and unfold appropriately.
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Chapter 15 Sheet Metal
Adding Walls to a Sheet Metal Part You cannot add walls to cylindrical or conical faces on sheet metal parts. To add a wall to a sheet metal part:
1.
Open a sketch on the face of a sheet metal part where the new wall will be attached.
2.
Select a linear edge of a planar face on the model to attach the wall to, and click Convert Entities the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities.
3.
Drag the vertices near existing bends a small distance away from the bends to allow for the bend radius.
4.
Click Extruded Boss/Base
5.
In the PropertyManager, under Direction 1:
on the Features toolbar, or click Insert, Boss/Base, Extrude.
a.
Select Blind in End Condition.
b.
Set a value for Depth
.
6.
Under Thin Feature, set Thickness
7.
Click OK
to the same value as the base part.
.
If a message appears warning of a disjoint body, click Reverse Direction click OK
15-16
on
again.
under Thin Feature, then
Sheet Metal Features When you click Insert Bends part.
or Insert, Sheet Metal, Bends, two distinct stages are applied to the sheet metal
•
The part is flattened and a bend allowance is added. The developed length is calculated, based on the bend radius and bend allowance.
•
The flattened part is restored to the folded state to create the bent version of the part.
Three features appear in the FeatureManager design tree that are specific to sheet metal operations. These three features represent a process plan for the sheet metal part: Sheet-Metal contains the definition of the sheet metal part. This feature stores the default bend parameter information (thickness, bend radius, bend allowance, auto relief ratio, and fixed entity) for the entire part. Flatten-Bends represents the flattened part. This feature contains information related to the conversion of sharp and filleted corners into bends. Each bend generated from the model is listed as a separate feature under Flatten-Bends. Bends generated from filleted corners, cylindrical faces, and conical faces are listed as RoundBends; bends generated from sharp corners are listed as SharpBends. The Sharp-Sketch listed under Flatten-Bends is the sketch that contains the bend lines of all sharp and round bends generated by the system. This sketch cannot be edited but can be hidden or shown. Process-Bends represents the transformation of the flattened part into the finished, formed part. Bends created from bend lines specified in the flattened part are listed under this feature. Flat-Sketch, listed under Process-Bends, is a placeholder for these bend lines. This sketch can be edited, hidden, or shown. Features listed after the Process-Bends icon in the FeatureManager design tree do not appear in the flattened view of the part.
Importing a Sheet Metal Part to SolidWorks If you have a sheet metal part with bends from another CAD system, you can import these parts, then convert them to SolidWorks sheet metal. The imported parts must be of uniform thickness to fold and unfold properly. To convert an imported part into a SolidWorks sheet metal part:
1.
Import a document into SolidWorks. See Importing Documents for more information.
2.
Click Insert Bends
3.
In the graphics area, select a face for Fixed Face or Edge
4.
Click OK
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Bends. .
.
The part converts to a SolidWorks sheet metal part. The FeatureManager design tree contains Sheet-Metal1 , Flatten-Bends1 , and Process-Bends1 features. The part can now be flattened and bent as a sheet metal part by toggling the suppression state of the Process-Bends feature.
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Chapter 15 Sheet Metal
Comparing Sheet Metal Design Methods Comparing Sheet Metal Design Methods You can better understand the features available in SolidWorks by comparing methods of creating sheet metal parts. There are two ways to create a sheet metal part: •
Build a part, then convert it to sheet metal.
•
Create the part as a sheet metal part using sheet metal-specific features. This eliminates extra steps because you create a part as sheet metal from the initial design stage.
Design a Sheet Metal Part from a Solid When you create a sheet metal part, you generally design the part in the folded state. This allows you to capture the design intent and the dimensions of the finished part. To create a sheet metal part of uniform thickness:
1.
Open a new part, and sketch a rectangle.
2.
Create a Base-Flange by clicking Base-Flange/Tab or Insert, Sheet Metal, Base Flange. The sheet metal features appear in the FeatureManager design tree.
3.
Now that the base for your part is created, add walls that bend from the base with a miter flange.
4.
or If you want to make a cut across a bend, click Unfold Insert, Sheet Metal, Unfold. This flattens the individual bends.
5.
Sketch a closed profile across the flattened bend, and Extrude the cut Through All.
6.
To restore the part to the bent state, click Fold Sheet Metal, Fold.
or Insert,
When you create a part initially out of sheet metal you use two features: Base-Flange and Miter Flange. However, if you build a solid, then convert it to sheet metal, you need more features: Base Extrude, Shell, Rip, and Insert Bends. It is much faster to create a part as sheet metal instead of creating a part, then converting it to sheet metal.
15-18
Design a Part from a Solid, Then Convert it to Sheet Metal It is possible to create a solid part, then convert it to sheet metal to add the bends and sheet metal features. To create a part of uniform thickness and convert it to sheet metal:
1.
Create a block with the Base-Extrude tool. Make the block 50mm on all sides.
2.
Shell the block to 1mm so the part is of uniform thickness. In Faces to Remove, select the faces as shown.
3.
To bend the part, rip the block between the edges of the tabs or Insert, Sheet Metal, Rip. Select the by clicking Rip edge to rip as shown.
4.
Convert the part to sheet metal by clicking Insert Bends or Insert, Sheet Metal, Bends.
5.
If you want to make a cut across a bend, drag the Rollback Bar before the Process-Bends feature in the FeatureManager design tree.
6.
Sketch a closed profile across one of the bends.
7.
Extrude the cut Through All.
8.
To restore the part to the bent state, drag the rollback bar to the bottom of the FeatureManager design tree.
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Chapter 15 Sheet Metal
Design a Sheet Metal Part from the Flattened State You may want to design a sheet metal part from the flattened state. In this case, you create a sheet metal part, then insert bend lines on which to fold the part. To create a sheet metal part from the flattened state:
1.
Open a new part.
2.
Create a sketch as shown. You do not have to dimension the part.
3.
Create a Base-Flange by clicking Base-Flange/Tab or Insert, Sheet Metal, Base Flange. The sheet metal features appear in the FeatureManager design tree.
4.
To bend the sheet metal part, sketch lines on the part as shown.
5.
Bend the part by clicking Sketched Bend , or Insert, Sheet Metal, Sketched Bend. The part bends at the sketched lines.
To add features that appear in the folded model:
There is no need to drag the rollback bar in order to add any additional tabs, cuts, or other features to the folded model. Instead, you can add features directly in the folded state; the features appear above the FlatPattern feature in the FeatureManager design tree. Designing a part with sheet metal-specific features uses fewer features and editing tools, and eliminates the use of the rollback bar. The sheet metal-specific features make it easier and faster to create a sheet metal part than designing a part, then converting it to sheet metal. SolidWorks includes sheet metal-specific features so you can create a part as sheet metal without having to convert it to sheet metal.
Design a Part from the Flattened State, Then Convert it to Sheet Metal It is possible to create a flattened part, then convert it to sheet metal to add the bends and sheet metal features. To create a flattened part and convert it to sheet metal:
15-20
1.
Open a new part.
2.
Create a sketch as shown. You do not have to dimension the sketch.
3.
Create a Base-Extrude feature that forms the flattened part.
,
4.
Convert the part to sheet metal by clicking Insert Bends or Insert, Sheet Metal, Bends.
5.
Bend the sheet metal part by adding bend lines to the FlatSketch. Sketch three lines on the Flat-Sketch as shown.
6.
Close the sketch. The sheet metal part bends on the lines you sketched.
7.
Once the sheet metal part is in its folded state, you can still add features to the part by dragging the Rollback Bar before the Sheet-Metal features in the FeatureManager design tree. This insures that the new features appear in both the bent and flattened states.
Reasons to Build a Part, then Convert it to Sheet Metal There are a few instances where it is to your advantage to build a part, then convert it to sheet metal. •
Imported Solid Bodies. If you import a sheet metal file with bends from another CAD system, the bends are already in the model. Using Insert Bends SolidWorks sheet metal part.
•
is your best option for converting the imported file to a
Conical Bends. Conical bends are not supported by the sheet metal-specific features, such as Base Flange, Edge Flange, and so on. Therefore, you must build the part using extrusions, revolves, and so on, then convert it to add bends to a conical sheet metal part.
Combining the Different Sheet Metal Design Methods Parts that are originally created as sheet metal have different features than parts that are created, and then converted to sheet metal. However, you can add sheet metal-specific features to parts converted to sheet metal. As soon as you add a sheet metal-specific feature, (a Miter Flange
, an Edge Flange
, and so on), the following occurs:
•
Flat-Pattern1
is added to the FeatureManager design tree, and suppressed.
•
Bends for new sheet metal features are stored under each individual feature instead of under Flatten-Bends1 or Process-Bends1
. Additionally, all pre-existing and new bends are listed under the Flat-Pattern1
feature. To flatten the part, unsuppress Flat-Pattern1
SolidWorks 2004 Reference Guide
rather than suppressing Process-Bends1
.
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Chapter 15 Sheet Metal
Other Sheet Metal Topics Bend Allowance and Bend Deduction Bend Allowance and Bend Deduction Options You can specify the bend allowance or bend deduction values for your part. Select from the following options: Bend Table K-Factor Bend Allowance Bend Deduction Bend Allowance and Bend Deduction You can choose either bend allowance or bend deduction calculations to determine the flat length of sheet stock to give the desired dimension of the bent part. Bend Allowance Calculations The following equation is used to determine the total flat length when bend allowance values are used: Lt = A + B + BA where: •
Lt is the total flat length
• •
A and B are shown in the illustration BA is the bend allowance value
Bend Deduction Calculations The following equation is used to determine the total flat length when bend deduction values are used: Lt = A + B - BD where:
15-22
•
Lt is the total flat length
• •
A and B are shown in the illustration BD is the bend deduction value
K-Factor K-Factor is a ratio that represents the location of the neutral sheet with respect to the thickness of the sheet metal part. When you select K-Factor as the bend allowance, you can specify a K-Factor bend table. The SolidWorks application also comes with a K-Factor bend table in Microsoft Excel format. This is located in\lang\English\Sheetmetal Bend Tables\kfactor base bend table.xls. Bend allowance with a K-Factor is calculated as follows: BA = Π ( R + KT )A ⁄ 180
where: BA = bend allowance R = inside bend radius K = K-Factor, which is t / T T = material thickness t = distance from inside face to neutral sheet A = bend angle in degrees (the angle through which the material is bent)
Bend Table Overview You can specify the bend allowance or bend deduction values for a sheet metal part in a bend table. The bend table also contains values for bend radius, bend angle, and part thickness. There are two types of bend tables that you can use: •
A text file with the .btl extension
•
An embedded Excel spreadsheet
A comparison of the two methods is shown as follows: Text File
Excel Spreadsheet
When you share your part with a colleague, you must remember to share your bend table as well.
When you share your part with a colleague, your bend table is automatically included because it is embedded.
Text tables can be edited in a variety of applications.
Excel spreadsheets can be edited in Microsoft Excel only.
NOTES: •
It is recommended that you use the Excel spreadsheet unless you have legacy bend tables from SolidWorks 2000 or earlier.
•
If you edit a bend table that has multiple bend thickness tables, the radii and angles must be the same. For example, if you insert a new bend radius value into a bend table with multiple bend thickness tables, you must insert the new value in all of the tables.
You can edit a bend table in a separate Excel window. Click Edit, Bend Table, Edit Table in New Window.
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Chapter 15 Sheet Metal
Bend Table - Text File A sample bend table for sheet metal operations is provided in\lang\english\Sheetmetal Bend Tables\sample.btl. To create your own bend table, copy and edit this bend table with any text editor. Bend tables created as a text file support the following: •
All bend table types (bend deduction, bend allowance, and k-factor).
•
All units of measure (meters, millimeters, centimeters, inches, and feet). Set the unit of measure in the Units row of the bend table.
A few items to note about bend tables in a text file: •
The sample bend table is provided only for informational purposes. The values in this table do not represent any actual bend allowance values.
•
If the thickness of the part or bend angle falls between values in the table, the software interpolates the values to calculate the bend allowance.
Bend Table - Excel Spreadsheet New bend tables that you create for SolidWorks are stored in an embedded Excel spreadsheet. You add bend table values into the cells of the spreadsheet, ensuring that the table is read properly by the SolidWorks software. Bend tables made in Microsoft Excel now support the following: •
All bend table types (bend deduction, bend allowance, and k-factor).
•
Multiple angles in a single bend table file.
To create a bend table:
1.
In a part, click Insert, Sheet Metal, Bend Table, New. If you get a message that says inserting a bend table may cause the developed length of the flat pattern to change, click Yes.
2.
In the dialog box: a.
Select an item in Units to set the unit of measurement.
b.
Select an item in Type to set the bend allowance or bend deduction.
c.
Type a path for File name, or click Browse to locate a path where you want to save the bend table.
d.
Click OK.
An embedded Excel window, containing the bend table spreadsheet, appears in the SolidWorks window. The bend table spreadsheet contains default radius, thickness, and angle values.
15-24
3.
Type the bend allowance or bend deduction values to the spreadsheet, depending on your choice for Type in step 2.
4.
Click outside the table, but within the SolidWorks graphics area, to close the spreadsheet.
Bend Allowance Value You can specify an explicit bend allowance for any sheet metal bend by entering the value when you create the bend. NOTE: By definition, the bend allowance is the arc length of the bend as measured along the neutral axis of the material.
Bend Deduction Value You can specify an explicit bend deduction for any sheet metal bend by entering the value when you create the bend. NOTE: By definition, the bend deduction is the difference between the bend allowance and twice the outside setback.
Using Forming Tools with Sheet Metal Forming Tools Forming tools act as dies that bend, stretch, or otherwise form sheet metal. The SolidWorks software includes some sample forming tools to get you started. They are stored in\data\Palette Forming Tools\. You can only insert forming tools from the Feature Palette window and you can apply them only to sheet metal parts. A sheet metal part has the Sheet-Metal1 feature in the FeatureManager design tree. You can create your own forming tools using many of the same steps you use to create any SolidWorks part. You apply forming tools to sheet metal parts to create form features such as louvers, lances, flanges, and ribs. Examine the sample forming tools before creating your own. You may find that by editing a sample forming tool, you can create a forming tool that meets your needs. Creating Forming Tools Forming tools act as dies that bend, stretch, or otherwise form sheet metal. When you create a forming tool, you must create two features: •
Base feature. Used as a temporary parent feature on which the boss feature is created.
•
Boss feature. Used as the actual forming tool.
After you create the boss feature, you delete the base feature.
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Chapter 15 Sheet Metal
To create a forming tool:
1.
Open a new part.
2.
Sketch a profile for the base feature on the horizontal plane centered on the origin. By default, the horizontal plane is the Top Plane. A typical profile for the base feature is a rectangle. Make sure the profile is big enough to accommodate the boss feature (forming tool). When you apply a forming tool to a sheet metal part, the origin lies where you drop the forming tool.
3.
Extrude the profile for the base feature upwards as shown.
4.
Create the boss feature below the horizontal plane. The boss feature can be an extrude or a revolve.
5.
Add additional features to the forming tool such as extrudes, revolves, fillets, chamfers, and so on. NOTES: The horizontal plane is the stopping surface of the forming tool. Therefore, the entire forming tool must lie below the stopping surface. The minimum radius of curvature of the forming tool must be greater than the thickness of the sheet metal part to which it is applied. To determine the minimum radius of curvature of the forming tool, click Tools, Check.
6.
Remove the base feature of the forming tool, so only the form feature remains: a.
Open a sketch on the bottom face of the base feature, and click Convert Entities
b.
.
Make an Extruded Cut and select Through All in End Condition.
7.
Indicate which faces of the forming tool create openings on sheet metal parts.
8.
Create a positioning sketch, if necessary.
9.
Save the part.
10. Add the tool to the Feature Palette window.
15-26
Creating Openings on Forming Tools Some types of form features, such as louvers and lances, create openings on sheet metal parts. To indicate which forming tool faces create openings, change the color of these faces to red. To create an opening on a forming tool:
1.
Right-click the face designed to create an opening, and select Properties under Face.
2.
In the dialog box, set Red to 255, Green to 0, and Blue to 0.
3.
Click OK.
4.
Click Rebuild
.
Create a Positioning Sketch for Forming Tool To edit the position of a form feature on a sheet metal part, you can create a positioning sketch on the top face of the forming tool. When you apply the forming tool to the sheet metal face, you use the positioning sketch to locate the form feature on the face of the sheet metal part. To create a positioning sketch for a forming tool:
1.
Open a sketch on the top face of the boss feature on the forming tool.
2.
Create a profile to locate the form feature on the sheet metal part. One method to create a profile is to click Convert Entities Sketch Tools, Convert Entities.
3.
Close the sketch, and rename the sketch if desired.
4.
To hide the positioning sketch so that it does not appear in the thumbnail graphic of the forming tool in the Feature Palette window, right-click the sketch in the FeatureManager design tree, and select Hide.
on the Sketch toolbar, or click Tools,
Working with Palette Items and Folders To copy a palette item:
Hold down the Ctrl key, then drag a palette item within the Feature Palette window. You can only copy an item this way in the same folder. The new item is named Copy of- . To rename a palette item:
You can rename the palette items and the folders, except the folders at the Palette Home level. Click-pauseclick the name in the Feature Palette window, and enter a new name. To edit a palette item:
1.
Right-click the item in the palette window, and select Edit Palette Item. - or Drag the item from the Feature Palette window and drop it in an empty area of the SolidWorks window (not an empty area of a document window). The part (.sldprt) or library feature (.sldlfp) document is opened in a new window.
2.
Edit the document as needed, then Save. The palette updates automatically to reflect the changes. NOTE: The thumbnail graphic reflects the newly saved view. Be sure to orient the part or assembly so that the graphic looks the way you want it to look.
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Chapter 15 Sheet Metal
To change the contents of a palette folder:
1.
In Windows Explorer, navigate to the directory you want to modify.
2.
Add, move, or delete the files as needed, using Windows file management commands.
3.
Click Reload
on the toolbar in the Feature Palette window to update the folders.
To delete a palette item:
Click the item in the Feature Palette window, and press Delete. The item is removed from the window, and the file is deleted from the corresponding folder. To delete a palette folder:
1.
Exit SolidWorks.
2.
Navigate to the directory to delete, move the contents to a new location, if necessary, then delete the directory.
Applying Forming Tools to Sheet Metal Parts You can only insert forming tools from the Feature Palette window and you can apply them only to sheet metal parts. A sheet metal part has the Sheet-Metal feature in the FeatureManager design tree. To apply a palette forming tool to a sheet metal part:
1.
In an existing sheet metal part, click Tools, Feature Palette, and navigate to the folder that contains the forming tools.
2.
Drag the forming tool from the Feature Palette window to the face you want to deform, but do not drop it yet. The face where you apply the forming tool corresponds to the stopping surface of the tool itself. By default, the tool travels downward. The material is deformed when the tool strikes the face where it is dropped. To toggle the direction of travel and strike the opposite side of the material, press the Tab key. Notice the preview as you toggle the direction.
3.
Drop the feature where you want it applied. If the forming tool includes an optional positioning sketch, that sketch is displayed when you drop the tool on the face.
4.
Locate the positioning sketch by dimensioning, adding relations, or modifying the sketch. As you add dimensions, the positioning sketch moves as a single entity. The absorbed sketch in the feature controls only the location of the feature, not its dimensions.
5.
In the Position form feature dialog box, click Finish. The forming tool is applied to the face, and the feature is added to the FeatureManager design tree with the name of the forming tool.
More Sheet Metal Topics Using Auto Reliefs The software automatically adds relief cuts wherever needed when inserting bends if you select Auto Relief. The software supports the following types of relief cuts: •
Rectangular
•
Tear
•
Obround
If you want to automatically add Rectangular or Obround reliefs, you must specify the Relief Ratio. Tear reliefs are of the minimum size required to insert the bend and flatten the part.
15-28
Relief Ratio The distance d represents the width of the Rectangular or Obround relief cut and the depth by which the side of the Rectangular or Obround relief cut extends past the bend region. The distance d is determined by the following equation: d = (relief ratio) * (part thickness) The bend region is represented by the dark gray area of the diagram.
The value of the relief ratio must be between 0.05 and 2.0. The higher the value, the larger the size of the relief cut added during insertion of bends. Changing Auto Reliefs You can change the type and size of a relief cut for a feature bend. A feature bend is different from an individual bend, in that the feature bend is an actual sheet metal feature. For example, when you have a Sketched Bend in the FeatureManager design tree, the Sketched Bend feature is the sheet metal feature, and SketchBend is the individual bend that is absorbed in the Sketched Bend feature. To change the type and size of a relief cut for a feature bend:
1.
In the FeatureManager design tree, right-click the feature bend you want to edit, and select Edit Feature.
2.
In the PropertyManager, select Custom Relief Type.
3.
Under Custom Relief Type: •
Set a relief cut in Auto Relief Type.
•
If you selected Rectangular or Obround, change the values for Relief Width Depth
4.
Click OK
and Relief
, or select Use relief ratio and set a value for Relief Ratio.
.
Edit Auto Reliefs You can edit auto relief cuts in sheet metal parts. For more information, select from the following: •
Edit a single auto relief
•
Edit all auto reliefs
NOTE:You cannot edit relief cuts in sheet metal parts created in versions prior to SolidWorks 99. Edit All Auto Reliefs You can change the type of auto reliefs automatically added to the bend regions in sheet metal parts. You cannot edit relief cuts in sheet metal parts created in versions prior to SolidWorks 99. To change the type of relief cut for all bends:
1.
Right-click the Sheet-Metal feature in the FeatureManager design tree and select Edit Feature.
2.
In the PropertyManager, under Auto Relief, change the type of relief cut.
3.
If you select Rectangular or Obround, specify the Relief Ratio.
4.
Click OK
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.
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Chapter 15 Sheet Metal
Rip Creates a rip feature along the selected model edges. A rip feature is commonly used in sheet metal parts, but you can add a rip feature to any part. To create a rip feature:
1.
2.
Create a part of uniform thickness with adjacent planar faces that form one or more linear edges or a chain of linear edges.
Click Rip
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Rip.
The Rip PropertyManager appears. 3.
On the model, select the internal linear edges to rip. Note the arrows that appear on each selected edge. By default, rips are inserted in both directions. To insert a rip in only one direction, click the name of the edge listed under Edges to Rip, and click Change Direction. The rip direction toggles every time you click Change Direction to one direction, then the other direction, then back to both directions.
4.
To change the gap distance, clear the Use default gap check box, and type a value in the Rip Gap
5.
Click OK
Both directions:
One direction:
15-30
.
box.
Bends The Bends PropertyManager allows you to create a sheet metal part. When you use the Insert Bends tool, you must create a solid body, then use Insert Bends to convert the part to sheet metal. Alternatively, you can create a part directly out of sheet metal with a Base-Flange. To convert a part to sheet metal:
1.
In a part made of uniform thickness, click Insert Bends Sheet Metal, Bends.
on the Sheet Metal toolbar, or click Insert,
The Bends PropertyManager appears. 2.
Under Bend Parameters, do the following: •
Select a Fixed Face or Edge
•
Set the Bend Radius
.
.
3.
Under Bend Allowance, select from the following options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
4.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
5.
If you want relief cuts added automatically, select the Auto Relief check box, then select the type of relief cut. If you select Rectangular or Obround, then you must specify a Relief Ratio.
6.
If desired, select an edge to rip under Rip Parameters •
Click Change Direction if you want to reverse the direction of the rip.
•
Clear the Use default gap check box if you want to set a gap distance, and type the value in the Rip Gap
7.
, and do the following:.
Click OK
box. .
The bends are added, and the part is converted to sheet metal. Edit Bends You can edit the bend parameters for a single bend, for a group of bends, or for your entire sheet metal part. The bend parameters include the default bend radius, and the bend allowance or bend deduction values. Select from the following: •
Edit a single bend.
•
Edit a group of bends.
•
Edit all the bends in your sheet metal part.
Reorder Bends You can reorder the bends in a sheet metal part in which bends have been inserted. To reorder bends in relation to each other:
1.
Right-click Flat-Pattern1 in the FeatureManager design tree, and select Reorder Bends. If you created the sheet metal part with the Insert Bends feature, right-click Process-Bends1, and select Reorder Bends.
2.
In the dialog box, click a bend name in the list, then click Move Up or Move Down to change the bend order.
3.
Repeat step 2 to move additional bends.
4.
Click OK.
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Chapter 15 Sheet Metal
Flattening Sheet Metal Bends You can flatten the bends in a sheet metal part in the following ways: •
To flatten the entire part, if the Flat-Pattern1 feature is present, unsuppress Flat-Pattern1, or click Flattened on the Sheet Metal toolbar. The bend lines are shown by default when you unsuppress Flat-Pattern1. To hide the bend lines, expand Flat-Pattern1, right-click Bend-Lines, and select Hide. When you flatten the entire part in this manner, corner treatments are applied to create a clean, flattened sheet metal part.
•
To flatten the entire part, if the Process-Bends1 feature is present, suppress Process-Bends1, or click Flattened
•
on the Sheet Metal toolbar.
To flatten one or more individual bends, add an Unfold
feature.
For faster system performance, only unfold the bends that you need for the task that you are performing. For example, when you add a cut across a bend, only unfold that one bend. No Bends You can roll back all bends from a sheet metal part in which bends have been inserted so that you can make additions, such as adding a wall. This is available only in sheet metal parts with Flatten-Bends1 and Process-Bends1 features. To roll back all bends from a sheet metal part:
Click No Bends on the Sheet Metal toolbar to roll back the bends up to Sheet-Metal1. The bend radius and bend allowance are rolled back. (The part is not flattened.) To restore all bends to the part:
Click No Bends
again.
Sheet Metal - Default Bend Parameters The presence of the Sheet-Metal1 feature in the FeatureManager design tree indicates that you have a sheet metal part. The Sheet-Metal1 feature contains the default bend parameters. To edit the default bend radius, bend allowance or bend deduction, or default relief type:
1.
Under Bend Parameters: •
On the model, select a linear edge on an end face of a cylindrical or conical face, or select a planar face for Fixed Face or Edge . The edge or face remains in place when the part is flattened. This step is not necessary if you start your sheet metal part from a Base Flange feature.
•
15-32
Set the Bend Radius
.
2.
Under Bend Allowance, select from the following: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
3.
If you selected K-Factor, Bend Allowance, or Bend Deduction, set a value.
4.
If you want relief cuts added automatically, select Auto Relief, then select the type of relief cut. If you selected Rectangular or Obround, then you must set a Relief Ratio.
5.
Click OK
.
Mirroring Sheet Metal Parts When you mirror a sheet metal part, many of the bends are mirrored as well. The only bends that are not mirrored are those that are normal to and coincident to the mirror plane; those bends are extended. To mirror a sheet metal part:
1.
In an existing sheet metal part, click Insert, Pattern/Mirror, Mirror. NOTE: If a message appears that says sheet metal features cannot be mirrored individually, click OK. The Mirror PropertyManager appears.
2.
Select a plane of symmetry or a planar face as the Mirror Face/Plane . Use Select Other from the shortcut menu if necessary.
3.
Select a body as the Bodies to Mirror
4.
Click OK
.
.
The entire part is mirrored as well as the sheet metal bends.
5.
Expand Mirror1 in the FeatureManager design tree and notice the new bends that include the mirrored geometry.
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Chapter 15 Sheet Metal
Cut Across Sheet Metal Bends You can make cuts across bend lines. To cut across sheet metal bends:
1.
In an existing sheet metal part, click Unfold
or Insert, Sheet Metal, Unfold.
The Unfold PropertyManager appears. 2.
In the graphics area: a.
Select a face as the fixed face. The selected face appears in the Fixed face
b.
box.
Select the bend you want to cut across. The selected bend appears in the Bends to unfold
3.
Click OK
box.
.
The selected bend only is unfolded. 4.
Sketch a closed profile across the flattened bend, and Extrude the cut Through All.
5.
To restore the part to the bent state, click Fold Metal, Fold.
or Insert, Sheet
The Fold PropertyManager appears. 6.
In the graphics area: a.
Select a face as the fixed face. The selected face appears in the Fixed face
b.
box.
Select the bend you want to fold. - or Click Collect All Bends to fold all bends. The selected bends appear in the Bends to fold
7.
Click OK
.
The selected bends fold.
15-34
box.
Normal Cut When adding a cut to a folded sheet metal part, you can select the Normal cut check box to ensure that the cut is created normal to the sheet metal thickness. The Normal cut check box is selected by default for sheet metal features, and is located in the Cut-Extrude PropertyManager. The effect of a Normal cut is illustrated below:
Sketch for cut
Without Normal cut
With Normal cut
Break Corner/Corner-Trim The Break Corner tool cuts away material from a folded sheet metal part on an edge or a face. The Corner-Trim tool cuts material away from a flattened sheet metal part on an edge or a face. If you use the Corner-Trim tool when your sheet metal part is in Flattened suppresses the feature when the part is folded.
mode, the SolidWorks software
To create a break corner or corner-trim on a sheet metal part:
1.
Create a sheet metal part.
2.
Click Break-Corner/Corner-Trim Corner.
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Break
The Break Corner PropertyManager appears. If the part is flattened, the Corner-Trim PropertyManager appears. 3.
Under Break Corner Options select from: •
Corner Edges and/or Flange Faces . In the graphics area, click the corner edges or flange faces to break. You can select corner edges, flange faces, or both. A preview of the break corner appears in the graphics area. The preview is not an exact representation of the geometry.
•
Preview of Break Corner/Corner-Trim
Internal corners only (flattened sheet metal parts only). Applies a corner trim to internal corners, as shown.
Preview of internal corners
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Chapter 15 Sheet Metal
4.
•
Break type. Click Chamfer
•
Distance
•
Radius
(straight edges) or Fillet
(round edges).
. Set a value for the chamfer distance. . Set a value for the fillet radius.
Under Relief Options (flattened sheet metal parts only) select from: •
Corner edges cuts.
. In the graphics area, click the corner edges to which you want to apply relief
A preview of the relief cuts appears in the graphics area. The preview is not an exact representation of the geometry. •
Relief type. Select a relief type to apply to the corner edge. If you select Circular or Bend Waist, set the Radius
5.
Click OK
. If you select Square, set the Side length
.
.
The selected corners are broken.
Chamfered break corners
Filleted break corners
example of corner edge Jog The Jog tool adds material to a sheet metal part by creating two bends from a sketched line. Some additional items to note about the Jog tool:
15-36
•
The sketch must contain only one line.
•
The line does not need to be horizontal or vertical.
•
The bend line does not have to be the exact length of the faces you are bending.
To create a jog feature on a sheet metal part:
1.
Sketch a line on the face of a sheet metal part where you want to create the jog. Alternatively, you can select the Jog feature before you create a sketch (but after you select a plane). When you select the Jog feature, a sketch opens on the plane.
2.
Click Jog on the Sheet Metal toolbar, or click Insert, Sheet Metal, Jog.
3.
In the graphics area, select a face for Fixed Face
4.
Under Selections, to edit the bend radius, clear Use default radius, and type a new value for Bend Radius
.
.
5.
6.
Under Jog Offset: •
Select an item in End Condition.
•
Set a value for Offset Distance
•
Select a Dimension position: Outside Offset
•
. Select Fix projected length if you want the face of the jog to stay the same length.
Under Jog Position, select: Bend Centerline Bend Outside
. , Inside Offset
, Material Inside
, or Overall Dimension
, Material Outside
, or
.
7. 8.
Set a value for Jog Angle . To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value.
9.
Click OK
.
Example of Fixed Projected Length In this example, the original length of the tab is preserved if you select the Fix projected length check box. If you clear the Fix projected length check box, no material is added to the tab to make the jog.
Original part
SolidWorks 2004 Reference Guide
Fix projected length selected
Fix projected length cleared
15-37
Chapter 15 Sheet Metal
Lofted Bend You can create a lofted bend in sheet metal parts. A lofted bend, similar to a loft feature, uses two sketches that are connected by a loft. The Base-Flange feature is not used with the Lofted Bend feature. Example of a Lofted Bend
Begin with two open profile sketches.
Use Lofted Bends to create a solid feature.
Lofted bend is complete.
The SolidWorks software contains several pre-made sheet metal parts created with lofted bends. These parts are located in\data\Palette Parts\sheetmetal\lofted bends. NOTES: •
When a lofted bend is represented with a lofted surface (B-spline), as is created by a square to circle profile, it cannot use K-Factor or Bend Allowance in the sheet metal calculations.
•
When a lofted bend is represented as a conical or cylindrical bend, such as a loft between concentric circular arcs, then it behaves in the same way as a cylindrical or conical bend in that it uses K-Factor or Bend Allowance to calculate the bends.
•
Lofted bends cannot be mirrored.
To create a lofted bend:
1.
Create two separate open profile sketches. Both sketches must conform to the following: • • •
The sketches must be open profiles. The profile openings should be aligned for flat-pattern accuracy. The sketches cannot have sharp edges.
2.
Click Lofted Bend on the Sheet Metal toolbar, or click Insert, Sheet Metal, Lofted Bends.
3.
In the graphics area, select both sketches. Make sure to select the points from which you want the path of the loft to travel. The sketch names appear under Profiles PropertyManager.
15-38
in the
4.
Examine the path preview. If necessary, click Move Up or Move Down to adjust the order of the profiles, or re-select the sketches to connect different points on the profiles.
5.
Set the Thickness for the sheet metal part.
6.
Click Reverse Direction
7.
Click OK
, if necessary.
.
Bend Deviation When you create a lofted bend, you can examine the surface area and curve lengths of the bend. These items are located in the Bend Deviation PropertyManager. To examine bend deviation:
1.
In the FeatureManager design tree: •
Right-click Flat-Pattern1 and select Unsuppress.
•
Click
•
Right-click Flatten-1, and select Bend Deviation.
to expand Flat-Pattern1.
The graphics area callouts display the bend deviation values for each edge. The bend deviation plane for the Bend Surface Area is the plane or face where the sketch is located. For example, if the material is extruded toward the inside of the model, bend deviation is measured from the outside face. The Bend Deviation PropertyManager appears, and displays the following: •
Under Bend Surface Area: o
Folded. Surface area of the lofted bend when in the folded state.
o
Flat. Surface area of the lofted bend when in the flattened state.
o
Deviation. Flat value minus the Folded value.
o
•
Under Curve Lengths: o
2.
Click OK
SolidWorks 2004 Reference Guide
Percentage change (%). Deviation value divided by the Folded value, multiplied by 100. Max deviation only. When selected, this shows the maximum deviation of the curve only.
.
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Chapter 15 Sheet Metal
Creating Sheet Metal Parts with Cylindrical Faces Parts with cylindrical faces can be made of sheet metal if they meet the following criteria: •
Any adjacent planar and cylindrical faces must be tangent.
•
At least one end face of any cylindrical face must have at least one linear edge.
To create a sheet metal part with cylindrical faces:
1.
Sketch an open contour arc. The arc can also be tangent to a line.
2.
Click Base-Flange/Tab
or Insert, Sheet Metal, Base Flange.
The Base Flange PropertyManager appears. 3.
4.
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Under Direction 1: •
Select an End Condition from the list.
•
Set the Depth
.
Under Sheet Metal Parameters: •
Set the Thickness
.
•
If necessary, select the Reverse direction check box to extend the feature in the opposite direction from that shown in the preview.
•
Set the Bend Radius
.
5.
Under Bend Allowance, select from the following bend allowance options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
6.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
7.
If you want relief cuts added automatically, select the Auto Relief check box, then choose the type of relief cut. If you choose Rectangular or Obround, then you must specify a Relief Ratio. NOTE: The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
8.
Click OK
.
The cylinder is now a sheet metal part.
NOTE: Only parts with exact analytic cylindrical faces can be unfolded. As a test, try to insert an axis on the cylindrical face. If you can insert an axis, the model is an exact cylinder. If you cannot insert an axis, then the model is not an exact cylinder and cannot be unfolded. However, sheet metal parts created with the Lofted Bends feature avoid this limitation and unfold appropriately. Creating Drawings of Sheet Metal Parts When you create a drawing of your sheet metal part, a flat pattern is automatically created. Drawings of sheet metal parts can also contain views of the bent sheet metal part. To create a drawing of a flat pattern:
1.
Open a new drawing.
2.
In the Model View PropertyManager, under Part/Assembly to Insert, select an item in Open documents, or click Browse to locate a sheet metal part. If the PropertyManager does not appear, click Model View Insert, Drawing View, Model.
3.
Click Next
4.
Under Orientation, select Flat Pattern in View Orientation
5.
Click in the drawing to place the view.
on the Drawing toolbar, or click
. .
A flat pattern configuration is created automatically with the bend lines visible. The bend region lines are not shown. 6.
Click OK
.
If you want to toggle the suppression of additional features in a flat pattern, create a part configuration of a flat pattern, then select a drawing view for it. To toggle the visibility of the bend lines in a flat pattern view:
1.
In the drawing window, expand Drawing View in the FeatureManager design tree to show the Flat-Pattern feature. Expand the Flat-Pattern feature.
2.
Right-click Bend-Lines and select Show or Hide.
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Chapter 15 Sheet Metal
To toggle the visibility of the bend region lines in a flat pattern view:
1.
Right-click the drawing view in the drawing sheet.
2.
Select Tangent Edge, Tangent Edges Visible or Tangent Edges Removed. - or Select Tangent Edge, Tangent Edges With Font to show bend region lines in the specified document Line Font. If the bend region lines do not appear, go back to the part window and right-click Flat-Pattern in the FeatureManager design tree. Select Edit Feature, and clear Merge faces. You may have to rebuild the drawing to see the tangent edges.
Flat Pattern The Flat-Pattern1 feature is intended to be the last feature in the folded sheet metal part. All features before Flat-Pattern1 in the FeatureManager design tree appear in both the folded and flattened sheet metal part. All features after Flat-Pattern1 appear only in the flattened sheet metal part. Some items to note about the flat-pattern feature: •
New features in folded part. When Flat-Pattern1 is suppressed, all features that you add to the part automatically appear before this feature in the FeatureManager design tree.
•
New features in flattened part. You flatten the entire sheet metal part by unsuppressing Flat-Pattern1. To add features to the flattened sheet metal part, you must first unsuppress Flat-Pattern1.
•
Reorder features. You cannot reorder sheet metal features to go below Flat-Pattern1 in the FeatureManager design tree. So, you cannot order a cut with the Normal cut option underneath Flat-Pattern1.
•
Modify parameters. You can modify the parameters of Flat-Pattern1 to control how the part bends, to enable or disable corner options, and to control the visibility of the bend region in the flattened sheet metal part.
To modify the parameters of the Flat-Pattern1 feature:
1.
Right-click Flat-Pattern1 in the FeatureManager design tree, and select Edit Feature.
2.
In the PropertyManager, under Parameters: •
In the graphics area, select a face that does not move as a result of the feature for Fixed face
•
Select Merge faces to merge faces that are planar and coincident in the flat pattern.
.
When selected, no lines are shown in the bend regions. • 3.
Select Simplify bends to straighten curved edges in the flat pattern.
Under Corner Options: •
Select Corner Treatment to apply smooth edges in the flat pattern.
•
Select Add Corner-Trim to apply relief cuts in the flat pattern. When selected, you can choose from: o
Break corners. Cuts away material from an edge or a face. Click Chamfer
o
as the Break type and set the Distance or Radius Relief type. Sets the relief type for any relief cuts needed.
o
Radius or Side length. Set the Radius
15-42
Click OK
.
or Side length for the Relief type.
Ratio to thickness. Sets the relief type radius to a specified ratio of the sheet metal thickness. When selected, set the Ratio of radius/distance to sheet metal thickness.
o
4.
or Fillet
.
Merge Faces When you select the Merge faces check box, no lines are shown in bend regions of the flat pattern. Here is an example of merged faces:
Merge faces selected
Merge faces not selected
Simplify Bends When you select the Simplify bends check box, curves are straightened out in the flat pattern. When this option is not selected, complex edges remain in the flat pattern. Here is an example of simplified bends:
Simplify bends selected
Simplify bends not selected
Corner Treatment When you flatten a sheet metal part by unsuppressing the Flat-Pattern feature, corner treatments are automatically applied to create a clean, flattened sheet metal part. The corner treatments are applied so the flat pattern is correct for manufacturing. To turn off corner treatments, right-click Flat-Pattern1, and select Edit Feature. In the PropertyManager, clear Corner Treatment. Here is an example of corner treatments:
Model with a miter flange
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Chapter 15 Sheet Metal
Flattened model without a corner treatment (using the Unfold
Flattened model with a corner treatment
feature)
Add Corner-Trim
Circular relief type
Square relief type
Bend waist relief type
Creating a Sheet Metal Flat Pattern Configuration You can create a configuration in a sheet metal part that shows the flattened part. To ensure that all features are shown in a flat pattern, you should create the flat pattern configuration after the entire design pattern of the part is complete. To create a flat pattern configuration:
1.
In a sheet metal part, create a new configuration.
2.
In the FeatureManager design tree: Right-click Flat-Pattern and select Unsuppress. - or Select Process-Bends and all of the features after it. Click Edit, Suppress, This Configuration to suppress all of the selected features.
15-44
Unfold/Fold With the Unfold and Fold tools, you can flatten and bend one, more than one, or all of the bends in a sheet metal part. This combination is useful when adding a cut across a bend. First, add an Unfold feature to flatten the bend. Next, add your cut. Lastly, add a Fold feature to return the bend to its folded state. For faster system performance, unfold and fold only the bends that you need for the task that you are performing. To add an Unfold feature:
1.
In a sheet metal part, click Unfold
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Unfold.
2.
In the graphics area, select a face that does not move as a result of the feature for Fixed face
3.
Select one or more bends as the Bends to unfold appropriate bends in the part.
4.
Click OK . The selected bends unfold.
.
, or click Collect All Bends to select all the
To add a Fold feature:
1.
In a sheet metal part, click Fold
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Fold.
2.
In the graphics area, select a face that does not move as a result of the feature for Fixed face
3.
Select one or more bends as the Bends to fold bends in the part.
4.
Click OK
.
, or click Collect All Bends to select all the appropriate
.
The selected bends fold.
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Chapter 15 Sheet Metal
15-46
16 Weldments
Weldments Toolbar The Weldments toolbar provides tools for creating weldment parts. Weldment Structural Member Gusset End Cap Fillet Bead Trim/Extend
Weldments - Structural Members When you add the first structural member to an existing layout sketch, adding the structural member defines the model as weldment feature. The weldment feature sets up a design functionality environment. It is not a feature in the same context as a fillet is a feature in the SolidWorks environment. When you insert a weldment feature, it activates the multibody environment by clearing the Merge result check box in the PropertyManager of features that add material. The weldment feature also acts as a placeholder for common custom properties that are inherited by all cut list items. All structural members include the following attributes: •
Structural members use profiles, for example an angle iron.
•
Profiles are identified by Type, Size, and Standard (iso and ansi inch). Each profile Type includes multiple sizes.
•
Structural members can include multiple segments, but all segments can use only one profile.
•
Multiple structural members, each with a different profile, can belong to the same weldment part.
•
Two structural members can only share a single point.
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Chapter 16 Weldments
Structural Member1
Structural Member2
You need to create a new structural member to add the vertical structural members to the top square structure. •
Structural members appear in the FeatureManager design tree as Structural Member1, Structural Member2, and so on. Bodies created by the structural members appear under Solid Bodies
.
•
You can create your own profiles (Type, Size, and Standard), and add them to the existing library of weldment profiles.
•
Weldment profiles are located in:\data\weldment profiles.
•
Structural members allow you to specify the pierce point of the profile, relative to the sketch segment used to create the structural member.
•
You can select structural members under Solid Bodies
, and create cut lists used in drawings.
To add structural members:
1.
Create a sketch.
Using linear sketch entities, you can create multiple 2D sketches with planes, create a 3D sketch, or combine 2D and 3D sketches.
16-2
2.
Click Structural Member
on the Weldments toolbar, or click Insert, Weldments, Structural Member.
3. 4.
To add multiple structural members, in the PropertyManager, click Keep Visible In the PropertyManager, under Selections:
.
•
Click in Standard and select iso or ansi inch.
•
Click in Type and select a Profile Type.
•
Click in Size and select a Profile.
•
To create the first structural member, select the first set of linear sketch entities in the graphics area as the Path segments.
As you select the structural members, Settings appears. Under Settings you can: •
Apply a corner treatment, or clear Apply corner treatment to specify a corner treatment later. For example, you can apply the corner treatment when you trim the structural members. You can also modify the corner treatment, allowing you to specify multiple corner treatments per structural member.
5.
•
Change Rotation Angle so that the structural member turns by a set number of degrees relative to the adjacent structural member.
•
Click Locate Profile to change the pierce point between the adjacent structural members. The default pierce point is the sketch origin.
Click OK
.
This clears Path segments, and allows you to apply additional, consecutive structural members. 6.
Select the second set of structural members. If necessary, you can apply a different Standard, Type, and Size.
7.
Click OK
to clear the Path segments, and to create additional structural members.
Weldments - Pierce Points (Locate Profile) The pierce point defines the location of the profile, relative to the sketch segment used to create the structural member. The default pierce point is the sketch origin in the profile library feature part. Any vertex or sketch point specified in the library feature profile can also be used as a pierce point.
Same profile with three different pierce points selected.
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Chapter 16 Weldments
To change a pierce point:
1.
Open an existing weldment part with structural members.
2.
Select a structural member in the FeatureManager design tree, and click Edit Feature.
3.
In the PropertyManager, under Settings, click Locate Profile. The system zooms in to the appropriate area. The graphics area displays the intersection between the last profiles you joined, using the default pierce point.
4.
Select any of the pierce points on the profile, or a sketch point that you added.
5.
Click OK
Rectangular tube profile with 11 pierce points. The pierce point is located at the default.
.
Weldments - Corner Treatments
No corner treatment
End Miter
End Butt1
End Butt2
Weldments - Change Corner Treatment You can change the corner treatment between adjacent structural members. To change a corner treatment:
1.
Right-click a structural member in the FeatureManager design tree and select Edit Feature.
2.
Select any of the points where structural members intersect.
The intersection point changes.
16-4
3.
Click the corner you want to modify. The Corner treatment pop-up toolbar appears.
4.
Click the corner treatment you want to apply, and click
End Trim 5.
End Miter
Click OK
End Butt1
.
End Butt2
.
Weldments - Trim and Extend You can trim structural members with planar faces so they butt up correctly in the weldment part. •
To trim a structural member with a planar face, such as a square tube, select one structural member as the Bodies to be Trimmed and another structural member as the Trimming Boundary.
•
To trim a structural member with a non-planar face, such as a pipe, use other trim tools such as Extruded Cut
.
1 - Bodies to be Trimmed 2 - Trimming Boundary
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Chapter 16 Weldments
To trim structural members with planar faces:
1.
Click Trim/Extend
2.
In the PropertyManager, under Corner Type, select a corner type.
End Trim
on the Weldments toolbar, or click Insert, Weldments, Trim/Extend.
End Miter
End Butt1
End Butt2
3.
Under Bodies to be Trimmed, select a structural member in the graphics area for Bodies.
4.
Under Trimming Boundary: •
Click Planar Face or Bodies. Selecting Planar Face as the Trimming Boundary is normally more efficient and offers better performance.
•
5.
Select an adjacent structural member in the graphics area as Face/Bodies.
Click OK
.
You should trim all corners in a weldment model.
16-6
Weldments - Adding Gussets Gussets reinforce the area between two, intersecting structural members with planar faces. There are two types of gussets:
•
Triangular Profile Triangular Profile Under Supporting Faces: •
Select Faces
. Select adjacent planar faces from two intersecting structural members.
•
Flip Profile D1 and D2 Parameters Profile Distance2.
. Flip the values between Profile Distance1 and
Under Profile: Set a value for Profile Distance1, and for Profile Distance2. Thickness. Set a Gusset Thickness thickness (inner, both, or outer side).
Inner Side
Both Sides
, and specify a side to the
Outer Side
Under Parameters: Locate a profile relative to the left and right edges of the structural member. Or, specify an offset distance from the edge to locate the gusset.
Profile Locates at Start Point
Profile Locates at Mid Point
Profile Locates at End Point
All location profiles shown above use Inner Side thickness.
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Chapter 16 Weldments
•
Polygonal Profile Polygonal Profile Under Supporting Faces: •
Select Faces . Select adjacent planar faces from two, intersecting structural members.
•
Flip Profile D1 and D2 Parameters . Flip the values between Profile Distance1 and Profile Distance2. Under Profile: Set values for Profile Distance1, Profile Distance2 and Profile Distance3. Select d4 to set a value for Profile Distance4. d4 defines the distance between the structural member and the vertex. - or Click a to set Profile Angle. a defines the angle between the two edges in the polygon that are adjacent to the structural members. Thickness. Set Gusset Thickness thickness (inner, both, or outer side).
Inner Side
Both Sides
, and specify a side to the
Outer Side
Under Parameters: Locate a profile relative to the left and right edges of the structural member. Or, specify an offset distance from the edge to locate the gusset. Click Flip Offset Direction
Profile Locates at Start Point
to change the offset direction.
Profile Locates at Mid Point
All profile locations shown above use Inner Side thickness.
16-8
Profile Locates at End Point
To add gussets:
1.
Click Gusset
2.
To add multiple gussets, in the PropertyManager, click Keep Visible
3.
Under Supporting Faces, select two adjacent, planar faces for Select Faces.
4.
Under Profile, click Triangular Profile or Polygonal Profile. •
on the Weldments toolbar, or click Insert, Weldments, Gusset. .
Set values for the appropriate profile distances. - or With Polygonal Profile, click a to set a Profile Angle.
•
• 5.
o
Inner Side
o
Both Sides
o
Outer Side
Set a value for Gusset Thickness
.
Under Parameters, set values to locate the gusset profile: •
6.
Select where to apply gusset Thickness:
Select a profile location: o
Profile Locates at Start Point
.
o
Profile Locates at Mid Point
.
o
Profile Locates at End Point
.
•
If necessary, select Offset and set an Offset Value.
•
Flip Offset Direction
Click OK
SolidWorks 2004 Reference Guide
. Change the offset direction.
.
16-9
Chapter 16 Weldments
Weldments - Fillet Weld Beads You can add full length, intermittent, or staggered fillet weld beads between any intersecting weldment entities such as structural members, plate weldments, or gussets. To add fillet weld beads:
1.
Click Fillet Bead
2.
To add multiple fillet beads, in the PropertyManager, click Keep Visible
3.
Under Arrow Side: a.
on the Weldments toolbar, or click Insert, Weldments, Fillet Bead. .
Select a Bead type. .
Annotation: 4 - Bead size. Radius of the fillet bead 3 - Bead length. Length of each bead segment. Only with Intermittent or Staggered. 6 - Bead pitch. Distance between the start of each bead. Only with Intermittent or Staggered.
Full length
Intermittent
Staggered. Creates fillet bead on both the Arrow Side and the Other Side. b.
Set a value for Bead size
.
c.
For Intermittent or Staggered types, set a Bead length and a Bead pitch.
d.
Clear Tangent propagation if necessary. Although you must select planar faces for the face sets, fillet weld beads can follow non-planar, tangent contours when you select Tangent propagation.
e.
Select a face as Face Set1
Gusset face
16-10
.
Structural member face
f.
Click in Face Set2
, then select a second, intersecting face.
Structural member face
Plate weldment face
The system assigns Virtual edges based on your selections for Face Set1 and Face Set2 . A fillet weld bead preview appears along the edges between the intersecting faces. 4.
Click Other Side. If you selected Staggered as the Bead type, the Other Side is already displayed. With Staggered as the Bead Type, apply the fillet weld bead to the opposite side.
Staggered bead type a.
Select a Bead type.
Annotation: 4 - Bead size. Radius of the fillet bead 3 - Bead length. Length of each bead segment. Only with Intermittent or Staggered. 6 - Bead pitch. Distance between the start of each bead. Only with Intermittent or Staggered.
Full length
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Intermittent
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Chapter 16 Weldments
Staggered. Creates fillet bead on both the Arrow Side and the Other Side. b.
Set a value for the Fillet Size
c.
For Intermittent or Staggered types, set a Bead length and a Bead pitch.
d.
Select a second face as Face Set1
.
Gusset face
Structural member face
e.
Click in Face Set2
, and select the second, intersecting face for the Arrow Side.
Structural member face
Plate weldment face
The system assigns the Virtual edges based on your selections for Face Set1
and Face Set2
A fillet weld bead preview appears along the edges between the intersecting entities. 5.
Click OK
.
Fillet weld bead between structural member and gusset
16-12
Fillet weld bead between structural member and plate weldment
.
Weldments - End Caps End caps close off open structural members. You can add end caps only to profiles with linear edges. To add end caps:
1.
Click End Cap
on the Weldments toolbar, or click Insert, Weldments, End Cap.
2.
To add multiple end caps, in the PropertyManager, click Keep Visible
3.
Under Parameters: •
Select a profile face for Face
•
Set a value for Thickness
.
. .
You can apply end caps to different open structural members. The opening depends on the structural member and the corner treatment you applied.
Select Face
End cap preview 4.
Under Offset: a.
Click Use thickness ratio to specify the offset distance of the end cap as a ratio of the thickness of the structural member that is being capped.
b.
Set a value for Thickness ratio
(maximum is 1).
- or a.
Clear Use thickness ratio.
b.
Set a value for Offset distance
c.
Click Chamfer corners if you want to add a chamfer to the corners.
d.
Set a value for Chamfer Distance
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.
.
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Chapter 16 Weldments
5.
Click OK
.
Repeat steps 3 through 5 to cap any remaining open profiles.
Creating Sub-Weldments You create sub-weldments to segment complex weldment models into more manageable entities. After you create sub-weldments, you can create the cut lists used in drawings. Any changes made to a sub-weldment model are reflected in the weldment model from which you created the sub-weldment. Sub-weldments can include any entity listed in the Solid Bodies
folder, including structural members, end caps,
gussets, weld fillet beads, and structural members trimmed with the Trim/Extend
tool.
To create a sub-weldment:
1.
In the FeatureManager design tree of the weldment model, expand the Solid Bodies
2.
Select the entities to include in the sub-weldment, using Shift or Ctrl to group-select.
folder.
The selected entities highlight in the graphics area. 3.
Right-click and select Create sub-weldment. A sub-weldment folder
4.
containing the selected entities appears under the Solid Bodies
Right-click the sub-weldment
folder.
folder and select Save to File.
The sub-weldment model opens in a new SolidWorks window, and the Save As dialog box appears. 5.
Accept or edit the name for File name, and click Save.
Weldment Drawings Drawings of weldments support:
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•
Views of entire weldment parts
•
Views of single bodies of weldment parts (Relative Views)
•
Weldment cut lists
•
Balloons
•
AutoBalloons
•
Alternating crosshatch for section views
Example of Weldment Cut List
Balloons in Weldment Drawings All configurations reference the same cut list for creating balloons. Balloon numbers remain associative to the cut list, even if they are created in another view. A balloon attached to a body in a drawing view of the entire weldment and a balloon attached to the same body in a drawing view showing only the body have the same item number. If you insert a balloon into a drawing view of a weldment and the drawing does not contain a cut list, you are prompted whether you want to create a cut list. If you delete a cut list, all balloons related to the cut list change their Item Number to 1.
Weldment Cut Lists To insert a weldment cut list in a drawing, first create cut list items in the weldment part document. Cut lists are tables. Example To create cut list items:
1.
In a weldment part document, under Solid Bodies, select bodies or sub-weldments to be included in a cut list item. You can group similar bodies, and sub-weldments, into one cut list item.
2.
Right-click and select Create cut list item. The bodies become absorbed features of the cut list item. The cut list item displays an instance number, plus the number of its weldment items in parentheses. Only top level items (bodies and sub-weldments) are listed in the cut list.
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Chapter 16 Weldments
To delete cut list items:
Select the cut list item and press Delete. The cut list item is deleted and the bodies remain under Solid Bodies. To insert a weldment cut list into a drawing:
1. 2.
In a drawing, click Weldment Cut List Cut List. Select a drawing view.
on the Annotation toolbar, or click Insert, Tables, Weldment
3. 4.
Specify properties in the Weldment Cut List PropertyManager, then click OK . If you did not select Attach to anchor in the PropertyManager, click in the graphics area to place the cut list
Configurations Weldments have two default configurations: Default and Default , where Default is a user-specified name. Different sizes of the same weldment are handled by configurations. The top level (a particular size of the body) is an configuration. Underneath the top level is a derived state that is an configuration. Weldment cut lists are always based on the Welded State configuration. Custom Properties Weldment cut lists include the item number (ITEM NO.) and quantity (QTY.) and cut list custom properties. Custom properties for cut lists are different from custom properties at the document level. In weldment parts, properties are included with cut list items created from structural members with Feature Palette profiles: •
DESCRIPTION
•
LENGTH
You can add properties to the cut list items. To add custom properties to cut list items:
1.
In the part document, right-click a Cut-List-Item and select Properties.
2.
In the Cut-List-Item Custom Properties dialog box:
3.
•
Type a property name in Name.
•
Type text or a value in Value.
•
Click Add.
Repeat step 2 as necessary, the click OK.
Weldment Cut List PropertyManager Specify properties for weldment cut lists. Table Template Click Browse for template insertion. Table Anchor Set the Anchored corner to:
16-16
to choose a standard or custom template. This option is available only during table
Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. Configurations Cut lists are usually based on the Welded State configuration. Keep Missing Item If cut list items have been deleted from the weldment since the cut list was created, you can keep the items listed in the table. If missing items are kept, select Strikethrough to display text for the missing item with strikethrough formatting. Item Numbers Start at. The cut list starts with the number displayed. Do not change item number. Click for item numbers to remain with their rows when columns are sorted or reordered. Table Format Click to access the Table Format PropertyManager.
Weldment Cut List Column PropertyManager Specify the columns to be included in a weldment cut list and their position in the table. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To access the Column PropertyManager, click at the head of a column when the pointer changes to
.
Column Properties For the selected column, choose one of the following column types, listed with its header title. You can edit the header in the Title box below. •
Item number. ITEM NO. Data in the Item Number custom property for the cut list items populates the column.
•
Quantity. QTY. Data in the Quantity custom property for the cut list items populates the column.
•
Cut list item name. The name of the cut list item (Cut-List-Item1, for example) in the part document populates the column.
•
User defined. Edit in Title for the column header. Enter data into the column manually.
•
Cut list item property. Custom properties for cut list items in the part document. Select a property from the list below and edit text for the column header in Title. Properties such as DESCRIPTION and LENGTH are available automatically for bodies created through the Feature Palette. You can add other custom properties for cut list items.
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Chapter 16 Weldments
Properties. List of document's custom properties, available when you specify Cut list item property under Column Properties. Title. Edit the text of the column header. Column position. Click Move Column Left
or Move Column Right
to move the selected column.
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Weldment Cut List PropertyManager. Table Format Click to access the Table Format PropertyManager.
Custom Properties in Weldments In a weldment part, the custom properties for the weldments feature and for the cut list represent a different list from the custom properties that are stored at the document level. The list of optional custom property names is located: lang\\weldments\weldmentproperties.txt. The profile library parts may carry any commonly used custom properties. For example, profiles supplied with the SolidWorks application include the custom property Description. In case of naming conflicts between the weldment feature and the weldment profile, the profile name takes precedence. Assign Custom Properties You can assign custom properties from three different sources: •
Profile sketch: Assign to the profile sketch any commonly used properties that are unique to the profile, and that you want inherited by the cut list item corresponding to a structural member feature. Description is such an example.
•
Weldment feature. Properties assigned to the weldment feature are propagated to all cut list items. This capability enables you to assign a property with a default value, which you can later edit for each cut list item. For example, you can add the Property Cost with a value in the appropriate monetary denomination.
•
Cut-List-Items . Cut list items inherit custom properties from the profile sketch and from the weldment feature. You can assign new properties or you can edit existing properties. For example, you can add the property Weight, and link that property to the model's mass properties. Creating the link between the two enables the SolidWorks application to calculate the weight of the first solid body in the cut list item. The system also computes and adds the property LENGTH for bodies generated by structural member features. The LENGTH property is not editable. Since the weight of only the first item is calculated from the cut list, the cut list should only include identical items.
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Custom Property Values Values that you assign as custom properties can be •
Constant. For example, the material assigned when creating the structural member profile.
•
Derived. o
Linked to dimension values.
o
Linked to mass properties.
Custom properties are required to generate a cut list with associative balloons for a multibody part. To add custom properties:
1.
Under Solid Bodies
, right-click a Cut-List-Item, and select Properties.
- or To assign custom properties at the highest propagation level, right-click the Weldment 2.
feature.
In the dialog box: a.
To assign a new name, type a value for Name, -or To assign an existing name, select one from the Name list.
b.
Select an item in Type.
c.
Type a value that is compatible with Type for Value. - or Select an item in Linked to value to associate the Value.
3. Click OK. The custom property is added.
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Chapter 16 Weldments
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17 SolidWorks Options
Overview of SolidWorks Options Customize functionality to suit your needs. Click Tools, Options to display system options and document property settings. Options Dialog Box Structure The SolidWorks Options dialog box structure emphasizes the difference between system options and document properties. The Options dialog box has two tabs: •
System Options. The system options are stored in the registry and are not part of the documents. Therefore, these changes affect all documents, current and future.
•
Document Properties. The document properties apply only to the current document, and the Document Properties tab is available only when a document is open. New documents get their document settings (such as Units, Image Quality, and so on) from the document properties of the template used to create the document. Use the Document Properties tab when you set up document templates.
The options listed on each tab are displayed in tree format on the left side of the dialog box. As you click an item in the tree, the options for the item appear on the right side of the dialog box. The title bar displays the title of the tab and the title of the options page. To access the Options dialog box:
You can access the Options dialog box in any of the following ways: •
Click Tools, Options. The Options dialog box appears with the System Options tab active.
•
Right-click in the FeatureManager design tree area and select Document Properties. (There must be no items selected in the FeatureManager design tree or graphics area in order to select Document Properties.) The Options dialog box appears with the Document Properties tab active.
•
Click Grid/Snap on the Sketch toolbar. The Options dialog box appears with the Grid/Snap page of the Document Properties tab active.
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Chapter 17 SolidWorks Options
System Options General System Options Lets you change general system options such as enabling the performance email option, the Confirmation Corner, and so on. To set general system options:
1.
Click Tools, Options, System Options, General.
2.
Select from the options described below.
3.
Click OK. •
Open last used document(s) at startup. Select Always or Never. Select Always if you want the documents that you used most recently to open automatically when you start the SolidWorks software.
•
Input dimension value. Specifies that the Modify dialog box is automatically displayed for the input of a new dimension value. Otherwise, you must double-click the dimension to change the value.
•
Single command per pick. Specifies that sketch and dimension tools clear after each use. (Double-clicking a tool causes it to remain selected for additional use.)
•
Show dimension names. Displays the dimension’s name as well as its value.
•
Show errors every rebuild. Displays an error message each time you rebuild the model, if errors are present.
•
Maximize document on open. Opens each document to its largest size within the SolidWorks window.
•
Use shaded face highlighting. Displays selected faces in a solid color (green by default). To specify a different highlight color, click Tools, Options, System Options, Colors, then select a different color for Selected Face, Shaded. Some third-party applications may require that you clear this option.
•
Show thumbnail graphics in Windows Explorer. Displays a thumbnail graphic instead of an icon in Windows Explorer for each SolidWorks part or assembly document. The graphic is based on the view orientation of the model when the document was last saved. A palette of 16 colors is used; if the model uses a color that is not available, a similar color is substituted. The thumbnail graphics are also used in the Open and Save As dialog boxes. If you do not see thumbnail graphics in the Open or Save As dialog boxes, you may have to open, then save your documents. When you re-open these dialog boxes, you will see the thumbnail graphics.
•
Use system separator for dimensions. Specifies that the default system decimal separator is used when displaying decimal numbers. o o
•
To set the system default, use the Windows Control Panel. To set a decimal separator different from the system default, clear the option, and type a symbol that you want to use (usually a period or a comma).
Use English language menus. If you specified the use of another language when installing the SolidWorks software, and the regional options in the Windows Control Panel are set to that language, select this option to change menus to English. You must exit and re-start SolidWorks for this change to take place.
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•
Use English language feature and file names. Displays feature names in the FeatureManager design tree and automatically created file names in English. Existing feature and file names in a foreign language do not update when you select this option. This option is available when: o o
Use English language menus is cleared. You are running the SolidWorks software on a foreign language operating system and you installed SolidWorks for that foreign language.
•
Enable performance email. Turns on and off the sending of email to SolidWorks Corporation regarding the performance and usage of the software.
•
Enable Confirmation Corner. Displays the Confirmation Corner in the upper right corner of the graphics area.
•
Auto-show PropertyManager. Displays the PropertyManager automatically. For example, if you edit a sketch and select a sketch feature to edit, the PropertyManager for the selected sketch feature appears automatically.
•
Save eDrawings data in SolidWorks document. Saves the SolidWorks document with eDrawings data so you can open the SolidWorks document in the eDrawings Viewer. If you select Save eDrawings data in SolidWorks document, you can override this option when you save your document. To override this option, click File, Save As, and clear Save eDrawing data.
•
Notify if SNL could not be obtained for eDrawings Save. Select if: You use SolidWorks Office and have a SolidNetWork License (SNL). If you save an eDrawings file, but there are no SolidWorks Office licenses available in SNL, you cannot save the eDrawings file as review-enabled. You can still save the file; however, it will not be review-enabled. It is helpful to have Notify if SNL could not be obtained for eDrawings Save selected so you know if the eDrawings file will be review-enabled. Your company may have several SolidWorks and SolidWorks Office licenses. If you use SolidWorks (not SolidWorks Office), and you save an eDrawings file, SNL searches for an available SolidWorks Office license so that you can save the file as review-enabled. Clear if: You use SolidWorks (not SolidWorks Office) and have a SolidNetWork License (SNL). If you use eDrawings without a SolidWorks Office license, eDrawings files are not saved as review-enabled. The notification message appears each time you save the eDrawings file unless Notify if SNL could not be obtained for eDrawings Save is cleared.
•
Custom property used as component description. Set or type a name to define a custom description label. For example, the Open dialog box has a Description label that displays the model description. Instead of displaying the Description label, you can display a label that you specify. If you change the Custom property used as component description in a document that has already been saved, you must manually add the new description to the Summary Information dialog box.
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Chapter 17 SolidWorks Options
Drawings Options You can set options for all drawings. To set options for drawings:
1.
Click Tools, Options, System Options, Drawings.
2.
Choose from the following options, then click OK.
Automatic placement of inserted dimensions from model. When selected, specifies that inserted dimensions are automatically placed at an appropriate distance from the geometry in the view. Display drawing view borders. When selected (the default), displays borders around individual drawing views. Automatically scale new drawing views. New drawing views are scaled to fit the drawing sheet, regardless of the paper size selected. Show contents while dragging drawing view. When selected, the model is displayed as you drag a view. When cleared, only the view boundary is shown while dragging. (Similar to Show window contents while dragging in Microsoft Windows.) Smooth dynamic motion of drawing view. When selected (the default), dynamic operations to drawings such as panning and zooming display smoothly. In most cases, keep the default. For some combinations of drawing size (small drawings in particular), graphics card, and system performance, operations such as panning and zooming may cause slower display performance. In such cases only, clear the Smooth dynamic motion of drawing view check box. Dynamic drawing view activation. When selected, the view closest to the pointer is activated automatically. To stop the dynamic activation temporarily, you can lock a view or the sheet. Right-click the view or sheet, and select Lock View Focus or Lock Sheet Focus. Right-click again, and select Unlock View Focus (or double-click another view) or Unlock Sheet Focus (or double-click any view) to return to dynamic mode. When cleared, double-click a drawing view to activate it, or right-click the view and select Activate View. To activate the sheet, double-click a blank area of the sheet or right-click the sheet and select Activate Sheet. Display new detail circles as circles. When selected, new profiles for detail views appear as circles. When cleared, the sketched profiles appear. Select hidden entities. When selected, you can select hidden (removed) tangent edges and edges that you have hidden manually. When you pass the pointer over hidden edges, the edges appear in phantom line font. Eliminate duplicate model dimensions on insert. When selected (the default), duplicate dimensions are not inserted into drawings when model dimensions are inserted. This option setting becomes the default setting for Eliminate duplicate model dimensions in the Insert Model Items dialog box. Allow auto-update when opening drawings. When selected, drawing views update automatically as the drawing document opens. Detail item snapping when dragging corner. When you click a corner and drag a detail item (for example, a note or dimension), the corner you clicked can infer to the corners of stationary detail items, and vice versa. Detail item snapping when dragging center. When you click the inside of a detail item (a note or dimension) and drag it, the center can infer to the center of stationary detail items, and vice versa. Print out-of-sync watermark. When selected, a watermark, SolidWorks Detached - Out-of-Sync Print, is printed on detached drawing printouts if the drawing is not synchronized with the model. Show Reference Geometry names in drawing. If selected, when reference geometry entities are imported into a drawing, their names appear. Automatically hide components on view creation. If selected, any components of an assembly not visible in a new drawing view are hidden and listed on the Hide/Show Components tab of the Drawing View Properties dialog box. The components are present, and all component information is loaded. The component names are transparent in the FeatureManager design tree. Display sketch arc centerpoints. When selected, sketch arc centerpoints are displayed in drawings.
17-4
Display sketch entity points. When selected, the endpoints of sketch entities are displayed as filled circles in drawing sheets and drawing sheet formats, but not in drawing views. Save tessellated data for drawings with shaded and draft quality views. If cleared, file size is reduced by not saving tessellated data in drawing documents with shaded and draft quality views. If needed, the data is read from the model file. In view-only mode and in eDrawings, nothing appears in the drawing view. For drawings with high quality and other display types, tessellated data is not used, so file size cannot be reduced. Print out-of-date drawing views with crosshatch. Specifies what happens when you Print (or Print Preview) a drawing that contains out-of-date views, with Automatic view update cleared. (If Automatic view update is selected, the views update automatically, and the crosshatch is removed whenever you print the drawing.) •
Prompt (default). Notifies you if the drawing contains out-of-date views, and asks how to proceed. When the dialog box appears, click Yes to print the drawing with crosshatch on the out-of-date views, or click No to print the drawing without crosshatch.
•
Always. The printed drawing always includes crosshatch on out-of-date views.
•
Never. The printed drawing never includes crosshatch on out-of-date views.
Detail view scaling. Specifies the scaling for detail views. The scale is relative to the scale of the drawing view from which the detail view is generated. Custom property used as Revision. Specify a document custom property to be regarded as the revision data when checking a document into PDMWorks (a SolidWorks Office Professional product).
Display Style Options You can set options for the default display of edges in all drawing documents. NOTE: The specified display types apply to new drawing views, except for new views created from existing views. If you create a new view from an existing view (a projected view, for example), the new view uses the display settings of the source view. To set the default display of edges in drawing documents:
1.
Click Tools, Options, System Options, Default Display Type.
2.
Choose from the following options, then click OK.
Default display for new drawing views Specifies the way parts or assemblies appear in drawings: •
Wireframe - All edges appear.
•
Hidden lines visible - Displays visible edges as specified in Line Font Options; displays hidden edges in gray.
•
Hidden lines removed - Displays only edges that are visible at the chosen angle; obscured lines are removed.
•
Shaded with edges - Parts appear in shaded mode with edges that would appear in Hidden lines removed mode displayed. You can specify a color for the edges, and set whether to use the specified color or a color slightly darker than the model color in the System Colors Options.
•
Shaded - Parts appear in shaded mode.
Display quality for new views •
High quality - model resolved.
•
Draft quality - model lightweight, used for faster performance with large assemblies.
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Chapter 17 SolidWorks Options
Default display of tangent edges in new drawing views If you selected Hidden lines visible or Hidden lines removed, select one of the following modes for viewing tangent edges (the transition edges between rounded or filleted faces): •
Visible - A solid line.
•
Use font - A line using the default font for tangent edges defined in Tools, Options, Document Properties, Line Font. (You must have a drawing document active to access this option.)
•
Removed - Not displayed.
Area Hatch/Fill Options You can set the hatch or fill options for any area hatch that you apply to a face or to a closed loop of a sketch entity in a drawing. To set area hatch options for all documents:
1.
Click Tools, Options, System Options, Area Hatch/Fill.
2.
Select from the options described below. The pattern is displayed in the preview window.
3.
Click OK.
Type of hatch or fill. Choose None, Solid, or Hatch. The subsequent options are available only for Hatch. The default color of the solid fill is black. You can change the color of the fill by selecting the area hatch in the graphics area and clicking Line Color on the Line Format toolbar. Pattern. Select a crosshatch pattern from the Pattern list. Scale. Type a scale value. Angle. Type an angle in degrees.
System Colors Lets you set the system defaults for colors used in drawings, assemblies, sketches, grid lines, background colors, and so on. You can also change the color scheme of the FeatureManager design tree or change the skin displayed in the PropertyManager. To set system colors:
1.
Click Tools, Options, System Options, Colors.
2.
Select from the options described below.
3.
Click OK.
System colors Displays a list of colors used for sketches, highlighting, and so on. Select an item in System colors, then click Edit to change the color. •
PropertyManager Color. Sets the background color for the PropertyManager.
•
PropertyManager Skin. Sets the background skin (image) for the PropertyManager. Skins take precedence over a color scheme in the PropertyManager. If you want the same color from the PropertyManager Color box to appear in the PropertyManager, set PropertyManager Skin to None.
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•
Reset All To Defaults. Resets all system colors back to the system default values.
•
Save As Scheme. Saves the set of colors you defined for the SolidWorks display. After you save a color scheme, you can select it from the Current Color Scheme list.
Additional Options •
Current Color Scheme. Displays the color scheme applied to the SolidWorks software. If you define a color scheme by saving your color choices with Save As Scheme, the color scheme appears in this list. Click Delete to delete a color scheme. After you click Delete, the path is gone. Click Cancel to undo the deletion, if necessary.
•
Use gradient background. Displays a gradient background for SolidWorks documents. Set System colors to Top Gradient Color or Bottom Gradient Color, then specify a color.
•
Match graphics area and FeatureManager backgrounds. Applies the same background color to the graphics area and FeatureManager design tree.
•
Use specified color for Shaded With Edges mode. Applies the specified color to model edges when the model is in Shaded With Edges mode. Set System colors to Edges in Shaded With Edges Mode, then specify a color. If you clear this option, the edges are slightly darker than the model color.
•
Use specified colors when editing parts in assemblies. Applies the specified color to the faces, features, and bodies of a part while it is being edited in an assembly. Set System colors to Assembly, Edit Part, then specify a color.
•
Go To Document Colors (parts and assemblies only). Opens the Document Properties - Colors dialog box to set document-specific colors.
Sketch Options Lets you set the default system options for sketching. To set the default sketching options:
1.
Click Tools, Options, System Options, Sketch.
2.
Select from the following options, then click OK. •
Use fully defined sketches. Requires sketches to be fully defined before they are used to create features.
•
Display arc centerpoints in part/assembly sketches. Displays arc centerpoints in sketches.
•
Display entity points in part/assembly sketches. Displays endpoints of sketch entities as filled circles. The color of the circle indicates the status of the sketch entity: Black = Fully defined Blue = Under defined Red = Over defined Green = Selected Over defined and dangling points are always displayed, regardless of this option.
•
Infer from model. Displays inferencing lines that relate to the lines and vertices of the underlying model when you are sketching on the face of an extruded part.
•
Prompt to close sketch. Displays a dialog box with the question, Close Sketch With Model Edges? if you create a sketch with an open profile, then click Extruded Boss/Base to create a boss feature. Use the model edges to close the sketch profile and select the direction in which to close the sketch.
•
Create sketch on new part. Opens a new part with an active sketch on the Front Plane.
•
Override Dims on Drag/Move. Overrides dimensions when you drag sketch entities or move the sketch entity in the Move or Copy PropertyManager. The dimension updates after the drag is complete. This option is also available in Tools, Sketch Settings, Override Dims on Drag/Move.
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Chapter 17 SolidWorks Options
•
Automatic relations. Automatically creates geometric relations as you add sketch elements. This option is also available in Tools, Sketch Settings, Automatic Relations.
•
Display plane when shaded. Displays the sketch plane when you edit a sketch in Shaded With Edges or Shaded mode. If the display is slow due to the shaded plane, it may be because of the Transparency options. With some graphics cards, the display speed improves if you use low transparency. To set a low transparency, click Tools, Options, System Options, Performance and clear High quality for normal view mode and High quality for dynamic view mode.
•
Display virtual sharps. Creates a sketch point at the virtual intersection point of two sketch entities. Dimensions and relations to the virtual intersection point are retained even if the actual intersection no longer exists, such as when a corner is removed by a sketched fillet or a sketched chamfer. (To set the display options for virtual sharps, click Tools, Options, Document Properties, Virtual Sharps.)
•
Over defining dimensions: o
o
Prompt to set driven state. Displays a dialog box with the question, Make Dimension Driven? when you add an over defining dimension to a sketch. Set driven by default. Sets the dimension to be driven by default when you add an over defining dimension to a sketch. Use Prompt to set driven state alone or with Set driven by default. Depending on your selections, one of four actions occur when you add an over defining dimension to a sketch: •
A dialog box appears that defaults to driven.
•
A dialog box appears that defaults to driving.
•
The dimension is driven.
•
The dimension is driving.
Display and Selection Options Lets you set system default options for the display and selection of edges, planes, and so on. To set display and selection options:
1.
Click Tools, Options, System Options, Display/Selection.
2.
Select from the options described below.
3.
Click OK.
Hidden edges displayed as Solid or Dashed. Select either solid lines or dashed lines to specify how hidden edges are displayed in Hidden Lines Visible mode in part and assembly documents. Selection of hidden edges
17-8
•
Allow selection in wireframe and HLV modes. Allows you to select hidden edges or vertices in Wireframe and Hidden Lines Visible modes.
•
Allow selection in HLR and shaded modes. Allows you to select hidden edges or vertices in Hidden Lines Removed, Shaded With Edges, and Shaded modes.
Part/Assembly tangent edge display Controls how tangent edges are displayed when the model is in Hidden Lines Removed or Hidden Lines Visible mode. •
As visible. Tangent edges displayed.
•
As phantom. Tangent edges display using the Phantom style line font (
•
Removed. Tangent edges are not displayed.
).
Edge display in shaded with edges mode Specifies how edges are displayed when the model is in Shaded With Edges mode. •
HLR. Any edges that would appear in Hidden Lines Removed mode are displayed in Shaded With Edges mode also.
•
Wireframe. All edges are shown in Shaded With Edges mode (like Wireframe).
Assembly transparency for in context edit Controls the transparency options when you edit assembly components. •
Opaque assembly. All components become opaque gray, except for the component you are editing, which becomes opaque pink.
•
Maintain assembly transparency. All components remain in their current state, except for the one you are editing, which becomes opaque pink.
•
Force assembly transparency. All components become transparent except the one you are editing, which becomes opaque pink. Use the slider to adjust the transparency level for Force assembly transparency. Move the slider to the right to make components more transparent.
Highlight all edges of features selected in graphics view. Specifies that all edges on the selected feature are highlighted when you click it. Dynamic highlight from graphics view. Specifies whether model faces, edges, and vertices are highlighted when you move the pointer over a sketch, model, or drawing. Show open edges of surfaces in different color. Makes it easier to differentiate between the open edges of a surface and any tangent edges or silhouette edges. To specify the edge color, click Tools, Options, System Options, Colors. Select Surfaces, Open Edges in System colors. Anti-alias edges. Smooths out jagged edges in Shaded With Edges, Wireframe, Hidden Lines Removed, and Hidden Lines Visible modes. To specify the anti-alias edge color, click Tools, Options, System Options, Colors. Select Edges in Shaded With Edges Mode in System colors. You must also select Use specified color for Shaded With Edges mode to use the color you selected.
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Chapter 17 SolidWorks Options
Example of anti-alias edges.
Anti-alias option selected
Anti-alias option cleared
You can customize the color of the edges. If you do not specify a color, the edges are slightly lighter or darker than the model color. Display shaded planes. Displays transparent shaded planes with a wireframe edge that have different front and back colors. To specify the shaded plane colors, click Tools, Options, Document Properties, Plane Display. Under Faces, click Front Face Color or Back Face Color to change the colors. Use the slider to adjust the transparency level for the planes. Move the slider to the right to make the planes more transparent. Enable selection through transparency. When selected, you can select opaque objects behind transparent objects in the graphics area. When cleared, you can select the nearest object regardless of transparency. Press Shift when you select objects to temporarily override the option. Display reference triad. Displays a reference triad to help orient you when viewing models. The reference triad is for display purposes only; you cannot select it or use it as an inference point. To specify the triad colors, click Tools, Options, System Options, Colors. Select any of the three axes to change: X axis of Reference Triad, Y axis of Reference Triad, or Z axis of Reference Triad in System colors.
Performance Options Lets you set system options related to performance. Changes to these settings do not affect documents that are already open. They only affect documents that are opened after the setting has been changed. To set performance options:
1.
Click Tools, Options, System Options, Performance.
2.
Select from the options described below.
3.
Click OK.
Verification on rebuild Contols the level of error checking when you create or modify features. For most applications, the default setting (off) is adequate, and results in a faster rebuild of the model.
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Transparency High-quality transparency is similar to looking through clear glass. Low-quality transparency (the default) is similar to viewing an object through a mesh or screen. •
High quality for normal view mode. While the part or assembly is not moving or rotating, the transparency is high quality. When moved or rotated with the pan or rotate tools, the application switches to low-quality transparency, enabling you to rotate the model faster. This is important if the part or assembly is complex.
•
High quality for dynamic view mode. High-quality transparency is retained while moving or rotating the model with the pan or rotate tools. Depending on your graphics card, this option may result in slower performance. If the display is slow when using transparent planes in Shaded With Edges or Shaded mode, it may be because of the Transparency you specified. With some graphics cards, the display speed improves if you do not use high-quality transparency.
Curvature generation Select one of the following options: •
Only on demand. Initial curvature display is slower, but uses less memory.
•
Always (for every shaded model). Curvature displays more quickly on the first display, but extra memory is always used (RAM and disk) for every part that you create or open.
Assemblies •
Automatically load components lightweight. Loads all the individual components in assemblies that you open as lightweight. Sub-assemblies are not lightweight, but the parts that they contain are lightweight. For more information, see Lightweight Parts.
•
Remove detail during zoom/pan/rotate. Removes small components and faces (both interior and exterior) from the graphics area when you zoom, pan, or rotate the model to improve system performance. When Remove detail during zoom/pan/rotate is enabled, the Optimize Zoom/Pan/Rotate option is available if you change the model. Click View, Display, or right-click in the graphics area and select View, Optimize Zoom/Pan/Rotate, to recalculate which components and faces should be hidden. Remove detail during zoom/pan/rotate is automatically disabled when you move or rotate a component, during mate animation, and during drag-and-drop animation. You can temporarily disable Remove detail during zoom/pan/rotate by holding down the Alt key.
•
Check out-of-date lightweight components. Lets you specify how you want the system to load lightweight components that are out-of-date. o o
o
•
Don’t check. Loads the assemblies without checking for out-of-date components. Indicate. Loads the assemblies and marks them with an icon if the assemblies contain an outof-date component, even if the assembly is not expanded. You can right-click an out-of-date toplevel assembly and select Set Lightweight to Resolved. Always Resolve. Resolves all out-of-date assemblies during load.
Resolve lightweight components. Some operations require certain model data that is not loaded in lightweight components. This option controls what happens when you request one of these operations in an assembly that has lightweight components. See also Loading Additional Model Data. o
o
Prompt. Resolves lightweight components each time one of these operations is requested. In the dialog box that appears, click Yes to resolve the components and continue, or click Cancel to cancel the operation. If you select Always resolve (before you click Yes or Cancel), the option is set to Always. Always. Automatically resolves lightweight components.
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•
Rebuild assembly on load. Lets you specify whether you want assemblies to be rebuilt, so components are updated when you open them. o
Prompt. Asks if rebuild is desired each time an assembly is opened. Click Yes or No in the dialog box that appears when you open the assembly. If you select Don’t ask me again (before you click Yes or No), the option is updated to reflect your choice (Yes changes the option to Always, No changes the option to Never).
o
Always. Always rebuilds assemblies when opening.
o
Never. Opens assemblies without rebuilding.
•
Automatically convert drawing views to draft quality when unloading components. Changes drawing views from high quality to draft quality when you set the model views to lightweight.
•
Mate animation speed. Enables animation of mates and controls the speed of the animation. When you add a mate, click Preview or OK in the PropertyManager to see an animation of the mate you just created. Move the slider to Off to disable mate animation.
Enable clipping for zoom limitation in Windows ME Lets you select a portion of the model and zoom in on only the selected portion. On the Windows ME operating system, there is a limit beyond which you cannot zoom in on a model. You can zoom in on small details very closely, but the display is slower. Update mass properties while saving document Updates the mass properties information when you save a document. This means that the next time you access the mass properties, the system does not need to recalculate them (if the document has not changed). The updating may slow performance, however. Use shaded preview Shows shaded previews to help you visualize features you create. You can rotate, pan, zoom, and set standard views while maintaining the shaded preview.
Use Software OpenGL Disables graphics adapter hardware acceleration and enables graphics rendering using only software. For many graphics cards, this results in slower performance. Select this option only if instructed to do so by technical support. If you select Use Software OpenGL, SolidWorks changes some of your options settings for optimum software performance. Click here to see the options that change. You can override any of these settings if desired. This option is automatically selected and unavailable for change if your graphics card does not support hardware acceleration, or does not support it for the current combination of resolution, number of colors, refresh rate, and so forth. Go To Image Quality Click Go To Image Quality to switch to the Document Properties - Image Quality dialog box to set image quality options.
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Performance Settings Use Software OpenGL selected •
Turn on: o
•
High quality for normal view mode
Turn off: o
High quality for dynamic view mode
o
Display shaded planes
o
Use gradient background
o
Display plane when shaded
o
Shadows
Use Software OpenGL cleared •
•
Turn on: o
High quality for normal view mode
o
High quality for dynamic view mode
o
Use gradient background
o
Display shaded planes
o
Shadows
Turn off Display plane when shaded
Assembly Options Lets you set the behavior for dragging components in an assembly. To customize Assemblies options:
1.
Click Tools, Options, System Options, Assemblies.
2.
Select Move components by dragging to allow components to move or rotate within their degrees of freedom when you drag them in the graphics area. When cleared, you can still move or rotate a component with the Move with Triad function or the Move Component
3.
and Rotate Component
tools.
Click OK.
Large Assembly Mode Options Lets you set options for Large Assembly Mode. Most of the options under Large Assembly Mode are duplicated on other pages of the Systems Options dialog box. The selections you make under Large Assembly Mode apply only when Large Assembly Mode is on. Set options for normal use (with Large Assembly Mode off), under Performance, Display/Selection, and so on. When Large Assembly Mode is on, you cannot access duplicated options except under System Options, Large Assembly Mode. To customize Large Assembly Mode options:
1.
Click Tools, Options, System Options, Large Assembly Mode.
2.
Change the settings then click OK.
General Options •
Large assembly threshold. This is the number of resolved components above which Large Assembly Mode activates or sends a message, depending on your settings. If you have already activated Large Assembly Mode, the threshold is ignored.
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Chapter 17 SolidWorks Options
•
Automatically activate Large Assembly Mode: o
Prompt. When you reach the threshold, a message gives you the option to activate Large Assembly Mode.
o
Never. Ignore the threshold.
o
Always. When you reach the threshold, Large Assembly Mode automatically activates.
NOTE: If you save an assembly with Large Assembly Mode active, SolidWorks ignores the Automatically activate Large Assembly Mode option the next time you open the assembly. The assembly opens with Large Assembly Mode active. •
Check out-of-date lightweight parts: o
o
o
Don't check. Load without checking for lightweight components. Select for the fastest performance. Indicate. Load the assemblies and mark them with an icon if the assemblies contain an out-ofdate part, even if the assembly is not expanded. You can right-click on an out-of-date top level assembly and select Set Out-of-date Lightweight to Resolved. Always resolve. All out-of-date components are resolved during loading.
•
Automatically load components lightweight. Loads your assembly with lightweight components.
•
Update mass properties while saving document. Recalculates the mass properties on save. Clear to improve performance.
•
Save auto recover info every. Specify how often to automatically save model information. Clearing this check box improves performance, but disables automatic save of your model.
Display Options To improve performance do the following:
•
Clear: o
o
o
•
Dynamic highlight from graphics view. Enables highlighting of entities in the graphics area as you move your cursor over the graphics area. Anti-alias HLR edges in shaded and fast HLR/HLV modes
o
Display shadows in shaded mode High quality transparency for normal view mode
o
High quality transparency for dynamic view mode
o
Use RealView graphics
o
•
Dynamic highlight from Feature Manager. Enables highlighting of entities in the graphics area as you move your cursor over the FeatureManager design tree.
Select: o
Remove detail during zoom/pan/rotate
o
Hide all planes, axes, sketches, curves, annotations, etc.
Select Only on demand in Curvature generation.
Drawings Options To improve performance do the following:
•
•
Clear: o
Show contents while dragging drawing view.
o
Smooth dynamic motion of drawing view.
o
Automatically load models for detached drawings.
Select: o
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Automatic hiding of components on view creation.
•
Select Hidden Lines Removed, Shaded, or Shaded with Edges in Default display style for new views.
•
Select Draft Quality in Default display quality for new views.
External References - Options Specifies how part, assembly, and drawing files with external references are opened and managed. To specify how SolidWorks manages references to external files:
1.
Click Tools, Options, System Options, External References.
2.
Change the settings then click OK.
External References •
Open referenced documents with read-only access. Specifies that all referenced documents will be opened for read-only access by default.
•
Don’t prompt to save read-only referenced documents (discard changes). Specifies that when a parent document is saved or closed, no attempt will be made to save its read-only, referenced documents.
•
Allow multiple contexts for parts when editing in an assembly. You can create external references to a single part from more than one assembly context. However, any individual feature or sketch within the assembly may only have one external reference.
•
Load referenced documents. Specifies whether to load the referenced documents when you open a part that is derived from another document (such as a base part, derived component part, part with a cavity feature, and so on.) o
o o
o
Prompt. Ask about loading externally referenced documents each time you open a document with external references. All. Opens all of the externally referenced documents. None. Does not open any of the externally referenced documents. External references may be shown as out of context until you open the externally referenced documents. Changed Only. Opens only the externally referenced documents that have changed since the last time you opened the original document.
•
Search file locations for external references. Specifies that SolidWorks should search the Referenced Documents list of folders in the File Locations Options dialog box. When cleared, the list is ignored.
•
Update out-of-date linked design tables to. Determines what happens to linked values and parameters if the model and the design table are out-of-sync. o
Prompt. The software prompts you when you open a document with a design table that is out-ofsync with the model.
o
Model. The design table updates with the model's values.
o
Excel. The model updates with the design table's values.
Assemblies •
Automatically generate names for referenced geometry. When this option is off, you can mate to parts for which you have read-only access because you are using the internal face IDs of the parts. Unless you will use component replacement, leave this option off, especially in a multi-user environment. When this option is on, you automatically create surface identifiers (for example: Face1, Face2) at the time you mate the part, therefore you need write access to the part, in most cases. Turn this option on if you intend to do component replacement using the same surface identifiers, remembering that you need write access to the parts you are using. (Rename the corresponding edges and/or faces on the replacement component to match the edge/face names on the original part.)
•
Update component names when documents are replaced. Clear this option only if you use the Component Properties dialog box to assign a component name in the FeatureManager design tree that is different from the filename of the component.
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Chapter 17 SolidWorks Options
Default Templates You can specify the folder and template file for automatically created parts, assemblies, and drawings. For example, when you import a file from another application or create a derived part, the default template is used for the new document. To specify a folder for document templates:
1.
Click Tools, Options.
2.
On the System Options tab, click Default Templates. The current path and folder for part, assembly, and drawing templates appears.
3.
To change the folder for one of the template types, click the browse button window.
next to the path display
In the New SolidWorks Document dialog box, select the new default template, then click OK. If you need to add a template that does not appear in this dialog box, add the template location with the File Locations option. 4.
5.
Select one of the following options: •
Always use these default document templates
•
Prompt user to select document template
Click OK.
File Locations Lets you specify and locate referenced documents. Folders are searched in the order in which they are listed in the Folders list. If one or more folders are selected in the Folders list, you can Delete existing folders and use Move Up or Move Down to change the folder search order. You can always Add new folders. To display file locations:
1.
Click Tools, Options, System Options, File Locations. The Show folders for box displays search paths for files of various types: •
Bend Tables
•
Library Feature Files
•
Revision Table Templates
•
Blocks
•
Macros
•
Sheet Formats
•
BOM Templates
•
Macro Feature Files
•
SolidWorks Journal File
•
Color Swatches
•
Material Databases
•
Textures
•
Custom Property File
•
Palette Assemblies
•
Web Folders
•
Dimension/Annotation Favorites
•
Palette Features
•
Weldment Profiles
•
Document Templates
•
Palette Forming Tools
•
Weldment Cut List Templates
•
Hole Callout Format File
•
Palette Parts
•
Weldment Property File
•
Hole Table Templates
•
Referenced Documents
When you select a file location for Macros, and then you run a macro, the software looks for a macro in the specified location. For instance, when you click Tools, Macro, Run, the Run Macro dialog box opens to the file location you specified. 2.
17-16
Click OK.
To add a folder for a file location:
1.
Click Tools, Options, System Options, File Locations.
2.
Select a folder type in Show folders for.
3.
Click Add to add a new directory path to the list.
4.
Browse in the Browse For Folder dialog box to locate the folder. If desired, click New Folder to create a new folder.
5.
Click OK.
To delete a folder from a file location:
1.
Click Tools, Options, System Options, File Locations.
2.
Select a folder type in Show folders for.
3.
Select the path in Folders and click Delete. After you click Delete, the path is gone. Click Cancel to undo the deletion, if necessary.
To change the folder search order in a file location list:
1.
Click Tools, Options, System Options, File Locations.
2.
Select a folder type in Show folders for.
3.
Select the path in Folders and click Move Up or Move Down as necessary. The paths for Referenced Documents are searched only if Search file locations for external references is selected in Tools, Options, System Options, External References. The paths for Palette Parts, Palette Forming Tools, Palette Features, Blocks, Custom Property Files, Macros, Macro Feature Files, and SolidWorks Journal Files are always searched, whether Search file locations for external references is selected or not.
FeatureManager Options Lets you set the default system options related to the FeatureManager design tree. To set the default FeatureManager design tree options:
1.
Click Tools, Options.
2.
On the System Options tab, click FeatureManager.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
FeatureManager Options •
Scroll selected item into view. Specifies that the FeatureManager design tree should automatically scroll to display the feature icon that is related to the selected items in the graphics area. If you have a very complex part or assembly, you may want to turn this option off. Then, when you want the FeatureManager design tree to scroll to a feature you can right-click the feature and select Go To Feature (in Tree).
•
Name feature on creation. When you create a new feature, the feature name in the FeatureManager design tree is automatically selected and ready for you to enter a name of your choice.
•
Arrow key navigation. Lets you use the arrow keys to traverse the FeatureManager design tree, and expand or collapse the design tree and its contents, as follows:
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Chapter 17 SolidWorks Options
•
o
Up arrow - Scrolls up the design tree
o
Down arrow - Scrolls down the design tree
o
Left arrow at top of design tree - Collapses the design tree
o
Right arrow at top of design tree - Expands the design tree
o
Left arrow on an item in the tree - Collapses the item to hide its contents
o
Right arrow on an item in the tree - Expands the item to display its contents, if any
Dynamic highlight. Specifies that the geometry in the graphics area (edges, faces, planes, axes, and so on) is highlighted when the pointer passes over the item in the FeatureManager design tree.
Spin Box Increments Lets you set the default incremental changes to the spin box values. To set the default spin box increment value:
1.
Click Tools, Options.
2.
On the System Options tab, click Spin Box Increments.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
Length increments Specifies the number of units added or subtracted when you click a spin box arrow to change a linear dimension value. You can set the values in English units or Metric units. Angle increments Specifies the number of degrees added or subtracted when you click a spin box arrow to change an angular dimension value.
View Rotation Options Lets you set the system defaults for view rotation. To set the default view rotation:
1.
Click Tools, Options.
2.
On the System Options tab, click View Rotation.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
Arrow keys Specifies the angle increment for view rotation when you use the arrow keys to rotate the model. Mouse speed Sets the speed of rotation when you use the mouse to rotate the model or assembly component. To get finer control and slower rotation, move the slider to the left. View animation speed Enables the animation-like display of changes in view orientation for part and assembly documents only. When you change from one view to another, the change occurs showing an animated sequence of frames between the old view and the new view. Move the slider to adjust the animation speed between Fast (default setting) and Slow. Move the slider to Off to turn off view animation.
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View animation occurs when you change views, including the following: •
View orientation commands (For example, Front, Isometric, and so forth)
•
Zoom to Area, Zoom to Fit, Zoom to Selection
•
Shift+ arrows to rotate 90 degrees
•
Any command where the system changes the view orientation automatically, such as extruding the first sketch of a part NOTE: View animation might not always work for extremely large-sized or complex documents.
Backup Options Lets you choose how often you want to make backup copies of your files and where you want to store the backups. To set the default options for making backups:
1.
Click Tools, Options.
2.
On the System Options tab, select Backups.
3.
Choose from the following options: •
Save auto recover info every changes. Select this check box and set the number of changes that should occur before information is automatically saved. NOTES: o
o o
In a part or assembly document, a change is a rebuild or an action that requires a rebuild, such as the addition of a feature. To disable auto recover, clear the check box. Auto recover files are saved in <default drive>:\\swxauto. For example: C:\Documents and Settings\user name\Local Settings\Temp\swxauto.
•
Number of backup copies per document. Specify the number of backup copies you want to save of part, assembly, or drawing documents. Scroll to 0 (for none) or up to 10.
•
Save backup files in the same location as the original. Select this check box to save the backup file in the same location as the original file. Backup files use the naming convention: Backup of <document name>.sld*.
•
Save backup copies in directory. Name a directory where all backup copies are stored by default. Type the path or use click to browse to the directory to use. This option is disabled if Save backup files in the same location as the original is selected.
4.
Click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box. NOTE: You should examine backup directories occasionally to make sure your backup copies do not use too much space.
Document Properties Detailing Options Set options for detailing in the active document. You can also set the detailing options in Document Templates. To set detailing properties:
1.
Click Tools, Options, Document Properties, Detailing.
2.
Change the detailing options to meet your standard detailing style, and click OK.
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Chapter 17 SolidWorks Options
Dimensioning Standard Select a dimensioning standard from the list: ISO, ANSI, DIN, JIS, BSI, GOST, or GB. The standard affects some detailing styles, such as weld symbols, surface finish symbols, and dimension arrows. Dual dimensions display. When selected, dimensions are displayed in two kinds of units. Choose whether the second dimension is displayed On top or On the right. Fixed size weld symbols. When cleared (default), the size of the weld symbol is scaled according to the dimension font size, and the size of the weld symbol changes if the dimension font size changes. When selected, the size of the weld symbol is dependent on the selected dimensioning standard, and the size of the weld symbol remains constant regardless of changes to the dimension font size. This option is not available for the GOST dimensioning standard. Display datums per 1982. Select this checkbox to use the 1982 standard for the display of datums. This option is available only if you use the ANSI dimensioning standard. Trailing zeros. Select one of three settings: •
Smart. Trailing zeros are trimmed for whole metric values. (Conforms to ANSI and ISO standards.)
•
Show. Dimensions have trailing zeros up to the number of decimal places specified in Tools, Options, Document Properties, Units.
•
Remove. All trailing zeros are removed. Tolerances are not affected by this option.
Alternate section display. The section line does not display across the drawing view; the arrow lines stop at the boundaries of the section cut. Centerline extension. This value controls the centerline’s extension length beyond the section geometry when it is in a drawing view. The default value is set according to standards, but you can change it. Select the value in the edit box and enter a new value. When a centerline length is modified, the new length is used the next time the section is rebuilt. Auto insert on view creation The following items are inserted automatically into all appropriate entities in new drawing views. •
Center marks. Add to arcs and circles.
•
Centerlines. Add to model faces with parallel edges.
•
Balloons. Add to all visible components, without duplicates in multiple views.
•
Dimensions marked for drawing. Add dimensions to models, without duplicates in multiple views. The dimensions are indicated in the part sketches as Mark for drawing.
Extension lines Gap. Set a value for the distance between the model and dimension extension lines. Beyond dimension line. Set a value for the length of the extension line beyond the dimension line. Example
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Datum features Display type. Select a default (Per Standard, Square, or Round (GB)) to appear in the Datum Feature PropertyManager. Next label. Type a letter to start the labels for datum feature symbols. Successive labels are in alphabetic order. Only uppercase letters are accepted. Surface finish symbols Display symbols per 2002. For ISO and related drafting standards, display surface finish symbols per 2002 standards. Center marks Size. Specifies the size of Center Marks, used with arcs and circles in drawings. Extended lines. Specifies whether the center mark lines are displayed. Centerline font. When selected, the lines in the center mark use the font specified for centerlines. Break lines Specify the following properties of break lines in a Broken View in a drawing. •
Gap. The distance between the break lines when they are inserted and after you break the view.
•
Extension. The length of the break lines beyond the model geometry.
Automatic update of BOM. When selected, if a Bill of Materials exists in a drawing, it automatically updates when relevant changes are made to the model. If you edit linked custom properties in a BOM and then rebuild the drawing, the properties are reset to the values in the Summary Info dialog box when this option is selected. Some manual edits are lost when the BOM is updated. Section Display Types Alternate Section Display Normal Section Display
Dimensions Options You can set options for dimensioning in the active document. To set dimensioning options:
1.
Click Tools, Options, Document Properties, Dimensions.
2.
Change the dimensioning options to meet your standards, and click OK.
Check Boxes Add parentheses by default. Reference dimensions in drawings are displayed within parentheses. Snap text to grid. The placement of dimension text snaps to the grid in a drawing or a sketch. Center between extension lines. Dimension text is centered between its extension lines. Include prefix inside basic tolerance box. For ANSI standard, any prefix added to a dimension with basic tolerance appears inside the tolerance box. Automatically jog ordinates. Ordinate dimensions are automatically jogged when inserted.
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Chapter 17 SolidWorks Options
Offset distances Specify values for the distances between baseline dimensions. •
•
From last dimension (B). The distance between dimension lines. This value is used for baseline dimensions and for Align Parallel/Concentric . SolidWorks automatically doubles the offset distance for dimensions displayed with tolerances. From model (A). The distance between the model and the first dimension for baseline dimensions. (Not used with Align Parallel/Concentric).
Arrows Style. Specify the default style of dimension arrows by selecting from the illustrated list. Outside, Inside, or Smart. Specify the placement of dimension arrows in relation to the extension lines. Smart arrows appear outside of extension lines if the space is too small to accommodate the dimension and the arrowheads. Display 2nd outside arrow (Radial). Check this option to specify that two outside arrows be displayed with radial dimensions. Arrows follow position of text (Radial). •
Arrow placement must be set to Smart.
•
When you drag radial dimensions inside or outside arcs or circles, the arrowheads move inside or outside with the dimensions.
Break dimension extension/leader lines Gap. Specify the gap in extension and leader lines when they are broken. Break around dimension arrows only. You can choose to have breaks occur only where the lines cross arrows. For ANSI standard, this option is selected by default. Bent leader length Specify the length of bent leaders. Text alignment Select Horizontal and Vertical default alignment for multiple lines of dimension text. Vertical alignment specifies where the leader is located relative to the text and applies only to certain standards, such as ANSI. Angle/linear-angled Display ANSI standard only. Select Use bent leaders to use bent leaders for: •
Dimensions of angles
•
Angular display of linear dimensions
Leaders Specify the alignment of dimension text with respect to the leaders. Precision Specify the dimension precision for the dimension value and tolerance values for Primary Units, Angular Units, and Alternate Units.
17-22
Tolerance Specify the type of tolerance, variation, font, and so on. See Dimension Tolerance Properties. You can set Tolerance display to None and then set the variations and font to defaults for the current document. When you modify the properties of a dimension, the default tolerance settings will be those set in these options.
Notes Options You can set note options for the active document. To set note options for the active document:
1.
Click Tools, Options, Document Properties, Notes.
2.
Choose from the following options, then click OK.
Text alignment Select Left, Right, or Center alignment for note text. Leader anchor Specify to which side of the note the leader should attach: Left, Right, or the side Closest to the attachment point. Leader style •
Leader style. Select Straight, Bent, or Underlined.
•
Leader length. Specify the distance between the leader bend and the text of the note for bent leaders.
Border •
Style - Select a style from the list. None results in text with leader, if a leader is specified, but no border enclosing the text.
•
Size - Select Tight Fit, expandable to tightly fit the text, or select a size to accommodate from one to five characters.
Balloons Options Set the default properties of balloons. To set default balloon properties:
1.
Click Tools, Options, Document Properties, Balloons.
2.
Specify the options described below, then click OK.
Single balloon Style. Select a style from the list. None results in text with leader, but no border enclosing the balloon. Size. Select a balloon size of Tight Fit, expandable to tightly fit any custom text you type in, or select a size to accommodate from one to five characters. Stacked balloons Style. Select a style from the list. None is not available for Stacked balloons. Size. Select a balloon size of Tight Fit, expandable to tightly fit any custom text you type in, or select a size to accommodate from one to five characters.
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Chapter 17 SolidWorks Options
Balloon text Upper. Select Item Number, Quantity, or Custom from the list for the upper section of a Circular Split Line balloon or for the whole balloon of all other styles. Lower. If the balloon style is Circular Split Line, the Lower box is available for you to select Item Number, Quantity, or Custom from the list. If you select Custom text, a window opens in the Balloon or Stacked Balloon PropertyManager for typing your text. Bent leaders Use bent leaders. Select for balloons to use bent leaders by default. Leader length. Enter a default value for the length of the leader nearest the balloon. AutoBalloon Layout Select a layout as the default for inserting autoballoons: Square Circular Top Bottom Left Right
Arrows Options You can set display options for arrows. The default options vary depending on the drafting standard specified in Tools, Options, Document Properties, Detailing. To set the options for displaying arrows:
1.
Click Tools, Options, Document Properties, Arrows.
2.
Specify the options described below, then click OK.
Size Specify the Height and Width of arrowheads, and the Length of the complete arrows, for leaders on dimensions, notes, and other annotations. Section/View Size Specify the Height and Width of arrowheads, and the Length of arrows, for section view lines and on view arrows (in auxiliary views, for example).
17-24
Attachments Specify the arrowhead styles to be used depending on where the leader is attached.
Virtual Sharp Display Options You can set display options for virtual sharps. To set the display options for virtual sharps:
1.
Click Tools, Options, Document Properties, Virtual Sharps.
2.
Select a style for the display of virtual sharps, and click OK.
Annotations Display Options You can specify the default display of annotations and select the types of annotations that you want to display by default. To set the default options for displaying annotations:
1.
Click Tools, Options, Document Properties, Annotations Display.
2.
Choose from the options described below, then click OK.
Display filter. To specify the annotation types to display by default, select Display all types, or clear Display all types and select individual types. Cosmetic threads
Shaded cosmetic threads
Datums
Geometric tolerances
Datum targets
Notes
Feature dimensions
Surface finish
Reference dimensions
Welds
Text scale (For part and assembly documents). When Always display text at the same size is cleared, you can specify a scale for the default size of annotation text.
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Chapter 17 SolidWorks Options
Select from the following options: •
Always display text at the same size. When selected, all annotations and dimensions are displayed at the same size regardless of zoom. Note that drawings have this option disabled and always zoom the text height.
•
Display items only in the view in which they are created. When selected, any annotation is displayed only when the model is viewed in the same orientation as when the annotation was added. Rotating the part or selecting a different view orientation removes the annotation from the display.
•
Display annotations / Display assembly annotations. When selected, all annotation types that are selected in the Display filter are displayed. For assemblies, this includes not only the annotations that belong to the assembly, but also the annotations that are displayed in the individual part documents.
•
Use assembly’s setting for all components. When selected, the display of all annotations matches the setting for the assembly document, regardless of the setting in the individual part documents. Use this option along with the Display assembly annotations check box to display different combinations of annotations.
•
Hide dangling dimensions and annotations. If you delete features in parts and assemblies, this option automatically hides the dangling dimensions and annotations in the drawings. If you suppress features, SolidWorks automatically hides dangling reference dimensions in the drawing; this option automatically hides dangling annotations.
•
If you use JIS dimensioning standards, specify the JIS surface finish size (either 1, 2, or 3 Characters or Custom Scale). If you select Custom Scale, specify the scale value in the Scale box.
Annotations Font Options You can specify the default font for various types of annotations (Note, Dimension, Detail, Section, View Arrow, Surface Finish, Weld Symbol, Tables, and Balloon). The font for Detail applies to the label on the detail circle, but not to the label on the detail view. The font for Section applies to the label on the section line, but not to the label on the section view. The labels for detail and section views are Notes and use the font for Note. To specify the default font for a type of annotation:
1.
Click Tools, Options, Document Properties, Annotations Font.
2.
Select an Annotation type in the list. The Choose Font dialog box appears.
3.
Select a Font, Font Style, Height, and Effect, then click OK.
4.
Repeat steps 2 and 3 to specify default fonts for other annotation types as needed, then click OK.
Tables Options Set options for tables in the active drawing document. To set options for tables:
1.
Click Tools, Options, Document Properties, Tables.
2.
Choose from the following options, then click OK.
Hole Table
Origin indicator . Specify the appearance of the indicator of the origin from which the software calculates hole positions by selecting a standard. Standard. Select a specific standard or Per Standard (the standard set in Detailing Options). Tag angle/Offset from profile center. Specify the position from the hole profile center of the tag that the software generates to identify each hole.
17-26
•
Angle
•
Offset
. Angle from a vertical line through the center of the hole. . Distance from the hole profile.
Alpha/numeric control. Specify whether the hole tag is alphabetic or numeric. Scheme. •
Combine same tags. Merge cells with the same tags (A1, A2, and so on as A). All the holes labeled with the same tag are part of a pattern, so the hole sizes are the same. The Size cells are merged and locations are not listed.
•
Combine same size. Merge cells of same size holes.
Location precision. The precision at which the X and Y locations of the holes are displayed. Show hole centers. An asterisk identifies the center of each hole. Automatic update of hole table. The table data updates when the model changes. Revision Table Symbol shapes. Select from a circle, square, triangle, or hexagon for the revision symbol. Alpha/numeric control. Specify whether the revision is alphabetic or numeric. •
Start from where user left. If you change control from alphabetic to numeric or vice versa, previous revisions remain as they are.
•
Change all. If you change control from alphabetic to numeric or vice versa, previous revisions (except any you have edited) change to the new format.
Bill of Materials Table Zero quantity. Select whether to display zero quantities with a dash (-) or a zero (0), or to leave the cell blank. Missing component. •
Keep the row for missing component.
•
Display with strikethrough text. Display text in rows for missing components with strikethrough.
View Labels Options Set options for detail, section, and auxiliary view labels in the active drawing document. To set options for view labels:
1.
Click Tools, Options, Document Properties, View Labels.
2.
Choose from the following options, then click OK.
The options for each type of view are the same except for the text under Name, which is DETAIL, SECTION, or AUXILIARY. Detail View, Section View, and Auxiliary View Per standard. The options below follow the standard specified in Tools, Options, Document Properties, Detailing (ANSI, ISO, and so on) and are not available for editing. Name. Select a title to appear in the view label. Label. Select whether the label letter corresponding to the label on the parent view appears in the view label. Scale. Select whether the word SCALE appears next to the scale.
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Chapter 17 SolidWorks Options
Delimiter. Select the delimiter between the two scale numbers and whether the scale appears in parentheses. If you select #X, the number in (#) can be an integer or a real number. Display. Display the view label with name and label stacked on top of the scale (Stacked), or all data on the same line (In-line).
Grid and Snap Options You can display a sketch grid in an active sketch or drawing and set options for the grid display and snap functionality. The options for grid spacing and minor grid lines per major lines apply to the rulers in drawings as well as to sketching and drawing grid lines. To set grid and snap options for the active document:
1.
Click Grid/Snap
on the Sketch toolbar, or click Tools, Options, Document Properties, Grid/Snap.
2.
Select from the options described below.
3.
Click OK.
Grid •
Display grid. Turns the sketch grid on or off.
•
Dash. Toggles between solid and dashed grid lines.
•
Automatic scaling. Automatically adjusts the display of the grid when you zoom in and out.
•
Major grid spacing. Specifies the space between major grid lines.
•
Minor-lines per major. Specifies the number of minor grid lines between major grid lines.
Snap •
Snap only when grid is displayed. Turns on grid snap only when Display grid is selected.
•
Snap to points. Turns snap on. When snap is on, points that you sketch or drag snap to the nearest intersection of grid lines (or to intermediate points, if Snap points per minor is greater than 1).
•
Snap points per minor. Sets the number of snap points between minor grid lines.
•
Snap to angle. Specifies that sketched lines snap to a pre-defined angle. Specify the angle to which sketched lines should snap. The inferencing pointer displays the specified angle as you sketch.
Units Options Lets you specify units for the active part, assembly, or drawing document. If you use small units such as angstroms, nanometers, microns, mils, or microinches, it is helpful to create templates as the basis for documents that use the units. The templates could include settings such as:
17-28
•
grid spacing
•
dimension witness line gap and bent leader length
•
dimension offset distances
•
note bent leader length
•
balloon bent leader length
•
arrow size and section view arrow size
•
text scale and Always display text at the same size
•
material density
To set units for the active document:
1.
Click Tools, Options, Document Properties, Units.
2.
Select from the options described below.
3.
Click OK.
Unit system Displays a unit system: •
MKS (meter, kilogram, second)
•
CGS (centimeter, gram, second)
•
MMGS (millimeter, gram, second)
•
IPS (inch, pound, second)
•
Custom. Lets you set the Length units, Dual units, Angular units, Density units, and Force.
Length units Displays the length units. If you set Unit system to Custom, select the units and set the Decimal places. Otherwise, you can only set Decimal places. If you select microinches, mils, inches, or feet & inches, select Decimal or Fractions. If you select Fractions, the following options are available: •
Round to nearest fraction
•
Denominator (Only dimensions that are evenly divisible by this denominator are displayed as fractions.)
If you select feet & inches, you can select Convert from 2'4" to 2'-4" format. The format for feet & inches in the SolidWorks software is 2'-4". If you import a document in the 2'4" feet & inches format, you can convert the document to 2'-4". Once you have converted the document to 2'-4" format, you cannot convert back to the 2'4" format. Dual units Displays a second type of units just as you specify the Length units. To show dual units in the SolidWorks software, select Dual dimensions display in the Detailing options. Angular units Displays the angular units. If you select Degrees or Radians, set the Decimal places. Density units Displays the Mass and Per unit volume units. Force Displays the force units.
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Chapter 17 SolidWorks Options
Document Colors Lets you set model, feature, and view mode colors for the active part or assembly document. NOTE: Document Colors is not available when you have a drawing document active. To set model, feature, and view mode colors:
1.
Click Tools, Options.
2.
On the Document Properties tab, select Colors.
3.
In the Model\Feature colors box, select the feature type or view mode type for which you want to edit the color representation. If you are working with an assembly, the only color choices are Shading and Hidden. These are the display colors for Shaded mode and Hidden Lines Visible mode.
4.
Click Edit to change the color used to display the selected item. Select a color from the Color palette or click Define Custom Colors and define a new color.
5.
Click OK and view the selection in the preview box.
6.
In an assembly, if you selected a color to display in Hidden mode, the Advanced button is available. You can select additional display qualities such as Shininess, Transparency, and so on.
7.
Additionally, you have the following options:
8.
•
Reset All To SolidWorks Defaults. Click this button to restore the original default color settings.
•
Apply same color to wireframe, HLR and shaded. Select this check box to use the same color for these view modes. (This option is available only for parts.)
•
Ignore feature colors. Select this check box to specify that feature colors are not used. (This option is available only for parts.)
•
Curvature. Click this button to define the colors associated with the radii of curvature.
•
Go To System Colors. Click this button to switch to the System Options - Colors dialog box.
Click OK to accept your changes, or click Cancel to exit the dialog box without saving the changes.
Material Properties Options Lets you set crosshatch options and material density for the active part. These options are not available for drawing or assembly documents. To set material properties options:
1.
In a part document, click Tools, Options.
2.
On the Document Properties tab, click Material Properties.
3.
Type the material density in the Density box. NOTE: You can type the density value with any units. For example, if the units of the part are grams and millimeters, you can use a density value of pounds and inches. The software converts the value to the document’s units when you click OK.
4.
5.
In the Area Hatch/Fill box, select from the following: •
None
•
Solid
•
Hatch
If you select Hatch, do the following: •
Select a crosshatch pattern from the Pattern list.
•
If necessary, set the Scale and Angle of the crosshatch pattern.
A preview of the pattern is displayed in the preview box.
17-30
6.
Click OK. NOTE: You can also change the Density from the Measurement Options dialog box. Click Tools, Mass Properties, Options, to access this dialog box.
Line Font Options You can set the style and weight of lines for various kinds of edges in drawing documents only. NOTE: The line font options are available only if the active document is a drawing document. To set the style and weight of lines in drawings:
1.
Click Tools, Options, Document Properties, Line Font.
2.
Change the settings for one or more type of edge, and click OK.
Type of edge Select an edge type from the list: Visible Edges, Hidden Edges, Sketch Curves, and so on. Style Choose a style from the list: Solid, Dashed, Phantom, Chain, and so on. Thickness Choose a thickness from the list: Normal, Thin, Thick, and so on. Preview Displays the selected line font.
Image Quality Lets you select the display quality that is most efficient for you. To set the image quality options for the active document:
1.
Click Tools, Options, Document Properties, Image Quality.
2.
Select from the following options, then click OK.
Shaded and draft quality HLR/HLV resolution Controls the tessellation of curved surfaces for shaded rendering output. A higher resolution setting results in slower model rebuilding but more accurate curves. When Draft Quality HLR/HLV Shaded settings control Shaded With Edges Lines Visible
, and Wireframe
, Shaded
, Hidden Lines Removed
is turned on, the , Hidden
views.
•
Low (faster) High (slower). Controls the image quality resolution settings. Move the slider to adjust the settings, or type a value for Deviation.
•
Deviation. Reports the maximum chordal deviation in effect at the various tuning levels. The chordal deviation value is greater at the Low (faster) setting, and decreases as the resolution becomes more finely tuned at the High (slower) setting.
•
Optimize edge length (higher quality, but slower). Increases image quality if, after you move the slider to the highest setting, you still want higher image quality. This option causes slower system performance and increased file size.
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Chapter 17 SolidWorks Options
•
Apply to all referenced part documents (assemblies only). Applies the settings to all of the part documents referenced by the active document.
•
Save tessellation with part document (parts only). Saves disk space and decreases save time when the part has detailed surfaces where the tessellation data is larger than the size of the geometry on disk. When you clear this option, nothing is displayed when the part is opened in: o
View-Only mode
o
SolidWorks Viewer
o
eDrawings (if you open the part directly in eDrawings)
Additionally, re-opening the part could take longer because the display is regenerated. Wireframe and high quality HLR/HLV resolution Controls the image quality of model edges in drawings. When Draft Quality HLR/HLV the Wireframe settings control Hidden Lines Removed
, Hidden Lines Visible
is turned off, , and Wireframe
views. Low (faster) High (slower). Increases image quality. Move the slider to Low (faster) if you want to redraw the screen more quickly and the display quality is not of great importance; move the slider to High (slower) for high display quality, but a slower redraw. If you notice problems with your HLR image display, move the slider to the right. Go To Performance Click Go To Performance to switch to the System Options - Performance dialog box.
Plane Display You can set the following plane display options for part and assembly documents: •
Face color
•
Transparency
•
Intersection display and color
NOTE: You must enable the Display shaded planes option to display shaded planes. To set the plane display:
17-32
1.
Open a part or assembly document.
2.
Click Tools, Options. On the Document Properties tab, click Plane Display.
3.
Under Faces, set the following options: •
Front Face Color. Displays the Color dialog box that you use to set the front face color of planes.
Front face color
Back face color
•
Back Face Color. Displays the Color dialog box that you use to set the back face color of planes.
•
Transparency. Controls the plane transparency (0% displays a solid face color; 100% displays no face color).
0% transparency
75% transparency
100% transparency
NOTE: Edges take the same color as the front and back faces, are not transparent, and are always displayed. 4.
Under Intersections, set the following options: •
Show intersections. Select or clear the Show intersections check box to display or hide the intersection of planes
Plane intersection lines displayed • 5.
Plane intersection lines hidden
Line Color. Displays the Color dialog box that you use to set the plane intersection line color.
Click OK to accept the changes, or Cancel to discard the changes and exit the dialog box.
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Chapter 17 SolidWorks Options
17-34
Index
Symbols $PRP 12-41 Numerics
1:1 scale output 13-10 2D IGES geometry 13-27 2D sketches in drawings 11-10 new 3-3 2D to 3D conversion 4-1 align sketches 4-6 create new sketch 4-10 extract sketches 4-5 extrude 4-7 import drawings 4-4 repair sketch 4-10 select chain 2-62 2D to 3D Toolbar 2-22 3 point arcs 3-59 3D curves in IGES 13-11, 13-29 3D models from 2D 4-1 3D sketches 3-68 3D frame points 3-51 coordinate systems 3-74 dimensions 3-75 Hole Wizard 6-77 line snap 3-69 lines 3-69, 3-70 sketch points 3-73 space handles 3-75 splines 3-49, 3-71 virtual sharps 3-75 A
absorbed feature 2-35 accelerator keys. See shortcut keys 2-18 ACIS files 13-17 edit imported features 13-4 export options 13-9 export units 13-9 export version 13-9 import 13-3, 13-7 import geometry 13-3 import options 13-7 import units 13-7 activate 11-5
SolidWorks 2004 Reference Guide
automatic view activation 17-4 configurations 10-1, 10-8 drawing sheets 11-4 drawing views 11-8 layers 11-58 add 15-28 corner trim 15-44 folders 2-50 forming tools to sheet metal parts 15-28 library features to parts 14-4 loft sections 6-104 palette features to assemblies 14-12 palette features to parts 14-10 relations in sketches 3-41 add-ins. See also translators eDrawings 13-24 PDF Files 13-33 SolidWorks MTS 13-39 advanced 9-68 color properties 7-9 component selection 9-68 mates 9-22, 9-23, 9-24 show/hide components 9-67 advanced smoothing 6-191 align 11-45 annotations 12-34 collinear/radial dimensions 12-24 concentric dimensions 12-23 dimensions 12-22 drawing views 11-49 grid 3-13 ordinate dimensions 12-17 parallel dimensions 12-23 sketches 4-6 with end faces 6-190 Align toolbar 2-22 align. See mating 9-13 aligned section views 11-42 alignment 11-45 aligned section views 11-42 auxiliary views 11-28 break view alignment 11-49 detail views 11-30 dimension text 17-21 drawing views 11-49
Index-1
mates 9-17 model views 11-19 projected views 11-26 relative to model views 11-22 section views 11-37 standard 3 views 11-17 alternate position views 11-43 ambient light 7-46 anchors 12-77 bill of materials 12-77 leaders 12-60, 12-64, 12-69, 17-23 tables 11-5, 12-77 angle mates 9-14, 9-19, 9-23 angular dimensions 3-37 between three points 3-37 between two lines 3-37 animate 13-24 drawings 13-24 mates 17-10 annotations 12-31 align 12-34 ANSI weld symbol 12-65 area hatch 12-66 assemblies 9-73 autoballoons 12-46 balloons 12-42, 17-23 blocks 12-69 center marks 12-48 centerlines 12-51 colors 11-56 cosmetic threads 12-54 datum feature symbols 12-58 datum targets 12-59 display filter 12-32, 17-25 dock points 12-35 dowel pin symbols 12-63 favorites 12-4 fonts 17-26 geometric tolerancing 12-60 hide/show 12-27 hole callouts 12-52 hyperlinks 2-42 insert into drawings 12-2, 12-3 layers 11-58 multi-jog leaders 12-35 multiple 12-33 notes 12-36, 17-23 options 12-31, 17-25, 17-26 parts 7-32 properties 12-32 stacked balloons 12-44 surface finish symbols 12-56 tables 12-76 underlined leader 12-38 weld symbols 12-64 Annotations toolbar 2-23 ANSI standard 17-19 1982 standard for datums 12-58 geometric tolerancing 12-60 tolerances 17-21 weld symbols 12-65 API - Application Programming Interface 2-91
Index-2
application protocols in STEP 13-37 arcs 3-60 3 point 3-59 3D arcs 3-68 centerpoint 3-59 dimensions 3-35, 3-38 in section lines 11-37 tangent 3-8, 3-59 area hatch 12-66 add to face or sketch 12-66 broken views 11-35 import 13-19 options 17-6 arrange icons 2-3 array of sketch entities 3-17, 3-25 arrows 12-12 aligned section views 11-42 auxiliary views 11-28 dimension display properties 12-10 dimension options 17-21 display options 17-24 flip in dimensions 12-6 mulit-jog leaders 12-35 projeced views 11-26 second arrow display 12-10 second outside arrow display 12-10 section views 11-37, 11-40 style 12-6, 12-12 assembiles envelops 9-66 features 9-55 mates 9-26 options 17-13 reorganize 9-38 assemblies 9-1 alignment condition 9-17 annotations 9-73 auto explode 9-69 bottom-up design 9-1 Collision Detection 9-74 colors 9-10 components 2-42, 9-4, 9-6, 9-9, 9-39, 9-62 configurations 10-4, 10-10, 10-12 create from split part 7-27 drawings 11-17, 11-40 Dynamic Clearance 9-76 envelopes 9-65, 9-66 exploded views 9-69, 9-70, 9-71 Feature Palette 14-7, 14-8 feature scope 9-56 FeatureManager design tree 9-2 features 9-49, 9-55 fix 9-11 float 9-11 hide 9-67 hole series 6-81 image quality 9-72 inferencing 9-6 interference detection 9-74 lightweight 9-61 loading component data 9-64 mates 9-8, 9-13, 9-17, 9-19, 9-25, 9-26, 9-28, 9-31
mirror components 9-51 molds 8-2 options 17-13 patterns 9-26, 9-49, 10-12 performance 9-61, 17-13 Physical Dynamics 9-75 Physical Simulation 9-33, 9-35 PropertyManager 9-10 reorder 9-53 reorganize 9-37, 9-38, 9-39, 9-61 roll back 9-53 save 9-6, 9-7, 9-46 send 2-20 show 9-67 sketches 3-11, 9-54 SmartMates 9-25 statistics 9-9 sub-assemblies 9-37, 9-39 suppress 9-28, 9-63, 9-64, 10-27 top-down design 9-1 transparency 9-48 weld beads 9-58 Assembly toolbar 2-24 at angle planes 5-2 attach dimensions 13-22 attachment point 12-24 dimension extension lines 3-38, 12-24 leaders 12-35, 12-36, 12-41, 12-60, 12-69, 17-24 auto explode 9-69 auto hatching 11-35, 11-38, 11-40 auto insert on view creation 12-6, 12-46, 12-48, 12-51, 17-19 auto reliefs 15-28, 15-29 autoballoons 12-46, 17-23 AutoCAD 2-91, 13-10 copying and pasting from 13-22 DXF/DWG files 13-19 font support 13-10 Mechanical annotation 13-19 moving from AutoCAD 2-91 proxy entities 13-19 XREFs 13-19 Autodesk Inventor files 13-17 autodimension 3-39 automatic 2-2 autoballoons 17-19 backups 2-2 center mark insertion 12-48, 17-19 centerline annotation insertion 12-51, 17-19 dimension insertion 17-19 drawing view update 11-45, 11-47 Fit tolerance 12-8, 12-29 inferencing 3-14 jog ordinates 12-17, 17-21 relations 3-40 save 17-19 solve 3-14 update of BOM 17-19 automatic mates. See SmartMates 9-25 autosize reference geometry 5-10 auto-start projected view 11-19 autotransitioning 3-8 auxiliary views 11-28, 11-51
SolidWorks 2004 Reference Guide
2D to 3D conversion 2-22 hide and show 11-51 label display 17-27 axes 5-12 broken views 11-35 hide 5-12 hole table datum origin 12-89 reference 5-12 show 5-12 B
background image 13-38 backups 2-2 automatic 2-2 options 17-19 balloons 12-42 auto insert 17-19 autoballoons 12-46 bill of materials 12-42, 12-81 options 17-23 stacked 12-44 base 6-44 center mark 12-50 extrude 6-45 flange 15-2 part 7-22 revolve 6-132, 6-151 scale 13-10 base point 12-69 baseline dimensions 12-17 bend allowance 15-22, 15-25 bend deduction 15-22, 15-25 bend deviation 15-39 bend table 15-24 bends 15-31 edit 15-23, 15-29, 15-31, 15-32 Excel file 15-23, 15-24 flat bends 15-13, 15-32 inserting 15-31 lofted 15-38 no bends 15-32 positions 15-13 reordering 15-31 round bends 15-13, 15-14 sharp bends 15-13 simplify 15-43 sketched bends 15-9 text file 15-23, 15-24 bent leader length 17-21 bilateral tolerance 12-28 bill of materials 12-81 anchor point 11-5, 12-77 balloons 12-42 child components 10-31 configurations 12-83 contents 12-84 custom properties 12-85 edit text 12-97 Excel-based 12-94, 12-99 insert 12-95 options 17-26 part numbers 12-98
Index-3
sort 12-85 stacked balloons 12-44 sub-assemblies 10-4, 10-31, 12-83 templates 12-78 bitmaps 11-5 in sheet formats 11-5 in sketches 3-67 black and white drawings 2-15 blanked surfaces on import 13-3 block settings 12-38 blocks 12-69 definitions 12-75 insert 12-69, 12-73 instances 12-74 bodies 6-149, 6-214, 7-10 bolt patterns 9-79, 9-89 bolts 9-77 BOM. See bill of materials 12-81 borders 12-38, 12-79, 17-23 boss 6-44 extrude 6-39 revolve 6-132, 6-151 thicken 6-195 bottom-up assembly design 9-1 bounding box 11-9 box selection 2-64 branch points 12-35 break alignment 11-49 break corner 15-35 break external references 9-43 break lines 11-35 break view 11-35 BREP 13-7, 13-11, 13-28, 13-34, 13-35 broken views 11-35 align with parent 11-46 break line gap 17-19 cut styles 11-37 broken-out section 11-34 C
CADKEY files 13-17 callouts 2-6, 3-43, 12-54 cam-follower mates 9-22 cap ends 6-46 capture mate references 9-17 capture type in TIFF 13-15 cascade window 2-3 casting parts (mold design) 8-2 CATIA graphics files 13-18 cavities 8-11 drafts 8-4 scaling factor 8-4 cells in tables 12-76, 12-80 center dimension text 12-13, 17-21 center marks 11-28, 12-48 centerlines 3-58 aligned section views 11-42 annotations 12-51 font for center marks 12-50, 17-19 lofts 6-101 section lines 11-37 section views 11-40
Index-4
centerpoint 3-59 arcs 3-59 rotate drawing views 11-49 centroid 5-14 CGR. See CATIA graphics files 13-18 chain 12-10 dimensions 12-10, 12-17 select 2-62 chamfer 6-7 dimensions 12-20, 12-21 feature 6-7 sketch 3-31 change assembly transparency 9-48 change URL 2-58 check 7-29 entity 7-31 face or edge 7-31 for out-of-date lightweight components 9-64 geometry 7-31 model geometry 7-30 planar surface 7-30 section views 11-41 sketch 3-16 sketch contours 3-16 child and parent relations 2-46, 11-9, 11-48 circles 3-55 detail views 11-30, 11-33 dimensions 3-36, 3-38 circular pattern 6-119, 12-48 circular sketch step and repeat 3-17 constrain spacing 3-19 fix radius 3-19 classification 12-8, 12-29 clearance 12-8, 12-29 click-click or click-drag 3-7 close 2-3 all documents 2-2, 2-3 sketches 3-21 closed corner 15-12 coincident mates 9-14, 9-20, 9-22 coincident relations 3-42 collapse 9-70 exploded views 9-70 FeatureManager design tree 2-46 collinear dimensions 12-24 Collision Detection 9-74 colors 17-6, 17-30 annotations 2-29, 11-56, 11-58, 12-6, 12-31 assembly instances 9-10 Color and Optics PropertyManager 2-37 component instances 9-72 curvature 7-39 display mode 11-56 document options 17-30 edit 7-7 faces or features 7-4, 7-8 layers 11-58 library features 14-5 material properties 7-5, 7-9 notes 11-56 parameter in design tables 10-33 parts in assemblies 9-72
print documents 2-15 sketch status 3-43 system options 17-6 tables 12-76 use assembly 9-72 combine parts 6-213 combine same sizes 12-88 combine same tags 12-88 combined features, MDT files 13-29 CommandManager 2-24 commands 2-83 comments 10-29 configurations 10-4 design tables 10-29 equations 7-16 summary info 7-33 component line font 11-55 component names 17-15 generate names for referenced geometry 17-15 update 17-15 components 9-4 assemblies 9-4, 9-10 Collision Detection 9-74 colors 9-72 configuration descriptions 2-45 configuration names 2-45 configurations 10-26 copy 9-51 derived 7-23 descriptions 2-44 drawings 11-17, 11-40, 11-55, 11-58 Dynamic Clearance 9-76 envelopes 9-65, 9-66 fix 9-11 float 9-11 hide 9-62, 9-67, 11-53 interference detection 9-74 layers 11-58 lightweight 9-61 loading additional data 9-64 mates 9-3, 9-13 mirror 9-51 molds 8-2 names 17-15 part numbers 10-28 patterns 9-49 Physical Dynamics 9-75 properties 9-9, 9-62, 9-67, 9-72 reorganize 9-37, 9-38, 9-39 replace 9-7 resolved 9-63, 9-64 select 9-66, 9-68 shared documents 2-42 show 9-62, 9-67 SmartMates 9-25 suppress 9-63, 9-64 visibility 9-62, 9-65 weld beads 9-58 composite curves 5-21 composite frames 12-62 compression scheme in TIFF 13-15 concentric 3-42
SolidWorks 2004 Reference Guide
dimensions 12-23 mates 9-14, 9-20 relations 3-42 ConfigurationManager 10-1 activate 10-1 split panel display 2-48 configurations activate 10-8 alternate position views 11-43 assemblies 10-10, 10-12 base parts 10-28 bill of materials 12-83 create manually 10-4 create with design tables 10-18 delete 10-13 derived 10-6 descriptions 2-45 dimensions 10-11, 12-26 edit 10-11 end conditions 10-10 equations 10-30 parts 10-8 previews 10-2 properties 10-4 sheet metal flat patterns 11-21 sketch dimensions 10-8 sketch planes 10-9 sketch relations 10-9 STEP files 13-37 weldment cut lists 16-15 confirm delete 2-35 confirmation corner 2-9, 17-2 conformance classes in STEP 13-37 conical 15-40 faces in sheet metal parts 15-15 holes for cosmetic threads 12-54 mates with conical features 9-26 connectors 6-9, 6-106 constrain all 3-19, 13-22 constraints. See relations 3-41 construction geometry. See also reference geometry 3-21 contents, bill of materials 12-84 contour map 6-201 contour selection 3-19 contour types for features 3-16, 3-17 conversion wizard 2-89 convert 2-89 2D to 3D 4-1 detached drawings 11-13 entities 3-22 lightweight drawings 11-16 older SolidWorks files 2-89 sketch lines to construction geometry 5-15 coordinate systems 5-13 3D sketches 3-74 scale parts 6-141 translate 5-13 copy 2-35 blocks 12-69 components 9-51 drag 2-7 drawing views 11-50
Index-5
entities from AutoCAD 13-22 features 7-4 options settings 2-90 planes 5-10 referenced files to server 2-58 references 9-46 sketch entities 3-8, 3-15 to clipboard 2-35 copy options wizard 2-90 corner 15-12 closed 15-12 treatment 15-42 trim 15-44 cosmetic threads 12-54 broken views 11-35 display 17-25 MDT files 13-29 pipe tap holes 6-88 tap holes 6-87 counterbore holes 6-84 countersink holes 6-85 create 3-3 configurations 10-4, 10-18 detached drawings 11-13 forming tools 15-25 new sketches 3-3, 3-4, 3-5, 4-10 openings on forming tools 15-27 palette items 14-8 sub weldments 16-14 crop views 11-33 crosshatch 11-10 area hatch 12-66 detail views 11-40 options 17-30 out-of-date drawing views 17-4 properties 12-68 section views 11-40 cursors. See pointers 3-6, 3-40 curvature 7-39 combs 3-52 display 7-41, 7-42 minimum 7-31 options 7-41 radius 7-40 sketch entities 3-52 curvature continuous 6-70 curve driven patterns 6-110 curved break line cut style 11-37 curves 5-15 composite 5-21 face curves 3-23 from file 5-17 helix 5-17 projected sketch onto face 5-18 projected sketch onto sketch 5-18 shape 6-144 sketches 3-22 spiral 5-17 split curves 3-32 split lines 5-20 through reference points 5-16 through XYZ points 5-16
Index-6
Curves toolbar 2-25 custom 11-7 drawing views 11-19 headers and footers 2-83 macro button 2-84 property values 11-7 scales 11-9, 11-21, 11-24, 11-27, 11-29, 11-31, 11-38 sheet formats 11-3, 11-6 table templates 12-79 template tabs 2-52 custom map SolidWorks to DXF 13-10 custom properties 7-33 bill of materials 12-85 design tables 10-32 drawings 11-4, 11-7, 12-41 in sheet formats 11-6 parts 7-33 weldments 16-18 custom standards 6-83 custom symbols. See blocks 12-69 customize commands 2-83 drawing sheet formats 11-5 headers and footers 2-83 keyboard 2-84 macro button 2-84 macros 2-93 menus 2-85 options 2-81, 2-86 SolidWorks 2-81 tolerance 13-7, 13-14 toolbars 2-86 cut 2-35 across sheet metal bends 15-34, 15-35 drawing views 11-50 extrude 6-50 normal cut 15-35 revolve 6-132 sketch entities 3-8 styles in broken views 11-37 thicken 6-195 to clipboard 2-35 tool 6-47 with surfaces 6-49 cut lists. See weldment cut lists 16-15 cylindrical faces in sheet metal parts 15-40 D
dangling 2-12 section views 11-41 sketch dimensions 7-4, 17-7 sketch geometry 3-43 dates, document properties 11-7, 12-41 datum feature symbols 12-58 datum origin 12-86, 12-89 datum targets 12-59 default 2-53 dimension properties 12-4 fonts 2-29 material properties 2-53 system colors 17-6 templates 2-53
view alignment 11-49 view rotation angle 11-49 defined in context relations 3-45 definition 12-69, 12-75 deform curve to curve deformation 6-9, 6-12 point deformation 6-19, 6-21 delete 2-35 area hatch 12-66 assembly components 9-6 background image 13-38 body 6-214 configurations 10-13 confirm 2-35 design tables 10-21 equations 7-15 faces 6-177 holes 6-179 layers 11-58 mates 9-28 patterns 6-128 relations 3-44 spline points 3-49 surfaces 6-177 tables 12-76 density 17-30 dependent 2-46 documents 9-42 drawing views 11-26, 11-28, 11-37 derived 3-11 configurations 10-6 drawing views 11-26 sketches 3-11 derived parts 7-21 base 7-22 components 7-23 edit 7-26 mirror 7-22 palette parts 14-10 design methods in assemblies 9-1 design tables base parts 10-28 colors 10-33 components 10-26, 10-27 configuration parameters 10-21, 10-23, 10-24 create 10-14, 10-18 custom properties 10-32 delete configurations 10-13 delete tables 10-21 dimensions 10-25, 10-32 edit 10-21, 10-36 Excel 10-14 expand sub-assemblies in BOMs 10-31 formatting 10-19 in drawings 10-35 lighting 10-31 MDT files 13-29 numerical configuration name 10-21 options 17-2 properties 10-5, 10-32 PropertyManager 10-17 saving 10-22
SolidWorks 2004 Reference Guide
split parts 10-32 suppress 10-27 user notes 10-33 detach segment on drag 3-22 detail circles 11-33 detail views 11-30 copy with parent view 11-50 detailed previews 6-215 hide with parent view 11-51 label display 17-27 modify 11-32 pin position 11-32 profile display 11-32, 17-4 scale 11-32, 17-4 detailing 12-1, 17-19 diagnostic tools 3-16, 3-45, 3-52, 9-28 diameters 3-36 circular dimensions 3-36 dimensions 12-6, 12-10 holes 6-86 holes for cosmetic threads 12-54 in revolve features 6-132 dimensions 3-33, 12-6 access 14-12 align 12-22, 12-23, 12-24 angular 3-37 arcs 3-35, 3-38 baseline 12-17, 17-21 chain 12-10, 12-14, 12-17 chamfer 12-20 circles 3-36, 3-38 configurations 10-11, 10-25, 12-26 copy 12-22 detached drawings 11-14 Dimension/Relations toolbar 2-26 dispaly 2-43 display 12-6 driven 12-10 dual 12-10, 17-19 equations 7-14 extension lines 3-38, 12-6, 12-24 favorites 12-4 foreshortened radius 12-10 hide/show 12-6, 12-27 hole callouts 12-52 horizontal 3-34, 3-35, 12-19 increment value 12-26 inserting into drawings 12-3 internal 14-12 layers 11-58 leaders 12-21 linear 3-34, 3-35, 12-10, 12-24 lines 12-6 link/unlink values 7-17 lock type 3-34, 12-19 mark for drawings 12-26, 17-19 midpoints 12-16 modify 3-33, 12-26 move 12-22 options 12-7, 17-2, 17-7, 17-19, 17-21, 17-25 ordinate 12-17, 12-19 overdefining 17-7
Index-7
override dimensions on drag 3-30, 17-7 parallel 12-19 parentheses 12-17 point-to-point 3-35 projected 11-10 properties 12-10 PropertyManager 12-8 radial 12-24 reference 12-16 selection 12-6 silhouette edges 12-16 sketches 3-33, 3-75, 10-8 standards 17-19 text 12-26, 12-32, 17-25 tolerance 12-28, 12-29 true 11-10 vertical 3-34, 3-35, 12-19 Dimensions/Relations toolbar 2-26 direction of lay 12-56 directional lights 7-47 display 7-42, 17-31 annotations 17-25 assembly annotations 9-73 auxiliary view arrows 11-28 axes in section views 11-40 background image 13-38 center points 17-4, 17-7 design tables in drawings 10-35 detail circle or profile 11-32 dimensions 12-6, 12-8, 12-21 drawing views 11-9, 11-45 entity points 17-4, 17-7 filter for annotations 7-32, 12-32, 17-25 Fit tolerances 12-29 image quality of assemblies 9-72 interfering bodies in HLR/HLG 9-72 modes 11-55, 11-56 OLE objects as icons 2-96 options 17-5, 17-19 quality 11-11 sketch status 17-7 surface cut in section views 11-42 symbols per 2002 12-56, 17-19 text at the same size 9-73 virtual sharps 17-7 display/delete relations 3-44 dissolve 9-39 library features 14-6 sub-assemblies 9-39 distance 3-33 mates 9-14, 9-21, 9-23 measure 7-18 offset 17-21 dock points 12-35 Document 2-82 document color options 17-30 document templates. See templates 2-52 documents 2-2 close all 2-3 colors 17-30 cycle between open 2-18, 2-53 in Windows Explorer 2-55
Index-8
names 12-41 open 2-53 print 2-13 properties 2-81, 11-7, 12-41 save 2-34 templates 2-52 windows 2-2 dome 6-30 dowel pin symbols 12-63 draft quality 2-68, 11-11, 11-16, 17-5 drafts 6-32 allow reduced angle 6-36 analysis 6-198 detailed previews 6-215 extrude 6-39, 6-50 mold design 8-4 neutral planes 6-32, 6-38 parting lines 6-35, 6-37 drag 2-7 and drop planes 5-2 blocks 12-69 break lines in broken views 11-35 components 9-4, 9-11, 9-12 detach sketch entity 3-22 detail view profiles 11-32 drawing views 11-50 edit assembly structure 9-37 feature handles to resize 6-208 FeatureManager design tree 2-56 files into assemblies 2-56 Internet Explorer 2-56 models into drawings 11-17 override dimensions 3-30 select 2-60 tables 12-76 drawing sheets 11-5 customizing sheet formats 11-5 delete 11-4 focus 11-8 formats 11-4, 11-5 multiple 11-4 reorder 11-8 setup 11-4 Drawing toolbar 2-26 drawing views activate 11-8 aligned section 11-42 alignment 11-49 alternate position 11-43 auxiliary 11-28 boundaries 11-9 broken 11-35 broken-out section 11-34 configuration 11-46 copy and paste 11-50 crop 11-33 derived 11-26 detail 11-30 empty 11-10, 11-25 exploded 11-26, 11-28, 11-30, 11-46 first and third angle projection 11-19 hide/show 11-51
isometric or projected dimensions 11-46 lock focus 11-8 model 11-19 perspective 11-19 predefined 11-24 projected 11-26 properties 11-46 relative to model 11-22 rotate 11-49, 11-50 scales 11-9 section 11-37, 11-41 select 11-1, 11-8 standard 11-17 standard 3 views 11-17 update 11-45, 11-47 drawings 11-1, 11-13 2D sketches 11-10 annotations 12-2 assemblies 11-8 component line font 11-55 construction geometry 3-21 design tables 10-35 detached 11-13 display modes 11-55 edge display 17-5 file size 11-13, 17-4 formats, sheets, and views 11-5 hide behind plane 11-53 hide edges 11-51 hide/show components 11-53 inferencing 3-14 insert model items 12-2 layers 11-58 lightweight 11-16 lines 11-55, 11-56, 17-31 move 11-48 names 11-3 new 11-3 OLE objects 11-45 options 11-2, 17-4 parts 4-4, 11-8 print 2-15, 2-16 reference geometry 12-2 save 11-1 scales 11-9 send 2-20, 11-12 sheet metal parts 15-41 show hidden edges 11-52 windows 11-8 driven dimensions 12-6, 12-10 duplicate entities in IGES 13-11 DXF/DWG files 13-19 attach dimensions 13-22 block import 12-69 constrain all 3-19, 13-22 copy/paste from AutoCAD 13-22 DWG preview 13-19 DXF 3D files 13-18 export 13-9, 13-10 export fonts 13-9, 13-10 export options 13-9, 13-10 export version 13-9, 13-10
SolidWorks 2004 Reference Guide
import 13-3 imported entities 13-22 insert 13-21 layer map export 13-10, 13-23 layers 11-58 line styles 13-10 mapping 13-23 View only 13-20 dynamic 7-3 drawing view activation 11-8, 17-4 feature editing 7-3 highlighting 2-59, 2-60 previews 2-68 transparency 2-79 Dynamic Clearance 9-76 E
edge display and selection 17-8 edge display in drawings 17-5 edge flange 15-3 edges 17-8 baseline dimensions 12-17 display options 17-8 hidden edge selection 17-8 highlighting 17-8 in drawings 11-51, 17-5 properties 7-8 edit 7-1 auto reliefs 15-29 bend parameters 15-29, 15-32 blocks 12-69 colors 7-7 configurations 10-11 crop views 11-33 definition 7-1 derived parts 7-26 design tables 10-21, 10-36 dimension access 14-12 equations 7-14, 7-15 exploded views 9-69, 9-71 features 7-1, 7-3 file locations 9-8 forming tools 14-9 imported features 13-4 joined parts 9-57 library features 14-5 macros 2-93 mates 9-8, 9-19 OLE objects 2-95 parts 7-20, 9-48 planes 3-12 seed features 6-129 sketches 3-2, 3-10, 3-12 tables 12-76 weld beads 9-58 eDrawings 13-11, 13-24, 13-25, 13-26 ellipses 3-57 email. See send mail 2-20 embed bitmaps in sheet formats 11-5 empty drawing views 11-10, 11-25 end conditions 6-39, 6-42, 10-10 entities 7-8
Index-9
IGES 13-28 offset 3-30 properties 7-8 envelopes 9-65 create 9-66 remove 9-66 select components 9-66 toggle visibility 9-65 equal length or radius 3-45 equations 7-14 comments and status 7-16 edit and delete 7-15 functions 7-16 in configurations 10-30 operators and constants 7-16 error reporting 2-12 errors in mates 9-31 Excel 17-2 bend table 15-24 bill of materials 12-99 design tables 10-14, 10-18 OLE objects 2-95 SolidWorks API 2-91 existing relations 3-41 exit sketch 3-11 explode blocks 12-69 Explode Sketch toolbar 2-27 exploded views 9-69 assemblies 9-69 collapse 9-70 edit 9-71 in drawings 11-8, 11-26, 11-28, 11-30, 11-46 lines 9-71 sketches 9-71 export documents 13-1, 13-2, 13-9 export options 13-9 ACIS files 13-9 DXF/DWG files 13-9, 13-10 eDrawings files 13-9, 13-11 IGES files 13-9, 13-11 multibody parts 13-16 Parasolid files 13-9, 13-13 STEP files 13-9, 13-13 STL files 13-9, 13-14 TIFF files 13-9, 13-15 VRML files 13-9 export sketch entities in IGES 13-11 extend entities 3-22 extend surface 6-157 extended lines 12-50, 17-19 extension lines 12-24 arcs and circles 3-38 display in dimensions 12-10, 12-13 flip 12-24 hide/show in dimensions 12-6 options 17-19, 17-21 external references 9-42 assemblies 9-42, 9-46 blocks 12-69, 12-75 break 9-43 file management 7-28 list 9-44
Index-10
lock 9-43 note properties 11-7 options 17-15 relations 3-45 rules 9-43 search file locations for 17-15 unlock 9-43 update path 9-43 external relations 3-45 extract sketches 4-5 extrude 6-44 2D to 3D conversion 4-7 boss/base 6-44, 6-45 cut 6-50 detailed previews 6-215 end conditions 6-42 surfaces 6-150 tabs on sheet metal parts 15-9 text 3-65 thin features 6-46 F
face curves 3-23 face fillets 6-70 help points 6-71 split lines 6-73 surfaces 6-156 faces 7-2 deletion 6-177 edit color 7-7 properties 7-8 replace 6-180, 6-181 fasteners 9-77 favorite dimensions and annotations 12-4 favorite hole types 6-80 add 6-81 delete 6-81 retrieve 6-81 update 6-81 feature control frames 12-62 Feature Palette window change dimensions 14-5 display 14-7 drag files into 2-56 edit items 14-9 forming tools 15-25 navigate 14-7 organize 14-7, 14-9 palette items 14-8 thumbnail graphics 14-9 feature statistics 7-28 feature-based mates 9-26 FeatureManager design tree add folders 2-50 assembly component icons 9-3 assembly conventions 9-2 blocks 12-69 color 17-6 component configuration descriptions 2-45 component configuration names 2-45 component descriptions 2-44 configuration descriptions 2-45
conventions 2-46 display by dependencies 9-2 display by features 9-2 displaying mates with components 9-2 drawings 11-8 external references 9-42 flyout 2-49 options 2-49 select drawing views 11-50 select from 2-50 sheet metal parts 15-17 split panel display 2-48 zoom to selection 11-8 features 6-1 accepting 2-9 assemblies 9-55, 9-56 boss/base 6-44, 6-132 chamfer 6-7 circular pattern 6-119 colors 7-7 combined 6-213, 13-29 contours 3-16 copy 2-7, 7-4 curve pattern 6-110 cut 6-47 deform 6-8, 6-9, 6-12, 6-19, 6-21 descriptions 2-43, 2-44 detailed preview 6-215 dome 6-30 draft analysis 6-198, 6-201 drafts 6-32, 6-35, 6-37, 6-38, 6-50 drag 2-7 edit 7-1, 7-2, 7-3 extrude 4-7, 6-39, 6-42, 6-44, 6-46, 6-50 fillets 6-57, 6-58, 6-60, 6-61, 6-62, 6-64, 6-67, 6-70, 6-71, 6-73
guide curves 6-97, 6-99, 6-101, 6-187, 6-189 hide and show bodies 6-175 holes 6-74 in-context 9-42 keep features 6-56 linear pattern 6-114 lofts 6-95, 6-96, 6-97, 6-99, 6-101, 6-104, 6-192 mirror 6-108, 6-125, 6-129 move 2-7, 6-208 out-of-context 9-42 parting lines 6-35, 6-37 patterns 6-108, 6-109, 6-123, 6-125, 6-126, 6-127 revolve 6-132 ribs 6-135, 6-138, 6-139 scale 6-141 scope 9-56 seed features 6-129 shape 6-142, 6-144 shells 6-145, 6-146 sketch driven pattern 6-121 suppress and unsuppress 7-21 sweeps 6-182, 6-183, 6-187, 6-189, 6-190, 6-193 table driven patterns 6-123 tangency 6-190, 6-191, 6-193 tapped hole 13-29 thicken 6-195
SolidWorks 2004 Reference Guide
thin 6-46, 6-94, 6-191 time-dependent 9-49 work 13-29 wrap 6-216 Features toolbar 2-27 file name extensions 2-52 favorites 12-4 sheet formats 11-6 table templates 12-78 file size 17-4 detached drawings 11-13 drawings 17-4 eDrawings 13-24 to send electronically 11-12 files 2-53 blocks 12-69, 12-75 external references 7-28 insert models into drawings 11-17 layers 11-58 locations 9-8, 17-16 names in notes 11-7 new 2-52 open 2-53 properties 7-33 save 2-34 sheet format files 11-6 fill 12-66, 17-6, 17-30 fill surface 6-164 fillets 6-57 constant radius 6-58 face blends 6-70, 6-71, 6-73 overflow type 6-59 radius 6-60 round corner 6-61 setback 6-62 sketch 3-31 surfaces 6-159 variable radius 6-64, 6-67 filter. See selection filter 2-63 find 2-50 in FeatureManager design tree 2-50 referenced documents 9-44 first angle projection 11-4, 11-19 first arc condition 12-10 Fit tolerances 12-8, 12-28, 12-29 fix component 9-11 fix relation 3-42 flag symbols 12-10 flange 15-2 base flange 15-2 edge flange 15-3, 15-4 miter flange 15-4, 15-6, 15-7 flatten 15-32 assembly hierarchy in IGES 13-9, 13-11 assembly hierarchy in Parasolid 13-9 sheet metal parts 15-32 flatten-bends 15-32, 15-44 flexible sub-assemblies 9-41 flip direction 11-40 dowel pin symbols 12-63 flat pattern view in drawings 11-21 section views in drawings 11-40
Index-11
flip side to cut 6-39 float components 9-11 folders 2-50 follow assembly order 12-42, 12-44, 12-83 Font toolbar 2-29 fonts AutoCAD support 13-10 component line font 11-55 detail circle label 11-31, 17-26 dimension text 12-8, 17-26 notes 12-38, 17-26 options 17-26 tables 12-79, 12-80 weld symbols 12-64, 12-65, 12-66, 17-26 foreshortened radius 12-10 form new sub-assemblies 9-37 forming tools 15-25 apply to sheet metal parts 15-28 create 15-25 edit 14-9 openings 15-27 positioning sketches 15-27 fractions 17-28 frame points 3-49 front 2-40 orientation 2-75, 3-4 plane 3-3 views 11-17 fully defined sketches 3-43 fundamentals of SolidWorks 2-1 G
gap 13-6, 17-21 break lines 11-35, 17-19 dimension lines 12-8, 17-21 GB standard 12-59, 17-19 gear mates 9-23 general 17-2 import options 13-7 system options 17-2 geometric characteristic symbol (GCS) 12-62 geometric relations 3-40 automatic 3-40 display/delete 3-44 sketch 3-41 geometric tolerancing 12-60 favorites 12-4 leaders, arrows, fonts 12-62 properties 12-62 geometry pattern 6-114, 6-121, 6-123, 6-127, 6-129 geometry-based mates 9-25 go to command 2-50 GOST standard 12-66, 17-19 gradient background 17-6 gravity 9-35 gray scale drawings 2-15 grid 17-28 align 3-13 options 17-28 snap 17-28 guide curves 6-97, 6-99, 6-101, 6-187, 6-189
Index-12
H
handles 2-6 hatch. See area hatch 12-66 HCG. See highly compressed graphics files 13-26 headers and footers 2-13, 2-83 helix 5-17 help 2-10 quick tips 2-91 SolidWorks 2-10 What's this? 2-10 help points 6-70 hems in sheet metal parts 15-10 hidden 11-55 edges in drawings 11-55 items 2-63 hidden lines removed 2-68, 2-69, 11-57, 17-5 hidden lines visible 2-68, 2-69, 11-57, 17-5 hide 9-62 assembly components 9-62, 9-67 axes 5-12 bodies 6-175 components in drawings 11-53 cosmetic threads 12-27 curvature combs 3-52 dimension extension lines 12-24 dimensions 12-27 drawing components behind plane 11-53 drawing views 11-51 edges in drawings 11-51 layers 11-58 planes 5-10 sketches in drawings 11-52 using envelopes 9-65 high quality 11-11 high trim curve accuracy in IGES 13-11 highlighting 2-59 highly compressed graphics files 13-26 HLR edges in shaded mode 11-55, 17-5 HLR. See hidden lines removed 2-69 hold lines in face fillets 6-71 hole callouts 12-8, 12-52 hole fit 12-8, 12-29 hole tables 12-86 add holes 12-88 datum origin 12-89 options 17-26 tags 12-86 hole wizard 6-77 callouts 12-52 custom standards 6-83, 6-84 favorites 6-81 parameters 6-80 placement 6-79 holes 6-77 3D sketches 6-77 add to table 12-86, 12-88 assemblies 6-81, 9-55 callouts 12-52 counterbore 6-84 countersink 6-85 delete. See surfaces 6-179 end conditions 6-76
fasteners 6-86 favorites 6-80, 6-81 features 6-74, 6-77 hole type 6-86 legacy 6-89 parameters 6-80, 6-86 pipe tap 6-88 placement 6-79 property 6-80 series 6-81 simple 6-74 standards 6-86 tap 6-87 wizard 6-77, 12-52 hollow feature. See shell 6-145 HOOPS files 13-27 horizontal 3-34 align drawing views 11-49 breaks 11-35 dimensions 3-34 ordinate dimensions 12-19 rotate views 11-49 hyperlinks 2-42 in notes 12-37 into drawings 11-17 I
icons 2-3 documents 2-2 FeatureManager 2-46 OLE objects 2-96 rebuild 2-50 IGES files 13-27 2D geometry 13-27 BREP export 13-11, 13-27 edit imported features 13-4 entity types 13-28 export 13-9 export options 13-9, 13-11 exported curves 13-29 exported surfaces 13-12 import 13-3 import hints 13-27 import options 13-7 import surfaces 13-3 import units 13-7 levels 13-29 open 2-53 image quality 9-72, 17-31 image type in TIFF 13-15 import 13-1 diagnosis 13-6 drawings into parts 4-4 files 13-1, 13-2, 13-3 formats 13-2 geometry 13-3 sheet metal parts 15-17 surfaces 13-3 import options 13-3, 13-7 ACIS files 13-7 general 13-7 IGES files 13-7
SolidWorks 2004 Reference Guide
STEP files 13-7 STL files 13-8 VDAFS files 13-7 VRML files 13-8 improve geometry. See simplify geometry 13-6 inches 17-28 in-context features 3-45, 9-42, 9-46, 9-47, 9-55 inferencing 3-14 annotations 12-34 lines 3-6, 3-14 pointers 3-6 to the assembly origin 9-6 inflection points 3-52 insert 12-2 blocks 12-69, 12-73 components into assemblies 9-4 configuration design tables 10-16 dimensions into drawings 12-2, 12-3 DXF/DWG files 13-21 imported geometry 13-3 model items into drawings 12-1, 12-2 SolidWorks data into other applications 2-97 spline points 3-49 inspection dimensions 12-10 instances 12-69 blocks 12-74 components in section views 11-40 holes in hole callouts 12-52 interference detection 9-74 internal dimensions 14-12 Internet open address 2-42 interrupt regeneration 7-32 intersection curves 3-24 invalid edges or faces 7-29 invalid solution found in sketches 3-43 invisible 12-38, 12-69 isometric views 2-75 iso-parametric. See face curves 3-23 item numbers 12-42 balloons 12-42 bill of materials 12-83, 12-85 weldment cut lists 16-16, 16-17 J
JIS standard 17-19 arrowhead style 12-8, 12-12 surface finish size 12-32, 12-57, 17-25 jog 15-36 lines 9-71 ordinate dimensions 12-17, 17-21 points 12-35 sheet metal parts 15-36 joined parts 9-56 create 9-56 edit 9-57 identify 9-58 JPEG files 13-29 jumps 11-17 auxiliary views to parent views 11-28 detail views to parent views 11-30 projected views to parent views 11-26 section views to parent views 11-37
Index-13
standard 3 views to parent views 11-17 stop current jump 2-41 justify text 12-8, 12-38 K
keep constrained corners in fillets 3-31 keep missing item 12-83, 16-16 keyboard 2-84 assign macros 2-93 customize 2-84 shortcuts 2-18 K-Factor 15-23 knit surfaces 6-161 L
labels 11-4 detail views 11-30, 11-32 display options 17-19 next datum 11-4 next view 11-4 options 17-27 section lines 11-42 section views 11-37, 11-40 large assembly mode 9-61, 11-1 Layer Toolbar 2-29 layers 11-58 area hatch 12-68 drawings 11-56, 11-58 IGES files 13-29 import/export 11-58 insert model items 12-2 layer toolbar 2-29 line fonts 11-55 tables 12-76 layout sketches in assemblies 9-54 leaders 12-13, 12-21 balloons 12-42 blocks 12-69, 12-74 display with dimensions 12-10, 12-21 flip in dimensions 12-24 geometric tolerancing 12-60 multiple 12-41, 12-42, 12-60 notes 12-36, 12-69, 17-23 options 17-21 perpendicular 12-60 surface finish symbols 12-56 legacy holes 6-89 levels in IGES files 13-29 library features 14-2 add to parts 14-4 colors 14-5 comparison with palette features 14-1 create 14-3 dissolve 14-6 edit 14-5 limitations 14-1 mandatory references 14-2 lighting 7-45 advanced 7-50 ambient 7-46 basic 7-50 basic controls 7-45
Index-14
cone 7-50 directional lights 7-47 in design tables 10-31 point lights 7-48 position 7-51 spot lights 7-49 lightweight 9-61 components 9-61, 9-64, 10-27 drawings 11-13, 11-16 Limit Mates 9-13 limit mates 9-23 Line Format toolbar 2-29 linear dimensions 3-34, 3-36, 12-6 linear patterns 6-114, 12-48 linear sketch step and repeat 3-25 constrain angle 3-26 fixed spacing 3-26 linear springs 9-34 lines 3-53 2D 3-53 3D 3-69, 3-70 aligned section views 11-42 autotransitioning 3-8 circular center mark 12-50 colors 11-56, 11-58, 12-66 connection center mark 12-50 explode 9-71 extended center mark 12-50 fonts 11-55, 11-56, 17-31 inferencing 3-6, 3-14 jog 9-71 options 17-31 radial center mark 12-50 section lines 11-37 size in center marks 12-48 snap in 3D sketches 3-69 styles 11-55, 11-56, 11-58 thickness 11-56, 11-58 weights 2-14, 11-55 link 2-95 bitmaps to sheet formats 11-5 blocks to file 12-75 dimension favorites 12-4 dimension values 7-17 drawing views to parent views 11-8 errors 11-7, 12-41 notes to documents 12-37 notes to properties 11-7, 12-41 OLE objects 2-95 to thickness 6-39 list 9-42 external references 9-42 hide/show components 11-53 load 13-23 DXF/DWG mapping file 13-23 models in detached drawings 11-13, 11-14 selection criteria for components 9-68 lock 9-43 dimensions 3-34, 12-19, 12-22 external references 9-43 light to model 7-47, 7-48 sheet focus 11-8
view focus 11-8 lofted bends 15-38 lofts 6-90 add sections 6-104 centerlines 6-101 guide curves 6-97, 6-99, 6-101 maintain tangency 6-93 non-planar profiles 6-95, 6-99 planar profiles 6-97 simple 6-91 split lines 6-96 surfaces 6-153 synchronization 6-106 tangent 6-101, 6-103, 6-192 loop selection 2-65 loops 2-61 M
Macro toolbar 2-30 macros customize 2-93 customize buttons 2-84 debug 2-93 edit 2-93 folder 2-93 hot keys 2-93 menus 2-93 new 2-92 pause 2-92 record 2-92 run 2-93 stop recording 2-93 mail. See send mail 2-20 mandatory references 14-2 manual update of drawing views 11-45 manufacturing network 2-90 map file in DXF/DWG 13-10 mark for drawings 12-6, 12-26, 17-19 mark size 12-50 mass properties 7-38 match faces and edges 13-5 mategroups 9-18 material properties 7-5, 7-9 options 17-30 parts 7-5, 7-9 setting default 2-53 material shrinkage (scaling factor) 8-4 materials 2-69 RealView graphics 2-72 supported graphics cards 2-71 Materials Editor PropertyManager 2-38 mathematical relations 7-14 mating 9-13 alignment condition 9-17 angle 9-14, 9-19, 9-23 animation 17-10 assembly components 9-13 automatic 9-25 cam-follower 9-22 coincident 9-14, 9-20 concentric 9-14, 9-20 delete mates 9-28
SolidWorks 2004 Reference Guide
diagnostics 9-28 distance 9-14, 9-21, 9-23 entities 9-15 errors 9-31 feature-based 9-26 FeatureManager design tree 9-2 gear 9-23 geometry-based 9-25 limit 9-23 mate reference 9-17 mategroups 9-18 parallel 9-14, 9-21 pattern-based 9-26 perpendicular 9-14, 9-21 replace entities 9-8 SmartMates 9-25 standard types 9-14, 9-15 suppress mates 9-28 symmetry 9-24 tangent 9-14, 9-22 viewing 9-3 maximum 7-29 edge gap 7-29 radius of curvature 7-29 vertex gap 7-29 MDT. See Mechanical Desktop files 13-29 measure 7-18 measurement options 7-19, 7-38 Mechanical Desktop files 13-29 menus 2-8, 2-86 assign macros 2-93 customize 2-85, 2-86 shortcut 2-8, 2-18 merge tables 12-76 Metastream files. See Viewpoint 13-39 mid surface 6-162 middle mouse button functions 2-78 midpoints 2-63, 5-15 dimensioning to 12-16 relations 3-42 select 2-63, 5-15 minimum radius of splines 3-53 mirror 6-108 components 9-51 features 6-129 parts 7-22 patterns 6-125 sketch entities 3-27 miter flange 15-4, 15-6, 15-7 model views 11-21 models 2-2 geometry 7-29, 7-30 in detached drawings 11-14 modify 12-26 dimensions 3-33, 10-11, 12-26 mates 9-8, 9-19 perspective 2-73 section line properties 11-42 sketches 3-9, 3-15 mold tools 8-2 cavity 8-11 parting lines 8-4
Index-15
parting surfaces 8-7 ruled surfaces 8-9 scaling factors 8-4 shut off surfaces 8-9 tooling split 8-9 undercut detection 8-4 Mold Tools toolbar 2-30 motors 9-33 mouse 2-7 drag 2-7 middle button 2-78 speed 17-18 wheel 2-78 move 9-11 assembly components 9-11, 17-13 drag 2-7 drawing views 11-48 drawings on sheet 11-48 features 6-208 no solve 3-15 ordinate dimensions zero position 12-17 planes 5-10 sketch entities 3-8 sketches 3-27 move/copy 3-15 moving frames 3-49 MTS. See Viewpoint files 13-39 multibody 7-10 cavity 8-9, 8-11 cut 6-47, 6-49 extrude 6-45 feature scope 9-56 hide and show 6-175 modeling techniques 7-10, 7-11, 7-12, 7-13, 7-14 revolve 6-132, 6-151 split parts 7-23 sweeps 6-152, 6-185 versus assemblies 7-10 multi-jog leaders 12-35 multiple 12-33 annotations 12-33 drafts in a rib 6-138 drawing sheets 11-4 leaders 12-36, 12-41, 12-42, 12-56, 12-60 notes 12-36 radius fillets 6-60 multi-threaded retrieval 2-53, 2-55 N
named views. See model views 11-19 names 17-15 drawing sheets 11-4 favorites 12-4 planes 5-8 update 17-15 neutral plane draft 6-38 new assembly document 2-51, 9-39 detached drawings 11-13 drawing document 2-51, 11-3 part document 2-51, 9-47 sketches 3-2, 3-6, 4-10
Index-16
template tabs 2-52 windows 2-3 newlink WP0900 10-1 newlink WP1283 14-6 no solution found in sketches 3-43 no solve move 3-15 normal to curve planes 5-2 not solved status 3-43 notes 12-36 balloons 12-42 borders 17-23 colors 11-56 favorites 12-4 hyperlinks 12-37 in blocks 12-38 in sheet formats 11-5 link to properties 11-7, 12-41 options 17-23 nuts 9-81, 9-86 O
object linking and embedding. See OLE objects 2-95 objects. See OLE objects 11-5 offset 3-30 entities 3-30 planes 5-2 surfaces 6-154 OLE objects 2-95 display as icons 2-96 display contents 2-96 edit 2-95 in drawings 11-5, 11-45 insert existing files 2-95 insert SolidWorks data into other applications 2-97 linking versus embedding 2-95 properties 2-97 reset size 2-97 on surface planes 5-2, 5-5 online help 2-10 open 2-53 configurations of documents 10-3 documents 2-53 documents in other formats 13-3 drawings 11-1, 11-16 existing SolidWorks documents 2-53 files 2-53 parts within assemblies 2-54 sketches 3-6 open Internet address 2-42 optimize surfaces 6-164 options 2-81, 2-86 annotations 12-31, 17-25, 17-26 area hatch 17-6 arrows 17-24 assemblies 17-13 backups 17-19 balloons 17-23 colors, document 17-30 colors, system 17-6 crosshatch 17-30 detailing 12-1, 17-19 dimensions 12-7, 17-21
display style 17-5 drawings 11-2, 17-4 edge display 17-5, 17-8 export 13-9, 13-10, 13-11, 13-13, 13-14, 13-15 external references 17-15 FeatureManager 2-49 file locations 17-16 fonts 17-26 grid 17-28 image quality 17-31 import 13-7, 13-8 large assembly 17-13 line font 17-31 material properties 17-30 notes 17-23 performance 17-10 sketch 17-7 snap 17-28 spin box increments 17-18 system 17-2 tables 17-26 twist control 6-193 units 17-28 view labels 17-27 view rotation 17-18 virtual sharps 17-25 wizard 2-90 ordinate dimensions 12-17, 17-21 orientation 2-75 aligned section views 11-42 auxiliary views 11-28 relative to model views 11-22 section lines 11-42 section views 7-35, 11-37 view 2-75 origins 5-14 coordinate systems 5-13 datum for hole table 12-88, 12-89 inferencing in assemblies 9-6 rotate views 2-79 sketches 3-5 orthographic 11-17 model views 11-19 projected views 11-26 relative to model views 11-22 standard 3 views 11-17 views in drawings 11-19 out-of-context features 9-42 output coordinate systems 5-13, 13-9 over defined 3-43 sketch dimensions/relations 3-43 sketch geometry 3-43 sketches 3-43 overflow type 6-59 overlapping parts. See interference detection 9-74 overlay views. See alternate position views 11-43 override dimensions on drag 3-30 P
page setup drawing colors 2-15 headers and footers 2-83
SolidWorks 2004 Reference Guide
line thickness 11-56 margins 2-15 palette features 14-6 add to assemblies 14-12 add to palette 14-8 add to parts 14-10 comparison with library features 14-1 derived parts 14-10 forming tools 15-28 limitations 14-1 mandatory references 14-2 sheet metal parts 15-28 pan 2-79 paper 2-13 margins 2-15 size 11-4 parabolas 3-61 parallel 12-19 dimensions 12-19 mates 9-14, 9-21 relations 3-42 parallel plane at point 5-2 parallelograms 3-65 parameters 10-33 color 10-33 configurations 10-21, 10-23, 10-24 holes 6-80 Parasolid files 13-33 edit imported features 13-4 export 13-9 export options 13-9 export version 13-9 import 13-3 import surfaces 13-3 open 2-53 parent scale 11-9 parent/child relations 2-43, 2-46, 7-20 parentheses 12-6, 12-17, 12-29, 17-21 part configuration 10-4, 10-8 part numbers 10-28 balloons 12-42 bill of materials 12-83 components 10-28 partial ellipse 3-57 partial sections 11-41, 11-42 parting lines 6-35 drafts 6-35 face blend fillet 6-71 molds 8-4 split lines 5-20 step drafts 6-37 parting surfaces 8-7 parts 7-1 annotations 7-32 assemblies 9-4, 9-47, 9-48 base parts 7-22 check 7-30, 7-31 colors 7-4, 7-7 configurations 10-1, 10-8 curvature 7-39 derived 7-21, 7-22, 7-23, 7-26 dimensions 7-17
Index-17
drawings 11-17 edit 7-1, 7-3, 7-20, 9-48 equations 7-14, 7-15, 7-16 feature statistics 7-28 features 7-1, 7-21 files 7-28 geometry 7-29, 7-30 insert 7-22 join 6-213, 9-56 lighting 7-45 lightweight 9-61 mass properties and section properties 7-38 material properties 7-5, 7-9, 17-30 measure size and distance 7-18, 7-19 mirror parts 7-22 multibody 7-10 parent/child 7-14 references 17-15 section views 7-35, 7-37 sketches 3-3 split 7-23 summary information 7-33 suppress and unsuppress 7-20, 7-21, 10-27 parts list. See bill of materials 12-95 paste 2-35 patch 6-177 boundary 6-164 faces 6-177 patterns 6-108 area hatch 12-68, 17-6 center marks 12-48 circular 6-119, 12-48 components in assemblies 9-49 control and modify 6-126 crosshatch 12-68, 17-30 curve driven 6-110 delete 6-128 geometry 6-127 linear 6-114, 12-48 mates 9-26 mirror feature 6-129 of patterns 6-109 seed feature 6-129 sketch driven 6-121, 6-123 sketches 3-17, 3-25 SmartMates 9-26 table driven 6-123 vary sketches 6-128 pause macro 2-92 PDF Files 13-33 perform full entity check and repair errors 13-7 performance 17-10 data 17-2 large assemblies 9-61, 17-13 lightweight drawings 11-16 performance options 17-10 perpendicular 3-42 leaders 12-60 mates 9-14, 9-21 relations 3-42 perspective 2-72 modify 2-73
Index-18
views in drawings 11-19 views in models 2-72 phantom lines 11-43 Physical Dynamics 9-75 Physical Simulation 9-33, 9-35 gravity 9-35 linear springs 9-34 motors 9-33 overview 9-33 record 9-35 replay 9-35 toolbar 2-32 pictures 3-67, 13-38 pierce relations 3-42, 6-187 pin detail views 11-32 pins 9-77 pipe tap holes 6-88 planes 5-2 at angle 5-2 autosize 5-10 colors 5-8 copy 5-10 creating 5-2 drag and drop 5-2 hide 5-10 hiding components 11-53 line and point 5-2 move 5-10 neutral 6-34 normal to curve 5-2 offset 5-2 on surface 5-2, 5-5 parallel plane at point 5-2 rename 5-8 resize 5-10 show 5-10 show intersections 5-8 sketches 3-3, 3-4, 3-12, 3-13, 10-9 through lines/points 5-2 transparent shaded 5-8 play macro 2-93 point lights 7-48 pointers 11-8 inferencing 3-6 relations 3-40 points 3-55 2D sketch entities 3-55 3D sketch entities 3-73 spline points 3-49 point-to-point dimensions 3-35 polygons 3-63 pop up tooltips 2-10 portrait page orientation 2-13 positioning sketches for forming tools 15-27 precision 12-12 display properties 12-10 options 17-21 PropertyManager 12-8 predefined views 11-21, 11-24 press 12-8, 12-29 previous view 2-80 print 2-13
3D 13-16 background 2-13 break lines in broken views 11-35 documents 2-13 drawings 2-15, 17-4 eDrawings 13-24 headers and footers 2-83 line weights 2-14 margins 2-15 preview 2-18 references 9-46 selection 2-16 setup 2-13 printer settings 2-13 Pro/ENGINEER files 13-33 profiles 11-30 crop views 11-33 detail circles 11-33 detail views 11-30, 11-32 lofts 6-95, 6-97, 6-99 sketch 15-4 sweep sections 6-187, 6-189 projected curves 5-15 replace a sketch 5-19 sketch onto face 5-18 sketch onto sketch 5-18 projected dimensions in drawings 11-10 projected tolerance zone 12-62 projected views 11-26 projection 11-19 during view rotation 11-49 first and third angle 11-4, 11-19 split lines 5-20 propagate 12-48, 12-51 properties 7-2 annotations 9-73, 12-32 assemblies 9-9, 9-73 bill of materials 12-95 components 9-9, 9-67 configurations 10-4, 12-98 custom 7-33, 12-41 datum targets 12-60 design tables 10-5, 10-32 documents 11-7 drawing sheets 11-4 drawing views 11-46 files 7-33 layers 11-58 OLE objects 2-97 sub-assemblies 9-9 PropertyManager 2-4 auto-show 17-2 overview 2-4 skin 17-6 split panel display 2-48 proportional splines 3-47 PTZ. See projected tolerance zone 12-62 publish eDrawings 13-24 Q
quality 13-14 drawing view display 11-11, 11-16
SolidWorks 2004 Reference Guide
STL files 13-14 quick tips 2-91 R
radial center mark lines 12-50 radial dimensions 12-19, 12-22, 12-24 radians 17-28 radiate surface 6-175 radius 12-10 arc dimensions 3-35 circular sketch step and repeat 3-19 control points 6-67 dimension display 12-6, 12-10 fillets 3-31, 6-60 of curvature 7-31, 7-39, 7-40 range, print 2-15 rapid prototyping files 13-37 read-only 17-15 block settings 12-38, 12-69 dimensions 12-10 drawing view properties 11-46 external references 17-15 open 2-53 reload/replace 2-42 realign drawing views 11-49 RealView graphics 2-72 rebuild 2-36 interrupt 7-32 models 2-36 symbol 2-50 updating drawing views 11-47 record macro 2-92 rectangles 3-64 redo 2-36 redraw 2-36 reference axis 5-12 reference dimensions 12-16 baseline 12-17 ordinate 12-17 parentheses 12-17, 17-21 reference edges for auxiliary views 11-28 reference geometry 5-1 axes 5-12 composite curves 5-21 convert sketch entities 5-15 curves 5-15 helix 5-17 insert into drawings 12-2, 12-4 planes 5-2 points 5-22 spiral 5-17 Reference Geometry toolbar 2-31 reference plane normal to edge 3-13 reference points 5-22 reference points in sketch driven patterns 6-123 referenced documents 17-15 load 17-15 open read-only 17-15 save read-only 17-15 search for 9-44 referenced files 17-16 in assemblies 9-8
Index-19
locations 9-8 refresh screen. See redraw 2-36 regenerate. See rebuild 2-36, 7-32 relations 3-42 add relations 3-41 automatic 3-40 callouts 3-43 dangling 7-4 display/delete 3-41 equal length/radii 3-45 geometric 3-40 mathematical 7-14 parent/child 2-46 replace entity 3-41 sketch relations in configurations 10-9 relative to model views 11-22 reload 2-42 shared documents 2-42 sheet format 11-4 remove crop view 11-33 removed tangent edge 11-57, 17-5 rename 7-28 features 2-43 files 7-28, 9-37, 9-38 flat pattern configuration 11-21 menu items 2-85 planes 5-1 reorder 9-39 assembly components 9-39, 9-53 bends 15-31 reorderfeatures 2-43 repair imported document 13-6 repair sketch 4-10 replace 9-7 assembly components 9-7 background images 13-38 mated entities 9-8 shared documents 9-7 sketch entities 3-44 surfaces 6-180 reset size of OLE objects 2-97 resize 7-3 features 6-208, 7-1, 7-3 planes 5-10 view boundaries 11-9 resolve 9-63 ambiguity 7-27 assembly components 9-63, 9-64 lightweight components 9-64 lightweight drawings 11-16 restore 3-33 broken views 11-35 dimensions 3-33 retain folder structure 2-58 reverse surface 6-164 revert model to earlier state 2-47 revision tables 12-91 custom property 17-4 options 17-26 symbols 17-26 revolve 6-132 features 6-132
Index-20
surfaces 6-151 ribs 6-135 detailed previews 6-215 drafts 6-138 linear and natural types 6-136, 6-138 open sketch 6-139 right 2-40, 3-4 right-mouse menus. See shortcut menus 2-8 rigid sub-assemblies 9-41 rip 15-30 roll back 9-53 assemblies 9-53 rollback bar 2-47 rotate 2-79 assembly components 9-12, 17-13 blocks 12-74 center marks 12-48 drawing views 11-49, 11-50 sketches 3-27 surface finish symbols 12-56 views 2-79 roughness 12-56 round corner fillets 6-61 row numbers 12-96 ruled surfaces 8-9 rulers in drawings 11-8 run macro 2-93 S
sat files (ACIS) 13-17 satisfied sketch dimensions/relations 3-43 save 2-34 assemblies 7-10, 9-6, 9-7, 9-46 assembly as multibody part 7-10 automatic save 17-19 blocks 12-69 design tables 10-22 dimensions 3-33 documents 2-34 drawings 11-1, 11-13 DXF/DWG mapping file 13-23 files 2-34 IGES assemblies in single files 13-11 properties in sheet formats 11-7 save as 2-34, 2-82, 7-10, 9-6, 9-7 save as copy 9-6, 9-7 selection criteria for components 9-68 sheet formats 11-6 table driven patterns 6-125 templates 2-52 VRML assemblies in single files 13-9 scale 6-141 automatic 11-9, 17-4 blocks 12-69, 12-74 custom 11-9 detail views 11-32, 17-4 drawings 11-4, 11-9 parent 11-9 parts 6-141 predefined views 11-24 print drawings 2-15 section lines 11-42
sketches 3-27 text of annotations 12-32, 17-25 scaling factor in mold design 8-4 scan equal 3-45 schematic 11-44 scope 9-56 assembly features 9-56 Collision Detection 9-74 multibody parts 9-56 Physical Dynamics 9-75 section views of assemblies 11-41 screen redraw 2-36 screws 9-77, 9-79 scroll. See pan 2-79 search 9-44 file locations for external references 9-44 results for assemblies 9-46 second arc condition 12-10 second arrow 12-10 second outside arrow 12-10 section display types 17-21 section lines 11-37 modify 11-40 stepped 11-37 straight 11-37 troubleshooting 11-41 section properties 7-38 section scope in drawings 11-40, 11-41 section views 11-37 aligned 11-42 assemblies 7-35, 11-40 auto hatching 11-38 broken-out 11-34 copy with parent view 11-50 create 2-73, 11-37 display only surface cut 11-42 drawings 11-37 hide with parent view 11-51 modify 11-40 partial 11-37 parts 7-35 planes 7-37 section line properties 11-42 Section View PropertyManager 2-74 selection 7-36 troubleshooting 11-41 VRML files 13-40 seed faces 6-161 seed features 6-110, 6-114, 6-119, 6-123, 6-129 select 2-60 area of drawing to print 2-15 chain 2-62 contours 3-19 drag select 2-60 from FeatureManager design tree 2-50 hidden entities 11-51, 17-4 in graphics area 2-60 loops 2-65 midpoints 2-63, 5-15 multiple items 2-60 other 2-63 select using envelope 9-66
SolidWorks 2004 Reference Guide
silhouettes 3-8 sketch entities 2-60 tables 12-76 tangency 2-65 through transparency 2-66, 17-8 views 11-8 selection 2-64 box 2-64 loop 2-65 partial loop 2-61 tangent 2-65 selection criteria for components 9-68 selection filter 2-63 hot keys 2-63 toolbar 2-63 send mail 2-20 assemblies 2-20 drawings 11-12 parts 7-32 service packs 2-91 set up drawing sheet 11-4 setback fillets 6-62 shaded 2-74 cosmetic threads 12-54, 17-25 preview 2-68, 17-10 sketch planes 3-12, 5-8 views 2-59, 2-74, 17-5 shaded with edges 2-75 shaft Fit 12-8, 12-29 shape 6-142, 6-144 feature adjustment controls 6-144 features 6-142 pressure and curve influence sliders 6-144 resolution slider 6-145 stretch and bend sliders 6-145 shared files 2-42 shared values 7-17 sheet formats 11-3 anchor points 11-5, 12-77 custom 11-5 lines 11-5 link notes to properties 11-7 new 11-3 new drawings 11-3 note text 11-5 save 11-6 sheet metal parts auto reliefs 15-28, 15-29 base flange 15-2 bends 15-9, 15-12, 15-13, 15-14, 15-22, 15-23, 15-24, 15-25, 15-29, 15-31, 15-32, 15-34
break corner 15-35 conical faces 15-15 cuts 15-34, 15-35 cylindrical faces 15-40 design methods 15-18, 15-19, 15-20, 15-21 drawings 11-21, 15-41 edge flange 15-3, 15-4 FeatureManager design tree 15-2, 15-17 flat pattern 15-32, 15-42 flat pattern configuration 11-21, 15-44 flatten 15-32
Index-21
fold 15-45 forming tools 15-25, 15-27, 15-28, 15-32, 15-42 hems 15-10 import 15-17 inserting bends 15-31 jog 15-36 lofted bends 15-38 mirror 15-33 miter flange 15-4, 15-6, 15-7 overview 15-1, 15-18, 15-19, 15-20, 15-21 rip 15-30 simplify bends 15-43 tabs 15-9 trim bends 15-8 unfold 15-32, 15-42, 15-45 walls 15-16 Sheet Metal toolbar 2-31 sheet properties 11-4 sheets. See drawing sheets 11-5 shells 6-145, 6-146, 6-147 shortcut 2-18 customize shortcut menus 2-86 keys 2-18 menus 2-8, 12-6 show 11-51 alignment 12-22 assembly components 9-62, 9-67 axes 5-12 bodies 6-175 component configuration descriptions 2-45 component configuration names 2-45 component descriptions 2-44 configuration descriptions 2-45 cosmetic threads 12-27, 12-54 curvature combs 3-52 dimension extension lines 12-24 dimensions 12-27 drawing views 11-51 edges in drawings 11-51 explode steps 9-71 feature descriptions 2-44 hidden edges in drawings 11-52, 17-4 hidden views 11-51 in design tables 10-26 planes 5-10 show annotation link errors 12-41 show STL info before saving file 13-14 sketches in drawings 11-52 using envelopes 9-65 shut-off surfaces 8-9 side views 11-17 silhouettes 3-8, 5-20, 12-16 simple hole 6-74 simplify 9-61 assemblies 9-61 bends 15-43 complex models 10-1 geometry 13-6 splines 3-49 simulation. See Physical Simulation 9-33 size features 6-208 sketch driven patterns 6-121
Index-22
sketch entities 3-57 arcs 3-59, 3-68 autodimension 3-39 centerlines 3-58 circles 3-55 copy 3-15, 3-27 ellipses 3-57 extend 3-22 lines 3-53, 3-69, 3-70 move 3-15, 3-27 parabolas 3-61 parallelograms 3-65 points 3-55, 3-73 polygons 3-63 rectangles 3-64, 3-65 rotate 3-15, 3-27 scale 3-15, 3-27 select 2-60 splines 3-46, 3-71 text 3-65 Sketch toolbar 2-32, 3-68 sketch tools 2-32 autodimension 3-39 chamfer 3-31, 3-58 circular step and repeat 3-17 construction geometry 3-21 convert entities 3-22 curvature combs 3-52 diagnostics 3-16, 3-45 extend 3-22 face curves 3-23 fillets 3-31, 3-58 intersection curves 3-24 linear step and repeat 3-25 mirror 3-27 modify 3-9 move/copy 3-15 offset entities 3-30 patterns 3-17, 3-25, 6-108 picture 3-67 select 2-60 split entities 3-32 trim entities 3-32 sketches 3-1 3D 3-68 align 4-6 assemblies 9-54 autodimension 3-39 broken views 11-35 close 3-11, 3-21 colors 3-43 complexity 3-5 copy 3-27 curves 3-22 cut 3-8 derived 3-11 dimensions 3-33, 10-8 edit 3-2, 3-10, 3-12 equations 3-33 exit 3-2, 3-11 extract 4-5 frame points 3-49
geometry 3-14, 3-21 grids 3-13 imported 13-22 in drawings 11-10, 11-28, 11-30, 11-37, 11-40, 11-42, 11-52, 11-56
inferencing 3-6, 3-14 modes 3-7, 3-8 move 3-9, 3-15 new 3-2, 3-6 no solve move 3-15 options 17-7 origins 3-5 parts 3-3 paste 3-8 patterns 3-17, 3-25, 6-123 planes 3-12, 3-13, 10-9 relations 3-40, 3-42, 3-43, 3-44, 10-9 repair 4-10 rotate 3-27 scale 3-27 select chain 2-62 splines 3-49 starting a sketch 3-3, 3-4, 3-5 status 3-43 status bar 3-5 skins 2-87, 17-6 slant extension lines 12-6, 12-24 SldTrans 1.0 (Pro/ENGINEER) 13-33 SldUG 1.0 (Unigraphics II) 13-39 Smart Fasteners 9-77 add nuts and washers 9-86 bolt patterns 9-89 bottom stack 9-78, 9-86 change type 9-85 configurations 9-89 defaults 9-78, 9-90 edit 9-85, 9-86, 9-87 flip 9-85 holes 9-77, 9-83 insert 9-78 overview 9-77 part numbers 9-88 patterns 9-83 PropertyManager 9-78 top stack 9-78, 9-86 unsupported hole types 9-83 update 9-90 SmartMates 9-25 feature-based 9-26 geometry-based 9-25 moving components 9-27 pattern-based 9-26 snap 17-28 3D sketches 3-69 blocks 12-69 dimension text 17-21 notes 12-36 software OpenGL 17-10 Solid Edge files 13-36 solid fill 12-66 SolidWorks 2-1 basic concepts 2-2
SolidWorks 2004 Reference Guide
fundamentals 2-1 service packs 2-91 subscription service 2-91 SolidWorks API 2-91 SolidWorks Office toolbar 2-33 SolidWorks web site 2-92 solve 3-14 equations 7-14 mategroups 9-18 move/copy 3-15 relations in imported drawings 3-19 sketch geometry 3-14 sort 12-76 space handles 3-75 spin box increments 3-33, 12-26, 17-18 spiral 5-17 splines 3-46 3D 3-71 curvature combs 3-52 fit spline 3-48 inflection points 3-52 insert points 3-49 minimum radius 3-53 moving frames 3-49 proportional 3-47 simplify 3-49 Spline Tools toolbar 2-33 split 2-48 bar 2-4 entities 3-32 hole series 9-87 panel display 2-43, 2-48 parts 7-23 tables 12-76 split lines 5-20 balloon style 12-42 drafts 6-35, 6-37 fillets 6-71, 6-73 lofts 6-96 projection 5-20 silhouette 5-20 surfaces 5-20 spot lights 7-49 springs 9-34 stacked balloons 12-44, 12-46, 17-23 standard 3 views 11-17, 11-19 standard mates 9-14, 9-15 Standard toolbar 2-33 Standard Views toolbar 2-40 standards 17-19 ANSI 1982 12-58 ANSI basic tolerances 17-21 holes 6-80, 6-86 surface finish symbols 12-56, 12-57, 17-19 welds 9-58 start command when creating new drawing 11-21 statistics, assembly 9-9 status bar 2-10, 3-5 STEP files 13-37 edit imported features 13-4 export 13-9, 13-13 import 13-3
Index-23
import options 13-37 import surfaces 13-3 import units 13-7 open 2-53 wireframe import 13-37 STL files (stereolithography) 13-37 export 13-9, 13-14 export options 13-9, 13-14 stop current jump 2-41 stop macro 2-93 stp files (STEP) 13-37 straight break line cut style 11-37 styles 11-56 cuts in broken views 11-35, 11-37 detail circles 11-32, 11-33 lines in drawings 11-55, 11-56 lines in layers 11-58 sub-assemblies 9-36 automatic change of editing focus 9-41 create 9-36 dissolve 9-39 editing limitations 9-41 flexible 9-41 forming a new 9-37 inserting a new 9-39 lightweight 9-61 manual change of editing focus 9-40 modify 9-36 rigid 9-41 summary 7-33 suppress 10-27 assembly components 9-63, 9-64 components or features in design tables 10-27 features 2-43, 7-2, 7-20, 7-21 mates 9-28 surface errors on import 13-3 surface finish symbols 12-4, 12-56, 17-25 surface flaws on import 6-164 surface representation in IGES 13-12 surfaces 6-148 bodies 6-149 colors 7-8, 17-8 cut 6-49, 6-195 delete 6-177, 6-179 draft analysis 6-198 drafts 6-32 extend 6-157 extruded 6-150 filled 6-164 fillets 6-64, 6-156, 6-159 hide and show bodies 6-175 import 13-3 knit 6-161 lofted 6-153 mid surface 6-162 molds 8-6, 8-7, 8-9 offset 6-154 optimize 6-164 parting 8-7 planar 6-149, 7-30 planes 5-2, 5-5 radiate 6-175
Index-24
replace 6-180 reverse 6-164 revolve 6-151 ruled 8-9 shut-off 8-9 swept 6-152 thicken 6-195 trim 6-170 untrim 6-172 Surfaces toolbar 2-40 sweeps 6-182 advanced smoothing 6-191 align with end faces 6-190 follow path 6-193, 6-194 follow path and guide curves 6-193 guide curves 6-187, 6-189 intermediate sections 6-189 keep normal constant 6-193 orientation 6-193, 6-194 overview 6-182 simple 6-183 smoothing 6-190 surfaces 6-152 tangency 6-191, 6-193 thin feature 6-183 symbols 12-10 flag 12-10 geometric tolerancing 12-62 in note text 12-10, 12-38 revision 12-91, 12-92, 17-26 symmetric relations 3-41 symmetric tolerance 12-8, 12-28 symmetry 3-58 about centerlines 3-58 mates 9-24 synchronize detached drawings 11-13 system color options 17-6 system options 2-81 T
table driven patterns 6-123, 6-125 table pattern coordinates 6-125 tables 12-76 anchors 12-77 bill of materials 12-81 columns 12-85, 12-90, 12-93, 16-17 custom templates 12-79 design tables 10-18 drag 12-76 edit 12-76 format 12-79, 12-80 hole tables 12-86 options 17-26 revision tables 12-91 templates 12-78, 12-79 weldment cut lists 16-15 tabs on sheet metal parts 15-9 tag name 12-38, 12-69 tags for hole tables 12-86, 12-89 tangent 3-42 arcs 3-59 lofts 6-101, 6-103, 6-192
mates 9-14, 9-22 selection 2-65 sketch relations 3-42 sweeps 6-190, 6-193 tangent edge display 11-57, 17-5 tangent to surface planes 5-5 tap holes 6-87 templates 2-52 bill of materials 12-78 create 2-52 default 2-53 file types 2-52 predefined views 11-24 schematic 11-44 tables 12-78, 12-79 tabs 2-52 view reference geometry 5-1 temporary axes 5-12 text 17-25 dimensions 12-22 extruded text on part 3-65 notes 12-36 size of annotations 12-32, 17-25 sketch 3-65 textures 2-39, 2-77 thicken surfaces 6-195 thickness 11-56, 11-58 thin features 6-45, 6-46, 6-94, 6-191 third angle projection 11-19 third party products. See add-ins 2-89 threads, cosmetic 12-54 through lines/points planes 5-2 thumbnail graphics 14-9 palette items 14-9 TIFF files 13-38 export 13-9, 13-15 export options 13-9, 13-15 import 13-38 tile graphics windows 2-3 time-dependent features 9-49 tip of the day 2-10 tolerances 12-28 chamfer dimensions 12-20 dimensions 12-28 Fit 12-8, 12-28, 12-29 geometric tolerancing 12-60 include prefix 17-21 options 17-21 simplify splines 3-49 toolbars 2D to 3D 2-22 Align 2-22 Annotations 2-23 arrange 2-21 Assembly 2-24 Curves 2-25 customize 2-86 Dimensions/Relations 2-26 dispaly or hide 2-21 Drawing 2-26 Explode Sketch 2-27 Features 2-27
SolidWorks 2004 Reference Guide
Font 2-29 Layer 2-29 Line Format 2-29 Macro 2-30 Mold Tools 2-30 Reference Geometry 2-31 Selection Filter 2-63 Sheet Metal 2-31 Simulation 2-32 Sketch 2-32 SolidWorks Office 2-33 Spline Tools 2-33 Standard 2-33 Standard Views 2-40 Surfaces 2-40 Tools 2-41 View 2-41 Web 2-41 Weldments 2-43 tooling split 8-9 tools 2-41 check 7-31 curvature 7-39 equations 7-14 mass properties and section properties 7-38 measure 7-18 Tools toolbar 2-41 tooltips 2-10 top 2-40 gradient color 17-6 orientation 2-75, 3-4 views 11-17 top-down assembly design 9-1 trailing zeros 17-19 transitional 12-8, 12-29 translate sketches 3-15 translators 13-2 ACIS 13-7, 13-9, 13-17 Autodesk Inventor 13-17 CADKEY 13-17 CATIA Graphics 13-18 DXF 3D 13-18 HCG 13-26 HOOPS 13-27 IGES 13-7, 13-11, 13-27, 13-28, 13-29 JPEG 13-29 Mechanical Desktop 13-29 Parasolid 13-13, 13-33 PDF Files 13-33 Pro/ENGINEER 13-33, 13-34, 13-35, 13-36 Solid Edge 13-36 STEP 13-7, 13-13, 13-37 STL 13-8, 13-14, 13-37 Unigraphics 13-39 VDAFS 13-7, 13-39 Viewpoint 13-39 VRML 13-8, 13-15, 13-40 ZGL 13-40 transparency 2-66, 2-79, 3-12, 5-8, 9-48, 9-62, 17-8, 17-10 triad 9-11, 9-12 move 9-11 rotate 9-12
Index-25
trigonometric functions in dimensions 3-33 trim 3-32 sheet metal bends 15-8 sketch segments 3-32 surfaces 6-170 trimmed surfaces in IGES 13-11 troubleshooting section views 11-41 True Position Tolerancing 12-62 true type dimensions 11-10 U
un-break broken views 11-35 under defined 2-46 sketch geometry 3-43 sketches 3-43 undercut detection 8-4 underlined leader 12-38 undo 2-36 Unigraphics II files 13-39 units 17-28 dimension properties 12-10 options 17-28 spin box increments 17-18 unlink values 7-17 unlock external references 9-43 unsuppress 7-21 components 10-27 features 7-2, 7-20, 7-21, 10-27 untrim surface 6-172 update 11-45 dependent drawing views 11-49 detached drawings 11-13 drawing views 11-45 paths in assemblies 9-43 section views 11-40 views in detached drawings 11-13 user notes in design tables 10-33 UV curves. See face curves 3-23 V
variable radius fillets 6-64 variable thickness shells 6-146 variables 12-52, 12-53 vary sketches in patterns 6-128 VBA 2-94 VDAFS files 13-39 edit imported features 13-4 export 13-9 import 13-3 import options 13-7 import surfaces 13-3 import units 13-7 open 2-53 vertical 3-34 align drawing views 11-49 breaks 11-35 dimensions 3-34 ordinate dimensions 12-19 rotate views 11-49 vertices 5-13 angular dimensions 3-37 baseline dimensions 12-17
Index-26
chamfers 6-7 coordinate system 5-13 end condition 6-76 reference points 5-22, 6-123 view 2-75 animation speed 17-18 axes 5-12 bodies 6-175 dependencies 9-2 features 9-2 mates 9-3 orientation 2-75 planes 5-10, 11-53 reference geometry 5-1 section 7-37, 11-37 temporary axes 5-12 view boundaries 11-9 detached drawings 11-13 resize 11-9 view label options 17-27 View only DXF/DWG 13-20 view only mode 2-53 view rotation options 17-18 View toolbar 2-41 view/hide toolbars 2-21 Viewpoint files 13-39 views 2-68 draft quality 2-68 hidden in gray 2-69 hidden lines removed 2-69 middle mouse button 2-78 new windows 2-3 orientation 2-75 pan 2-79 perspective 2-72 previous 2-80 quality 11-11 RealView graphics 2-72 rotate 2-79 shaded 2-74 shaded with edges 2-75 SolidWorks Viewer 2-78 textures 2-77 view-only mode 2-78 wireframe 2-78 zoom 2-80, 2-81 virtual sharps 3-58, 3-75, 17-25 visible 10-26 components in a design tables 10-26 cosmetic threads 12-54 edges in drawings 11-55 layers 11-58 tangent edge display 11-57, 17-5 Visio 11-44 Visual Basic for Applications 2-94 VRML files 13-40 edit imported features 13-4 export 13-9 export options 13-9 import 13-3 import surfaces 13-3 open 2-53
W
walls in sheet metal parts 15-16 washers 9-82, 9-86 watermarks 11-13, 11-16 web folders change URL 2-58 copy referenced files to server 2-58 opening files from 2-57 overview 2-57 saving files to 2-57 Web support 2-42 open address 2-42 stop jump 2-41 Web toolbar 2-41 weld beads 9-58 automatic weld symbols 9-60 create 9-58 edit 9-58 select faces 9-60 standards 9-58 types 9-58 weld symbols 12-64 ANSI 12-65 display 17-19 edit 12-64 favorites 12-4 fonts 17-26 GOST 12-66 insert 12-64 options 17-19 properties 12-64 weldment cut lists 16-15 anchor 12-77 configurations 16-15 custom properties 16-15 item numbers 16-16 templates 12-78 weldments 16-1 corner treatments 16-4 custom properties 16-18 cut lists 16-15 end caps 16-13 fillet weld beads 16-10 gussets 16-7 structural members 16-1 sub weldments 16-14 trim and extend 16-5 weldment drawings 16-14
SolidWorks 2004 Reference Guide
Weldments toolbar 2-43 What's this? 2-10 What's wrong? 2-12 windows 2-2 cascade 2-3 close all 2-2 drawings 11-8 new 2-3 tile 2-3 Windows Explorer 2-55 wireframe 2-78, 17-5 witness lines. See extension lines 12-24 wizards 2-90 conversion 2-89 copy options 2-90 holes 6-77 work features, MDT files 13-29 wrap 6-216 X
X display 12-20 x_b or x_t files (Parasolid) 13-33 xmt_bin or xmt_txt files (Parasolid) 13-33 XREFs 13-19 Z
zebra stripes 7-42, 7-44 zeros 17-19 color default 10-33 configuration parameter default 10-24 leading 17-19 trailing 17-19 ZGL files 13-40 zig zag break line cut style 11-37 zone 12-93 zoom 2-81 in/out 2-81 to area 2-80 to fit 2-80 to selection 2-81, 11-8
Index-27
Index-28
© 1995-2004, SolidWorks Corporation 300 Baker Avenue Concord, Massachusetts 01742 USA All Rights Reserved U.S. Patents 5,815,154; 6,219,049; 6,219,055; 6,603,486; 6,611,725 and certain foreign patents. U.S. and foreign patents pending. SolidWorks Corporation is a Dassault Systemes S.A. (Nasdaq:DASTY) company. The information and the software discussed in this document are subject to change without notice and should not be considered commitments by SolidWorks Corporation. No material may be reproduced or transmitted in any form or by any means, electronic or mechanical, for any purpose without the express written permission of SolidWorks Corporation. The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of this license. All warranties given by SolidWorks Corporation as to the software and documentation are set forth in the SolidWorks Corporation License and Subscription Service Agreement, and nothing stated in, or implied by, this document or its contents shall be considered or deemed a modification or amendment of such warranties. SolidWorks® is a registered trademark of SolidWorks Corporation. SolidWorks 2004 is a product name of SolidWorks Corporation. FeatureManager® is a jointly owned registered trademark of SolidWorks Corporation. Feature Palette™, PhotoWorks™, and PDMWorks™ are trademarks of SolidWorks Corporation. ACIS® is a registered trademark of Spatial Corporation. FeatureWorks® is a registered trademark of Geometric Software Solutions Co. Limited. GLOBEtrotter® and FLEXlm® are registered trademarks of Globetrotter Software, Inc. Other brand or product names are trademarks or registered trademarks of their respective holders.
COMMERCIAL COMPUTER SOFTWARE - PROPRIETARY U.S. Government Restricted Rights. Use, duplication, or disclosure by the government is subject to restrictions as set forth in FAR 52.227-19 (Commercial Computer Software - Restricted Rights), DFARS 227.7202 (Commercial Computer Software and Commercial Computer Software Documentation), and in the license agreement, as applicable. Contractor/Manufacturer: SolidWorks Corporation, 300 Baker Avenue, Concord, Massachusetts 01742 USA Portions of this software are copyrighted by and are the property of Electronic Data Systems Corporation or its subsidiaries, copyright© 2004 Portions of this software © 1988, 2000 Aladdin Enterprises. Portions of this software © 1996, 2001 Artifex Software, Inc. Portions of this software © 2001 artofcode LLC. Portions of this software © 2004 Bluebeam Software, Inc. Portions of this software © 1999, 2002-2004 ComponentOne Portions of this software © 1990-2004 D-Cubed Limited. Portions of this product are distributed under license from DC Micro Development, Copyright © 1994-2002 DC Micro Development, Inc. All rights reserved Portions © eHelp Corporation. All rights reserved. Portions of this software © 1998-2004 Geometric Software Solutions Co. Limited. Portions of this software © 1986-2004 mental images GmbH & Co. KG Portions of this software © 1996 Microsoft Corporation. All Rights Reserved. Portions of this software © 2001, SIMULOG. Portions of this software © 1995-2004 Spatial Corporation. Portions of this software © 2003-2004, Structural Research & Analysis Corp. Portions of this software © 1997-2004 Tech Soft America. Portions of this software © 1999-2004 Viewpoint Corporation. Portions of this software © 1994-2004, Visual Kinematics, Inc. This software is based in part on the work of the Independent JPEG group. All Rights Reserved
Contents
Chapter 1
SolidWorks 2004 Reference Guide
Scope ................................................................................................................................................................................. 1-1 Discounted Printing Offer ................................................................................................................................................. 1-1 Conventions ....................................................................................................................................................................... 1-1 Resources ........................................................................................................................................................................... 1-2
Chapter 2
SolidWorks Fundamentals
SolidWorks Fundamentals ................................................................................................................................................. 2-1 Basic Concepts .................................................................................................................................................................. 2-2 Document Windows .......................................................................................................................................................... 2-2 Cascade ....................................................................................................................................................................... 2-3 Tile Horizontally - Tile Vertically ............................................................................................................................. 2-3 Arrange Icons ............................................................................................................................................................. 2-3 Close All ..................................................................................................................................................................... 2-3 New Window .............................................................................................................................................................. 2-3 PropertyManager Overview .............................................................................................................................................. 2-4 Callouts and Handles ......................................................................................................................................................... 2-6 Drag and Drop ................................................................................................................................................................... 2-7 Shortcut Menu ................................................................................................................................................................... 2-8 Accepting Features ............................................................................................................................................................ 2-9 Pop-up Tooltips ............................................................................................................................................................... 2-10 Help ................................................................................................................................................................................. 2-10 What's Wrong? ................................................................................................................................................................ 2-12 Print ................................................................................................................................................................................. 2-13 Page Setup ................................................................................................................................................................ 2-13 Line Weights ............................................................................................................................................................ 2-14 Margins ..................................................................................................................................................................... 2-15 Printing Drawings .................................................................................................................................................... 2-15 Print Selection .......................................................................................................................................................... 2-16 Custom Scale Examples ........................................................................................................................................... 2-17 Print Preview ............................................................................................................................................................ 2-18 Keyboard Shortcuts ......................................................................................................................................................... 2-18 Send Mail ......................................................................................................................................................................... 2-20 Toolbars ........................................................................................................................................................................... 2-21 Toolbars .................................................................................................................................................................... 2-21 2D to 3D Toolbar ..................................................................................................................................................... 2-22 Align Toolbar ........................................................................................................................................................... 2-22 Annotations Toolbar ................................................................................................................................................. 2-23 Assembly Toolbar .................................................................................................................................................... 2-24 CommandManager ................................................................................................................................................... 2-24 Curves Toolbar ......................................................................................................................................................... 2-25 Dimensions/Relations Toolbar and Menus .............................................................................................................. 2-26
SolidWorks 2004 Reference Guide
i
Drawing Toolbar ......................................................................................................................................................2-26 Explode Sketch Toolbar ...........................................................................................................................................2-27 Features Toolbar .......................................................................................................................................................2-27 Font Toolbar .............................................................................................................................................................2-29 Layer Toolbar ...........................................................................................................................................................2-29 Line Format Toolbar .................................................................................................................................................2-29 Macro Toolbar ..........................................................................................................................................................2-30 Mold Tools Toolbar ..................................................................................................................................................2-30 Reference Geometry Toolbar ...................................................................................................................................2-31 Sheet Metal Toolbar .................................................................................................................................................2-31 Simulation Toolbar ...................................................................................................................................................2-32 Sketch Toolbar ..........................................................................................................................................................2-32 SolidWorks Office Toolbar ......................................................................................................................................2-33 Spline Tools Toolbar ................................................................................................................................................2-33 Standard Toolbar ......................................................................................................................................................2-33 Save ...................................................................................................................................................................2-34 Save As ..............................................................................................................................................................2-34 Cut .....................................................................................................................................................................2-35 Copy ..................................................................................................................................................................2-35 Paste ..................................................................................................................................................................2-35 Delete ................................................................................................................................................................2-35 Undo ..................................................................................................................................................................2-36 Redo ..................................................................................................................................................................2-36 Rebuild ..............................................................................................................................................................2-36 Redraw ..............................................................................................................................................................2-36 Color And Optics PropertyManager .................................................................................................................2-37 Materials Editor PropertyManager ....................................................................................................................2-38 Texture PropertyManager .................................................................................................................................2-39 Show Web Toolbar ............................................................................................................................................2-39 Standard Views Toolbar ...........................................................................................................................................2-40 Surfaces Toolbar .......................................................................................................................................................2-40 Tools Toolbar ...........................................................................................................................................................2-41 View Toolbar ............................................................................................................................................................2-41 Web Toolbar .............................................................................................................................................................2-41 Stop Current Jump .............................................................................................................................................2-41 Reload Documents ............................................................................................................................................2-42 Insert Hyperlink .................................................................................................................................................2-42 Open Internet Address .......................................................................................................................................2-42 Weldments Toolbar ..................................................................................................................................................2-43 FeatureManager Design Tree ..........................................................................................................................................2-43 FeatureManager Design Tree ...................................................................................................................................2-43 Show Feature's Description ...............................................................................................................................2-44 Show Component's Description ........................................................................................................................2-44 Show Component's Configuration Name ..........................................................................................................2-45 Show Component's Configuration Description .................................................................................................2-45 Show Configuration's Description ....................................................................................................................2-45 FeatureManager Design Tree Conventions ..............................................................................................................2-46 Parent/Child Relationships .......................................................................................................................................2-46 Rollback Bar .............................................................................................................................................................2-47 Split Panel Display ...................................................................................................................................................2-48 Flyout FeatureManager Design Tree ........................................................................................................................2-49 FeatureManager Options ..........................................................................................................................................2-49 Selecting from the FeatureManager Design Tree .....................................................................................................2-50 Find in FeatureManager Design Tree .......................................................................................................................2-50 Add Folders ..............................................................................................................................................................2-50 Opening New and Existing Documents in SolidWorks ..................................................................................................2-51 New SolidWorks Document .....................................................................................................................................2-51
ii
Default Templates .....................................................................................................................................................2-52 Creating Additional Template Tabs ..........................................................................................................................2-52 Setting Default Material Properties ..........................................................................................................................2-53 Open ..........................................................................................................................................................................2-53 Opening Documents from Part or Assembly Windows ...........................................................................................2-54 Multi-Threaded Retrieval .........................................................................................................................................2-55 SolidWorks Documents in Windows Explorer .........................................................................................................2-55 Drag and Drop Files to a SolidWorks Document .....................................................................................................2-56 Web Folders Overview ....................................................................................................................................................2-57 Web Folders Overview .............................................................................................................................................2-57 Web Folders - Saving and Opening Files .................................................................................................................2-57 Change URL .............................................................................................................................................................2-58 Copy Referenced Files to Server ..............................................................................................................................2-58 Selection ...........................................................................................................................................................................2-59 Highlighting ..............................................................................................................................................................2-59 Select .........................................................................................................................................................................2-60 Select Partial Loop ....................................................................................................................................................2-61 Select Chain ..............................................................................................................................................................2-62 Select Other ..............................................................................................................................................................2-63 Midpoint Selection ....................................................................................................................................................2-63 Selection Filter ..........................................................................................................................................................2-63 Selection Filter Hot Keys ..........................................................................................................................................2-63 Box Selection ............................................................................................................................................................2-64 Loop Selection ..........................................................................................................................................................2-65 Tangent Selection .....................................................................................................................................................2-65 Select through Transparency ....................................................................................................................................2-66 Viewing Models ...............................................................................................................................................................2-67 Applying Color and Optic Properties .......................................................................................................................2-67 Draft Quality HLR/HLV ...........................................................................................................................................2-68 Shaded and Dynamic Previews ................................................................................................................................2-68 Hidden Lines Removed ............................................................................................................................................2-69 Hidden Lines Visible ................................................................................................................................................2-69 Applying, Creating, and Editing Materials ...............................................................................................................2-69 Materials - Supported Graphics Cards ..............................................................................................................2-71 Materials - General Information ........................................................................................................................2-71 Materials - Visual Properties .............................................................................................................................2-71 Materials - Physical Properties ..........................................................................................................................2-72 Materials - Crosshatch .......................................................................................................................................2-72 RealView Graphics ............................................................................................................................................2-72 Perspective ................................................................................................................................................................2-72 Modify Perspective ...................................................................................................................................................2-73 Creating a Section View ...........................................................................................................................................2-73 Section View PropertyManager ................................................................................................................................2-74 Shaded .......................................................................................................................................................................2-74 Shaded With Edges ...................................................................................................................................................2-75 Shadows ....................................................................................................................................................................2-75 Orientation ................................................................................................................................................................2-75 Add a Named View ..................................................................................................................................................2-77 Textures ....................................................................................................................................................................2-77 Wireframe .................................................................................................................................................................2-78 Manipulating Models .......................................................................................................................................................2-78 Middle Mouse Button Functions ..............................................................................................................................2-78 Pan ............................................................................................................................................................................2-79 Rotate View ..............................................................................................................................................................2-79 Previous View ...........................................................................................................................................................2-80 Zoom to Fit ...............................................................................................................................................................2-80 Zoom to Area ............................................................................................................................................................2-80
SolidWorks 2004 Reference Guide
iii
Zoom In/Out .............................................................................................................................................................2-81 Zoom to Selection .....................................................................................................................................................2-81 Customizing SolidWorks .................................................................................................................................................2-81 Overview of SolidWorks Options ............................................................................................................................2-81 Document Templates ................................................................................................................................................2-82 Customize Commands ..............................................................................................................................................2-83 Customize Headers and Footers ...............................................................................................................................2-83 Customize Keyboard ................................................................................................................................................2-84 Customize Macro Button ..........................................................................................................................................2-84 Customize Menus .....................................................................................................................................................2-85 Customize Options ...................................................................................................................................................2-86 Customize Toolbars ..................................................................................................................................................2-86 Skins .........................................................................................................................................................................2-87 SolidWorks Tools ............................................................................................................................................................2-89 Add-Ins .....................................................................................................................................................................2-89 Conversion Wizard ...................................................................................................................................................2-89 Copy Options Wizard ...............................................................................................................................................2-90 Manufacturing Network ...........................................................................................................................................2-90 Moving from AutoCAD ...........................................................................................................................................2-91 Quick Tips ................................................................................................................................................................2-91 SolidWorks API ........................................................................................................................................................2-91 SolidWorks Service Packs ........................................................................................................................................2-91 SolidWorks Web Site ...............................................................................................................................................2-92 Recording and Playing Macros ........................................................................................................................................2-92 New Macro ...............................................................................................................................................................2-92 Record/Pause Macro .................................................................................................................................................2-92 Edit Macro ................................................................................................................................................................2-93 Run Macro ................................................................................................................................................................2-93 Stop Macro ...............................................................................................................................................................2-93 Assign a Macro to a Shortcut Key or Menu .............................................................................................................2-93 VBA ..........................................................................................................................................................................2-94 Object Linking and Embedding - OLE ............................................................................................................................2-95 Object Linking vs. Embedding .................................................................................................................................2-95 Object .......................................................................................................................................................................2-95 Display Content .................................................................................................................................................2-96 Display as Icon ..................................................................................................................................................2-96 Reset Size ..........................................................................................................................................................2-97 Inserting SolidWorks Data in Other Applications ....................................................................................................2-97 OLE Object Property ................................................................................................................................................2-97
Chapter 3
Sketching
Sketching in SolidWorks ...................................................................................................................................................3-1 Sketch ................................................................................................................................................................................3-2 Sketch on the Face of a Part ..............................................................................................................................................3-3 Starting a New 2D Sketch ..................................................................................................................................................3-3 Starting the Sketch .............................................................................................................................................................3-4 Starting the Sketch .............................................................................................................................................................3-5 Working in a Sketch ..........................................................................................................................................................3-5 Opening a New Sketch ......................................................................................................................................................3-6 Inferencing Pointers and Lines ..........................................................................................................................................3-6 Sketch Modes .....................................................................................................................................................................3-7 Autotransitioning ...............................................................................................................................................................3-8 Silhouettes ..........................................................................................................................................................................3-8 Cutting, Copying, and Pasting in Sketches ........................................................................................................................3-8 Modify Sketch ...................................................................................................................................................................3-9 Edit Sketch .......................................................................................................................................................................3-10 Exit Sketch .......................................................................................................................................................................3-11
iv
Derived Sketch .................................................................................................................................................................3-11 Sketch Plane References ..................................................................................................................................................3-12 Edit Sketch Plane .............................................................................................................................................................3-12 Shaded Sketch Plane ........................................................................................................................................................3-12 Reference Plane Normal to Edge .....................................................................................................................................3-13 Sketch Tools .....................................................................................................................................................................3-13 Align Grid .................................................................................................................................................................3-13 Automatic Inferencing Lines ....................................................................................................................................3-14 Automatic Solve .......................................................................................................................................................3-14 No Solve Move .........................................................................................................................................................3-15 Move or Copy PropertyManager ..............................................................................................................................3-15 Check Sketch for Feature Usage ...............................................................................................................................3-16 Allowed Contour Types ............................................................................................................................................3-16 Circular Sketch Step and Repeat ..............................................................................................................................3-17 Constrain Spacing and Fixed Options ......................................................................................................................3-19 Constrain All .............................................................................................................................................................3-19 Contour Selection .....................................................................................................................................................3-19 Close Sketch to Model ..............................................................................................................................................3-21 Construction Geometry .............................................................................................................................................3-21 Convert Entities ........................................................................................................................................................3-22 Detach Segment on Drag ..........................................................................................................................................3-22 Extend Entities ..........................................................................................................................................................3-22 Face Curves ..............................................................................................................................................................3-23 Intersection Curve .....................................................................................................................................................3-24 Linear Sketch Step and Repeat .................................................................................................................................3-25 Fixed Spacing in Linear Sketch Step and Repeat .....................................................................................................3-26 Constrain Angle in Linear Sketch Step and Repeat ..................................................................................................3-26 Mirror Entities ..........................................................................................................................................................3-27 Move, Rotate, Scale, or Copy ...................................................................................................................................3-27 Offset Entities ...........................................................................................................................................................3-30 Override Dims on Drag/Move ..................................................................................................................................3-30 Sketch Chamfer ........................................................................................................................................................3-31 Sketch Fillet ..............................................................................................................................................................3-31 Sketch Fillet PropertyManager .................................................................................................................................3-32 Split Entities ..............................................................................................................................................................3-32 Trim Entities .............................................................................................................................................................3-32 Dimensions and Relations ................................................................................................................................................3-33 Dimensions ...............................................................................................................................................................3-33 Horizontal Dimension .......................................................................................................................................3-34 Vertical Dimension ............................................................................................................................................3-34 Lock Dimensions ...............................................................................................................................................3-34 Point-to-Point Dimensions ................................................................................................................................3-35 Point-to-Point Dimensions ................................................................................................................................3-35 Arc Dimensions .................................................................................................................................................3-35 Arc Dimensions .................................................................................................................................................3-35 Circular Dimensions ..........................................................................................................................................3-36 Circular Dimensions ..........................................................................................................................................3-36 Angular Dimensions Between Two Lines .........................................................................................................3-37 Angular Dimensions ..........................................................................................................................................3-37 Angular Dimensions Between Three Points ......................................................................................................3-37 Dimensions Between Arcs or Circles ................................................................................................................3-38 Autodimension ..........................................................................................................................................................3-39 Geometric Relations .................................................................................................................................................3-40 Automatic Relations .................................................................................................................................................3-40 Add Relations/Properties PropertyManager .............................................................................................................3-41 Sketch Relations .......................................................................................................................................................3-42 Sketch Relations Callouts .........................................................................................................................................3-43
SolidWorks 2004 Reference Guide
v
Sketch Geometry Status ...........................................................................................................................................3-43 Sketch Status Conventions .......................................................................................................................................3-43 Display/Delete Relations PropertyManager .............................................................................................................3-44 Scan Equal ................................................................................................................................................................3-45 External vs. Defined in Context ...............................................................................................................................3-45 Splines ..............................................................................................................................................................................3-46 Splines ......................................................................................................................................................................3-46 Proportional Splines .................................................................................................................................................3-47 Spline PropertyManager ...........................................................................................................................................3-47 Fit Spline ..................................................................................................................................................................3-48 Simplify Spline .........................................................................................................................................................3-49 Insert Spline Point ....................................................................................................................................................3-49 Moving Frame ..........................................................................................................................................................3-49 Frame Point PropertyManager .................................................................................................................................3-50 3D Frame Point PropertyManager ............................................................................................................................3-51 Curvature Combs ......................................................................................................................................................3-52 Curvature Scale ........................................................................................................................................................3-52 Inflection Points ........................................................................................................................................................3-52 Minimum Radius ......................................................................................................................................................3-53 2D Sketching ...................................................................................................................................................................3-53 Line ...........................................................................................................................................................................3-53 Line PropertyManager ..............................................................................................................................................3-54 Points ........................................................................................................................................................................3-55 Point PropertyManager .............................................................................................................................................3-55 Circle ........................................................................................................................................................................3-55 Circle PropertyManager ...........................................................................................................................................3-56 Ellipse .......................................................................................................................................................................3-57 Partial Ellipse ............................................................................................................................................................3-57 Ellipse PropertyManager ..........................................................................................................................................3-57 Centerlines ................................................................................................................................................................3-58 Virtual Sharp ............................................................................................................................................................3-58 Centerpoint Arc ........................................................................................................................................................3-59 Tangent Arcs ............................................................................................................................................................3-59 3 Point Arc ................................................................................................................................................................3-59 Arc PropertyManager ...............................................................................................................................................3-60 Parabolas ...................................................................................................................................................................3-61 Parabola PropertyManager .......................................................................................................................................3-62 Polygons ...................................................................................................................................................................3-63 Polygon PropertyManager ........................................................................................................................................3-63 Rectangles .................................................................................................................................................................3-64 Parallelograms ..........................................................................................................................................................3-65 Text ...........................................................................................................................................................................3-65 Sketch Text PropertyManager ..................................................................................................................................3-66 Sketch Picture ...........................................................................................................................................................3-67 Sketch Picture PropertyManager ..............................................................................................................................3-68 3D Sketching ...................................................................................................................................................................3-68 3D Sketching ............................................................................................................................................................3-68 Line Snap ..................................................................................................................................................................3-69 3D Lines ...................................................................................................................................................................3-70 3D Line PropertyManager ........................................................................................................................................3-70 3D Splines ................................................................................................................................................................3-71 3D Spline PropertyManager .....................................................................................................................................3-72 3D Points ..................................................................................................................................................................3-73 3D Point PropertyManager .......................................................................................................................................3-73 3D Circle PropertyManager .....................................................................................................................................3-74 Coordinate System - 3D Sketching ..........................................................................................................................3-74 Space Handle ............................................................................................................................................................3-75
vi
Dimensioning a 3D Sketch .......................................................................................................................................3-75 Virtual Sharps - 3D Sketch .......................................................................................................................................3-75 3D Arc PropertyManager .........................................................................................................................................3-75
Chapter 4
2D to 3D Conversion
2D to 3D Conversion Overview ........................................................................................................................................4-1 2D to 3D Toolbar ...............................................................................................................................................................4-4 Importing Drawings into Part Documents .........................................................................................................................4-4 Extracting Sketches ............................................................................................................................................................4-5 Aligning Sketches ..............................................................................................................................................................4-6 Extruding in 2D to 3D ........................................................................................................................................................4-7 Cutting in 2D to 3D ............................................................................................................................................................4-8 Additional Conversion Tools ...........................................................................................................................................4-10 Repair Sketch ............................................................................................................................................................4-10 Create Sketch from Selections ..................................................................................................................................4-10
Chapter 5
Reference Geometry
Reference Geometry Overview ..........................................................................................................................................5-1 Updating Reference Geometry in Document Templates ...................................................................................................5-1 Planes .................................................................................................................................................................................5-2 Creating Planes ...........................................................................................................................................................5-2 Changing Plane Names ...............................................................................................................................................5-8 Plane Display ..............................................................................................................................................................5-8 Hiding or Showing Planes ........................................................................................................................................5-10 Moving, Resizing, and Copying Planes ....................................................................................................................5-10 Automatic Sizing of Planes and Axes ......................................................................................................................5-10 Axis Overview .................................................................................................................................................................5-12 Reference Axis .................................................................................................................................................................5-12 Reference Axis .................................................................................................................................................................5-13 Coordinate System ...........................................................................................................................................................5-13 Coordinate System PropertyManager ..............................................................................................................................5-14 Origin ...............................................................................................................................................................................5-14 Centroid ............................................................................................................................................................................5-14 Converting Sketch Lines to Construction Geometry .......................................................................................................5-15 Curve Overview ...............................................................................................................................................................5-15 Curve Through XYZ Points ......................................................................................................................................5-16 Curve Through Reference Points ..............................................................................................................................5-16 Curve from File .........................................................................................................................................................5-17 Helix and Spiral ........................................................................................................................................................5-17 Helix/Spiral PropertyManager ..................................................................................................................................5-18 Projecting Sketched Curves ......................................................................................................................................5-18 Replacing a Sketch of a Projected Curve .................................................................................................................5-19 Split Lines .................................................................................................................................................................5-20 Composite Curve ......................................................................................................................................................5-21 Reference Points ..............................................................................................................................................................5-22 Point PropertyManager ....................................................................................................................................................5-22
Chapter 6
Features
Features Overview .............................................................................................................................................................6-1 Features Toolbar ................................................................................................................................................................6-2 Feature Previews ................................................................................................................................................................6-4 Chamfers ............................................................................................................................................................................6-7 Deform ...............................................................................................................................................................................6-8 Deform ........................................................................................................................................................................6-8 Deform Curve to Curve ..............................................................................................................................................6-9 Deform Feature Using Curve to Curve ...............................................................................................................6-9 Deform Feature Curve to Curve Options ..........................................................................................................6-12
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Deform Point ............................................................................................................................................................6-19 Deform Feature Using Point .............................................................................................................................6-19 Deform Feature Point Options ..........................................................................................................................6-21 Domes ..............................................................................................................................................................................6-30 Drafts ...............................................................................................................................................................................6-32 Draft Overview .........................................................................................................................................................6-32 Draft Feature .............................................................................................................................................................6-32 Draft with Neutral Plane ...........................................................................................................................................6-33 Parting Line Draft .....................................................................................................................................................6-35 Allow Reduced Angle Option ..................................................................................................................................6-36 Parting Line with Step Draft .....................................................................................................................................6-37 Tapered and Perpendicular Draft Steps ....................................................................................................................6-38 Extrudes ...........................................................................................................................................................................6-38 Extrude Feature ........................................................................................................................................................6-38 Extrude Feature Overview ........................................................................................................................................6-39 Extruded Boss/Base ..................................................................................................................................................6-44 Boss/Base-Extrude ...................................................................................................................................................6-45 Extrude Thin Feature ................................................................................................................................................6-46 Cut Feature ...............................................................................................................................................................6-47 Cutting Tools ............................................................................................................................................................6-47 Surface Cut ...............................................................................................................................................................6-49 Extruded Cut .............................................................................................................................................................6-50 Fillets ...............................................................................................................................................................................6-53 Fillet ..........................................................................................................................................................................6-53 Fillet Overview .........................................................................................................................................................6-57 Constant Radius Fillet ..............................................................................................................................................6-58 Multiple Radius Fillet ...............................................................................................................................................6-60 Round Corner Fillet ..................................................................................................................................................6-61 Setback Fillet ............................................................................................................................................................6-62 Variable Radius Fillet ...............................................................................................................................................6-64 Using Variable Radius Control Points .....................................................................................................................6-67 Full Round Fillet .......................................................................................................................................................6-69 Face Fillet .................................................................................................................................................................6-70 Face Fillet with Hold Line ........................................................................................................................................6-71 Face Fillet with Split Line ........................................................................................................................................6-73 Holes ................................................................................................................................................................................6-74 Simple Hole ..............................................................................................................................................................6-74 Creating a Simple Hole ............................................................................................................................................6-76 End Condition Types ................................................................................................................................................6-76 Hole Wizard ..............................................................................................................................................................6-77 Hole Wizard Overview ......................................................................................................................................6-77 Hole Wizard on a Plane .....................................................................................................................................6-78 Hole Wizard Hole Placement ............................................................................................................................6-79 Favorite Hole Types ..........................................................................................................................................6-80 Property ......................................................................................................................................................6-80 Parameters ..................................................................................................................................................6-80 Delete Favorite Hole .........................................................................................................................................6-81 Retrieve Favorite Hole ......................................................................................................................................6-81 Update Favorite Hole ........................................................................................................................................6-81 New Favorite Name ..........................................................................................................................................6-81 Hole Series ........................................................................................................................................................6-81 Hole Wizard Holes ............................................................................................................................................6-83 Hole Wizard Custom Standards .................................................................................................................6-83 Edit Hole Wizard Standards .......................................................................................................................6-83 Hole Wizard - Edit Standards Data ............................................................................................................6-84 Counterbore ................................................................................................................................................6-84 Dynamic Changes with Counterbore Holes ...............................................................................................6-85
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Countersink ................................................................................................................................................6-85 Dynamic Changes with Countersink Holes ...............................................................................................6-86 Hole ............................................................................................................................................................6-86 Dynamic Changes with Regular Holes ......................................................................................................6-87 Tap ..............................................................................................................................................................6-87 Dynamic Changes with Tap Holes .............................................................................................................6-88 Pipe Tap ......................................................................................................................................................6-88 Dynamic Changes with Pipe Tap Holes .....................................................................................................6-89 Legacy ........................................................................................................................................................6-89 Lofts .................................................................................................................................................................................6-90 Loft Overview ...........................................................................................................................................................6-90 Loft Features .............................................................................................................................................................6-91 Loft with Thin Feature ..............................................................................................................................................6-94 Loft Thin Feature Samples .......................................................................................................................................6-95 Loft with Non-Planar Profile ....................................................................................................................................6-95 Loft with Split Line ..................................................................................................................................................6-96 Loft with Guide Curve and Planar Profile ................................................................................................................6-97 Loft with Guide Curve and non-Planar Profile .........................................................................................................6-99 Recommendations for Lofts with Guide Curves ....................................................................................................6-101 Loft Side Tangency .................................................................................................................................................6-101 Loft with Centerline ................................................................................................................................................6-101 Loft with Start and End Tangency Control .............................................................................................................6-103 Add Loft Section .....................................................................................................................................................6-104 Loft Synchronization ..............................................................................................................................................6-106 Patterns and Mirroring ...................................................................................................................................................6-108 Pattern and Mirror Overview ..................................................................................................................................6-108 Patterns of Patterns .................................................................................................................................................6-109 Curve Driven Pattern Overview .............................................................................................................................6-110 Curve Driven Pattern ..............................................................................................................................................6-110 Linear Pattern ..........................................................................................................................................................6-114 Circular Pattern .......................................................................................................................................................6-119 Sketch Driven Patterns ...........................................................................................................................................6-121 Table Driven Patterns .............................................................................................................................................6-123 Save Table Pattern Coordinates .......................................................................................................................6-125 Load Table Pattern Coordinates ......................................................................................................................6-125 Mirror Pattern .........................................................................................................................................................6-125 Control and Modify Patterns ..................................................................................................................................6-126 Geometry Pattern .............................................................................................................................................6-127 Vary Sketch .....................................................................................................................................................6-128 Pattern Deletion ...............................................................................................................................................6-128 Seed Feature ....................................................................................................................................................6-129 Mirror Feature .........................................................................................................................................................6-129 Revolves .........................................................................................................................................................................6-132 Revolved Boss/Base ...............................................................................................................................................6-132 Revolve Features ....................................................................................................................................................6-132 Ribs ................................................................................................................................................................................6-135 Rib Overview ..........................................................................................................................................................6-135 Rib - Linear and Natural Type ................................................................................................................................6-138 Rib Feature ..............................................................................................................................................................6-139 Scaling ............................................................................................................................................................................6-141 Shapes ............................................................................................................................................................................6-142 Shape Feature ..........................................................................................................................................................6-142 Shape Feature Controls Tab ....................................................................................................................................6-144 Shells ..............................................................................................................................................................................6-145 Shell Features ..........................................................................................................................................................6-145 Shell with Multi-Thickness Faces ..........................................................................................................................6-146 Shell Feature Diagnostics .......................................................................................................................................6-147
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Surfaces ..........................................................................................................................................................................6-148 Surfaces Overview ..................................................................................................................................................6-148 Surfaces Toolbar .....................................................................................................................................................6-148 Surface Bodies ........................................................................................................................................................6-149 Surface Features .....................................................................................................................................................6-149 Planar Surface .................................................................................................................................................6-149 Extruded Surface .............................................................................................................................................6-150 Revolved Surface ............................................................................................................................................6-151 Swept Surface ..................................................................................................................................................6-152 Lofted Surface .................................................................................................................................................6-153 Offset Surface ..................................................................................................................................................6-154 Radiating a Surface from a Parting Line .........................................................................................................6-155 Surface Face Blend Fillet ................................................................................................................................6-156 Surface Controls .....................................................................................................................................................6-157 Extend Surface ................................................................................................................................................6-157 Fillet Surface ...................................................................................................................................................6-159 Knit Surface .....................................................................................................................................................6-161 Mid Surface .....................................................................................................................................................6-162 Fill Surface ......................................................................................................................................................6-164 Trim Surface ....................................................................................................................................................6-170 Untrim Surface ................................................................................................................................................6-172 Radiate Surface ...............................................................................................................................................6-175 Hide and Show Bodies ....................................................................................................................................6-175 Delete Face ......................................................................................................................................................6-177 Delete Hole ......................................................................................................................................................6-179 Replace Face ...................................................................................................................................................6-180 Sweeps ...........................................................................................................................................................................6-182 Sweep Overview .....................................................................................................................................................6-182 Simple Sweep .........................................................................................................................................................6-183 Sweeps Feature .......................................................................................................................................................6-185 Sweeps with Mulltiple Profiles ..............................................................................................................................6-187 Sweeps with Guide Curves .....................................................................................................................................6-187 Recommendations for Sweeps with Guide Curves ................................................................................................6-189 Preview Intermediate Sweep Sections ....................................................................................................................6-189 Sweeps Options ......................................................................................................................................................6-190 Sweep Options .................................................................................................................................................6-190 Sweep Options Align with End Faces .............................................................................................................6-190 Example of Sweep with Thin Features ...........................................................................................................6-191 Example of Merge Smooth Faces Option in Sweeps ......................................................................................6-191 Sweep Options Advanced Smoothing .............................................................................................................6-191 Sweep Options Maintain Tangency ................................................................................................................6-191 Loft Tangency Options ....................................................................................................................................6-192 Start and End Tangency Options for Sweeps ..................................................................................................6-193 Orientation/Twist Control Option ...................................................................................................................6-193 Orientation/Twist Type - Follow Path ............................................................................................................6-194 Thicken ..........................................................................................................................................................................6-195 Tools for Features ..........................................................................................................................................................6-198 Analysis of Features ...............................................................................................................................................6-198 Draft Analysis Overview .................................................................................................................................6-198 Draft Analysis .................................................................................................................................................6-201 Deviation Analysis ..........................................................................................................................................6-205 Manipulation of Features ........................................................................................................................................6-208 Move/Size Features with Feature Handles ......................................................................................................6-208 Move/Copy Bodies ..........................................................................................................................................6-209 Combine Bodies ..............................................................................................................................................6-213 Delete Body .....................................................................................................................................................6-214 Choose Option .................................................................................................................................................6-214
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Select Detailed Preview ...................................................................................................................................6-215 Wrap ...............................................................................................................................................................................6-216
Chapter 7
Parts
Overview and Editing Parts ...............................................................................................................................................7-1 Parts Overview ............................................................................................................................................................7-1 Edit Definition ............................................................................................................................................................7-1 Properties of Features and Faces ................................................................................................................................7-2 Dynamic Feature Editing ............................................................................................................................................7-3 Copying Features ........................................................................................................................................................7-4 Color of Parts ..............................................................................................................................................................7-4 Material Properties and Appearance of Parts .............................................................................................................7-5 Appearance and Material Properties ...........................................................................................................................7-6 Edit Color ....................................................................................................................................................................7-7 Entity Property ............................................................................................................................................................7-8 Advanced Properties ...................................................................................................................................................7-9 Multibody Parts ................................................................................................................................................................7-10 Multibody Overview .................................................................................................................................................7-10 Multibody Parts Versus Assemblies .........................................................................................................................7-10 Modeling Techniques ...............................................................................................................................................7-11 Body Intersection ...............................................................................................................................................7-11 Bridging .............................................................................................................................................................7-12 Local Operations ...............................................................................................................................................7-12 Symmetry Modeling ..........................................................................................................................................7-13 Tool Body Modeling .........................................................................................................................................7-14 Controlling Parts ..............................................................................................................................................................7-14 Parent and Child Relations .......................................................................................................................................7-14 Equations ..................................................................................................................................................................7-14 Edit and Delete Equations .................................................................................................................................7-15 Operators and Constants ....................................................................................................................................7-16 Equation Comments and Status .........................................................................................................................7-16 Shared Values ...........................................................................................................................................................7-17 Measure .....................................................................................................................................................................7-18 Measurement Options ...............................................................................................................................................7-19 Dependency Editing ..................................................................................................................................................7-20 Suppress and Unsuppress Features ...........................................................................................................................7-21 Derived Parts ............................................................................................................................................................7-21 Insert Part ..................................................................................................................................................................7-22 Mirror Part ................................................................................................................................................................7-22 Derive Component Part ............................................................................................................................................7-23 Split and Save Bodies ...............................................................................................................................................7-23 Edit Derived Parts .....................................................................................................................................................7-26 Create Assembly .......................................................................................................................................................7-27 Resolve Ambiguity ...................................................................................................................................................7-27 File Management with External References .............................................................................................................7-28 Feature Statistics .......................................................................................................................................................7-28 Model Geometry Overview ......................................................................................................................................7-29 Selected Items Check Entity .....................................................................................................................................7-29 Checking Model Geometry .......................................................................................................................................7-30 Checking a Planar Surface ........................................................................................................................................7-30 Checking Part Faces or Edges ..................................................................................................................................7-31 Check Entity .............................................................................................................................................................7-31 Finding the Minimum Radius of Curvature ..............................................................................................................7-31 Interrupt Regeneration ..............................................................................................................................................7-32 Send To .....................................................................................................................................................................7-32
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Displaying Parts Information ...........................................................................................................................................7-32 Displaying Annotations in Parts ...............................................................................................................................7-32 Summary Information ..............................................................................................................................................7-33 Summary Info – Custom and Configuration Specific ..............................................................................................7-33 Edit List ....................................................................................................................................................................7-35 Section Views Overview ..........................................................................................................................................7-35 Section View Selection .............................................................................................................................................7-36 Section Views in Models ..........................................................................................................................................7-37 Using Viewing Planes for Section Views ................................................................................................................7-37 Mass Properties and Section Properties ...................................................................................................................7-38 Curvature ..................................................................................................................................................................7-39 Curvature Options ....................................................................................................................................................7-41 Curvature Display .....................................................................................................................................................7-41 Zebra Stripes .............................................................................................................................................................7-42 Zebra Stripes on Boundaries ....................................................................................................................................7-44 Lighting ............................................................................................................................................................................7-45 Lighting Overview ....................................................................................................................................................7-45 Basic Lighting Controls ............................................................................................................................................7-45 Ambient Light ..........................................................................................................................................................7-46 Directional Light Properties .....................................................................................................................................7-47 Point Light Properties ...............................................................................................................................................7-48 Spot Light Properties ................................................................................................................................................7-49 Lighting - Basic ........................................................................................................................................................7-50 Lighting - Advanced .................................................................................................................................................7-50 Lighting - Position and Direction .............................................................................................................................7-51
Chapter 8
Mold Design
Mold Tools Toolbar ...........................................................................................................................................................8-1 Understanding Mold Design ..............................................................................................................................................8-2 Mold Tools - Undercut Detection ......................................................................................................................................8-3 Scaling Factor and Draft in Mold Design ..........................................................................................................................8-4 Mold Tools - Parting Lines ................................................................................................................................................8-4 Mold Tools - Ruled Surfaces .............................................................................................................................................8-6 Mold Tools - Shut Off Surfaces .........................................................................................................................................8-6 Mold Tools - Parting Surfaces ...........................................................................................................................................8-7 Mold Tools - Tooling Split ................................................................................................................................................8-9 Interlock Surface ..............................................................................................................................................................8-10 Finishing the Interlock Surface ........................................................................................................................................8-10 Mold Tools - Insert Cavity ..............................................................................................................................................8-11
Chapter 9
Assemblies
Assemblies .........................................................................................................................................................................9-1 Design Methods .................................................................................................................................................................9-1 The FeatureManager Design Tree in an Assembly ...........................................................................................................9-2 Component Icons in the FeatureManager Design Tree .....................................................................................................9-3 Viewing Mates ...................................................................................................................................................................9-3 Adding Components to an Assembly ................................................................................................................................9-4 Insert Components ......................................................................................................................................................9-4 Adding Components from an Open Document Window ...........................................................................................9-5 Adding Components from Windows Explorer ...........................................................................................................9-5 Adding Components from Internet Explorer ..............................................................................................................9-5 Adding Components by Dragging and Dropping .......................................................................................................9-5 Inferencing to the Assembly Origin ...........................................................................................................................9-6 Deleting Components from an Assembly ..........................................................................................................................9-6 Saving an Assembly and Its Components .........................................................................................................................9-6 Saving an Assembly in Various Ways ...............................................................................................................................9-7 Replace Components .........................................................................................................................................................9-7
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Reload Documents .............................................................................................................................................................9-8 Edit Referenced File Locations ..........................................................................................................................................9-8 Replace Mated Entities ......................................................................................................................................................9-8 Assembly Statistics ............................................................................................................................................................9-9 Component Properties ........................................................................................................................................................9-9 Assembly Instance Color .................................................................................................................................................9-10 Arranging Components ....................................................................................................................................................9-10 Assembly PropertyManager .....................................................................................................................................9-10 Positioning Components in an Assembly .................................................................................................................9-10 Fixing the Position of a Component .........................................................................................................................9-11 Moving a Component ...............................................................................................................................................9-11 Rotating a Component ..............................................................................................................................................9-12 Assembly Mates ........................................................................................................................................................9-13 Mate PropertyManager ......................................................................................................................................9-13 Standard Mates ..................................................................................................................................................9-14 Standard Mates by Entity ..................................................................................................................................9-15 Mate Alignment .................................................................................................................................................9-17 Mate Reference ..................................................................................................................................................9-17 Mategroups ........................................................................................................................................................9-18 Modifying a Mating Relationship .....................................................................................................................9-19 Angle Mate ........................................................................................................................................................9-19 Coincident Mate ................................................................................................................................................9-20 Concentric Mate ................................................................................................................................................9-20 Distance Mate ....................................................................................................................................................9-21 Parallel and Perpendicular Mates ......................................................................................................................9-21 Tangent Mate .....................................................................................................................................................9-22 Cam-Follower Mates .........................................................................................................................................9-22 Gear Mates .........................................................................................................................................................9-23 Limit Mates .......................................................................................................................................................9-23 Symmetry Mate .................................................................................................................................................9-24 SmartMates ...............................................................................................................................................................9-25 Geometry-Based Mates .....................................................................................................................................9-25 Feature-Based Mates .........................................................................................................................................9-26 Pattern-Based Mates ..........................................................................................................................................9-26 Adding SmartMates While Moving Components .............................................................................................9-27 Deleting a Mating Relationship ................................................................................................................................9-28 Suppressing a Mating Relationship ..........................................................................................................................9-28 Mate Diagnostics ......................................................................................................................................................9-28 Conflicting Mates ..............................................................................................................................................9-29 Design Errors and Mating .................................................................................................................................9-30 Errors in Solving Mates .....................................................................................................................................9-31 In-Context Mating Conflicts ..............................................................................................................................9-31 Mates to Dangling Geometry ............................................................................................................................9-31 Mating Conflicts with Sketch Relations ............................................................................................................9-32 Physical Simulation ..................................................................................................................................................9-33 Linear or Rotary Motors ....................................................................................................................................9-33 Linear Springs ...................................................................................................................................................9-34 Gravity ...............................................................................................................................................................9-35 Recording and Replaying a Simulation .............................................................................................................9-35 Sub-assemblies .................................................................................................................................................................9-36 Working with Sub-assemblies ..................................................................................................................................9-36 Forming a New Assembly from Existing Components ............................................................................................9-37 Dragging Components to Edit the Assembly Structure ............................................................................................9-37 Assembly Structure Editing ......................................................................................................................................9-38 Changing the Order of Components .........................................................................................................................9-39 Inserting a New Sub-assembly .................................................................................................................................9-39 Dissolving a Sub-assembly .......................................................................................................................................9-39
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Changing the Editing Focus Manually .....................................................................................................................9-40 Automatic Change of Editing Focus ........................................................................................................................9-41 Limitations in Sub-assembly Editing .......................................................................................................................9-41 Flexible Sub-Assemblies ..........................................................................................................................................9-41 Working with Parts Within an Assembly ........................................................................................................................9-42 Working with Parts within an Assembly ..................................................................................................................9-42 External References ..................................................................................................................................................9-42 Understanding the Update Path ................................................................................................................................9-43 Locking and Breaking External References .............................................................................................................9-43 Rules for External References ..................................................................................................................................9-43 List External References ...........................................................................................................................................9-44 Searching for Referenced Documents ......................................................................................................................9-44 Search Results ..........................................................................................................................................................9-46 Saving Assemblies with In-context Features ...........................................................................................................9-46 Editing Parts in the Assembly Context .....................................................................................................................9-47 Creating a Part in an Assembly ................................................................................................................................9-47 Editing a Part in an Assembly ..................................................................................................................................9-48 Transparency During Part Editing ............................................................................................................................9-48 Time-Dependent Features ........................................................................................................................................9-49 Tips for Mating with Time-Dependent Features ......................................................................................................9-49 Adding a Component Pattern ...................................................................................................................................9-49 Linear Component Pattern ................................................................................................................................9-50 Circular Component Pattern ..............................................................................................................................9-50 Feature Driven Pattern ......................................................................................................................................9-51 Mirror Components - Overview ...............................................................................................................................9-51 Mirror Components Step 1: Selections .............................................................................................................9-52 Mirror Components Step 2: Filenames .............................................................................................................9-53 Mirror Components Step 3: Orientation ............................................................................................................9-53 Reorder and Roll Back in Assemblies ......................................................................................................................9-53 Assembly Layout Sketch ..........................................................................................................................................9-54 Example of Using an Assembly Layout Sketch .......................................................................................................9-54 Assembly Features ....................................................................................................................................................9-55 Creating an Assembly Feature ..................................................................................................................................9-55 Feature Scope ...........................................................................................................................................................9-56 Joining Parts .............................................................................................................................................................9-56 Creating a Joined Part .......................................................................................................................................9-56 Editing a Joined Part .........................................................................................................................................9-57 Identifying the Parts in a Joined Part ................................................................................................................9-58 Weld Beads ...............................................................................................................................................................9-58 Weld Types .......................................................................................................................................................9-58 Creating and Editing Weld Beads .....................................................................................................................9-58 Surface Delta and Radius ..................................................................................................................................9-59 Weld Face Selection Tips ..................................................................................................................................9-60 Automatic Weld Symbols .................................................................................................................................9-60 Simplifying Assemblies ...................................................................................................................................................9-61 Simplifying Large Assemblies .................................................................................................................................9-61 Large Assembly Mode .............................................................................................................................................9-61 Lightweight Components .........................................................................................................................................9-61 Toggling the Visibility .............................................................................................................................................9-62 Component Suppression States ................................................................................................................................9-63 Loading Additional Model Data ...............................................................................................................................9-64 Comparison of Components Suppression States ......................................................................................................9-64 Assembly Envelopes ................................................................................................................................................9-65 Apply Envelope ........................................................................................................................................................9-65 Creating Assembly Envelopes ..................................................................................................................................9-66 Removing Assembly Envelopes ...............................................................................................................................9-66 Select Using Envelope ..............................................................................................................................................9-66
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Component Selection by Properties ..........................................................................................................................9-67 Advanced Hide/Show Components ..........................................................................................................................9-67 Advanced Component Selection ...............................................................................................................................9-68 Saving and Reloading Selection Criteria ..................................................................................................................9-68 Displaying Assemblies .....................................................................................................................................................9-69 Exploding an Assembly View ..................................................................................................................................9-69 Assembly Exploder ...........................................................................................................................................9-69 Exploding and Collapsing an Exploded View ...................................................................................................9-70 Alternative Method for Editing an Exploded View ..........................................................................................9-71 Explode Line Sketch ..........................................................................................................................................9-71 Jog Line .............................................................................................................................................................9-71 Image Quality in Assemblies ....................................................................................................................................9-72 Color and Appearance in Assemblies .......................................................................................................................9-72 Annotations in Assemblies .......................................................................................................................................9-73 Preventing Interference Between Components ................................................................................................................9-74 Interference Detection ..............................................................................................................................................9-74 Collision Detection ...................................................................................................................................................9-74 Physical Dynamics ....................................................................................................................................................9-75 Dynamic Clearance ...................................................................................................................................................9-76 Smart Fasteners ................................................................................................................................................................9-77 Smart Fasteners Overview ........................................................................................................................................9-77 Smart Fasteners PropertyManager ............................................................................................................................9-78 Smart Fasteners Bolts and Screws ............................................................................................................................9-79 Smart Fasteners Nuts ................................................................................................................................................9-81 Smart Fasteners Washers ..........................................................................................................................................9-82 Unsupported Hole Types ..........................................................................................................................................9-83 Editing Smart Fasteners ............................................................................................................................................9-85 Smart Fasteners Hardware Stacks ............................................................................................................................9-86 Drag-and-Drop Editing of Smart Fasteners ..............................................................................................................9-87 Smart Fasteners Part Numbers ..................................................................................................................................9-88 Mark Up-to-date .......................................................................................................................................................9-88 Configuring Bolt Patterns in Smart Fasteners ..........................................................................................................9-89 Smart Fasteners Defaults ..........................................................................................................................................9-90
Chapter 10 Configurations Configurations Overview .................................................................................................................................................10-1 ConfigurationManager .....................................................................................................................................................10-1 Show Preview ..................................................................................................................................................................10-2 Configurations and In-context Components ....................................................................................................................10-2 Configure Document ........................................................................................................................................................10-3 Configure Document for View / Configurations .............................................................................................................10-3 Manual Configurations ....................................................................................................................................................10-4 Creating a Configuration Manually ..........................................................................................................................10-4 Add Configuration/Configuration Properties ...........................................................................................................10-4 Properties for Newly Inserted Items .........................................................................................................................10-5 Derived Configurations ............................................................................................................................................10-6 Activating a Configuration .......................................................................................................................................10-8 Configurable Items for Parts .....................................................................................................................................10-8 Sketch Dimensions in Configurations ...............................................................................................................10-8 Sketch Planes in Configurations ........................................................................................................................10-9 Sketch Relations in Configurations ...................................................................................................................10-9 End Conditions in Configurations ...................................................................................................................10-10 Configurable Items for Assemblies ........................................................................................................................10-10 Modifying a Configuration Dimension ..................................................................................................................10-11 Editing a Configuration ..........................................................................................................................................10-11 Special Assembly Configurations ...........................................................................................................................10-12 Component Configurations in an Assembly ...........................................................................................................10-12
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Deleting a Configuration ........................................................................................................................................10-13 Design Table Configurations .........................................................................................................................................10-14 Creating a Design Table .........................................................................................................................................10-14 Creating a Design Table as a Separate Excel File ..................................................................................................10-14 Inserting a Design Table .........................................................................................................................................10-16 Design Table PropertyManager ..............................................................................................................................10-17 Add Rows and Columns .........................................................................................................................................10-18 Creating Configurations with a Design Table ........................................................................................................10-18 Formatting a Design Table .....................................................................................................................................10-19 Manually Add Parameters in a Design Table .........................................................................................................10-21 Numerical Configuration Name .............................................................................................................................10-21 Editing a Design Table ...........................................................................................................................................10-21 Deleting a Design Table .........................................................................................................................................10-21 Saving Design Tables .............................................................................................................................................10-22 Deleting a Configuration ........................................................................................................................................10-22 Specifying Design Table Parameters ......................................................................................................................10-23 Specifying Design Table Parameters ..............................................................................................................10-23 Summary of Design Table Parameters ............................................................................................................10-24 Dimensions in Design Tables ..........................................................................................................................10-25 Dimensions ......................................................................................................................................................10-26 Component Configuration ...............................................................................................................................10-26 Component Visibility ......................................................................................................................................10-26 Component Suppression State .........................................................................................................................10-27 Suppression of Features ..................................................................................................................................10-27 Base Parts ........................................................................................................................................................10-28 Component Part Number .................................................................................................................................10-28 Comment .........................................................................................................................................................10-29 Equations in Configurations ............................................................................................................................10-30 Expand in BOM ..............................................................................................................................................10-31 Lighting in Design Tables ...............................................................................................................................10-31 Split Parts ........................................................................................................................................................10-32 Custom Properties ...........................................................................................................................................10-32 User Notes .......................................................................................................................................................10-33 Color Parameter ...............................................................................................................................................10-33 Design Tables in Drawings ....................................................................................................................................10-35 Design Tables in Drawings .............................................................................................................................10-35 Displaying a Design Table in a Drawing ........................................................................................................10-35 Design Table in a Drawing ..............................................................................................................................10-36 Editing a Design Table in a Drawing ..............................................................................................................10-36
Chapter 11 Drawings Drawings Overview .........................................................................................................................................................11-1 Getting Started in Drawings ............................................................................................................................................11-2 Setting Options for Drawing Documents .................................................................................................................11-2 Creating a Drawing ...................................................................................................................................................11-3 Sheet Format/Size .....................................................................................................................................................11-3 Sheet Properties ........................................................................................................................................................11-4 Multiple Drawing Sheets ..........................................................................................................................................11-4 Sheet Formats, Sheets, and Views ............................................................................................................................11-5 Customizing Sheet Formats ......................................................................................................................................11-5 Saving Sheet Formats ...............................................................................................................................................11-6 Linking Notes to Document Properties ....................................................................................................................11-7 The Drawing Window ..............................................................................................................................................11-8 Views of Parts and Assemblies ................................................................................................................................11-8 View Boundaries ......................................................................................................................................................11-9 Scales in Drawings ...................................................................................................................................................11-9 Dimension Type .....................................................................................................................................................11-10
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Crosshatch in Drawings ..........................................................................................................................................11-10 2D Sketching in Drawings ......................................................................................................................................11-10 Quality in Drawings ................................................................................................................................................11-11 Convert to Draft Quality .........................................................................................................................................11-12 Sending Drawing Documents Electronically ..........................................................................................................11-12 Types of Drawing Documents .......................................................................................................................................11-13 Drawing Documents ...............................................................................................................................................11-13 Detached Drawings .................................................................................................................................................11-13 Working in Detached Drawings .............................................................................................................................11-14 Lightweight Drawings ............................................................................................................................................11-16 Standard Drawing Views ...............................................................................................................................................11-17 Standard Drawing Views ........................................................................................................................................11-17 Standard 3 View .....................................................................................................................................................11-17 Standard 3 View PropertyManager .................................................................................................................11-19 First Angle and Third Angle Projection ..........................................................................................................11-19 Model View ............................................................................................................................................................11-19 Model/Predefined/Empty View PropertyManager .................................................................................................11-21 Relative to Model View ..........................................................................................................................................11-22 Relative View PropertyManager in Drawings ................................................................................................11-23 Relative View PropertyManager in Models ....................................................................................................11-24 Drawing View Orientation ..............................................................................................................................11-24 Predefined Views ....................................................................................................................................................11-24 Empty Views ..........................................................................................................................................................11-25 Derived Drawing Views ................................................................................................................................................11-26 Derived Drawing Views .........................................................................................................................................11-26 Projected View ........................................................................................................................................................11-26 Projected View PropertyManager ...........................................................................................................................11-27 Auxiliary View .......................................................................................................................................................11-28 Auxiliary View PropertyManager ..........................................................................................................................11-29 Detail View .............................................................................................................................................................11-30 Detail View PropertyManager .........................................................................................................................11-31 Modifying a Detail View .................................................................................................................................11-32 Detail Circle Styles ..........................................................................................................................................11-33 Crop View ...............................................................................................................................................................11-33 Broken-out Section .................................................................................................................................................11-34 Broken-out Section PropertyManager ....................................................................................................................11-35 Broken View ...........................................................................................................................................................11-35 Broken View Break Line Styles .............................................................................................................................11-37 Section Views in Drawings ....................................................................................................................................11-37 Section View PropertyManager ......................................................................................................................11-38 Modifying Section Views ................................................................................................................................11-40 Section Views of Assemblies ..........................................................................................................................11-40 Section Scope ..................................................................................................................................................11-41 Troubleshooting Section Views ......................................................................................................................11-41 Modifying Section Line Properties .................................................................................................................11-42 Aligned Section View .............................................................................................................................................11-42 Alternate Position View ..........................................................................................................................................11-43 Alternate Position PropertyManager ......................................................................................................................11-44 Position Schematic PropertyManager .....................................................................................................................11-44 OLE Items in Drawings ..........................................................................................................................................11-45 Drawing View Update ............................................................................................................................................11-45 Drawing View Alignment and Display ..........................................................................................................................11-45 Drawing View Alignment and Display ..................................................................................................................11-45 Manipulating Views ................................................................................................................................................11-46 Drawing View Properties ................................................................................................................................11-46 Multiple Views PropertyManager ...................................................................................................................11-47 Updating Views ...............................................................................................................................................11-47
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Move Drawing .................................................................................................................................................11-48 Moving Drawing Views ..................................................................................................................................11-48 Aligning Views ...............................................................................................................................................11-49 Rotating Views ................................................................................................................................................11-49 Rotate Drawing View ......................................................................................................................................11-50 Copying and Pasting Views ............................................................................................................................11-50 Hiding and Showing ...............................................................................................................................................11-51 Hiding and Showing Views .............................................................................................................................11-51 Hiding and Showing Edges .............................................................................................................................11-51 Hiding and Showing Sketches .........................................................................................................................11-52 Show Hidden Edges ........................................................................................................................................11-52 Hide/Show Components ..................................................................................................................................11-53 Hide Behind Plane ...........................................................................................................................................11-53 Displaying ...............................................................................................................................................................11-55 Component Line Font ......................................................................................................................................11-55 Drawing View Display Modes ........................................................................................................................11-55 Line Format .....................................................................................................................................................11-56 Tangent Edge Display Overview ....................................................................................................................11-57 Tangent Edge Display .....................................................................................................................................11-57 Layers ..............................................................................................................................................................11-58
Chapter 12 Detailing Detailing Overview ..........................................................................................................................................................12-1 Detailing Overview ..................................................................................................................................................12-1 Setting Detailing Options .........................................................................................................................................12-1 Inserting Model Items ...............................................................................................................................................12-1 Insert Model Items ....................................................................................................................................................12-2 Inserting Annotations into Drawings ........................................................................................................................12-3 Inserting Dimensions into Drawings ........................................................................................................................12-3 Inserting Reference Geometry into Drawings ..........................................................................................................12-4 Favorites ...................................................................................................................................................................12-4 Add or Update a Favorite .........................................................................................................................................12-6 Dimensions in Drawings ..................................................................................................................................................12-6 Dimensions Overview ..............................................................................................................................................12-6 Setting Dimensions Options .....................................................................................................................................12-7 Dimension PropertyManager ....................................................................................................................................12-8 Symbol ....................................................................................................................................................................12-10 Dimension Properties .............................................................................................................................................12-10 Value ...............................................................................................................................................................12-11 Name ...............................................................................................................................................................12-11 Full Name ........................................................................................................................................................12-11 Units ................................................................................................................................................................12-11 Font ..................................................................................................................................................................12-12 Arrow Style .....................................................................................................................................................12-12 Arrows .............................................................................................................................................................12-12 Display as inspection dimension .....................................................................................................................12-12 Read only .........................................................................................................................................................12-12 Dimension Precision .......................................................................................................................................12-12 Dimension Display ..........................................................................................................................................12-13 Driven ..............................................................................................................................................................12-13 Display with parentheses .................................................................................................................................12-13 Display as dual dimension ...............................................................................................................................12-13 Display with solid leader .................................................................................................................................12-13 Use document's second arrow .........................................................................................................................12-13 Display second outside arrow .........................................................................................................................12-14 Display as chain dimension .............................................................................................................................12-14 Diameter dimension ........................................................................................................................................12-14
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Foreshortened radius .......................................................................................................................................12-14 Dimension to inside of arc ...............................................................................................................................12-15 Display as linear dimension .............................................................................................................................12-15 First arc condition, Second arc condition ........................................................................................................12-15 Layer ................................................................................................................................................................12-15 Dimension Units/Chamfer Dimension Units ..........................................................................................................12-16 Dimensioning to Midpoints ....................................................................................................................................12-16 Reference Dimensions ............................................................................................................................................12-16 Parentheses .............................................................................................................................................................12-17 Baseline Dimensions ..............................................................................................................................................12-17 Ordinate Dimensions ..............................................................................................................................................12-17 Horizontal Ordinate Dimensions ............................................................................................................................12-19 Vertical Ordinate Dimensions ................................................................................................................................12-19 Parallel Dimensions ................................................................................................................................................12-19 Chamfer Dimensions ..............................................................................................................................................12-20 Dimension Leaders/Text .........................................................................................................................................12-21 Leader/Text Display for Chamfer Dimensions .......................................................................................................12-21 Moving and Copying Dimensions ..........................................................................................................................12-22 Aligning Dimensions ..............................................................................................................................................12-22 Align Dimensions Parallel/Concentric ...................................................................................................................12-23 Align Collinear/Radial Dimensions ........................................................................................................................12-24 Dimension Extension Lines ....................................................................................................................................12-24 Modify Text of Dimension .....................................................................................................................................12-26 Modify Dimension ..................................................................................................................................................12-26 Specify Configurations ...........................................................................................................................................12-27 Increment ................................................................................................................................................................12-27 Hide/Show Annotations ..........................................................................................................................................12-27 Dimension Tolerance ..............................................................................................................................................12-28 Fit Tolerances .........................................................................................................................................................12-29 Annotations ....................................................................................................................................................................12-31 Annotations Overview ............................................................................................................................................12-31 Annotations Options Overview ..............................................................................................................................12-31 Annotation Properties .............................................................................................................................................12-32 Multiple Annotations ..............................................................................................................................................12-33 Aligning Annotations ..............................................................................................................................................12-34 Multi-jog Leaders ...................................................................................................................................................12-35 Notes .......................................................................................................................................................................12-36 Hyperlinks in Notes .........................................................................................................................................12-37 Note PropertyManager ....................................................................................................................................12-38 Note Properties ................................................................................................................................................12-39 Multiple Leaders .....................................................................................................................................................12-41 Link to Property ......................................................................................................................................................12-41 Balloons ..................................................................................................................................................................12-42 Balloon PropertyManager .......................................................................................................................................12-44 Stacked Balloons ....................................................................................................................................................12-44 Stacked Balloon PropertyManager .........................................................................................................................12-46 AutoBalloons ..........................................................................................................................................................12-46 AutoBalloon PropertyManager ...............................................................................................................................12-47 Center Marks ..........................................................................................................................................................12-48 Center Mark PropertyManager ...............................................................................................................................12-50 Centerline Annotations ...........................................................................................................................................12-51 Hole Callouts ..........................................................................................................................................................12-52 Hole Callout Variables ...........................................................................................................................................12-53 Cosmetic Threads ...................................................................................................................................................12-54 Cosmetic Thread PropertyManager ........................................................................................................................12-55 Surface Finish Symbols ..........................................................................................................................................12-56 Surface Finish PropertyManager ............................................................................................................................12-57
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Datum Feature Symbols .........................................................................................................................................12-58 Datum Feature PropertyManager ...........................................................................................................................12-59 Datum Targets ........................................................................................................................................................12-59 Datum Target PropertyManager .............................................................................................................................12-60 Geometric Tolerancing ...........................................................................................................................................12-60 Geometric Tolerance Properties ......................................................................................................................12-62 Geometric Tolerance Options .........................................................................................................................12-62 Dowel Pin Symbols ................................................................................................................................................12-63 Weld Symbols ........................................................................................................................................................12-64 Weld Symbol Properties ..................................................................................................................................12-64 ANSI Weld Symbol Properties .......................................................................................................................12-65 GOST Weld Symbol Properties ......................................................................................................................12-66 Area Hatch/Fill .......................................................................................................................................................12-66 Area Hatch/Fill Properties ......................................................................................................................................12-68 Blocks .....................................................................................................................................................................12-69 Insert Block PropertyManager ........................................................................................................................12-73 Block Instance PropertyManager ....................................................................................................................12-74 Attributes .........................................................................................................................................................12-74 Block Definition PropertyManager .................................................................................................................12-75 Tables .............................................................................................................................................................................12-76 Annotation Tables ..................................................................................................................................................12-76 Table Anchors ........................................................................................................................................................12-77 Table Templates .....................................................................................................................................................12-78 Custom Table Templates ........................................................................................................................................12-79 Table Format PropertyManager .............................................................................................................................12-79 Table Cell PropertyManager ..................................................................................................................................12-80 Bill of Materials ......................................................................................................................................................12-81 Bill of Materials PropertyManager .................................................................................................................12-83 Bill of Materials Contents ...............................................................................................................................12-84 Bill of Materials Column PropertyManager ....................................................................................................12-85 Bill of Materials Sort .......................................................................................................................................12-85 Hole Tables .............................................................................................................................................................12-86 Hole Table Add Holes .....................................................................................................................................12-88 Hole Table PropertyManager ..........................................................................................................................12-88 Hole Table Axis PropertyManager .................................................................................................................12-89 Hole Table Insert PropertyManager ................................................................................................................12-89 Hole Table Column PropertyManager ............................................................................................................12-90 Revision Tables ......................................................................................................................................................12-91 Revision Table PropertyManager ....................................................................................................................12-92 Revision Table Column PropertyManager ......................................................................................................12-93 Excel-based Bill of Materials ........................................................................................................................................12-94 Bill of Materials Overview .....................................................................................................................................12-94 Bill of Materials Templates ....................................................................................................................................12-94 Bill of Materials - Inserting ....................................................................................................................................12-95 Bill of Materials - Configuration ............................................................................................................................12-95 Bill of Materials - Contents ....................................................................................................................................12-96 Bill of Materials - Control ......................................................................................................................................12-96 Bill of Materials - Edit Text ...................................................................................................................................12-97 Bill of Materials - Part No. Column .......................................................................................................................12-98 Bill of Materials - Multiple Configurations ............................................................................................................12-98 Bill of Materials - Save as Excel File .....................................................................................................................12-99 Bill of Materials - Custom Properties ...................................................................................................................12-100
Chapter 13 Import/Export Importing and Exporting Files .........................................................................................................................................13-1 Importing/Exporting SolidWorks Documents .................................................................................................................13-2 Importing Documents ......................................................................................................................................................13-3
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Importing Geometry .........................................................................................................................................................13-3 Editing Imported Features ................................................................................................................................................13-4 Open - Match Faces and Edges of Imported Features .....................................................................................................13-5 Import Diagnosis ..............................................................................................................................................................13-5 Import Diagnosis PropertyManager .................................................................................................................................13-6 General Import Options ...................................................................................................................................................13-7 STL and VRML Import Options ......................................................................................................................................13-8 Exporting Documents and Setting Options ......................................................................................................................13-9 ACIS Export Options ................................................................................................................................................13-9 DXF/DWG Export Options ....................................................................................................................................13-10 eDrawings Export Options .....................................................................................................................................13-11 IGES Export Options ..............................................................................................................................................13-11 Surface Representation ...........................................................................................................................................13-12 Parasolid Export Options ........................................................................................................................................13-13 STEP Export Options .............................................................................................................................................13-13 STL Export Options ................................................................................................................................................13-14 TIFF Export Options ...............................................................................................................................................13-15 VRML Export Options ...........................................................................................................................................13-15 Exporting Multibody Documents ..................................................................................................................................13-16 Print3D ...........................................................................................................................................................................13-16 File Types .......................................................................................................................................................................13-17 ACIS Files (*.sat) ...................................................................................................................................................13-17 Autodesk Inventor Files ..........................................................................................................................................13-17 CADKEY Files .......................................................................................................................................................13-17 CATIA Graphics Files ............................................................................................................................................13-18 DXF 3D Files ..........................................................................................................................................................13-18 DXF/DWG Files (*.dxf, *.dwg) .............................................................................................................................13-19 DXF/DWG View Only ....................................................................................................................................13-20 DXF/DWG View Only PropertyManager .......................................................................................................13-21 Inserting DXF/DWG Files ..............................................................................................................................13-21 Copying and Pasting from AutoCAD to SolidWorks .....................................................................................13-22 Imported DXF/DWG Entities ..........................................................................................................................13-22 DXF/DWG Mapping .......................................................................................................................................13-23 eDrawings ...............................................................................................................................................................13-24 Saving Drawing Sheets in eDrawing Files .............................................................................................................13-25 Saving Configurations in eDrawing Files ...............................................................................................................13-26 Highly Compressed Graphics Files ........................................................................................................................13-26 HOOPS Files ..........................................................................................................................................................13-27 IGES Files (*.igs, *.iges) ........................................................................................................................................13-27 IGES Entity Types ..................................................................................................................................................13-28 IGES Levels ............................................................................................................................................................13-29 IGES 3D Curves .....................................................................................................................................................13-29 JPEG Files ..............................................................................................................................................................13-29 Mechanical Desktop Files .......................................................................................................................................13-29 Parasolid Files (*.x_t, *.x_b) ..................................................................................................................................13-33 PDF Files ................................................................................................................................................................13-33 Pro/ENGINEER Files .............................................................................................................................................13-33 Importing Pro/ENGINEER Part Files Into SolidWorks .........................................................................................13-34 Importing Pro/ENGINEER Assembly Files Into SolidWorks ...............................................................................13-35 Exporting SolidWorks Documents as Pro/ENGINEER Files ................................................................................13-36 Solid Edge Files ......................................................................................................................................................13-36 STEP Files (*.step) .................................................................................................................................................13-37 STL Files (*.stl) ......................................................................................................................................................13-37 TIFF Files (*.tif) .....................................................................................................................................................13-38 Inserting TIFF Files ................................................................................................................................................13-38 Unigraphics II Files ................................................................................................................................................13-39 VDAFS Files (*.vda) ..............................................................................................................................................13-39
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Viewpoint Files ......................................................................................................................................................13-39 VRML Files (*.wrl) ................................................................................................................................................13-40 ZGL Files ................................................................................................................................................................13-40
Chapter 14 Library Features and the Feature Palette Window Library Features and the Feature Palette Window ..........................................................................................................14-1 Palette Features and Library Features - Similarities and Differences .............................................................................14-1 Mandatory References .....................................................................................................................................................14-2 Library Features ...............................................................................................................................................................14-2 Library Features ........................................................................................................................................................14-2 Creating a Library Feature ........................................................................................................................................14-3 Adding a Library Feature to a Part ...........................................................................................................................14-4 Insert Library Feature Wizard ..................................................................................................................................14-5 Editing a Library Feature ..........................................................................................................................................14-5 Change Dimensions ..................................................................................................................................................14-5 Adding Color ............................................................................................................................................................14-5 Dissolving a Library Feature ....................................................................................................................................14-6 Feature Palette Window ...................................................................................................................................................14-6 Feature Palette Window ...........................................................................................................................................14-6 Feature Palette Window Overview ...........................................................................................................................14-6 Displaying the Feature Palette Window ...................................................................................................................14-7 Organizing Feature Palette Items .............................................................................................................................14-7 Creating a Palette Item .............................................................................................................................................14-8 Thumbnail Graphics .................................................................................................................................................14-9 Working with Palette Items and Folders ..................................................................................................................14-9 Palette Parts as Derived Parts .................................................................................................................................14-10 Adding Palette Items to Documents .......................................................................................................................14-10 Adding a Palette Feature to a Part ...................................................................................................................14-10 Edit This Sketch ..............................................................................................................................................14-11 Edit Dimension Access ...................................................................................................................................14-12 Internal Dimensions ........................................................................................................................................14-12 Adding a Palette Part to an Assembly .............................................................................................................14-12
Chapter 15 Sheet Metal Sheet Metal ......................................................................................................................................................................15-1 Designing Sheet Metal with Sheet Metal Features ..........................................................................................................15-2 Base Flange ..............................................................................................................................................................15-2 Examining the FeatureManager Design Tree ...........................................................................................................15-2 Edge Flange ..............................................................................................................................................................15-3 Profile Sketch ...........................................................................................................................................................15-4 Miter Flange .............................................................................................................................................................15-4 Miter Flange - Arc Sketches ..............................................................................................................................15-6 Miter Flange - Sketch Creation .........................................................................................................................15-6 Miter Flange - Edge Selection ...........................................................................................................................15-7 Bend Positions ..........................................................................................................................................................15-7 Trim Side Bends .......................................................................................................................................................15-8 Sheet Metal Tab ........................................................................................................................................................15-9 Sketched Bend ..........................................................................................................................................................15-9 Hem ........................................................................................................................................................................15-10 Closed Corner .........................................................................................................................................................15-12 Designing a Solid Body, then Converting it to Sheet Metal ..........................................................................................15-13 Bend Types .............................................................................................................................................................15-13 Creating a Sheet Metal Part Using Sharp Bends ....................................................................................................15-13 Creating a Sheet Metal Part Using Round Bends ...................................................................................................15-14 Creating Sheet Metal Parts with Conical Faces .....................................................................................................15-15 Adding Walls to a Sheet Metal Part .......................................................................................................................15-16 Sheet Metal Features ..............................................................................................................................................15-17
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Importing a Sheet Metal Part to SolidWorks ..........................................................................................................15-17 Comparing Sheet Metal Design Methods ......................................................................................................................15-18 Comparing Sheet Metal Design Methods ...............................................................................................................15-18 Design a Sheet Metal Part from a Solid ..................................................................................................................15-18 Design a Part from a Solid, Then Convert it to Sheet Metal ..................................................................................15-19 Design a Sheet Metal Part from the Flattened State ...............................................................................................15-20 Design a Part from the Flattened State, Then Convert it to Sheet Metal ................................................................15-20 Reasons to Build a Part, then Convert it to Sheet Metal ........................................................................................15-21 Combining the Different Sheet Metal Design Methods .........................................................................................15-21 Other Sheet Metal Topics ..............................................................................................................................................15-22 Bend Allowance and Bend Deduction ....................................................................................................................15-22 Bend Allowance and Bend Deduction Options ...............................................................................................15-22 Bend Allowance and Bend Deduction ............................................................................................................15-22 K-Factor ...........................................................................................................................................................15-23 Bend Table Overview ......................................................................................................................................15-23 Bend Table - Text File .....................................................................................................................................15-24 Bend Table - Excel Spreadsheet ......................................................................................................................15-24 Bend Allowance Value ....................................................................................................................................15-25 Bend Deduction Value ....................................................................................................................................15-25 Using Forming Tools with Sheet Metal ..................................................................................................................15-25 Forming Tools .................................................................................................................................................15-25 Creating Forming Tools ..................................................................................................................................15-25 Creating Openings on Forming Tools .............................................................................................................15-27 Create a Positioning Sketch for Forming Tool ................................................................................................15-27 Working with Palette Items and Folders .........................................................................................................15-27 Applying Forming Tools to Sheet Metal Parts ................................................................................................15-28 More Sheet Metal Topics ........................................................................................................................................15-28 Using Auto Reliefs ..........................................................................................................................................15-28 Changing Auto Reliefs ....................................................................................................................................15-29 Edit Auto Reliefs .............................................................................................................................................15-29 Edit All Auto Reliefs .......................................................................................................................................15-29 Rip ...................................................................................................................................................................15-30 Bends ...............................................................................................................................................................15-31 Edit Bends .......................................................................................................................................................15-31 Reorder Bends .................................................................................................................................................15-31 Flattening Sheet Metal Bends ..........................................................................................................................15-32 No Bends .........................................................................................................................................................15-32 Sheet Metal - Default Bend Parameters ..........................................................................................................15-32 Mirroring Sheet Metal Parts ............................................................................................................................15-33 Cut Across Sheet Metal Bends ........................................................................................................................15-34 Normal Cut ......................................................................................................................................................15-35 Break Corner/Corner-Trim ..............................................................................................................................15-35 Jog ....................................................................................................................................................................15-36 Lofted Bend .....................................................................................................................................................15-38 Bend Deviation ................................................................................................................................................15-39 Creating Sheet Metal Parts with Cylindrical Faces .........................................................................................15-40 Creating Drawings of Sheet Metal Parts .........................................................................................................15-41 Flat Pattern .......................................................................................................................................................15-42 Merge Faces .....................................................................................................................................................15-43 Simplify Bends ................................................................................................................................................15-43 Corner Treatment .............................................................................................................................................15-43 Add Corner-Trim .............................................................................................................................................15-44 Creating a Sheet Metal Flat Pattern Configuration .........................................................................................15-44 Unfold/Fold .....................................................................................................................................................15-45
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Chapter 16 Weldments Weldments Toolbar .........................................................................................................................................................16-1 Weldments - Structural Members ....................................................................................................................................16-1 Weldments - Pierce Points (Locate Profile) .............................................................................................................16-3 Weldments - Corner Treatments ..............................................................................................................................16-4 Weldments - Change Corner Treatment ...................................................................................................................16-4 Weldments - Trim and Extend .........................................................................................................................................16-5 Weldments - Adding Gussets ..........................................................................................................................................16-7 Weldments - Fillet Weld Beads .....................................................................................................................................16-10 Weldments - End Caps ..................................................................................................................................................16-13 Creating Sub-Weldments ...............................................................................................................................................16-14 Weldment Drawings ......................................................................................................................................................16-14 Weldment Cut Lists .......................................................................................................................................................16-15 Weldment Cut List PropertyManager ............................................................................................................................16-16 Weldment Cut List Column PropertyManager ..............................................................................................................16-17 Custom Properties in Weldments ..................................................................................................................................16-18
Chapter 17 SolidWorks Options Overview of SolidWorks Options ...................................................................................................................................17-1 System Options ................................................................................................................................................................17-2 General System Options ...........................................................................................................................................17-2 Drawings Options .....................................................................................................................................................17-4 Display Style Options ...............................................................................................................................................17-5 Area Hatch/Fill Options ...........................................................................................................................................17-6 System Colors ...........................................................................................................................................................17-6 Sketch Options ..........................................................................................................................................................17-7 Display and Selection Options .................................................................................................................................17-8 Performance Options ..............................................................................................................................................17-10 Performance Settings ..............................................................................................................................................17-13 Assembly Options ..................................................................................................................................................17-13 Large Assembly Mode Options ..............................................................................................................................17-13 External References - Options ................................................................................................................................17-15 Default Templates ..................................................................................................................................................17-16 File Locations .........................................................................................................................................................17-16 FeatureManager Options ........................................................................................................................................17-17 Spin Box Increments ..............................................................................................................................................17-18 View Rotation Options ...........................................................................................................................................17-18 Backup Options ......................................................................................................................................................17-19 Document Properties .....................................................................................................................................................17-19 Detailing Options ....................................................................................................................................................17-19 Dimensions Options ...............................................................................................................................................17-21 Notes Options .........................................................................................................................................................17-23 Balloons Options ....................................................................................................................................................17-23 Arrows Options ......................................................................................................................................................17-24 Virtual Sharp Display Options ...............................................................................................................................17-25 Annotations Display Options .................................................................................................................................17-25 Annotations Font Options .......................................................................................................................................17-26 Tables Options ........................................................................................................................................................17-26 View Labels Options ..............................................................................................................................................17-27 Grid and Snap Options ...........................................................................................................................................17-28 Units Options ..........................................................................................................................................................17-28 Document Colors ....................................................................................................................................................17-30 Material Properties Options ....................................................................................................................................17-30 Line Font Options ...................................................................................................................................................17-31 Image Quality .........................................................................................................................................................17-31 Plane Display ..........................................................................................................................................................17-32
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1 SolidWorks 2004 Reference Guide
Dear SolidWorks Customer, We are pleased to introduce the SolidWorks Reference Guide, a new publication available to SolidWorks Subscription Service members. This publication includes the entire contents of SolidWorks® 3D mechanical design software online help documentation in an easy-to-navigate Adobe® Acrobat® PDF format, making it easier for you to find the technical information you need quickly. In addition, we offer convenient printing options for any customer who wishes to obtain a printed version of this document, which is approximately 1,000 pages long. For details, please visit the “guides” section of the SolidWorks Support web site or click to http://www.solidworks.com/pages/services/subscription/ReferenceGuide.html. We welcome your feedback concerning the SolidWorks Reference Guide. Please send comments and suggestions via email to [email protected]. We appreciate your support as an active member of the SolidWorks community! Sincerely,
John J. McEleney CEO, SolidWorks Corporation
Scope The information in the Reference Guide comes from the SolidWorks Online Help for SolidWorks 2004 Service Pack 1. The Reference Guide does not include information on the add-ins such as the PhotoWorks software or the eDrawings software. The purpose of the Reference Guide is to provide a linear, easily printed version of the SolidWorks Online Help. SolidWorks Corporation is responding to your enhancement requests for a way to easily print the help, quickly return to previous topics, and mark pages for later reference. Please note: •
The text in the Reference Guide matches the text in the SolidWorks Online Help; it has not been rewritten for printed format. The text might seem awkward at times because it originates from context-sensitive help.
•
The order of the topics in the Reference Guide might seem awkward at times. SolidWorks Corporation made its best attempt to arrange the topics of the SolidWorks Online Help in the most logical order.
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Some page breaks may come at awkward times. A decision was made to forfeit some ideal placement of page breaks in favor of fewer pages in the book.
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All Related Topics buttons in the SolidWorks Online Help were deleted from the Reference Guide.
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Chapter 1 SolidWorks 2004 Reference Guide
Conventions The Reference Guide uses the following font and icon conventions: •
bold - Indicates a user interface element such as a menu item, tooltip, title of a dialog box, and so on.
•
- Represents a note or a tip. It is not a link; the information follows the icon. Notes and tips provide timesaving steps and helpful hints.
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hyperlinks - Indicates a hyperlink to another section of the Reference Guide. You can click hyperlinks in the .pdf file to be taken to another section. Hyperlinks do not change to cross-references with a page number in any printed versions of the book.
Resources Some of the resources provided by SolidWorks Corporation to aid you in learning the software are: •
Quick Tips - Pop-up messages that appear while you create SolidWorks documents. These messages give hints and options based on the current SolidWorks mode. Access: Click Help, Quick Tips.
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Introducing SolidWorks book - Discusses basic concepts and terms used throughout SolidWorks. The book uses a bathroom vanity to illustrate various tools and functions in the software. Access: Click Help, Introducing SolidWorks, or read the printed manual that is shipped to new customers.
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What's New book - Highlights the new functionality with step-by-step examples for many of the new functions. Access: Click Help, What's New Manual, or read the printed manual that is shipped to subscription customers.
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Online Tutorial - Includes step-by-step examples that teach the functionality of the SolidWorks product and its add-ins. Access: Click Help, Online Tutorial.
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Moving from AutoCAD - Assists AutoCAD users in learning some of the differences between SolidWorks and AutoCAD. Access: Click Help, Moving from AutoCAD.
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Glossary - Contains definitions of solid modeling and SolidWorks-specific terms. Access: Click the Glossary tab in the SolidWorks Online Help.
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Design Portfolio - Showcases parts created with SolidWorks, provides a high level overview of design intent, and presents potential design implementations. Access: Click Help, Design Portfolio.
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Release Notes - Contains information about new and changed functionality at every Service Pack. Access: Click Help, SolidWorks Release Notes.
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2 SolidWorks Fundamentals
SolidWorks Fundamentals What is SolidWorks 2004? SolidWorks® 2004 is mechanical design automation software that takes advantage of the familiar Microsoft® Windows® graphical user interface. This easy-to-learn tool makes it possible for mechanical designers to quickly sketch ideas, experiment with features and dimensions, and produce models and detailed drawings. This chapter discusses some basic concepts and terminology used throughout the SolidWorks software. It provides an overview of the following topics:
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Basic Concepts
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The FeatureManager Design Tree
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Opening New Documents and Using Templates
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Opening Existing SolidWorks Documents
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What's Wrong?
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Shortcut Menus
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View Modes
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Selection Methods
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Print and Print Preview
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SolidWorks Service Packs
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Converting Older SolidWorks Files to SolidWorks 2003
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Getting Help and Visiting the SolidWorks Web Site
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Using the Macro Tools
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Object Linking and Embedding (OLE)
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SolidWorks Application Programming Interface (API)
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Chapter 2 SolidWorks Fundamentals
Basic Concepts •
A SolidWorks model consists of parts, assemblies, and drawings.
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Typically, you begin with a sketch, create a base feature, and then add more features to your model. (You can also begin with an imported surface or solid geometry.)
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You are free to refine your design by adding, changing, or reordering features.
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Associativity between parts, assemblies, and drawings assures that changes made to one view are automatically made to all other views.
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You can generate drawings or assemblies at any time in the design process.
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The SolidWorks software lets you customize functionality to suit your needs.
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Click Tools, Options on the main menu to display the available System Options and Document Properties tabs.
•
The SolidWorks software saves your work for you. The auto recover option automatically saves information about your active part, assembly, or drawing document so you do not lose your work in case of a system crash. To set this option, click Tools, Options. On the System Options tab, click Backups and select Save auto recover info every
Document Windows In the SolidWorks application, each part, assembly, and drawing is referred to as a document, and each document is displayed in a separate window. (Each drawing document can contain multiple drawing sheets, though.)
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•
You can have multiple part, assembly, and drawing document windows open at the same time. Also, you can have multiple views of the same document visible at the same time.
•
To arrange the windows, you can drag them by their title bars, and you can resize them by dragging a corner or border. Also, from the Window menu, you can select Cascade, Tile Vertically, or Tile Horizontally.
•
To organize your SolidWorks window, you can minimize open documents. Click Minimize in the upper right corner of the document border. An icon appears in the lower part of the SolidWorks window. If the icon is not visible, it may be behind another open document. Resize any open documents as necessary. Click Window, Arrange Icons to arrange them at the bottom of the SolidWorks window.
•
Click Window, Close All to close all open documents. You are prompted to save any unsaved documents.
Cascade Arranges all SolidWorks document windows so they overlap with all their title bars visible. To cascade document windows:
Click Window, Cascade.
Tile Horizontally - Tile Vertically Arranges and shrinks the open SolidWorks document windows so they are all visible. To tile the document windows:
•
Click Window, Tile Horizontally to display the windows horizontally on your screen.
•
Click Window, Tile Vertically to display the windows vertically on your screen.
NOTE: If you have many SolidWorks documents open, the display will be both vertical and horizontal.
Arrange Icons Lines up all minimized document icons in evenly spaced rows at the bottom of the SolidWorks window. To arrange minimized document icons:
Click Window, Arrange Icons.
Close All Closes all open documents. If a new or changed document has not been saved, the program asks you to confirm whether you want to save the document or rebuild the part. To close all documents:
1.
Click Window, Close All.
2.
Respond to confirmation requests from the SolidWorks application to save or not save documents when they are closed.
New Window Creates a new window for viewing the active part, assembly, or drawing. To open another view in a new window:
1.
Click Window, New Window.
2.
Adjust the size and location of the new window, as desired. (To hide the FeatureManager design tree in the new window, drag the right edge of the FeatureManager design tree to the left edge of the window.) NOTE: This window is just another view of the same document. You can set the zoom, rotation, and view mode (wireframe, hidden removed/gray, or shaded) for each window independently, but any changes you make to the model will be reflected simultaneously in both windows.
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PropertyManager Overview More functions now use the PropertyManager instead of dialog boxes, which allows your graphics to be displayed instead of hidden by dialog boxes. Description The PropertyManager contains the following items: •
PropertyManager Title Block. Contains the feature icon and feature name
•
OK
, Cancel
, Preview
(Not shown are Keep Visible Undo
, and Help , Back
buttons.
, Next
, and
buttons.)
•
Group Boxes. Contain Group Box title label icons
• •
Group Box Open and Group Box Closed icons Selection Boxes. Available for making selections in the graphics area or in the FeatureManager design tree. When active they are pink. When you click an item in the selection box, the selected item is easier to identify in the graphics area, because the highlighted edges are bolder:
Edge is selected in PropertyManager - easier to identify in graphics area
, buttons and
Edge is not selected in PropertyManager - harder to identify in graphics area
Color Schemes You can apply pre-defined color schemes to the PropertyManager. To apply a pre-defined color scheme to the PropertyManager:
1.
Click Tools, Options, System Options, Colors.
2.
Select None in PropertyManager Skin. Skins take precedence over a color scheme in the PropertyManager.
3.
Select a color in Current Color Scheme. The colors in PropertyManager Color and PropertyManager Skin may change according to the color you selected in Current Color Scheme.
4.
Click OK. When you display the PropertyManager, the new color scheme appears.
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Entering Values and Accepting or Cancelling Commands When you have the PropertyManager displayed, there are several ways to enter values and accept commands. To enter values and accept commands:
Original part with Depth
1.
set to 10.
Set Depth to 30, but do not press Enter.
Press Enter and the preview updates.
In the Extrude PropertyManager, under Direction 1, set Depth
Press Enter again and the part updates to show the new value.
to 30, but do not press Enter.
The preview does not change because you have not yet accepted the new value. 2.
Press Enter. The preview now updates to show the new Depth
because you accepted the new value.
3.
At this point, if you want to cancel the Extrude command and retain the original depth, press Esc. However, you want to accept the new value.
4.
Press Enter again. The Extrude command is accepted. The part updates to show the new value, and the PropertyManager closes.
Deleting and Clearing Selections In the PropertyManager, you can right-click items in a list to delete them from the selection. For example, to delete a face selection from the Shell PropertyManager, right-click the name of the face in the list and select Delete. You can also right-click anywhere inside the list, and select Clear Selections to delete all of the items in the list. Split Bar The split bar separates the PropertyManager from the graphics area. If you drag the split bar back and forth, it snaps into position at the optimum width for displaying the PropertyManager. When you create new documents, the split bar opens at the optimum width. You can drag the split bar to resize the windows, as necessary.
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Callouts and Handles Callouts Callouts are text-filled boxes that appear in the graphics area when you use certain tools. Callouts help you easily distinguish between different entities. For example, these callouts show the sweep profile and the sweep path. You can drag these callouts to reposition them, but you cannot use them to change any properties of the entity to which they refer
Some callouts, such as those for chamfers, display figures that you can edit to manipulate the size of the entity.
In this example, you can edit the callout in the graphics area. Handles Handles allow you to dynamically click, move, and set certain parameters without leaving the graphics area. The handle color is set in Tools, Options, System Options, Colors, in the System colors box. Active handles are the Highlight color. Inactive handles are the Inactive Entities color. Handles span the length of extrusions. Drag the handle to the desired extrude depth, and the handle spans that length. You can also drag the pointer (instead of the handle) to the desired extrude depth. Click the handle, then drag the pointer in either direction
One handle has one arrow head, and the other handle has two arrow heads, to help you see which direction the handle applies to.
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Drag and Drop SolidWorks supports several drag and drop operations for features. •
Reordering features. You can change the order in which features are rebuilt by dragging them in the FeatureManager design tree. Place the pointer on a feature name, press the left mouse button, and drag the feature name to a new position in the list. (As you drag up or down the tree, each item that you drag over highlights. The feature name that you are moving drops immediately below the currently highlighted item when you release the mouse button.) If the reorder operation is legal, a
pointer appears; if it is not legal, a
pointer appears.
NOTE: A reorder operation is legal as long as the parent feature precedes its child feature. For more information, see Parent/Child Relationships. You can create folders in the FeatureManager design tree, and drag and drop features into the folders. Example: The Cut-Extrude feature was made before the Shell feature was added.
In the Feature Manager design tree, the Shell feature icon was dragged and dropped before Cut-Extrude icon.
•
Moving and copying features. You can move or copy features by dragging them in the model.
To move a feature to a new place on a model:
While holding down the Shift key, drag the feature to a different location. Release the mouse button to drop the feature on a planar face of the model. Example:
To move more than one feature at a time, hold down the Ctrl key as you select the features, then hold down the Shift key while you drag the features. To create a copy of the feature on a model:
Point at a planar face on the feature and hold down the Ctrl key while you drag the feature. Drop the copy on a planar face of the model.
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To copy a feature from one part to another part:
Tile the windows, then hold down the Shift key, point at a planar face on the feature, then drag and drop the feature from one window to another. - or You can also use the Copy
and Paste
tools on the Standard toolbar.
Shortcut Menu You have access to a variety of tools and commands on the shortcut menu while you work in the SolidWorks software. When you move the pointer over geometry in the model, over items in the FeatureManager design tree, or over the SolidWorks window borders, right-click to access a shortcut menu of commands that are appropriate for wherever you clicked. Shortcut menus include: • • •
Headings to denote sections of the menu. User-defined names if you apply custom names to features, components, and so on. Groups of related menu items.
To add or delete an item in a SolidWorks menu:
1.
Display the shortcut menu where you want to add or delete a menu item and select Customize Menu. Each item currently visible in the menu is preceded by
.
This menu is for customization purposes only. You cannot run a command from this menu. 2.
To add menu items, select the empty check boxes. To delete menu items, clear the selected check boxes.
3.
Click anywhere outside of the menu to save your changes, or press Enter. To cancel your changes, press Esc.
To restore the shortcut menus to default values or to show all menu items:
1.
Click Tools, Customize, or right-click over the toolbar area (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
2.
On the Options tab, under Shortcut customization: •
Click Show All to display all shortcut menu items.
•
Click Reset to Defaults to reset all shortcut menu items to the default display. Click the same buttons under Menu customization to update SolidWorks menus.
3.
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Click OK.
You can access the "more commands menu" by selecting the double-down arrows the double-down arrows, the shortcut menu expands to offer more menu items.
in the menu. When you click
The double-down arrows appear after you have executed at least one command in the menu. If you have not executed a command in the menu, or if the menu contains fewer than 12 items, the double-down arrows do not appear. The shortcut menu provides an efficient way to work without continually moving the pointer to the main pull-down menus or the toolbar buttons. For instance, with the shortcut menu, you can: •
Select a tool without moving your pointer to the toolbar
•
Open and close sketches
•
Change or view the properties of an item
•
Rename a feature or dimension with the Properties dialog box
•
Hide or show a sketch, plane, axis, or assembly component by right-clicking an item in the FeatureManager design tree or in the graphics area
•
Temporarily roll a model back to an earlier state by right-clicking any feature in the FeatureManager design tree and selecting Rollback
•
Open an assembly component for editing
•
Access the dimension tools and an annotations menu when in a drawing
•
Access the toolbars list when you click a SolidWorks window border
Accepting Features You have several streamlined ways to accept features you create. After creating a preview of a feature, you can: •
Right-click and select OK or Cancel from the shortcut menu.
•
Right-click when the pointer changes to without accepting the values.
to accept the preview, or click to return to the preview
Confirmation Corner Another way to accept features is to use the Confirmation Corner. You can: •
Click the OK or Cancel icons that appear in the Confirmation Corner of the SolidWorks graphics area.
•
Click the Exit Sketch icon in the Confirmation Corner to finish the sketch or click the Delete Sketch icon to discard changes to the sketch.
To turn off the Confirmation Corner, click Tools, Options, General, System Options, and clear Enable Confirmation Corner.
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PropertyManager In an active PropertyManager, you can: •
Click OK
•
Click Cancel
or press Enter. or press Esc.
Pop-up Tooltips Pop-up tooltips guide you when building models. Pop-up tooltips appear with an informational message, then disappear after a few seconds. Here are some examples of pop-up tooltips: Sheet Metal Example. This pop-up tooltip appears when you insert a fold in a sheet metal part. In the Fold PropertyManager, if you select BaseBend1 under Bends to fold, the popup tooltip warns you that the selected bend is already folded. Offset Example. If you try to offset a spline sketch, a pop-up tooltip advises you that you can only sketch offset lines and arcs.
Help If you have questions while you use SolidWorks, you can find answers in several ways: •
SolidWorks User Interface
Use the following tools to get help with items in the SolidWorks window: o
PropertyManagers and dialog boxes. In an active PropertyManager or dialog box, click Help , click the Help button, or press F1.
o
o
o
•
What's This. Click What's This on the Standard toolbar, then click a FeatureManager design tree, ConfigurationManager, PropertyManager, or toolbar item for help on that item. Tooltips. Provides information about tools on toolbars, PropertyManagers, and dialog boxes. When you pause the pointer over a tool for a brief time, a tooltip appears to display the name of the tool. Status Bar. Provides a brief description in the Status Bar at the bottom of the SolidWorks window as you move the pointer over a tool or click a menu item.
SolidWorks Online User's Guide
Provides assistance while you work. To access this resource, click Help on the Standard toolbar, or click Help, SolidWorks Help Topics. The help also contains a glossary of terms.
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•
Quick Tips
Displays a set of pop-up messages that appear while you create SolidWorks documents. Quick Tips give hints and options based on the current SolidWorks mode. Most of the messages have hyperlinks; click a hyperlink to see the associated item in the SolidWorks window. To access this resource, click Help, Quick Tips. Quick Tips are not available when the Online Tutorial is active. •
SolidWorks API and Add-Ins Help Topics
Provides assistance while you work on the SolidWorks Application Programming Interface (API) or other API add-in products. To access this resource, click Help, SolidWorks API and Add-Ins Help Topics. •
Moving from AutoCAD
Helps you transition from 2D AutoCAD to 3D SolidWorks. It compares terms and concepts, explains SolidWorks approaches to design, and provides links into SolidWorks help, tutorials, and other resources. To access this resource, click Help, Moving from AutoCAD. •
Introducing SolidWorks
Introduces concepts and design processes in a high-level approach. It does not give step-by-step procedures on how to create a model; instead, it guides you through the design process by illustrating how to plan models, make parts, build assemblies, then create drawings. This book is shipped to new customers. Introducing SolidWorks is available as an Adobe Acrobat file if you installed the manuals during the installation of the SolidWorks software. To access this resource, click Help, Introducing SolidWorks. •
Online Tutorial
Contains lessons that provide an online alternative to the Introducing SolidWorks book, and helps new users build models faster. To access this resource, click Help, Online Tutorial. o
o
o
•
The Online Tutorial includes several step-by-step lessons that cover SolidWorks topics and several add-in applications. You can execute some SolidWorks commands directly from the Online Tutorial. This is helpful when you need to open a sample part. Click a link, and the SolidWorks software automatically opens the part so you do not have to browse directories to locate the part. When you click a toolbar button in the Online Tutorial window, the corresponding button highlights in the SolidWorks software to help you locate the tool.
Design Portfolio
Contains part examples that help you understand how to combine the various SolidWorks tools to meet your design needs and requirements. To access this resource, click Help, Design Portfolio. •
What's New Manual
Provides information about new functionality in SolidWorks. The What's New Manual is available as an Adobe Acrobat file if you installed the manuals during the installation of the SolidWorks software. To access this resource, click Help, What's New Manual. •
Tip of the Day
Gives helpful hints about the SolidWorks software when you open a new SolidWorks session. To access this resource, click Help, Tip of the Day. To see a tip each time you start a SolidWorks session, select Show tips at startup in the Tip of the Day dialog box. •
Service Packs
Access SolidWorks service packs that are regularly posted on the SolidWorks Web site. These service packs contain software updates and enhancements to the SolidWorks software. Service packs are available for SolidWorks Subscription Service customers only. To check for a new service pack, click Help, Service Packs. •
SolidWorks Release Notes
Provides the latest information about operating systems, graphics cards, new functionality in the latest service pack, and so on. To access this resource, click Help, SolidWorks Release Notes.
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•
About SolidWorks
Displays information about the SolidWorks software. To access this resource, click Help, About SolidWorks. In the dialog box, click Connect to get information from the SolidWorks Web site. For information about add-in applications you installed, click Help, About
Partner Solutions
Provides access to the SolidWorks Solution Program Partner Web site. To access this resource, click Help, Partner Solutions.
What's Wrong? Lets you view rebuild errors or warnings in a part or assembly. When there is a rebuild error, the SolidWorks software cannot create the model geometry. When there is a warning, model geometry is still created. Some common rebuild errors include: •
Dangling Dimensions or Relations. Dimensions or relations to an entity that no longer exists
•
Features that cannot be rebuilt, such as a fillet that is too large
You can identify rebuild errors or warnings by icons in the FeatureManager design tree: Icon
Description Indicates an error with the model. This icon appears on the document name at the top of the FeatureManager design tree, and on the feature that contains the error. Indicates an error with a feature. This icon appears on the feature name in the FeatureManager design tree. Indicates a warning underneath the node indicated. This icon appears on the document name at the top of the FeatureManager design tree, and on the parent feature in the FeatureManager design tree whose child feature issued the error. Indicates a warning with a feature. This icon appears on the specific feature in the FeatureManager design tree that issued the warning.
If a document or feature has both an error and a warning, the
icon is displayed.
To review rebuild errors or warnings with the What's Wrong functionality:
Right-click the sketch, feature, part, or assembly name and select What’s Wrong? to display the error. The Rebuild Errors dialog box automatically appears when the error is first generated. The dialog box includes:
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•
Asterisks. If an error message has a prefix of **, click the message to highlight the problem area on the model.
•
Show errors. Displays error messages.
•
Show warnings. Displays warning messages.
•
Display What's Wrong during rebuild. Automatically displays errors each time you rebuild the model. This option affects only the current SolidWorks session.
•
Display full message. Displays the complete message whenever there is an error. Otherwise, an abbreviated message is displayed.
Print Prints the active document. To print the active document:
1.
Click File, Print.
2.
In the dialog box, select from the following options: •
Document Printer o
Name. Specifies the printer.
o
The system provides read-only information about the printer’s status, type, and location.
o
Properties. Sets options that are specific to the selected printer.
o
•
•
System Options o
Line Weights. Specifies the line weights that work best with your printer or plotter.
o
Margins. Specifies values for the top, bottom, left, and right margins for the document.
Document Options o
•
Page Setup. Specifies page setup options and advanced printer options such as scale, orientation, resolution, and so on.
Header/Footer. Specifies headers and footers for the active document.
Print range o
All. Prints all pages of the document.
o
Pages (Drawings only). Prints the sheets you specify.
o
Selection (Drawings only). Prints a selected area of a drawing sheet at a scale you specify.
• Select from the following options. The last set state is remembered on subsequent prints during the current SolidWorks session only. o
Number of copies. Sets the number of copies to print.
o
Print background. Prints the window background, in addition to the model or drawing.
o
o
3.
Print to file. Prints to a file instead of the printer. Type a name for the file in the Print to File dialog box. Convert draft quality drawing views to high quality (Drawings only). Converts the current draft quality view into high quality for printing purposes only.
Click OK.
Page Setup Allows you to change printer settings. You must have a SolidWorks document open to set printer settings. To change printer settings:
1.
Click File, Page Setup.
2.
In the dialog box, select from the following options: •
Printer Settings. Select one of the following: o
o
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Use system settings. Prints the document with Windows print settings, and allows you to change these settings as needed. Use this document's settings. Overrides system print settings with the print settings saved in the current document, and applies any changes to these settings in the current document only. System print settings remain unchanged.
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o
Set each drawing sheet individually. Specify the settings for each sheet in the drawing by selecting a drawing sheet in Settings for. In subsequent files that you print, the SolidWorks software remembers the last setting you selected.
•
Resolution and Scale. Set the scale for the printed document. o
Same as window (parts and assemblies only). Prints the current view of the graphics area.
o
Scale to fit (drawings only). Prints the drawing sheet to fit the paper size.
o
Scale. Prints the document at a scaled value (in percent) that you specify.
o
High Quality (drawings only). The SolidWorks software determines the optimum resolution for the printer and paper size combination, generates the raster output and prints it accordingly. When you select High Quality, click File, Print, Properties to set any advanced properties for the selected printer. If there are options for improved raster output, selecte them to get the highest quality printed output.
•
•
Paper. Select: o
Size. Sets the paper size on which you want to print the document.
o
Source. Sets the printer tray where the paper is located.
Drawing Color. Select one of the following: o
o
o
•
3.
Automatic. Sends color information if the printer or plotter driver reports that it is capable of printing color. Otherwise, the SolidWorks software sends black and white information. Color / Gray scale. Sends color data to the printer or plotter regardless of the capabilities that the printer or plotter driver reports. Black and white printers generally print colored entities in gray scale or dithered with this option. Use this option where a color printer or plotter prints in black and white with the Automatic setting. Black and white. Sends all entities to the printer or plotter in black and white regardless of the printer or plotter color capabilities.
Orientation. Select: o
Portrait. Prints the document with a vertical page orientation.
o
Landscape. Prints the document with a horizontal page orientation.
Click OK.
Line Weights You can set the line weights in an active document that work best with your printer or plotter. These settings are saved for all open SolidWorks documents. To set line weights:
1.
Click File, Print.
2.
In the dialog box, under System Options, click Line Weights.
3.
In the Line Weights dialog box, type a value for the line weights (Thin, Normal, Thick, and five additional line thickness settings). If you use specific Line Thickness the settings in the Line Weights dialog box.
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values in a SolidWorks drawing, the lines print according to
4.
Click OK.
5.
Click OK to close the Print dialog box and print the document.
Margins You can set values for the top, bottom, left, and right margins for the printed document. These settings are saved for all SolidWorks documents. To set print margins:
1.
Click File, Print. The Print dialog box appears.
2.
Under System Options, click Margins. The Margins dialog box appears.
3.
Clear the Use printer’s margins check box. NOTE: The Use printer's margins check box prints the document with the printer's default margin values. If you modified the values in the Margins dialog box, select this check box to view the printer's default margin values.
4.
Set the Top, Bottom, Left, and Right margins to the desired values.
5.
Click OK.
6.
Click OK to close the Print dialog box and print the document.
Printing Drawings You can print or plot an entire drawing sheet, or just a selected area of the sheet. You have the option to print in black and white (the default) or in color. You can specify different settings for individual drawing sheet. For basic information about printing and plotting any SolidWorks document, see Print. To specify settings for individual drawing sheets:
1.
Click File, Page Setup. Under Individual Drawing Sheet Control, select Set each sheet individually.
2.
Select a sheet from the Settings for list, and choose settings for the sheet.
3.
Repeat step 2 for each sheet, or leave any sheet at the default settings, and click OK.
To print a drawing in color:
1.
In a drawing, modify the colors of the entities as desired. For information about changing the color, style, and thickness of entities, see Component Line Font, Line Format, and Layers.
2.
Click File, Page Setup. Under Drawing Color, select one of the following, then click OK: •
Automatic. SolidWorks detects the printer or plotter capabilities and sends color information if the printer or plotter driver reports that it is capable of printing color. Otherwise, SolidWorks sends black and white information.
•
Color / Gray scale. SolidWorks sends color data to the printer or plotter regardless of the capabilities that the printer or plotter driver reports. Black and white printers generally print colored entities in gray scale or dithered with this option. Use this option where a color printer or plotter prints in black and white with the Automatic setting.
•
Black and white. SolidWorks sends all entities to the printer or plotter in black and white regardless of the printer or plotter color capabilities.
3.
Click File, Print. In the Print dialog box, under Name, select a printer that supports color.
4.
Click Properties, verify that any options required for color printing are specified appropriately, then click OK. (The options vary for different printers.)
5.
Click OK to print. When the specified printer is set up for color printing, Print Preview displays the drawing in color also.
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To print the whole drawing sheet:
1.
Click File, Print. In the Print dialog box, under Print range, click All or specify the Pages you want to print.
2.
Under Scale, click the Scale To Fit check box to print the entire sheet on the page, or clear the check box and specify a Scale value (by percent).
3.
Click OK.
To print a selected area of a drawing sheet:
1.
Click File, Print. In the Print dialog box, under Print range, click Selection, and click OK. The Print Selection dialog box appears, and a selection frame is displayed on the drawing sheet. The frame reflects the current printer settings (page size, orientation, and so on) as defined under File, Page Setup, Print Setup.
2.
Select a scale factor to apply to the selected area. •
Model scale (1:1). This is the default. This means that the selected area is printed at actual size; a model dimension of 100mm is printed at 100mm. The default sheet scale is used to calculate the correct print size; therefore, for views that use a scale different than the default sheet scale, you may need to use a custom scale to achieve the desired result.
•
Sheet scale (n:n). The selected area is printed as it appears on the full sheet. If the drawing size and the paper size are the same, the entire sheet is printed. Otherwise, only the selected area is printed, as it would appear on the full sheet.
•
Custom scale. The selected area is printed at a scale factor you define. Enter the values you want in the boxes, then click Apply scale. You can use Custom scale to focus on a particular area of a drawing sheet.
When you change the scale factor, the selection frame size changes accordingly. 3.
Drag the selection frame to position it over the area you want to print. You can drag the entire frame, but you cannot drag the individual sides to control the selected area. You can pan or zoom the view, or change the sheet while the selection frame is displayed.
4.
Click OK to print the selected area.
Print Selection Lets you specify an area of the drawing sheet to print. To specify an area of the drawing sheet to print:
1.
In an open drawing, click File, Print.
2.
In the dialog box, under Print range, click Selection, then click OK. The Print Selection dialog box appears, and a selection frame appears on the drawing sheet. The frame reflects the current printer settings (such as page size, and orientation) as defined in the Page Setup dialog box.
3.
Select a scale factor to apply to the selected area: •
Model scale (1:1). The selected area is printed at actual size; a model dimension of 100mm is printed at 100mm. The default sheet scale is used to calculate the correct print size; therefore, for areas that use a scale different than the default sheet scale, you may need to use a custom scale to get the desired result.
•
Sheet scale (1:1). The selected area is printed as it appears on the full sheet. If the drawing size and the paper size are the same, the entire sheet is printed. Otherwise, only the selected area is printed.
•
Custom scale. The selected area is printed at a scale factor you define. Type the values you want in the boxes, then click Apply scale.
Click Example to see Custom scale examples.
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4.
Drag the selection frame to position it over the area you want to print. You can pan or zoom the view while the selection frame is displayed. The pointer changes to
5.
as you position the selection frame.
Click OK to print the selected area.
Custom Scale Examples Drawing Sheet Scale
Custom Scale for Printing
1:1
1:1
Printed Output
A 1 inch x 1 inch box prints at the same scale (1 inch x 1 inch). 1:1
2:1
A 1 inch x 1 inch box prints as a 2 inch x 2 inch box, even though the dimension values remain the same. (Conversely, if you set the custom scale to 1:2, the box prints at 0.5 inches x 0.5 inches.) 1:2
1:1
A 1 inch x 1 inch box prints as a 1 inch x 1 inch box. However, only one-fourth of the drawing sheet prints because the drawing is zoomed in to get the box to the 1:1 scale.
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D-Landscape 1:1
A-Landscape 1:1
A 1 inch x 1 inch box prints as a 1 inch x 1 inch box because the drawing sheet scales are the same. However, only oneeighth of the drawing sheet prints because an A-Landscape sheet is oneeighth the size of a D-Landscape sheet.
Print Preview Previews the image of the active document before you send it to the printer. To preview a print job:
Click Print Preview
on the Standard toolbar, or click File, Print Preview.
Keyboard Shortcuts Keyboard shortcut keys are available for every menu item. Look for the underlined letters on the main menu bar. If you do not see the underlined letters on the main toolbar, press Alt. Press Alt and the underlined letter to display the menu. For example, press Alt+F to display the File menu. Also, look for the underlined letter for each of the menu items. When the menu is displayed, pressing an underlined letter activates the related command. For example, press Alt+F to display the File menu, then press C to close your files. Some commands also have shortcut keys that are displayed on the menu beside the command. For example, the combination Ctrl+N opens a new file.
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This table lists commonly used default keyboard shortcuts: Action Model Views Rotate the model: • horizontally or vertically • horizontally or vertically 90 degrees • clockwise or counterclockwise Pan the model Zoom in Zoom out Zoom to Fit Previous View View Orientation View Orientation menu Front Back Left Right Top Bottom Isometric Selection filters Filter Edges Filter Vertices Filter Faces Toggle Selection Filter toolbar Toggle selection filters (on/off) File menu items New SolidWorks document Open document Open From Web Folder Make Drawing from Part Make Assembly from Part Save Print Additional keyboard shortcuts Access online help when in a PropertyManager or dialog box Rename an item in the FeatureManager design tree (this works for most items) Rebuild the model Force rebuild the model and rebuild all of its features Redraw the screen Cycle between open SolidWorks documents Line to arc/arc to line (sketch mode) Undo Cut Copy Paste Delete Next window Close window
Key Combination
Arrow keys Shift+Arrow keys Alt+ left or right Arrow keys Ctrl+Arrow keys Z z f Ctrl+Shift+Z Spacebar Ctrl+1 Ctrl+2 Ctrl+3 Ctrl+4 Ctrl+5 Ctrl+6 Ctrl+7 e v x F5 F6 Ctrl+N Ctrl+O Ctrl+W Ctrl+D Ctrl+A Ctrl+S Ctrl+P F1 F2 Ctrl+B Ctrl+Q Ctrl+R Ctrl+Tab a Ctrl+z Ctrl+ x Ctrl+ c Ctrl+ v Delete Ctrl+F6 Ctrl+F4
Additionally, you can customize the keyboard shortcut keys to suit your style of working.
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Send Mail Sends the current SolidWorks document to another system using your electronic mail application. To mail a part or sketch to another computer:
1.
Click File, Send To. Your electronic mail application responds with its usual dialog box.
2.
Type your mail password, the mailing address, and any other information required by your mail application.
To mail an assembly or drawing to another computer:
1.
Click File, Send To.
2.
In the dialog box, select one of the following: •
•
A list of the referenced documents and their locations, the number of documents, and the combined size of the documents is displayed. If the size of the mail is large, it can cause transmission problems. If you choose to send the assembly or drawing and referenced documents, you do not have to send all of the referenced files. You can click: •
Attach. Attaches the selected reference document to the mail message. (The paper clip icon is added.)
•
Remove. Removes the selected reference document from the mail message. (The paper clip icon is replaced.)
•
Attach All. Attaches all of the reference documents to the mail message. (The paper clip icon is added.) If an assembly document has lightweight components, this dialog box does not appear.
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3.
Click OK.
4.
Type your mail password, the mailing address, and any other information required by your mail application.
Toolbars Toolbars Displays or hides toolbars. See the following: 2D to 3D
Font
Sketch
Align
Layer
SolidWorks Office
Annotation
Line Format
Spline Tools
Assembly
Macro
Standard
Curves
Mold Tools
Standard Views
Dimensions/Relations
Reference Geometry
Surfaces
Drawing
Selection Filter
Tools
Explode Sketch
Sheet Metal
View
Features
Simulation
Web Weldment
Toolbars for installed add-in products are available. These are available only if you select the toolbar from the View, Toolbars menu. You can use flyout toolbars to save space in the graphics area. When you click a flyout button associated with the flyout button appears.
, the toolbar
You can add flyout buttons to any toolbar, including the CommandManager. To make toolbars visible:
1.
Click Tools, Customize.
2.
On the Toolbars tab, under Toolbars, select the toolbars that you want to display; clear the toolbars that you want to hide.
3.
Click OK.
To add a toolbar button to a toolbar:
1.
Click Tools, Customize, Commands.
2.
In the dialog box, select a toolbar in Categories. To add a flyout button, select Flyout Toolbars.
3.
Under Buttons, drag a toolbar button to a toolbar in the SolidWorks window.
4.
Click OK.
To access hidden toolbar buttons:
Occasionally a toolbar is longer than the length of your screen. If this occurs, click the arrows toolbar to access the hidden toolbar buttons.
at the end of the
To move a toolbar:
Click the start or edge of the toolbar and drag. If you drag a toolbar to an edge of the SolidWorks window, the toolbar docks to the edge automatically. - or If you drag a toolbar away from the window edge, it becomes a floating palette. If you accidentally move a toolbar and you want to move it back to its original position, double-click the toolbar title.
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2D to 3D Toolbar The 2D to 3D tools help you convert a 2D drawing to a 3D part. Some of the tools can be used in any sketches. Front. The selected sketch entities become the front view in converting to a 3D part. Top. The selected sketch entities become the top view in converting to a 3D part. Right. The selected sketch entities become the right view in converting to a 3D part. Left. The selected sketch entities become the left view in converting to a 3D part. Bottom. The selected sketch entities become the bottom view in converting to a 3D part. Back. The selected sketch entities become the back view in converting to a 3D part. Auxiliary. The selected sketch entities become an auxiliary view in converting to a 3D part. You must select a line in another view to specify the angle of the auxiliary view. Create Sketch from Selections. The selected sketch entities become a new sketch. You can extract a sketch, for example, and then modify it before creating a feature. Repair Sketch. You can fix errors in a sketch so that the sketch can be used to extrude or cut a feature. Typical errors can be overlapping geometry, small gaps, or many small segments that are collected into a single entity. Align Sketch. Select an edge in one view to align to the edge selected in a second view. The order of selection is important. Extrude. Extrude a feature from the selected sketch entities. You do not have to select a complete sketch. Cut. Cut a feature from the selected sketch entities. You do not have to select a complete sketch.
Align Toolbar The Align toolbar provides tools for aligning annotations such as Notes, Geometric Tolerance Symbols, and so on. See Aligning Annotations. Leftmost Rightmost Uppermost Lowermost Space evenly across Space evenly down Center Horizontal Center Vertical Compact Horizontal Compact Vertical
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Annotations Toolbar The Annotations toolbar provides tools for adding notes and symbols to a drawing, part, or assembly document. Only those annotations that are appropriate for the active document are available; the other tools are displayed in gray. Note Surface Finish Geometric Tolerance Balloon AutoBalloon Stacked Balloon Datum Feature Symbol Weld Symbol Datum Target Insert Block Model Items Center Mark Centerline Hole Callout Cosmetic Thread Multi-jog Leader Dowel Pin Symbol Hole Table Bill of Materials Revision Table Design Table Weldment Cut List
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Assembly Toolbar The Assembly toolbar controls the management, movement, and mating of components. Insert Components New Part New Assembly Large Assembly Mode Hide/Show Components Change Transparency Change Suppression State Edit Component Smart Fasteners Mate Move Component Rotate Component Replace Components Replace Mate Entities Exploded View Explode Line Sketch Interference Detection Change Assembly Transparency Simulation Toolbar
CommandManager The CommandManager is a context-sensitive toolbar that dynamically updates based on the toolbar you want to access. By default, it has toolbars embedded in it based on the document type. When you click a button in the control area, the CommandManager updates to show that toolbar. For example, if you click Sketches in the control area, the Sketch toolbar appears in the CommandManager.
Use the Command Manager to access toolbar buttons in a central location and to save space for the graphics area.
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To access the CommandManager:
1.
Click Tools, Customize.
2.
In the dialog box, on the Toolbars tab, select Enable CommandManager.
3.
Click OK.
To use the CommandManager:
Click a button in the control area. The CommandManager updates to show the toolbar associated with the button you clicked. - or Click
next to a button in the control area.
The flyout toolbar associated with the button you clicked appears. To add buttons to the control area of the CommandManager:
When you add a button to the control area of the CommandManager, the button appears in the current document type only. For example, if you add the Reference Geometry button to the control area of the CommandManager while in a part document, it does not appear in the CommandManager for an assembly document. 1.
Right-click anywhere in the CommandManager and select Customize CommandManager.
2.
In the menu, select the toobars to add.
3.
Click anywhere outside the menu to save your changes, or press Enter. - or -
1.
Click Tools, Customize.
2.
On the Commands tab:
3.
a.
Select Flyout Toolbars in Categories.
b.
Under Buttons, drag the button to the control area of the CommandManager.
Click OK.
The Layer toolbar is not available in the CommandManager. To turn off the toolbar button descriptions:
Right-click anywhere in the CommandManager and select Show Description to clear the check mark.
Curves Toolbar The Curves toolbar provides tools for creating and using curves. Project Curve Split Line Composite Curve Curve Through XYZ Points Curve Through Reference Points Helix and Spiral
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Dimensions/Relations Toolbar and Menus The Dimensions/Relations toolbar and the Tools, Dimensions and Tools, Relations menus provide tools to dimension and to add and delete geometric relations. Not all toolbar buttons have corresponding menu items; conversely, not all menu items have corresponding toolbar buttons. Smart Dimension Horizontal Dimension Vertical Dimension Baseline Dimension Oridinate Dimension Horizontal Ordinate Dimension Vertical Ordinate Dimension Chamfer Dimension Autodimension Add Relation Display/Delete Relations Scan Equal Align Ordinate Constrain All
Drawing Toolbar The Drawing toolbar provides tools for aligning dimensions and creating drawing views. Align Collinear/Radial Align Parallel/Concentric Hide/Show Annotations Detail View Section View Aligned Section View Projected View Standard 3 View Auxiliary View Named View
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Relative View Predefined View Empty View Update View Crop View Broken-out Section Alternate Position View Area Hatch/Fill
Explode Sketch Toolbar With the Explode Sketch tools, you can add route lines to assembly explode line sketches and 3D sketches, and add jogs to sketch lines. Route Line Jog Line
Features Toolbar The Features toolbar provides tools for creating model features. The set of features icons is very extensive so not all of them are included on the default Features toolbar. You can customize this toolbar by adding and removing icons to suit your working style and frequent tasks. See Customize Toolbars for more information. Extruded Boss/Base Revolved Boss/Base Sweep Loft Thicken Extruded Cut Revolved Cut Swept Cut Lofted Cut Thickened Cut Cut with Surface Fillet Chamfer
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Rib Scale Shell Draft Simple Hole Hole Wizard Dome Shape Deform Wrap Move/Size Features Suppress Unsuppress Unsuppress with Dependents Linear Pattern Circular Pattern Mirror Feature Curve Driven Pattern Sketch Driven Pattern Table Driven Pattern Split Combine Join Delete Solid/Surface Imported Geometry Insert Part Move/Copy Bodies Library Feature
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Font Toolbar You can specify the font, font size, font style, and justification for selected notes, dimensions, and geometric tolerances. You can also reset the font properties to the document defaults. The Font toolbar is active only when notes, dimensions, or geometric tolerances are selected. Balloon text and view labels (Section View, Detail View, and so on) are notes and can be formatted with the Font tools. To specify a font:
1.
Select notes, dimensions, or symbols to format. Hold down Ctrl to make multiple selections.
2.
Select from the following font properites: •
Font. Select a font type from the list of font sets available on your system.
•
Font Size. Select the point size to use. The corresponding font size in the document’s default unit of measure is displayed in the next box. (The measurement corresponds to the actual height of the tallest character in the font set.)
•
Font Style. Click the icons for Bold, Italic, or Underline, or a combination of these.
•
Justification. Click the icons for Left Justify, Center Justify, or Right Justify to justify Note text.
To reset text to the document default font:
1.
Select a formatted item.
2.
Click Document Font
.
The text returns to the document font, size, style, and justification.
Layer Toolbar The Layer toolbar contains a list of layers in the active drawing and a tool for specifying the properties of layers. Layer Properties
Line Format Toolbar The Line Format toolbar provides tools for changing the appearance of individual lines, edges, and sketch entities in a drawing. Layer Properties Line Color Line Thickness Line Style Hide Edge Show Edge Color Display Mode
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Macro Toolbar The Macro toolbar controls macro recording, playback, and editing. Run Macro Stop Macro Record\Pause Macro New Macro Edit Macro
Mold Tools Toolbar The Mold Tools toolbar provides tools for creating molded parts and assemblies. Scale Parting Lines Ruled Surface Parting Surfaces Tooling Split Cavity Draft Split Line Offset Surface Ruled Surface Radiate Surface Planar Surface Knit Surface Draft Analysis Undercut Detection
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Reference Geometry Toolbar The Reference Geometry toolbar provides tools for creating and using reference geometry. Plane Axis Coordinate System Point Mate Reference
Sheet Metal Toolbar The Sheet Metal toolbar provides tools for creating and using sheet metal parts. Insert Bends Flatten No Bends Rip Base-Flange/Tab Miter Flange Fold Unfold Sketched Bend Edge Flange Closed Corner Hem Break-Corner/Corner-Trim Jog Lofted-Bend
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Simulation Toolbar The Simulation toolbar contains the tools for using Physical Simulation. Stop Record or Playback Calculate Simulation Reset Components Replay Simulation Linear Motor Rotary Motor Linear Spring Gravity
Sketch Toolbar The tools on the Sketch toolbar affect the entire sketch, rather than individual sketch entities. The Sketch toolbar controls selection, sketch creation, sketch modification, and the sketch grid.
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Select
Circle
Face Curves
Grid/Snap
Ellipse
Mirror Entities
Sketch or Exit Sketch
Partial Ellipse
Sketch Fillet
3D Sketch
Parabola
Sketch Chamfer
Modify Sketch
Spline
Offset Entities
Move or Copy Entities
Polygon
Fit Spline
Rotate or Copy Entities
Rectangle
Trim Entities
Scale or Copy Entities
Parallelogram
Extend Entities
No Solve Move
Point
Split Entities
Line
Centerline
Construction Geometry
Centerpoint Arc
Text
Tangent Arc
Convert Entities
3 Point Arc
Intersection Curve
Linear Sketch Step and Repeat Circular Sketch Step and Repeat Sketch Picture
SolidWorks Office Toolbar The SolidWorks Office toolbar allows you to activate any add-in application included in the SolidWorks Office package. The SolidWorks Office toolbar is unavailable if you did not install SolidWorks 2004 with a SolidWorks Office registration code. PhotoWorks release 2 SolidWorks Animator eDrawings 3D Instant Website SolidWorks Toolbox SolidWorks Utilities FeatureWorks
Spline Tools Toolbar Use tools on the Spline Tools toolbar to control properties of a sketched spline. The Spline tool is on the Sketch toolbar. Spline Point Show Inflection Points Show Minimum Radius Show Curvature Combs Simplify Spline
Standard Toolbar The Standard toolbar controls file management and model regeneration. New Open Save Make Drawing from Part/Assembly Make Assembly from Part/Assembly Print Print Preview Cut
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Copy Paste Delete Undo Redo Rebuild Redraw Edit Color Edit Material Edit Texture Toggle Selection Filter Toolbar Web Toolbar Help What's This? Save Saves the active document to disk. To save a document:
Click Save
or File, Save, or press Ctrl+S.
NOTE: When you save a new document, the Save As dialog box opens so that you can enter a filename or accept a default filename. Save As Saves the active document to disk with a new name or saves it in a different format for export to another application. To save a document with a new filename or format:
1.
Click File, Save As.
2.
In the dialog box, click the Save in box to browse to the location where you want to save the document. Use the locations sidebar to help navigate to the location where you want to save your document. The locations sidebar is available in certain operating systems only.
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3.
Type a name for File name.
4.
Select from the following options, if necessary: •
Save as type. Saves the file in another file format. You can also export files.
•
Description. Provides a description of the model.
•
Save as copy. Saves the document to a new filename without replacing the active document.
•
Save eDrawing data. Saves the document with eDrawings data so you can open the document in the eDrawings Viewer. If you selected Save eDrawings data in SolidWorks document in Tools, Options, System Options, General, you can override this option when you save your document. To override this option, clear Save eDrawing data.
5.
•
References. Displays a list of the documents referenced by the currently selected assembly or drawing. You can edit the locations of the listed files.
•
Down arrow (next to the Save button). Accesses Add to Favorites to create a shortcut to the selected document in your Favorites folder.
Click Save. The document is saved in the location you specified.
Cut Removes the selected items and places them on the Microsoft Windows Clipboard. To cut:
1.
Select the item(s) to cut.
2.
Click Cut
, or Edit, Cut, or press Ctrl+X.
Copy Copies one or more selected items to the Microsoft Windows Clipboard. To copy:
1.
Select one or more items to copy.
2.
Click Copy
, or Edit, Copy, or press Ctrl+C.
Paste Copies the contents of the Clipboard to the current sketch, part, assembly, or drawing document. To paste the contents of the Clipboard:
1.
2.
If necessary, select an appropriate destination for the item being pasted. For example: •
If the Clipboard contains a sketch, select a face or a plane to paste the sketch on.
•
If the Clipboard contains an extruded or revolved feature or a hole, select a face to paste the feature on.
Click Paste
or Edit, Paste, or press Ctrl+V.
Delete Removes one or more selected items. To delete an item:
1.
Select one or more items to delete.
2.
Click Delete
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on the Standard toolbar, click Edit, Delete or press Delete.
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3.
4.
In the dialog box, select: •
Also delete absorbed features. Deletes features that were used to create the item to be deleted listed in And All Dependent Items.
•
Also delete all child features. Deletes features dependent on a previously built feature listed in And All Dependent Items.
Click Yes. If you selected more than one item in step 1, click Yes to All to delete all of the items.
Undo Reverses recent changes you have made, when possible. To undo your last action:
Click Undo
or Edit, Undo, or press Ctrl+Z.
To undo multiple operations:
1.
Click Undo List (to the right of the Undo button) to see the list of actions that are available to undo. The most recent actions are at the top of the list.
2.
Select any action on the list. The action you selected and all actions above it on the list are reversed.
Redo Reverses recent Undo commands you have made, when possible. Redo is available only for sketches in part and assembly documents. To redo your last Undo action:
Click Redo
or Edit, Redo, or press Ctrl+Y.
To redo multiple Undo operations:
1.
Click Redo List (to the right of the Redo button) to see the list of Undo actions that are available to redo. The most recent actions are at the top of the list.
2.
Select any action on the list. The action you selected and all actions above it on the list are redone.
Rebuild Rebuilds the model with any changes that you made. To rebuild the model:
Click Rebuild
or Edit, Rebuild, or press Ctrl+B.
NOTE: When you reorder an imported feature or any other feature with no parent or child, the part does not rebuild - only the FeatureManager design tree rebuilds. Redraw Refreshes the screen, but does not rebuild the part. To refresh the screen:
Click Redraw
or View, Redraw, or press Ctrl+R.
NOTE: Use Redraw to refresh the screen if the graphics do not appear to be complete.
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Color And Optics PropertyManager Use the Color And Optics PropertyManager to apply color and optical properties to selected entities in a model. Selection •
•
Selection filters. Helps you select geometric entities in the model. o
Select Faces
o
Select Features
o
Select Surfaces
o
Select Components
o
Select Bodies
o
Select Parts
(assemblies only)
(assemblies only)
Remove Color. Deletes the color and optical properties from the selected geometry.
Favorite • •
Current Color. Displays the currently selected color in the swatch. Select or Create a Swatch. Displays pre-defined swatches included with the SolidWorks software.
•
Click Create New Swatch to define a custom swatch. Select Existing Color or Add Color. Displays the colors contained in the selected swatch.
•
Add Current Color to Swatch
•
Remove Current Color from Swatch
. Adds the selected color to a custom swatch. . Removes the selected color from a custom swatch.
Color Properties • •
Current Color. Displays the current color of the selected entity. Pick a Color. Displays all colors in the color palette.
• • •
RGB. Defines a color with red, green, and blue values. HSV. Defines a color with hue, saturation, and value entries. Numeric. Allows you to enter numeric values for RGB or HSV: o
Red Component of Color
o
Hue Component of Color
o
Green Component of Color
o
Saturation Component of Color
o
Blue Component of Color
o
Value Component of Color
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Optical Properties •
Transparency. Controls the degree to which light passes through the model.
•
•
Ambience. Approximates the intensity of a light source illuminating a surface from all directions without attenuation or shadowing.
•
•
Diffusion. Controls the intensity of the light on the surface. Diffusion is dependent on its angle to a light source but independent of the position of the viewer.
•
Specularity. Controls the intensity of the light on the surface. Specularity is dependent on the position of the light source and the position of the viewer. Shininess. Controls the reflectivity of the light.
Emissivity. Controls the intensity of radiated light.
Configurations • • •
This configuration All configurations Specify configuration
Materials Editor PropertyManager You can create parts from a specific material with the Materials Editor PropertyManager. The material and its properties propagate to COSMOSWorks, COSMOSXpress, PhotoWorks release 2, mass properties and material properties. The Material icon to a part.
appears in the FeatureManager design tree regardless of whether you applied a material
The Materials Editor PropertyManager controls: Materials •
Select a Material Database. Displays pre-defined material libraries included with the SolidWorks software, or displays custom material libraries.
•
Remove Material. Deletes the material from the model.
•
Create/Edit Material. Creates a new material or edits an existing material.
Visual Properties •
Advanced graphics. Allows you to display the model in RealView or Standard graphics.
•
RealView. Applies a 3D material to the model that dynamically changes when you rotate the model. RealView display applies only if you have a supported graphics card.
•
Standard. Applies a 2D texture to the model. You can control the: o
Scale
. Adjusts the grain of the texture.
o
Angle
o
Blend color. Blends the part color with the texture color.
. Adjusts the rotation of the texture.
•
Use material color. Applies the color shown to the model. This option is not available with all materials.
•
Use material crosshatch. Applies the crosshatch pattern assigned to the material when used as a section view in a drawing.
Physical Properties Displays the physical properties associated with the selected material.
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Texture PropertyManager Apply textures to geometric entities in a model. The Texture PropertyManager controls: Selection •
•
Selection filters. Helps you select geometric entities in the model. The available selection filters are: o
Select Faces
o
Select Features
o
Select Surfaces
o
Select Components
o
Select Bodies
o
Select Parts
(assemblies only)
(assemblies only)
Remove Textures. Deletes the texture from the selected entity.
Texture Selection •
Texture File Locations. Displays pre-defined texture libraries included with the SolidWorks software, or displays custom texture libraries.
•
Texture Tree. Displays 2D texture files.
•
Last 10 Used Textures. Displays the last 10 textures you used.
Texture Properties •
Texture Preview. Displays a preview image of the selected texture.
•
Scale
•
Angle
•
Blend color. Blends the part color with the texture color.
. Adjusts the grain of the texture. . Adjusts the rotation of the texture.
Configurations •
This configuration
•
All configurations
•
Specify configuration
Show Web Toolbar Displays or hides the Web toolbar. To access the Web toolbar when it is hidden:
•
Click Web Toolbar
on the Standard toolbar to display the Web icons.
•
Click Web Toolbar
again to hide the Web toolbar when it is not needed.
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Standard Views Toolbar The Standard Views toolbar provides tools to rotate the model, assembly, or sketch to one of the preset standard views. Front Back Left Right Top Bottom Isometric Trimetric Dimetric Normal To -- a view that is perpendicular to the selected plane or planar face
Surfaces Toolbar The Surfaces toolbar provides tools for creating and modifying surfaces. Extruded Surface Revolved Surface Swept Surface Lofted Surface Offset Surface Radiate Surface Knit Surface Planar Surface Extended Surface Trimmed Surface Filled Surface Mid-Surface Replace Face Delete Face Untrim Surface
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Tools Toolbar The Tools toolbar provides tools for measuring and defining the mass properties of models and for creating equations. Measure Equations Mass Properties Design Table Feature Statistics Deviation Analysis COSMOSXpress. Click Tools, COSMOSXpress.
View Toolbar The View toolbar controls: View Orientation
Hidden Lines Removed
Previous View
Shaded With Edges
Zoom to Fit
Shaded
Zoom to Area
Draft Quality HLR/HLV
Zoom In/Out
Perspective
Zoom to Selection
Shadows In Shaded Mode
Rotate View
Section View
Pan
Curvature
Wireframe
Zebra Stripes
Hidden Lines Visible
RealView Graphics
Web Toolbar The Web toolbar provides support for working over the Internet. Stop Current Jump Reload\Replace Insert Hyperlink Open Internet Address Stop Current Jump Stops the jump that you are attempting. To stop the current local or Internet jump:
Click Stop Current Jump
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Reload Documents Allows you to Reload documents. This is useful if you have read-only access to a document and you want to reload the latest version with any changes made by a colleague. To reload a document:
1.
Click File, Reload in a part or assembly document, or right-click a component in an assembly and select Reload.
2.
Select Open as read-only if you do not want to save any changes to the file. NOTE: If you have write-access to a sub-assembly then you reload it as read-only, you still have writeaccess to the individual components of the sub-assembly. You must reload each of the sub-assembly components as read-only to relinquish write-access privileges.
3.
Click OK. See also Replace Components.
Insert Hyperlink Creates a hyperlink to a document on the Internet, your local network, or on your own hard drive. When you select a hyperlink, the associated document or Web site opens. To create an embedded hyperlink:
1.
Click Insert Hyperlink
on the Web toolbar, or click Insert, Hyperlink.
The Insert Hyperlink dialog box appears. 2.
Type the path in the Link to file or URL box, or click Browse and browse to the document to which you want to link. The path appears in the Path box.
3.
Select the Use relative path for hyperlink check box if you want to specify a directory path relative to the current location instead of the full path.
4.
Click OK to accept the path. The path appears in the graphics area.
To delete an embedded hyperlink:
Click the hyperlink path, then press Delete. Open Internet Address Allows you to specify a Web site or document to view. If the specified path is to a local SolidWorks document, it opens in the SolidWorks application. Other documents and Web sites open in your Internet browser. To open an Internet link:
1.
Click Open Internet Address
on the Web toolbar.
The Open Internet Address dialog box appears.
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2.
Type the address of the document, folder, or computer on the Internet, or click the Browse button and browse to the document or location that you want.
3.
Click OK to continue to open the Internet address; click Cancel to end the operation and close the dialog box.
Weldments Toolbar The Weldments toolbar provides tools for creating weldment parts. Weldment Structural Member Gusset End Cap Fillet Bead Trim/Extend
FeatureManager Design Tree FeatureManager Design Tree The FeatureManager design tree on the left side of the SolidWorks window provides an outline view of the active part, assembly, or drawing. This makes it easy to see how the model or assembly was constructed or to examine the various sheets and views in a drawing. The FeatureManager design tree and the graphics area are dynamically linked. You can select features, sketches, drawing views, and construction geometry in either pane. You can split the FeatureManager design tree and either display two FeatureManager instances, or combine the FeatureManager design tree with the ConfigurationManager or PropertyManager. The FeatureManager design tree makes it easy to: •
Select items in the model by name.
•
Identify and change the order in which features are created. You can drag and drop items in the FeatureManager design tree list to reorder them. This changes the order in which features are regenerated when the model is rebuilt.
•
Display the dimensions of a feature by double-clicking the feature’s name.
•
Rename items by slowly clicking two times on a name to select it and then entering a new name.
•
Suppress and Unsuppress part features and assembly components.
•
View parent/child relations by right-clicking a feature in the list, then selecting Parent/Child.
•
Display the following items: o
Feature descriptions
o
Component descriptions
o
Component configuration names
o
Component configuration descriptions
The FeatureManager design tree provides the following folders and tools: •
Use the rollback bar to temporarily roll the model back to an earlier state.
•
, and selecting Add a new equation, edit, or delete an equation by right-clicking the Equations folder the action you want. (The Equations folder appears when you add the first equation to a part or assembly.)
•
Control the display of dimensions and annotations by right-clicking the Annotations folder
•
Add or modify a material applied to a part by right-clicking the Material icon
•
Add or modify light sources in the Lighting folder
•
View all solid bodies that the document contains in the Solid Bodies folder
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.
. .
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•
View all surface bodies that the document contains in the Surface Bodies folder
.
•
Add your own custom folders, and drag features into the folders to reduce the length of the FeatureManager design tree.
•
Move between the FeatureManager design tree, the PropertyManager, the ConfigurationManager, and Add-In tabs by selecting the tabs at the top of the left pane.
Show Feature's Description In part, assembly, and drawing documents, you can display feature descriptions in the FeatureManager design tree. To show feature descriptions:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Feature’s Description. The FeatureManager design tree displays the feature descriptions. By default, feature names and feature descriptions are the same. You must specify a new feature description in order for it to appear in the FeatureManager design tree. •
•
To change a feature description in a part or assembly, rightclick the feature, select Properties, and type a new Description. To change a feature description in a drawing, you must change the feature description in the part or assembly file.
Feature descriptions
Show Component's Description In part, assembly, and drawing documents, you can display component descriptions in the FeatureManager design tree. Component descriptions can also be displayed in the ConfigurationManager of parts and assemblies. To show component descriptions:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Components’s Description. The FeatureManager design tree displays the component descriptions. NOTES: •
•
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By default, component names and component descriptions are the same. You must specify a new component description in the component part file so it appears in the FeatureManager design tree. Component descriptions appear only if you selected Description in Custom property used as custom description in the General system options. You can select a different item for Custom property used as custom description, but you must set a value for that custom property on the Custom tab of the Summary Information dialog box.
Component description
Show Component's Configuration Name In part, assembly, and drawing documents, you can display component configuration names in the FeatureManager design tree. To show component configuration names:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Components’s Configuration Name. The FeatureManager design tree displays the component configuration names.
Component configuration name Show Component's Configuration Description In part, assembly, and drawing documents, you can display component configuration descriptions in the FeatureManager design tree. Component configuration descriptions can also be displayed in the ConfigurationManager of parts and assemblies. To show component configuration descriptions:
At the top of the FeatureManager design tree, right-click the part, assembly, or drawing name, and select Tree Display, Show Components’s Configuration Description. The FeatureManager design tree displays the component configuration descriptions. By default, component configuration names and component configuration descriptions are the same. You must specify new component configuration descriptions so they appear in the FeatureManager design tree. You change a component configuration description in the part file.
Component configuration description
Show Configuration's Description In part or assembly documents, you can display configuration descriptions in the ConfigurationManager. By default, configuration names and descriptions are the same. You must specify new configuration descriptions so they appear in the ConfigurationManager. To change a configuration’s description, right-click the configuration in the ConfigurationManager, select Properties, and type a new Description. To show configuration descriptions:
In the ConfigurationManager, right-click the part or assembly name at the top of the tree, and select Tree Display, Show Configuration’s Description. The ConfigurationManager displays the configuration descriptions.
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Chapter 2 SolidWorks Fundamentals
FeatureManager Design Tree Conventions The FeatureManager design tree uses the following conventions: •
A
symbol to the left of an item’s icon indicates that it contains associated items, such as sketches. Click to expand the item and display its contents.
To collapse all expanded items at once, right-click the document name at the top of the tree, and select Collapse Items. •
Sketches in the FeatureManager design tree are preceded by (+) if they are over defined; they are preceded by (–) if they are under defined; they are preceded by (?) if the sketch could not be solved. (There is no prefix if the sketch is fully defined.)
•
Features are preceded by the rebuild symbol part.
•
Assembly components in the FeatureManager design tree are preceded by (+) if their position is over defined; they are preceded by (–) if their position is under defined; they are preceded by (?) if their position could not be solved; they are preceded by (f) if their position is fixed (locked in place).
•
Assembly mates are preceded by (+) if they are involved in over defining the position of components in the assembly; they are preceded by (?) if they could not be solved.
•
In an assembly, each instance of the component is followed by a number in angle brackets
•
The state of external references is displayed in the FeatureManager design tree, as follows: o
o
if a change has been made that requires the rebuild of the
If a part or feature has an external reference, its name is followed by –>. The name of any feature with external references is also followed by –>. If an external reference is currently out of context, the feature name and the part name are followed by ->?
o
The suffix ->* means that the reference is locked.
o
The suffix ->x means that the reference is broken.
Parent/Child Relationships Displays the parents and children of a selected feature, sketch, axis, plane, curve, or surface. A parent feature is an existing feature upon which others depend. For example, an extrude is the parent feature to a fillet that rounds its edges. When new features are built upon other features, their existence depends upon the previously-built feature. The new feature is called a child feature. For example, a hole is the child of the solid in which it is cut. To display parent/child relationships:
1.
In the model or in the FeatureManager design tree, right-click the item whose parent/child relationship you want to display.
2.
Select Parent/Child from the menu. The dialog box shows the Parents and Children of the selected feature.
3.
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In this dialog box, you can: •
Right-click an item in the Parents or Children list, and select an option from the shortcut menu, such as Edit Sketch or Edit Feature.
•
Expand features to see additional parent/child relationships.
•
Resize the dialog box to see all of the items listed.
Rollback Bar Temporarily reverts the model to an earlier state, suppressing recently added features. You can add new features or edit existing features while the model is in the rolled-back state. You can use the rollback bar to roll back to absorbed features, roll forward, roll to previous, or roll to the end of models. You can roll back a part with the Rollback Bar in the FeatureManager design tree. The rollback bar is a yellow and black line which turns blue when selected. Drag the bar up or down the FeatureManager design tree to step forward or backward through the regeneration sequence.
You can also use the shortcut menu to roll a model back to an earlier state. Right-click any feature in the FeatureManager design tree and select Rollback. To revert a part to an earlier state:
1.
Place the pointer over the rollback bar in the FeatureManager design tree. The pointer changes to
2.
.
Click the rollback bar. The bar changes color from yellow and black to blue.
3.
Drag the rollback bar up the FeatureManager design tree until it is above the feature(s) you want rolled back. - or Click the rollback bar and use the up and down arrow keys on the keyboard to move the rollback bar up or down. To enable this use of the arrow keys, click Tools, Options, System Options, FeatureManager, and select Arrow key navigation.
4.
To roll forward again, drag the rollback bar to the bottom of the FeatureManager design tree. Icons in the FeatureManager design tree are gray and unavailable when they are rolled back.
To roll back to absorbed features:
1.
In the FeatureManager design tree, click the
to expand the absorbed features within the parent feature.
2.
Right-click an absorbed feature, and select Rollback. A message appears that tells you the absorbed feature will be temporarily unabsorbed for editing purposes.
3.
Click OK.
4.
Drag the rollback bar below the feature you selected in step 2. The feature is unabsorbed and ready for editing.
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To roll a model forward:
1.
Roll the model back to an earlier state in the FeatureManager design tree.
2.
Right-click a rolled back feature in the FeatureManager design tree, and select Roll Forward. The model rolls forward to the selected feature.
To roll a model to its previous state:
1.
Roll the model back to an earlier state in the FeatureManager design tree.
2.
Right-click any feature in the FeatureManager design tree, and select Roll to Previous. The model rolls back to its previous state.
To roll to the end of a model:
1.
Roll the model back to an earlier state in the FeatureManager design tree.
2.
Right-click a rolled back feature in the FeatureManager design tree, and select Roll to End. The model rolls to its original state.
Split Panel Display You can display a split instance of the panel adjacent to the graphics area, usually the FeatureManager design tree. A split display is not limited to duplicate FeatureManager design trees. You can select any combination of the following: •
FeatureManager design tree
•
PropertyManager
•
ConfigurationManager
•
Third party applications that use the panel
This option is available either alone or in conjunction with Window, New Window. Without opening a new window, you can display the same part, assembly or drawing, along with any combination of the panels. With complex designs, for example, you can: •
Display different sections of the part, drawing, or assembly, expanded or collapsed
•
View different details for configurations
•
Pick different selections from each panel
To split the FeatureManager design tree:
1.
Place the pointer at the top of the FeatureManager design tree until it changes to
.
2.
Drag the bar down below the last item in the FeatureManager design tree.
3.
Release the mouse to display a duplicate FeatureManager design tree, below the first. Each instance of the FeatureManager design tree panel displays a set of tabs.
4.
Select the tabs that are appropriate for the panels that you want to display: PropertyManager, ConfigurationManager, FeatureManager design tree, or the panel of a third party application.
To close the split FeatureManager design tree:
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1.
Place the pointer at the top of the duplicate FeatureManager design tree until it changes to
2.
Drag the bar up until it meets the top of the original FeatureManager design tree.
3.
Release the mouse to close the display of the duplicate FeatureManager design tree.
.
Flyout FeatureManager Design Tree The flyout FeatureManager design tree allows you to view both the FeatureManager design tree and the PropertyManager at the same time. The flyout FeatureManager design tree automatically appears when a PropertyManager is active. To expand the flyout FeatureManager design tree, you can: •
Click
next to the document name in the flyout FeatureManager design tree
•
Click the PropertyManager title
The flyout FeatureManager design tree is transparent so you can see the model underneath it.
PropertyManager (left) and flyout FeatureManager design tree (right)
FeatureManager Options Lets you set the default system options related to the FeatureManager design tree. To set the default FeatureManager design tree options:
1.
Click Tools, Options.
2.
On the System Options tab, click FeatureManager.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
FeatureManager Options •
Scroll selected item into view. Specifies that the FeatureManager design tree should automatically scroll to display the feature icon that is related to the selected items in the graphics area. If you have a very complex part or assembly, you may want to turn this option off. Then, when you want the FeatureManager design tree to scroll to a feature you can right-click the feature and select Go To Feature (in Tree).
•
Name feature on creation. When you create a new feature, the feature name in the FeatureManager design tree is automatically selected and ready for you to enter a name of your choice.
•
Arrow key navigation. Lets you use the arrow keys to traverse the FeatureManager design tree, and expand or collapse the design tree and its contents, as follows o
Up arrow - Scrolls up the design tree
o
Down arrow - Scrolls down the design tree
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•
o
Left arrow at top of design tree - Collapses the design tree
o
Right arrow at top of design tree - Expands the design tree
o
Left arrow on an item in the tree - Collapses the item to hide its contents
o
Right arrow on an item in the tree - Expands the item to display its contents, if any
Dynamic highlight. Specifies that the geometry in the graphics area (edges, faces, planes, axes, and so on) is highlighted when the pointer passes over the item in the FeatureManager design tree.
Selecting from the FeatureManager Design Tree There are several ways to select items directly from the FeatureManager design tree. •
Select features, sketches, planes, and axes in the model by clicking their names in the FeatureManager design tree.
•
Select multiple consecutive items in the FeatureManager design tree by holding the Shift key while you select. Click the first item, hold down Shift, and click the last item.
•
Select multiple items in the graphics area, or select non-consecutive items in the FeatureManager design tree by holding the Ctrl key while you select.
•
Perform a text search of the FeatureManager design tree by right-clicking an item in the FeatureManager design tree (except Material or Lighting) and selecting Go To.
Find in FeatureManager Design Tree Lets you do a text search of the FeatureManager design tree for an item. To search the FeatureManager design tree:
1.
Right-click the name of the part, assembly, or drawing at the top of the FeatureManager design tree, and select Go To. - or Right-click the name of a part, feature, sketch, plane, or assembly in the FeatureManager design tree, and select Go To. The Find In FeatureManager Design Tree dialog box appears.
2.
Enter the name of the item (or a part of the name) in the Find what box.
3.
Click Find Next.
4.
Continue to click Find Next until the name of item you are searching for scrolls into view. By default, the tree is searched from the top to the bottom. If you want to reverse the search direction, clear the Start from the top check box.
Add Folders In part or assembly documents, you can add folders to the FeatureManager design tree. You can rename new folders and drag additional features into the new folders. This reduces the length of the FeatureManager design tree. When you select a folder that you added in the FeatureManager design tree, the features in the folder are highlighted in the graphics area. Similarly, when you select a feature in the graphics area that is in a folder you created, the folder is highlighted and expands to show the highlighted feature in the FeatureManager design tree. You can insert features into folders by one of two ways: automatically or manually. You can place any set of continuous features or components into an individual folder. You cannot use Ctrl to select non-continuous features. This maintains parent-child relationships. You cannot add new folders to existing folders.
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To create a new folder and insert features automatically:
In the FeatureManager design tree, right-click a feature and select Add to New Folder. A new folder appears in the FeatureManager design tree. The feature you right-clicked is now in the new folder. You can rename the folder and drag additional features into the folder. To create a new folder and insert features manually:
In the FeatureManager design tree, right-click a feature and select Create New Folder. A new folder appears in the FeatureManager design tree. You can rename the folder and drag additional features into the folder. When you manually drag a feature onto a folder name, the pointer changes to
.
To remove features from a folder:
1.
In the FeatureManager design tree, drag the feature from the folder onto the folder icon The pointer changes to
2.
.
.
Release the mouse button. The feature is removed from the folder, and appears just below the folder.
Opening New and Existing Documents in SolidWorks New SolidWorks Document Creates a new document. New documents use templates as the basis for their format and properties. Templates include user-defined parameters, such as units of measure or other detailing standards. Templates allow you to maintain as many different styles of documents for parts, drawings, or assemblies as you need. A document template can be a part, drawing, or assembly that you saved as a template. To create a new SolidWorks document:
1.
Click New on the Standard toolbar, click File, New, or click New Document in the Welcome to SolidWorks 2004 dialog box.
2.
The New SolidWorks Document dialog box has two versions. Click the appropriate button for the version you want to access: •
Novice. Uses a simpler version of the dialog box, which provides explanations of part, assembly, and drawing documents. If you have the Online Tutorial active, then open a new document, a tutorial template opens. The tutorial template uses the appropriate units, view orientations, and so on, for the tutorial lessons.
•
Advanced. Uses a modified version of the dialog box that shows template icons on various tabs. When you select a document type, a preview of the template appears in the Preview box. In the Advanced version, you can: o
Add your own tabs for storing templates.
o
Click the tutorial tab to access the tutorial template.
o
Click Large Icons
o
Click List
o
to display items with large icons.
to display items with small icons.
Click List Details to display information about each item in the window, including columns for file size and date modified.
3.
Click the type of document you want to open.
4.
Click OK.
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Default Templates You can specify the folder and template file for automatically created parts, assemblies, and drawings. For example, when you import a file from another application or create a derived part, the default template is used for the new document. To specify a folder for document templates:
1.
Click Tools, Options.
2.
On the System Options tab, click Default Templates. The current path and folder for part, assembly, and drawing templates appears.
3.
To change the folder for one of the template types, click the browse button window.
next to the path display
In the New SolidWorks Document dialog box, select the new default template, then click OK. If you need to add a template that does not appear in this dialog box, add the template location with the File Locations option. 4.
5.
Select one of the following options: •
Always use these default document templates
•
Prompt user to select document template
Click OK.
Creating Additional Template Tabs When you open a new SolidWorks document, you select a template for that document from a tab in the advanced version of the New SolidWorks Document dialog box. Initially, all the documents are listed on the same tab, but you can create additional custom tabs on which you can organize your templates. Custom tabs help manage your templates in the following ways: •
Placement - Create folders on any drive, including hard drives, floppy drives, or network drives.
•
Access - Share the contents of network folders, or restrict access to folders if required.
•
Organization - Arrange folder contents to reflect your work environment.
To create a new tab on the advanced version of the New SolidWorks Document dialog box:
1.
In Windows Explorer, create a new folder in the location that you want. For example, you could put a set of templates that you designed in a special folder called:
2.
In the SolidWorks software, click Tools, Options, System Options, File Locations.
3.
Select Document Templates in Show folders for.
4.
Click Add and browse in the Browse For Folder dialog box to find the location of the folder you created in step 1.
5.
Click OK.
6.
Click OK again to close the System Options - File Locations dialog box.
7.
Create a new template and, using Save As, browse to the folder you created in step 1 and name the new template. After you save a template to the new folder, a new tab appears in the advanced version of the New SolidWorks Document dialog box that is named after the folder you specified.
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Setting Default Material Properties You can set the following default material properties for your part or assembly document templates: •
Ambient. How light is reflected and scattered by other objects
•
Diffuse. How light is scattered equally in all directions on the surface
•
Specularity. How surfaces exhibit highlights
•
Shininess. How solid objects alternate between a glossy, reflective surface and a dull, matte surface
•
Transparency. How much light passes through the surface
•
Emission. How light projects from the surface
To set the default material properties for a document template:
1.
Click File, New. The New SolidWorks Document dialog box appears with an available set of templates.
2.
Double-click the part or assembly icon for the type of template that you want to create.
3.
Click Tools, Options, and on the Document Properties tab, click Colors. NOTE: Only options on the Document Properties tab are saved in a document template.
4.
In the Model\Feature colors list, select Shading, then click Advanced. The Advanced Properties dialog box appears.
5.
Set the material properties as desired, then click OK.
6.
Click OK to close the Document Properties - Colors box.
7.
Click File, Save As. The Save As dialog box appears.
8.
9.
In the Save as type list, select a template type: •
Part Templates (*.prtdot)
•
Assembly Templates (*.asmdot)
Type a name in the File name box. The extension is added automatically.
10. Browse to the folder where you want to save your template, then click Save.
Open Opens an existing part, drawing, or assembly document. Also used to import files from other applications. To open an existing part, assembly, or drawing document:
1.
Click Open
on the Standard toolbar, click File, Open, or press Ctrl+O.
2.
In the dialog box, select a file type in Files of type.
3.
Browse to select the part, drawing, or assembly document, or the file from another application that you want to open. NOTES: •
The Description label displays a description if you added one to the model.
•
Use the locations sidebar to help navigate to the location where you want to open your document. The locations sidebar is available in certain operating systems only.
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4.
Select from the following options, if necessary: •
Down arrow o
o
•
(Next to the Open button):
Open as Read-Only. Allows another user to have write access to the document while you have the document open. You cannot save or change the part in Read-Only mode. Add to Favorites. Creates a shortcut to the selected document in your Favorites folder.
Preview. Displays a preview of the SolidWorks part, assembly, or drawing document in the dialog box without opening it. Select a configuration name in Configurations to see a preview of the specified model configuration. If the Preview box does not display the configuration preview, open the document, then open each configuration, and save the document. The next time you open the document, the Preview box shows the selected preview.
5.
•
Advanced. Opens the Configure Document dialog box (assemblies only).
•
View-Only. Opens the part document only for viewing. (Only documents saved in SolidWorks 98 or later may be opened in View-Only mode.) If you are in a part or assembly document, you can change to edit mode by right-clicking in the graphics area and selecting Edit.
•
Lightweight. Opens the assembly or drawing document with lightweight parts.
•
References. Displays a list of the documents referenced by the currently selected assembly or drawing. You can edit the locations of the listed files.
Click Open to open the document, or double-click the configuration name under Configurations to open a specified configuration of the document. If you are opening files from a previous release of SolidWorks, the file may open more slowly than you would like. The Conversion Wizard converts the files so they open more rapidly.
Opening Documents from Part or Assembly Windows While you are editing an assembly, you can open its associated component documents (parts or sub-assemblies) in their own windows. Any changes that you make to the components automatically update the assembly. While you are editing a part with in-context features, you can open the assembly document where the features were created. To open a component from an assembly document:
1.
In the assembly window, right-click a component.
2.
Select Open part or Open Assembly. The component document opens in a separate window.
To open an assembly from a part document:
1.
In the part window, right-click a feature or sketch in the FeatureManager design tree or graphics area that has an external reference.
2.
Select Edit In Context. The assembly that contains the update path for the selected feature opens in a separate window.
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Multi-Threaded Retrieval Documents saved in recent SolidWorks releases are retrieved in multi-threaded mode. (Documents saved in releases prior to SolidWorks 98 cannot be retrieved in multi-threaded mode.) When you retrieve a large part, drawing, or assembly document, the document immediately displays in a view-only state while the actual document and all its components are retrieved in the background. During the view-only state, you can use all functions supported in the SolidWorks Viewer (Zoom, Rotate, and so on), but you cannot switch to another document or start to open another document. After the retrieval is complete, SolidWorks changes to the normal edit state.
SolidWorks Documents in Windows Explorer Use Windows Explorer to see thumbnail images and to access custom property information for SolidWorks documents. To see thumbnail images of SolidWorks documents in Windows Explorer:
Thumbnail images are available only if you use Windows XP, Windows 2000, or Windows Server 2003. 1.
In Windows Explorer, open a folder that contains SolidWorks documents.
2.
Click View, Thumbnails. A thumbnail image of each SolidWorks document in the folder is displayed. If you set up Windows Explorer to show preview images, a preview of the SolidWorks document also appears when the document is selected. You can also view thumbnail icons of SolidWorks parts and assemblies in Windows Explorer. The icon is based on the view orientation of the model when the document was last saved. To enable this functionality, click Tools, Options, System Options, General, and select Show thumbnail graphics in Windows Explorer. You may need to restart SolidWorks and Windows Explorer to see the thumbnail icons in these applications.
To preview a part, drawing, or assembly from Windows Explorer (Windows NT only):
Right-click the name of the part, drawing, or assembly in Windows Explorer, and select Quick View. To access custom property information for SolidWorks documents in Windows Explorer:
If you save custom property information in the Summary Information dialog box, the following properties appear in Windows Explorer: • Description •
Revision
•
Status
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Additionally, Type, Size, Last Saved By and Number of sheets are shown automatically. You cannot save this information in the Summary Information dialog box. 1.
In Windows Explorer, open a folder that contains SolidWorks documents.
2.
Move the pointer over a SolidWorks document. The custom property information is displayed.
To open a SolidWorks document from Windows Explorer:
In Windows Explorer, do one of the following: •
Double-click the name of the SolidWorks document.
•
Right-click the name of the SolidWorks document and select Open.
•
Drag and drop the SolidWorks document (or any document supported by the SolidWorks software) into an empty area of the SolidWorks window, not occupied by another document window.
Drag and Drop Files to a SolidWorks Document •
Drag and drop a part or assembly from Windows Explorer to an open SolidWorks assembly window to add an instance of the part or sub-assembly to the assembly.
•
Drag and drop a part or assembly from Windows Explorer to an open and empty SolidWorks drawing document to create a Standard 3 View drawing of the part or assembly.
•
Drag and drop a zipped (.zip) file into an empty SolidWorks window, or an empty area of an open SolidWorks document. The SolidWorks software opens the zipped files based on where you drop the zipped file. For example, if you drag and drop a .zip file that contains several models into an empty SolidWorks window, each model opens in its own window. The .zip file can contain any file type supported by the SolidWorks software. If the .zip file contains several SolidWorks files and an imported file, such as a .igs file, the .igs file opens in a separate window. NOTES: o
•
If the .zip file contains models that are not on your local computer (if you dragged the .zip file from the Internet), the Browse For Folder dialog box appears for you to download the .zip file to a location on your local computer.
Drag and drop hyperlinked SolidWorks part files from Internet Explorer, version 4.0 or later, to: o
the Feature Palette window
o
a new, empty part document
o
an empty area of a SolidWorks window
o
a drawing or assembly document
If you drop the file into a drawing or an assembly, you are prompted to name the new file on your local disk.
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•
Drag and drop between open documents. Drag a part name from the FeatureManager design tree of an open part file to insert it into an open assembly document.
•
Drag a part or assembly name from the FeatureManager design tree to a drawing document.
Web Folders Overview Web Folders Overview Web Folders is a SolidWorks tool that allows multiple users to share and work on SolidWorks part, assembly, or drawing documents, as well as other file formats, across the Internet. A Web Folder is a shortcut to a web server. Creating a Web Folder You need to create a Web Folder on a web server. Contact your system administrator for assistance. Using Web Folders Requirements: •
The web server must support Web Folders. Check with your system administrator or Internet service provider to see whether your web server supports Web Folders.
•
You must have Microsoft Internet Explorer version 5.0 or greater installed on your computer. If you are installing Internet Explorer, choose the Customize option and then select Web Folders under Web Authoring Components. If Internet Explorer is already installed, contact your system administration for assistance in adding Web Folders.
Accessing Web Folders For users to access a Web Folder you create on a web server, they must have an account on the web server. There are two options for allowing others to access your Web Folder: •
Users have an account on the server.
•
The user's account has the permission to access your Web Folder. Contact your system administrator for information on sharing a Web Folder with other users.
For users to be able to open and edit a SolidWorks document you place on a Web Folder: •
They must have access to the Web Folder.
•
They must have the SolidWorks software installed. If they do not have the SolidWorks software, they can view the SolidWorks document with SolidWorks Explorer.
Web Folder Security Your system administrator determines the Web Folder security policy when they set up access for other users. Contact your system administrator for security information.
Web Folders - Saving and Opening Files You can save a file to a web folder, or open a file from a web folder. To save a file to a web folder:
1.
Create a web folder on a computer with a web server. See your systems administrator to help you set up a web folder on a server.
2.
In SolidWorks, open the file that you want to save to the web folder.
3.
Click File, Save To Web Folder. The Save To Web Folder dialog box appears. The file name of the open file appears in the File name box.
4.
Click the arrow
in the URL box, and select the URL of the web folder on the server.
NOTE: If the web server requires a password, the Enter Network Password dialog box appears. Enter the User Name and Password, then click OK. The web folder opens, and the default folders are displayed. 5.
Double-click the web folder where you want to save the file.
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6.
Click Save. •
If you are saving a part or drawing document, it is saved to the web folder.
•
If you are saving an assembly document, the Copy Referenced Files To Server dialog box appears. Set the desired options, then click OK to save the referenced files to the web folder.
NOTE: When working with part and assembly documents, certain SolidWorks operations generate a Save As dialog box. You cannot save a document to a web folder from the Save As dialog box. To open a file from a web folder:
1.
Click File, Open From Web Folder. The Open From Web Folder dialog box appears.
2.
Click the arrow
in the URL box, and select the URL of the web folder on the server.
If the web server requires a password, the Enter Network Password dialog box appears. Enter the User Name and Password, then click OK. The web folder opens, and the default folders are displayed. 3.
Double-click the web folder that contains the file. All files in that folder appear in the dialog box window.
4.
Select the desired file and click Open. The file opens in SolidWorks.
Change URL With the Change URL dialog box, you can change where on the web server you save referenced files. To change where on the web server you save referenced files:
1.
In the Copy Referenced Files To Server dialog box, select one or more of the files in the Current Reference list.
2.
Click Change URL. The Change URL dialog box appears.
3.
Under New Location, type the new URL location where you want to save the referenced files.
4.
Click OK in the Change URL dialog box.
5.
Click OK in the Copy Referenced Files To Server dialog box. The referenced files are copied to the new URL location.
Copy Referenced Files to Server An assembly document references files called components. Use this dialog box to copy these referenced files to a web folder on a server. To copy referenced files to a web folder:
1.
Open a SolidWorks assembly document.
2.
Click File, Save To Web Folder. The Save To Web Folder dialog box appears. The file name of the open file appears in the File name box.
3.
Click the arrow
in the URL box, and select the web folder where you want to save the files.
If the web server requires a password, the Enter Network Password dialog box appears. If it does not require a password, go to step 5. 4.
Type the User Name and Password, then click OK. The web folder opens, and the default folders are displayed.
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5.
Double-click the web folder where you want to save the file.
6.
Click Save. The Copy Referenced Files To Server dialog box appears with the following information:
7.
•
Current Reference. The current path to the assembly components.
•
Copy the referenced files to. The new path to the web folder where you want to copy the assembly component.
•
Retain Folder Structure check box. Select to retain the same folder structure in the web folder as shown under the Current Reference list.
The following buttons are available: •
Select All. Click to select all files listed under Current Reference. Selected files show a check mark next to them. Only selected files are copied to the web folder.
•
Deselect All. Click to clear all selected files listed under Current Reference.
•
Change URL. Click to display the Change URL dialog box, which is used to change the location of referenced files that you are saving to a web folder. NOTE: At least one file under Current Reference must be selected to use the Change URL dialog box.
8.
Click OK. The referenced files are saved to the web folder.
Selection Highlighting Selected Items Items that you select are highlighted in a solid style font.
Edges that you select highlight as thick solid lines.
Edges of faces that you select highlight as thin solid lines.
To set the selected items highlighting color:
1.
Click Tools, Options, System Options Colors.
2.
Click Selected Item 1 in System colors, then click Edit.
3.
Select a color from the Color palette or click Define Custom Colors and define a new color, then click OK.
4.
Click OK again to close the System Options - Colors dialog box.
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To set the highlight color for faces that you select while in Shaded With Edges or Shaded view mode:
In Shaded With Edges select.
or Shaded
view modes, you can control the color used to highlight faces that you
1.
Click Tools, Options, System Options, Colors.
2.
Click Selected Item 1 in System colors, then click Edit.
3.
Select a color from the Color palette or click Define Custom Colors and define a new color, then click OK.
4.
Click OK again to close the System Options - Colors dialog box. To turn this option off, click Tools, Options, System Options, General, and clear Use shaded face highlighting. Selected faces in Shaded With Edges and Shaded view modes are then highlighted as thin lines.
Dynamic Highlighting When you move the pointer over an edge or a face, edges highlight as thick solid lines; edges of faces highlight as thin solid lines. This is the same highlighting functionality as for selected items. In drawings, edges dynamically highlight as thin phantom lines and edges of faces dynamically highlight as thin dashed lines. Dynamic highlighting is turned on as the default. To turn off dynamic highlighting, click Tools, Options, System Options, Display/Selection and clear Dynamic highlight from graphics view. To set the dynamic highlighting color:
1.
Click Tools, Options, System Options, Colors.
2.
Click Selected Item 1 in System colors, then click Edit.
3.
Select a color from the Color palette or click Define Custom Colors and define a new color, then click OK.
4.
Click OK again to close the System Options - Colors dialog box.
Select Select Select to:
lets you select sketch entities when you are working in a sketch. In a sketch or drawing document, use
•
select sketch entities
•
drag sketch entities or endpoints to reshape the sketch
•
select a model edge or face
•
drag a selection box around multiple sketch entities
•
select a dimension to drag to a new location
•
double-click a dimension that you want to modify
To select items:
1.
Click Select
or Tools, Select.
2.
Click the item that you want to select. Notice that items change color as the pointer passes over them. This dynamic highlighting helps you locate the item to select.
To select multiple items:
Hold down the Ctrl key while you click the items that you want to select.
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To box-select:
Depending on the type of document you are in, you can drag a selection rectangle around the items you want to select. All items that are completely inside the selection rectangle are selected. The following table shows which items are selected when you box-select in a specified document: Document
Item selected
Parts
edges
Assemblies
components
Drawings
annotations
Select Partial Loop Imported models can contain many small edges. To repair or edit imported models, you often need to select a series of connecting edges. When surfaces or solids contain small edges, use Select Partial Loop to choose a chain of connecting edges. The chain direction is based on the relative position of the second open edge that you select: •
Left of midpoint. Chain moves left.
•
Right of midpoint. Chain moves right.
The chain always includes the first edge you first selected. To use Select Partial Loop with solid bodies, the selected edges must be on the same face. To select a partial loop:
Loop direction, with edge 1 and edge 2
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1.
Select the first edge in the chain.
2.
Press Ctrl select the second edge, and do either of the following: •
Position the pointer left of the midpoint to create a chain that moves left.
•
Position the pointer right of the midpoint to create a chain that moves right.
Right of midpoint selected 3.
Right-click and choose Select Partial Loop.
Select Chain You can select a chain of entities attached to the selected entity in both directions until a branch is encountered. To select a chain of sketch entities:
Right-click a sketch entity and choose Select Chain. The entities of sketch geometry such as rectangles and polygons are selected. If the geometry includes branches, the chain stops at the branch. You can continue the selection manually. You can hold Ctrl and select multiple chains.
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Select Other Selects items that are hidden by other items. To select hidden items:
1.
Point at the item you want to select and right-click.
2.
Click Select Other. The pointer changes to
3.
.
Click the right mouse button to step through the items that lie under the point where you clicked. Click the left mouse button when the desired item is highlighted.
Midpoint Selection You can select the midpoint of an entity to create other entities such as planes or axes. To select a midpoint:
Right-click an edge, then click Select Midpoint. The midpoint appears as a circle on the edge.
Selection Filter Use a Selection Filter to help you select specific items in the graphics area or the drawing sheet area. For example, you can set a Selection Filter to filter only model faces. When you select items in the model, only faces can be selected. Selection Filters make it easy to identify the specified items when the pointer passes over them. To toggle the display of the Selection Filter toolbar, click Toggle Selection Filter Toolbar toolbar, or press F5. •
on the Standard
The first three buttons on the Selection Filter toolbar allow you to specify the behavior of the Selection Filter: Toggle Selection Filters. Turns selected filters on or off. You can also press F6. Clear All Filters. Clears all of the selected filters. Select All Filters. Selects all of the filters.
•
The rest of the buttons on the Selection Filter toolbar are filters. Select the filters that match the items you want to select in the graphics area. When a Selection Filter is active, the pointer changes to
.
Selection Filter Hot Keys •
To hide or show the Selection Filter toolbar, press F5.
•
To turn all the selected filters on or off, press F6.
•
To activate or deactivate specific filters, use the following hot keys.
Filter for edges
Press e
Filter for faces
Press x
Filter for vertices
Press v
NOTE: When a Selection Filter is active, the pointer changes to
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Box Selection You can select all entity types in parts, assemblies, and drawings by dragging a selection box. You can select multiple groups of entities by pressing the Ctrl key while dragging multiple box selections. The default geometry type selected is as follows: •
Part documents - edges
•
Assembly documents - components
•
Drawing documents - sketch entities, dimensions, and annotations
You can set up different selection types with the selection filters. In drawings, hidden edges and faces are not selected. To use box selection to select multiple edges in a part:
1.
Drag a selection box around the left face.
2.
Press Ctrl and drag to select the right side of the part.
The edges of the left face are highlighted.
The left side edges remain selected. The right side edges are highlighted and added to the selection.
NOTE: To enable selection of hidden edges, click Tools, Options, System Options, Display/Selection. Under Selection of hidden edges, select the Allow selection in wireframe and HLV modes and Allow selection in HLR and shaded modes check boxes, as desired.
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Loop Selection You can select a loop of connecting edges using the right mouse button, and then apply a feature such as fillet or chamfer to the selection. Hidden edges are selected in all view modes. To do a loop selection:
1.
Right-click the edge as shown.
2.
The edge becomes highlighted and the shortcut menu appears.
Click Select Loop. The edges of the entire outer loop of the front face become highlighted. The handle indicates the face whose edge is loop selected.
3.
Click the handle to change the loop selection to the edges of the other connecting face. The edges of the top face become highlighted. The handle changes to indicate the new face whose edge is loop selected.
Tangent Selection You can select a group of tangent curves, edges, or faces, with the right mouse button. You can then apply a feature, such as fillet or a chamfer, to the selection. Hidden edges are selected in all view modes. To do a tangent selection:
1.
Right-click the face as shown. The face becomes highlighted and the shortcut menu appears.
2.
Click Select Tangency. All five of the tangent faces become highlighted.
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Select through Transparency You can select opaque objects through transparent objects. This includes opaque components through transparent components in an assembly as well as interior faces, edges, and vertices through transparent faces in a part. As you move the pointer over opaque geometry that is behind transparent geometry, the opaque faces, edges, and vertices highlight. Click to select the highlighted geometry in the graphics area.
NOTES: •
For purposes of selection, transparent means more than 10 percent transparent. Entities less than 10 percent transparent are considered opaque.
•
If the entire model is transparent, (or opaque), use Select Other to select an object.
Keyboard Shortcuts You can use keyboard shortcuts to change which entities the pointer selects first:
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•
To select geometry on a transparent entity with an opaque object behind it, press Shift when selecting.
•
To select the part you are editing through an opaque component, press Tab when selecting.
Viewing Models Applying Color and Optic Properties Use the Color and Optics PropertyManager to apply colors and optical properties such as transparency and ambience to a model.
To apply color or optical properties to a selected entity:
1.
Click Edit Color
on the Standard toolbar, or click Edit, Appearance, Color.
2.
Set the properties in the Color And Optics PropertyManager as necessary.
3.
Click OK
.
To add a custom color swatch to the PropertyManager:
1.
Click Edit Color
on the Standard toolbar, or click Edit, Appearance, Color.
2.
In the PropertyManager, under Favorite: a.
Click Create New Swatch
.
b.
In the Save As dialog box, type a swatch name for File name, then click Save. The file extension is .sldclr. The swatch name appears in Select or Create a Swatch.
c.
To add a color to the swatch: i.
Under Color Properties, define the color you want to add.
ii.
Under Favorite, click Add Current Color to Swatch
.
The color is added to the swatch.
d.
To remove a color from the swatch: i.
Click a color in the custom swatch that you do not want to keep.
ii. Click Remove Selected Swatch Color The color is removed from the swatch.
3.
Click OK
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Draft Quality HLR/HLV Draft Quality HLR/HLV displays complex parts, assemblies, and drawings faster when your model is in Hidden Lines Removed or Hidden Lines Visible mode. Use Draft Quality HLR/HLV with any model for the following benefits: •
Real-time rotation. You can control the rotation speed, and display the entire model in real time.
•
Dynamic HLR/HLV recalculation. HLR/HLV displays during model rotation.
•
Resolution and performance. Image resolution and performance are dependent on the settings in the Document Properties- Image Quality dialog box. You can balance image quality (resolution) with performance. In drawing documents, the following functionality is not available with Draft Quality HLR/HLV:
•
Detail, Crop, Broken, or Alternate Position Views
•
Hide/Show Edge
•
Layers
Line Fonts and Component Line Fonts remain thin solid lines. To change the display of Hidden Lines Removed and Hidden Lines Visible to faster mode:
Click Draft Quality HLR/HLV
on the View toolbar, or click View, Display, Draft Quality HLR/HLV.
Shaded and Dynamic Previews Shaded Previews Shaded previews help you visualize features that you create. For example, when you create an extrude feature, as soon as the Extrude PropertyManager appears, the feature is shown as a shaded preview. You can rotate, pan, zoom, and set standard views while maintaining the shaded preview. NOTE: To improve performance, you can turn shaded previews off in the System Options - Performance dialog box.
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Dynamic Previews When you create or edit a feature that supports dynamic previews, you see a dynamic preview in the graphics area of how the model changes when you move the pointer. At first, a shaded preview appears. Click a handle of the shaded preview, then drag the pointer to see the dynamic preview.
Click the handle, as shown
Drag the pointer to see the dynamic preview
Hidden Lines Removed Displays the model with all edges that are not visible from the current view angle removed. To display the model with hidden lines removed:
Click Hidden Lines Removed
or View, Display, Hidden Lines Removed.
Hidden Lines Visible Displays the model with all edges that are not visible from the current view angle in gray. To display the model with hidden lines visible:
Click Hidden Lines Visible
on the View toolbar, or click View, Display, Hidden Lines Visible.
You can display hidden edges as either solid or dashed lines. To change the display style, click Tools, Options, System Options, Display/Selection.
Applying, Creating, and Editing Materials You can apply a material to a part, and create or edit a material with the Materials Editor PropertyManager. The material and its properties propagate to COSMOSWorks, COSMOSXpress, PhotoWorks release 2, mass properties and material properties. The Material icon appears in the FeatureManager design tree regardless of whether you applied a material to a part.
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To apply a material to a part:
1.
In an open part, click RealView Graphics Graphics.
on the Standard toolbar, or click View, Display, RealView
If you do not have a supported graphics card, RealView Graphics is unavailable. You do not need to use RealView Graphics to apply a material to a part. 2.
Click Edit Material
on the Standard toolbar, or click Edit, Appearance, Material.
3.
Set the properties in the Materials Editor PropertyManager as necessary.
4.
Click OK
.
The material is applied to the part, and the material name appears in the FeatureManager design tree next to the Material icon
.
To create a custom material:
When you create a material, you derive the properties from a SolidWorks default material, then change the properties as necessary to create a different material. 1.
In an open part, click Edit Material
on the Standard toolbar, or click Edit, Appearance, Material.
2.
In the PropertyManager, under Materials: a.
Click an item in Select a Material Database to specify the material library where you want to create a material.
b.
Expand a material classification, then select a material.
c.
Click Create/Edit Material.
3.
Set the properties as necessary on the General Information, Visual Properties, Physical Properties, and Crosshatch tabs.
4.
Click OK.
5.
Click OK
to close the PropertyManager.
To edit a custom material:
You cannot edit SolidWorks default materials. You can, however, edit materials that you created.
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1.
In an open part, click Edit Material
on the Standard toolbar, or click Edit, Appearance, Material.
2.
In the PropertyManager, under Materials: a.
Click a database you created in Select a Material Database to specify the material library that contains the material you want to edit.
b.
Select a material that you created.
c.
Click Create/Edit Material.
3.
Set the properties as necessary on the General Information, Visual Properties, Physical Properties, and Crosshatch tabs.
4.
Click OK.
5.
Click OK
to close the PropertyManager.
To delete a material from a part:
1.
In a part with a material applied to it, click Edit Material Appearance, Material.
on the Standard toolbar, or click Edit,
2.
In the PropertyManager, under Materials, click Remove Material.
3.
Click OK
.
The material is removed from the part and the material name is removed from the Material icon FeatureManager design tree.
in the
Materials - Supported Graphics Cards The following Nvidia® Quadro® graphics cards support RealView Graphics
display:
•
Quadro FX 2000
•
Quadro4 750 XGL
•
Quadro FX 1000
•
Quadro4 700 XGL
•
Quadro4 980 XGL
•
Quadro4 700 Go GL
•
Quadro4 900 XGL
•
Quadro FX Go700 (for Dell™ Precision™ M60 Mobile Workstation only)
•
Quadro4 780 XGL
•
Quadro FX 500
Materials - General Information The General Information tab controls the following properties when you create or edit a material: Database Selection Displays the material libraries: •
Solidworks Materials. A pre-defined library that contains SolidWorks materials. You cannot create or edit materials in this library.
•
Material Classification Displays the material classes in your custom material databases. Material Name Displays the material names in your custom material databases. Materials - Visual Properties The Visual Properties tab controls the following properties when you create or edit a material: RealView Graphics Lists all of the 3D materials used to display models using RealView Graphics. Although you can select a material from this list, it does not appear if you do not have a supported graphics card. Texture Lists all of the 2D textures available in the Texture PropertyManager.
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PhotoWorks Material Lists all of the materials available in PhotoWorks release 2, if you have the add-in product. When you render a model, this material is propagated to PhotoWorks release 2. Color Lists all of the colors used in the Color And Optics PropertyManager. Materials - Physical Properties The Physical Properties tab controls the following properties when you create or edit a material: Material Properties Displays the physical properties for the material. You can change the Value only. If you enter a unit for Value, the units update according to the units you set in the Document Properties - Units dialog box. Materials - Crosshatch The Crosshatch tab controls the following properties when you create or edit a material: Crosshatch •
None. No crosshatch is associated with the material.
•
Solid. A solid black crosshatch is associated with the material.
•
Hatch. A crosshatch with Scale and Angle is associated with the material. The Pattern list displays available crosshatches.
RealView Graphics When you apply a material to a part, use RealView Graphics to display the model with realistic-looking materials. RealView Graphics is available with supported graphics cards only. To turn on RealView Graphics:
Click RealView Graphics on the View toolbar, or click View, Display, RealView Graphics. You can turn off RealView Graphics when your assembly is in large assembly mode.
Perspective Displays a perspective view of the model. A perspective view is the view normally seen by the eye. Parallel lines recede into the distance to a vanishing point. You can create a Named View in a drawing of a perspective view of a model. To display the model in Perspective view:
Click Perspective
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on the View toolbar, or click View, Display, Perspective.
Modify Perspective Perspective is related to the size of the object being observed and the distance of that object from the observer. You can modify the perspective by specifying the Object Sizes Away value in the Perspective PropertyManager. The smaller the value, the greater the amount of perspective distortion. To change the perspective:
1.
With Perspective
selected, click View, Modify, Perspective.
The Perspective View PropertyManager appears. 2.
Under Observer Position, type a value in the Object Sizes Away
3.
Click OK
box.
.
Creating a Section View A section view displays a view of the model cut through the part or assembly. When you create a section view, then toggle the view off and on, the section view state is retained. Zebra stripes are not available with an active section view.
To create a section view:
1.
In a part or assembly document, click Section View Section View.
on the View toolbar, or click View, Display,
2.
In the PropertyManager, under Section 1, set the properties in the Section View PropertyManager as necessary.
3.
To create additional section views, select Section 2 and Section 3, then repeat step 2. You can use the same planes to create additional section views. Section 3 is unavailable until Section 2 is selected.
4.
Click OK
.
To save a section view:
1.
In the Section View PropertyManager, under Options, click Save View.
2.
In the Named View dialog box, type a name for View name.
3.
Click OK. The Orientation dialog box appears with the new section view.
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Section View PropertyManager Displays a view of the model cut through the part or assembly. When you create a section view, you use planes or faces as references to make the model cut. The Section View PropertyManager controls: Section 1 and Section 2 •
Planes. Selects the Front Plane section view.
•
Reference Section Plane/Face. Displays the plane or face to create the section view. Reverse Section Direction
, Top Plane
, and Right Plane
that you can use to create the
changes the direction of the cut to the opposite side.
•
Offset Distance
.
•
X Rotation
. Rotates the reference section along the X-axis.
•
Y Rotation
. Rotates the reference section along the Y-axis.
•
Edit Color. Changes the color of the section view while the PropertyManager is active. The colors are used only while the PropertyManager is active. The colors are not displayed after the section view is created.
Section 3 This section appears after you select Section 2. Use Section 2 and Section 3 to create additional section views in the model. Options •
Save View. Saves the section view as a named view in the Orientation dialog box. If you insert a saved section view in a drawing, only the view orientation and perspective view data are shown. The actual section view is not visible.
•
Reset. Resets the selections to the default values.
•
Show section cap. Displays the section view with the color specified in the Edit Color box. Clear this option to see inside the model.
Shaded Displays a shaded view of the model. When you select a face on a model that is in shaded view, the entire face is highlighted. To display a model in shaded view:
Click Shaded on the View toolbar, or click View, Display, Shaded. You can control: • • •
The color of shaded parts. The color of individual part faces. The light intensity and direction on the shaded parts.
When in shaded view, the sketch plane is displayed as a translucent plane. This behavior is controlled by the Display plane when shaded option. Click Tools, Options, System Options, Sketch.
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Shaded With Edges Displays a shaded view of the model with edges visible. To display a model in Shaded With Edges view:
Click Shaded With Edges on the View toolbar, or click View, Display, Shaded With Edges. You can also control the color of the shaded edges.
Shadows Displays a shadow under the model. When shadows are displayed, the light appears from the top-most part of the model in the current view. The shadow does not dynamically change positions when you rotate the model. NOTE: When you have shadows enabled, system performance is slower during dynamic view operations (zoom, pan, rotate, and so on). To turn on shadows:
Click Shadows In Shaded Mode
on the View toolbar, or click View, Display, Shadows In Shaded Mode.
NOTE: To change the placement of the shadow, turn Shadows In Shaded Mode off, rotate the model, then turn the shadows on again.
Orientation Rotates and zooms the model or drawing to a preset view. You can select from the standard views (Normal To, Front, Back, Isometric, and so on for a model, Full Sheet for a drawing) or add your own named views to the list. You can return your model or drawing to a previous view by clicking Previous View can undo the last 10 view changes.
, on the View toolbar. You
To select a view:
Click Standard Views
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Viewing Models Normal To To display a model in Normal To view:
1.
2.
In the model, select one of the following: •
Plane or planar face
•
Cylindrical or conical face
•
Any feature created with a single sketch
Click Standard Views
, and select Normal To
If you click Normal To
.
again, the model flips 180°.
To select a view orientation with Normal To:
With this method, the first face you choose is parallel to the screen and the second face you choose is at the top of the view. 1.
Hold down Ctrl and select two planar faces. The second planar face cannot be parallel to the first.
2.
Click Standard Views
, and select Normal To
.
Orientation Dialog Box To display the Orientation dialog box:
Do one of the following: •
Click View Orientation
•
Click View, Modify, Orientation.
on the View toolbar.
•
Press the Space Bar.
•
Right-click in a drawing sheet and select Zoom/Pan/Rotate, View Orientation. To keep the Orientation list open, click
in the dialog box.
To add a new named view to the Orientation dialog box:
1.
Use the Rotate, Zoom, and Pan commands to create the desired view.
2.
With the Orientation dialog box open, click New View
3.
In the Named View dialog box, type a name for View name, and click OK.
.
The name appears at the top of the list of views. You can display the view by double-clicking its name. To delete a named view from the Orientation dialog box:
You can delete a named view from the Orientation dialog box only if you created the named view with the above procedure. In the Orientation dialog box, select the named view you want to delete and press Delete.
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To change the orientation of the standard model views in the Orientation dialog box:
1.
In the Orientation dialog box, double-click one of the named views to select the new orientation. For example, if you want what is currently the Left view to become the front view, double-click Left.
2.
Click (do not double-click) the name of the standard view you want to assign to the current orientation of the model. For example, click Front if you want the current view to become the front.
3.
Click Update Standard Views selected view.
4.
Click Yes to confirm the update.
. This updates all of the standard views so they are relative to the
To return all standard model views to their default settings in the Orientation dialog box:
1.
In the Orientation dialog box, click Reset Standard Views
2.
Click Yes to confirm the update.
.
Add a Named View The Named View dialog box appears when you select New View in the Orientation dialog box. 1.
Use the Rotate, Zoom, and Pan commands to create the desired view.
2.
Enter a descriptive name for the view, and click OK. Display the named view by double-clicking on its name in the Orientation list.
Textures Use the Texture PropertyManager to apply 2D textures to part and assembly documents for a more realistic finish.
To apply a texture to a part or assembly document:
1.
In a part or assembly document, click Edit Texture Appearance, Texture.
on the Standard toolbar, or click Edit,
2.
Set the properties in the Texture PropertyManager as necessary. You cannot apply textures to weld beads or cosmetic threads.
3.
Click OK
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To create custom textures:
1.
Create a folder in your installation directory where you want to store texture files.
2.
Place any files to use as textures in the folder you created in step 1. The images must be in .jpg, .bmp, or .png format.
3.
In the SolidWorks software, click Tools, Options, System Options, File Locations.
4.
Select Textures in Show folders for, then click Add.
5.
In the Browse For Folder dialog box, browse to the folder you created in step 1.
6.
Click OK. The next time you apply a texture, the folder path appears in the Texture PropertyManager in the Texture File Locations list, and you can select your custom textures. When you create a custom texture, you can also apply the texture to a material when you create or edit a material.
Wireframe Displays all the edges of the model. To display the model in wireframe:
Click Wireframe
on the View toolbar, or click View, Display, Wireframe.
Manipulating Models Middle Mouse Button Functions Three-button Mouse If you use a three-button mouse, you can dynamically use the following view commands: •
Pan all document types - Hold down Ctrl and drag with the middle mouse button. (In an active drawing, you do not need to hold down Ctrl.)
•
Rotate part or assembly - Drag with the middle mouse button.
•
Zoom all document types - Hold down Shift and drag with the middle mouse button.
•
The middle mouse button acts the same as the left mouse button if one of the dynamic view commands (Zoom In/Out
, Pan
, or Rotate View
on the View toolbar) is active.
If you open the part or assembly in View-Only mode or in the or in SolidWorks Viewer, you can only rotate the part or assembly with the middle mouse button if it was saved with Fast HLR/HLV , Shaded With Edges , or Shaded
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mode.
Wheel-type Mouse If you use a wheel-type mouse, you can zoom in to the position of the pointer instead of the center of the graphics area by spinning the wheel backwards. This is the default behavior. If the pointer is outside of the graphics area, the center of the model zooms into view. While rolling the mouse wheel, you must keep the pointer on the area where you want to zoom. To turn this function off, click View, Modify, Zoom About Screen Center. Zoom the view in or out by spinning the wheel forward or back. The model zooms to the center of the screen. This can also be combined with the middle mouse button rotate command by holding down the wheel while you spin it. To use the wheel to pan the view, hold down Shift while you spin the wheel. If you select an entity by pressing down and releasing the mouse wheel, you can then rotate the model around the selected entity by holding down the mouse wheel while moving the mouse. Often the settings for the wheel override the SolidWorks software settings. To change this, SolidWorks recommends that you turn off the wheel when using the SolidWorks software. This is done in the Windows Control Panel for the mouse. If this fails, check with the manufacturer for a new driver or for issues concerning the current mouse drivers.
Pan Scrolls the part, assembly, or drawing in the document window. To pan with the mouse:
1.
Click Pan
or View, Modify, Pan.
The pointer changes to 2.
.
Hold the mouse button down and drag in the direction you want to scroll.
To pan with the arrow keys:
Hold down the Ctrl key and use the Arrow keys. To pan with the middle mouse button:
Hold down the Ctrl key and the middle mouse button, then drag in the direction you want to pan.
Rotate View Rotates the model view. When you rotate a part or assembly with high-quality transparency, the application dynamically switches to a lowquality transparency, enabling you to rotate the model faster. Once you complete the rotation, the model switches back to high-quality transparency. This is especially important if your part or assembly is complex. Optionally, you can choose to retain high-quality transparency while rotating or moving the model with the rotate or pan tools. Depending on your graphics card, this option may result in slower performance. TIP: To set the type of transparency, click Tools, Options, and on the System Options tab, select Performance. Select the appropriate transparency options.
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To rotate the model view:
1.
Click Rotate View
or View, Modify, Rotate.
2.
Press the mouse button and drag to rotate the view. NOTE: Click View, Modify, Rotate About Screen Center to rotate the view around the center of the screen or the origin of the model. TIP: Use the arrow keys to rotate the view vertically or horizontally. (Hold down Shift to rotate in 90-degree increments). Hold down Alt and use the left-right arrow keys to rotate clockwise or counterclockwise.
To rotate the view about a selected vertex, edge, or face:
1.
Click Rotate View
or View, Modify, Rotate.
2.
Click the vertex, edge, or face to rotate about.
3.
Press the mouse button and drag to rotate the view.
NOTE: To change the speed of the view rotation, click Tools, Options, and on the System Options tab select View Rotation. Use the Mouse speed slider to change the speed of rotation; in the Arrow keys box, you can change the angle increment used when rotating with the arrow keys.
Previous View After moving your model to one or more views, you can return your model or drawing to a previous view. You can undo the last 10 view changes. To see previous views:
Click Previous View
on the View toolbar.
Zoom to Fit Zooms in or out so you can see the entire model, assembly, or drawing sheet. To see the entire model:
Click Zoom to Fit
on the View toolbar, or click View, Modify, Zoom to Fit.
Zoom to Area Zooms in to an area that you select by dragging a bounding box. To zoom in to a selected area:
1.
Click Zoom to Area
2.
Point at one corner of the area you want to enlarge. The pointer changes to
on the View toolbar, or click View, Modify, Zoom to Area.
.
3.
Press the mouse button and drag the bounding box diagonally to enclose the area.
4.
Release the mouse button. The view is zoomed in to the selected area.
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Zoom In/Out Zooms in and out. To zoom in or out:
1.
Click Zoom In/Out
on the View toolbar, or click View, Modify, Zoom In/Out.
2.
Press the mouse button and drag up (toward the top of the screen) to zoom in, or drag down to zoom out.
TIP: Press z to zoom out or Shift+Z to zoom in. NOTE: If you have a wheel-type mouse, you can zoom in to the position of the pointer instead of the center of the graphics area by spinning the wheel backwards. This is the default. If the pointer is outside of the graphics area, the center of the model zooms in to view. You do not need Zoom In/Out enabled when you use the wheel to zoom. To turn this function off, click View, Modify, Zoom About Screen Center. The model zooms to the center of the screen. While rolling the mouse wheel, you must keep the pointer on the area where you want to zoom.
Zoom to Selection Zooms in on a portion of the model, assembly, or drawing that you select. To zoom to selection:
1.
Click an entity to which you want to zoom, or hold Ctrl and click several entities.
2.
Click Zoom to Selection
on the View toolbar, or click View, Modify, Zoom to Selection.
The view is zoomed in to the selected entity.
Customizing SolidWorks Overview of SolidWorks Options Customize functionality to suit your needs. Click Tools, Options to display system options and document property settings. Options Dialog Box Structure The SolidWorks Options dialog box structure emphasizes the difference between system options and document properties. The Options dialog box has two tabs: •
System Options. The system options are stored in the registry and are not part of the documents. Therefore, these changes affect all documents, current and future.
•
Document Properties. The document properties apply only to the current document, and the Document Properties tab is available only when a document is open. New documents get their document settings (such as Units, Image Quality, and so on) from the document properties of the template used to create the document. Use the Document Properties tab when you set up document templates.
The options listed on each tab are displayed in tree format on the left side of the dialog box. As you click an item in the tree, the options for the item appear on the right side of the dialog box. The title bar displays the title of the tab and the title of the options page.
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To access the Options dialog box:
You can access the Options dialog box in any of the following ways: •
Click Tools, Options. The Options dialog box appears with the System Options tab active.
•
Right-click in the FeatureManager design tree area and select Document Properties. (There must be no items selected in the FeatureManager design tree or graphics area in order to select Document Properties.) The Options dialog box appears with the Document Properties tab active.
•
Click Grid/Snap on the Sketch toolbar. The Options dialog box appears with the Grid/Snap page of the Document Properties tab active.
Document Templates Templates are documents (part, drawing, and assembly documents) that include user-defined parameters. When you open a new part, drawing, or assembly, you select a template to use for your new document. Templates allow you to maintain as many different documents for parts, drawings, or assemblies as you need. A template can be a part, drawing, or assembly document that you saved as a template. For example, you can create: •
A document template using millimeters and another template using inches
•
A document template using ANSI and another template using ISO dimensioning standard
You can organize your document templates by placing them on different tabs in the New SolidWorks Document dialog box. TIP: If you use small units of measure such as angstroms, nanometers, microns, mils, or microinches, you might want to create specific templates as the basis for documents that use the units. The templates could include settings for such Document Properties as: •
grid spacing
•
extension line and break line gap
•
dimension offset distance and break dimension gap
•
note bent leader length
•
balloon bent leader length
•
arrow size and section view arrow size
•
text scale and text display size
•
material density
To create a template:
1.
Click New
on the Standard toolbar, or click File, New.
The New SolidWorks Document dialog box appears with an available set of templates. 2.
Double-click the appropriate icon for the type of template that you want to create: Part, Assembly, or Drawing.
3.
Click Tools, Options. On the Document Properties tab, select options to customize your new document template, then click OK. NOTE: Only options on the Document Properties tab are saved in a document template.
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4.
Click File, Save As.
5.
In the Save as type list, select a template type: •
Part Templates (*.prtdot)
•
Assembly Templates (*.asmdot)
•
Drawing Templates (*.drwdot)
6.
Type a name in the File name box. The extension is added automatically.
7.
Browse to the folder where you want to save your template, then click Save.
Customize Commands Adds, removes, and rearranges command buttons to customize your toolbars. You can: •
add command buttons and place them on more than one toolbar
•
remove command buttons that you never use
•
rearrange command buttons on toolbars, or move command buttons from one toolbar to another
To customize command buttons on your toolbars:
1.
With a document open, click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
2.
On the Commands tab, under Categories, select the toolbar that you want to change.
3.
Under Buttons, point at the toolbar button to see the tooltip that describes the button. If you click the button, a definition appears under Description.
4.
Do any of the following to customize the command buttons: To... Add a command button or place it on more than one toolbar Remove a command button from a toolbar Rearrange a command button on a toolbar Move a command button from one toolbar to another
5.
Then... In the Customize dialog box, click and drag a button to any toolbar. In the SolidWorks window, click and drag the button from the toolbar to the graphics area. In the SolidWorks window, click and drag the button from the toolbar to another area of the toolbar. In the SolidWorks window, click and drag a button from one toolbar to a different toolbar.
Click OK.
Customize Headers and Footers You can specify headers and footers for the active document before printing. To create a header or footer:
1.
Click File, Print. The Print dialog box appears.
2.
Under Document Options, click Header/Footer. The Header/Footer dialog box appears.
3.
Select a predefined header or footer from the Header and Footer lists. - or Click Custom Header or Custom Footer to create a unique header or footer and do the following: a.
Select an area of the document where you want the header or footer to appear: Left section, Center section, or Right section.
b.
Select the items you want to appear on the page (Page Numbers Date
c.
, Time
, or Filename
, Number of Pages
,
).
Click OK.
The Header preview and Footer preview boxes update according to the items you selected. 4.
Click OK to close the Header/Footer dialog box.
5.
Click OK to close the Print dialog box and print the document.
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Customize Keyboard Customizes your keyboard to suit your style of working with SolidWorks. To customize your keyboard:
1.
With a document open, click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
2.
Click the Keyboard tab.
3.
Click the appropriate buttons to Assign a new shortcut key, Remove a shortcut key, or Reset All shortcut keys to their original state. Customization options:
4.
•
Categories. Select the menu that contains the command you want.
•
Commands. Select the command for which you want to assign or remove a shortcut key.
•
Press new shortcut key. Type a single key or a combination of keys.
•
Current keys. Displays the current shortcut key for the selected command.
•
Description. Displays the description for the selected command.
Click OK.
Customize Macro Button When you create a macro, you can assign a bitmap to the macro button on the toolbar. The SolidWorks software includes sample bitmaps, or you can create your own bitmap. You can also specify which method (a procedure that operates on an object) within a macro you want to run. For more information, see the SolidWorks API Help Topics. If you create a bitmap for a macro button, the bitmap must meet these requirements: •
Dimension = 16 x 16 pixels
•
Color = 16 colors
•
Background color = white
To run a specific macro method and create a custom macro button:
1.
With a document open, click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
2.
In the dialog box, on the Commands tab:
3.
a.
Select Macro in Categories.
b.
Under Buttons, drag the Macro
button to any toolbar in the SolidWorks window.
In the Customize Macro Button dialog box: a.
Under Appearance: i.
Click Choose Image.
ii.
In the Icon path dialog box, select a bitmap image (*.bmp), then click Open. The SolidWorks software provides bitmap images to use as custom buttons. These are located in
iii. If necessary, type a Tooltip and Prompt message, which provides a brief description of the function of the tool on the status bar.
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b.
Under Action: i.
Click
and open the macro you want to use.
ii.
If necessary, select a Method. When you select a method, only that method runs in the macro. The method is in the form: <module_name>.<method_name>.
iii. Click OK.
4.
c.
Type a key in Shortcut to assign a shortcut key to the macro.
d.
Click OK.
Click OK again to close the Customize dialog box.
To edit a customized macro button:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when creating custom macro buttons.
2.
Right-click the customized macro button in the toolbar that you want to edit.
3.
In the Customize Macro Button dialog box, edit the macro as necessary, then click OK.
4.
Click OK again to close the Customize dialog box.
Customize Menus Customizes a SolidWorks menu to suit your style of working. To add or delete an item in a SolidWorks menu:
1.
Click the menu you want to add or delete a menu item and select Customize Menu. Each item currently visible in the menu is preceded by
.
This menu is for customization purposes only. You cannot run a command from this menu. 2.
To add menu items, select the empty check boxes
. To delete menu items, clear the selected check boxes
. 3.
Click anywhere outside of the menu to save your changes, or press Enter. To cancel your changes, press Esc.
To set SolidWorks menus or shortcut menus to default values or to show all menu items:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
2.
3.
On the Options tab, under Shortcut customization or Menu customization, click: •
Show All. Displays all menu items.
•
Reset to Defaults. Resets all menu items to the default display.
Click OK.
To customize a SolidWorks menu:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
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2.
On the Menus tab, click the appropriate buttons to Rename a menu item, Remove or Add a menu item, or Reset All menus to their original state. Customization options: Categories. Select the menu to change. Commands. Select the command to add, rename, relocate, or remove. Change what menu. Displays the code name of the selected menu. Position on menu. Lets you select a menu position, including Auto, At Top, or At Bottom. Name of command. Displays the code name of the selected command. Description. Displays the description of the selected command.
3.
Click OK.
Customize Options If you customized SolidWorks menus or shortcut menus, you can set them back to default values or show all menu items. To set SolidWorks menus or shortcut menus to default values or to show all menu items:
1.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize. You must have a SolidWorks document active when customizing menus.
2.
3.
On the Options tab, under Shortcut customization or Menu customization, click: •
Show All. Displays all menu items.
•
Reset to Defaults. Resets all menu items to the default display.
Click OK.
Customize Toolbars Customizes, displays, or hides toolbars. You can position toolbars and set their visibility based on the document type (part, assembly, or drawing). You can also set which toolbars are visible for when there are no documents open. The SolidWorks software remembers which toolbars to display and where to display them for each document type. For example, with a part document open, you can choose to display only the Standard and Features toolbars. Whenever you create or open any part document, only these toolbars are displayed. Meanwhile, for an assembly document, you can choose to display only the Assembly and Selection Filter toolbars. Whenever you create or open an assembly document, only these toolbars are displayed. To customize which toolbars appear for part, assembly, or drawing documents:
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1.
Open a part, assembly, or drawing document.
2.
Click Tools, Customize, or right-click any toolbar (not the CommandManager) and select Customize.
3.
On the Toolbars tab, select the toolbars you want to display and clear the toolbars you want to hide. Your selections apply to the type of SolidWorks document that is currently open.
4.
Select from the following options: •
Large icons. Displays large toolbar buttons.
•
Show tooltips. Displays a note to identify each toolbar button when you pause the pointer over a button.
•
Use large tooltips. Displays expanded tooltips that show both the name of a toolbar button and a brief description of its functionality. This is available only when Show tooltips is selected.
5.
Click: •
OK to accept the changes.
•
Reset to undo the changes and return to previous settings
•
Cancel to discard the changes and close the dialog box.
You can move toolbars as desired. Toolbars can be either docked in one of the toolbar areas or floating. To move a toolbar:
Click the start or edge of the toolbar and drag. If you drag a toolbar to an edge of the SolidWorks window, the toolbar docks to the edge automatically. - or If you drag a toolbar away from the window edge, it becomes a floating palette.
Skins You can apply skins as background images to the PropertyManager. Skins are images that appear behind the PropertyManager data, similar to this wood sample skin. You can also create your own PropertyManager buttons. Only bitmap (.bmp) files are supported as skins. SolidWorks offers sample skins for your use. The sample skins are located in
1.
Click Tools, Options, System Options, Colors.
2.
Under System colors, select an item in PropertyManager Skin. To disable skins, select None.
3.
Click OK. When you activate the PropertyManager, the skin appears.
To create a customized skin bitmap file:
1.
Open your graphics editing software and create a bitmap file. You can use any color (including true colors), resolution, or size setting.
2.
Save the skin as
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To customize the PropertyManager buttons:
After you create your background skin bitmap file, you can customize any of the OK, Cancel, Help, Keep Visible, Back, Next, Preview, and Undo buttons. You are encouraged to customize all buttons so they match. If you do not customize a button with a skin, the default SolidWorks button is applied. The button colors are blended to the background color. If you have dark background colors, the default buttons may be difficult to read. 1.
Create the skin bitmap file as described in the procedure above.
2.
Create the button skin bitmap file with your graphics editing software, using the following guidelines: •
File Name. The button skin bitmap file name must be <skin_bitmap_file_name>__
3.
•
Display States. You must display the button in four states: off, on, mouse over, and unavailable. Here is an example using the Cancel button:
•
Pixel Size. Each individual button state must be 32 by 32 pixels. Therefore, each group of four buttons must be 32 pixels high and 128 pixels wide. Here is an example of the pixel size using the Cancel button.
•
Colors. The buttons can have a color palette of 2, 8, 16, or 256 colors. True colors are not supported.
•
Transparency. To set any part of the button skin bitmap file to transparent, set the RGB color for that area to 255, 0, 255. Transparent areas display the color and design used in the background skin bitmap file. Here is an example using the OK button:
Add the button skin bitmap files to
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SolidWorks Tools Add-Ins Lets you integrate other compatible software applications with your installed SolidWorks software. The add-in software applications must be installed on your computer. To use another software application along with SolidWorks:
1.
Click Tools, Add-Ins. The list of installed, compatible software appears in the dialog box.
2. 3.
Select one or more applications that you want to use. Click OK. Some add-in applications provide a tab at the top of the FeatureManager design tree panel. The tab contains information related to the specific add-in.
These tabs include the SolidWorks Animator tab at the far right.
You can also add an add-in application's toolbar to the SolidWorks window.
Conversion Wizard When you open a SolidWorks document from an earlier version, it may take more time than you are used to experiencing. After the document has been opened and saved, subsequent opening time returns to normal. The SolidWorks Conversion Wizard automatically converts all of your SolidWorks documents from an earlier version to the current SolidWorks format. Depending on how many files you have, the conversion process may take a while, but once it is done, the documents open more rapidly. Once a document is converted, you can no longer open the file in the older SolidWorks version. To access the Conversion Wizard, click the Microsoft Start button, then click Programs, SolidWorks 2004, SolidWorks Tools, Conversion Wizard. The Conversion Wizard has the following options: •
Create a backup for files to convert. Backs up all of your files before the conversion. If you choose to back up your SolidWorks files, the Conversion Wizard copies the files to a sub-folder named Solidworks Conversion Backup. The wizard asks you for the location of the files to be converted, and leads you through the process.
•
Include subfolders. Converts all SolidWorks documents in the main folder and its subfolders.
•
Visibility: o
o
Run SolidWorks in background. The SolidWorks software runs while the files are being converted, but it is invisible to the user. Show SolidWorks window. The SolidWorks software runs while the files are being converted, and is visible to the user.
•
Save pre-2003 drawings with "Automatic update of BOM". Sets the option, Automatic update of BOM, which automatically updates a drawing's Bill of Materials when changes are made to the model for all drawings created prior to SolidWorks 2003.
•
Convert drawings to Detached Drawings format automatically. Converts all converted drawing documents to Detached format.
•
Ignore files with missing references. Documents dependent on missing reference files are not converted.
•
Backup Folder: o
Path. Displays the location where the backup files are saved. Click Browse to change the location.
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At the end of the conversion process, two report files exist in the folder to which you directed the conversion: •
Conversion Wizard Log.txt. Contains a list of files that converted.
•
Conversion Wizard Failed.txt. Contains a list of files that did not convert.
Copy Options Wizard When you select options for the SolidWorks application, those options settings are saved in a registry file. To maintain uniformity among the SolidWorks users at your location, you or your network administrator can use the Copy Options Wizard to apply the same options to other SolidWorks installations on your network. To use the Copy Options Wizard:
1.
Click the Microsoft Windows Start button, then click Programs, SolidWorks 2004, SolidWorks Tools, Copy Option Wizard.
2.
In the dialog box: •
To capture your SolidWorks options information from the registry file, select An existing user and select your name. - or -
•
To capture SolidWorks options from a registry file you created, select A previously created registry file, then click Browse to locate the file.
3.
Click Next.
4.
Under SolidWorks option settings destination, select: •
Users and computers on the network. Copy the SolidWorks options directly to Both users and computers, Only users, or Only computers on the network. Depending on the option you choose, the next dialog box allows you to select the users or computers to which the settings will apply. - or -
•
Create a registry file. The SolidWorks registry options of the current system are copied to a swOptions.reg file that you can use with SolidWorks supported operating systems. Copy this swOptions.reg file to another computer and double-click the file. The registry options are automatically copied to the registry of the new computer.
5.
Click Next.
6.
Click Finish.
Manufacturing Network The Manufacturing Network is an online directory of SolidWorks-enabled service vendors. This directory lists contract design and manufacturing companies who can help reduce your product's time to market. Each company in the directory is a SolidWorks user; there is no need to translate SolidWorks documents to an intermediate file format. The Manufacturing Network is free of charge. NOTE: You need an Internet connection to access the Manufacturing Network. To access the Manufacturing Network:
Click Tools, Manufacturing Network. - or In your Internet browser, go to http://www.solidworks.com/swmn.
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Moving from AutoCAD Moving from AutoCAD supports users in the transition from 2D AutoCAD to 3D SolidWorks. It compares terms and concepts, explains SolidWorks approaches to design, and provides links into SolidWorks Help, tutorials, and other resources. To access Moving from AutoCAD:
Click Help, Moving from AutoCAD.
Quick Tips Quick Tips are a set of pop-up messages that appear while you create SolidWorks documents. These messages give hints and options based on the current SolidWorks mode. Most of the messages have hyperlinks; click the hyperlink to see the associated item in the SolidWorks window. Quick Tips are not available when the Online Tutorial is active. There are four icons associated with the Quick Tips status. These appear in the lower-right corner of the SolidWorks window: Icon
Status Available, but not currently displayed Currently displayed Not available Temporarily disabled
To turn on Quick Tips:
Click Help, Quick Tips or click
.
To turn off Quick Tips:
Click Help, Quick Tips, or click
.
Quick Tips are mode-specific. For example, if you have Quick Tips displayed when you have a part document open, then you click , Quick Tips are no longer displayed in part modes. However, if you open an assembly document, Quick Tips reappear.
SolidWorks API The SolidWorks Application Programming Interface (API) is a COM programming interface to the SolidWorks software. The API contains hundreds of functions that you can call from Visual Basic (VB), Visual Basic for Applications (VBA), VB.NET, C++, C#, or SolidWorks macro files. These functions provide the programmer with direct access to SolidWorks functionality. To access the API help, click Help, SolidWorks API and Add-Ins Help Topics. There are tips, code fragments, and examples of API functions on the SolidWorks Web page: www.solidworks.com/api.
SolidWorks Service Packs If you are a SolidWorks subscription customer, you can take advantage of SolidWorks service packs that are regularly posted on the SolidWorks Web site. These service packs contain software updates and enhancements to the SolidWorks software. To check for a new service pack, click Help, Service Packs, and click the Check button. Select the Check for a new service pack once a week check box if you want the software to automatically check the SolidWorks Web site once a week.
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SolidWorks Web Site If your computer is connected to the Internet, you can visit the SolidWorks Web site to learn more about SolidWorks Corporation and its products. To access the SolidWorks Web site:
1.
Click Help, About SolidWorks.
2.
In the dialog box, click Connect.
Recording and Playing Macros New Macro You can create a new macro from the Macro toolbar or from a menu item. Creating a new macro is different from recording a macro. When you create a new macro, you program the macro directly from your macro editing application. When you record a macro, you create the macro from within the SolidWorks software. To create a new macro:
1.
Click New Macro
on the Macro toolbar, or click Tools, Macro, New.
The New Macro dialog box appears. 2.
Type a File name.
3.
Click Save. Your macro editing application opens where you can create a new macro.
Record/Pause Macro You can record operations performed with the SolidWorks user interface and replay them with SolidWorks macros. A macro contains the equivalent calls to the API functions that were made when the operations were performed with the user interface. A macro can record your mouse clicks, menu choices, and keystrokes to play back later. You can create a new macro without recording one first. To record a macro:
1.
Click Record\Pause Macro
on the Macro toolbar, or click Tools, Macro, Record.
2.
Perform the steps you want to record.
3.
When you are done, click Stop Macro
4.
In the dialog box, type a name for File name and click Save. (The .swp extension is automatically added to the filename.)
on the Macro toolbar, or click Tools, Macro, Stop.
To pause while recording a macro:
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Click Record\Pause Macro
or Tools, Macro, Pause.
Click Record\Pause Macro
again to continue recording.
Edit Macro Edits or debugs a macro that you recorded previously. To edit a macro:
1.
Click Edit Macro
on the Macro toolbar, or click Tools, Macro, Edit.
If you have previously edited macros, you can select the macro directly from the menu when you click Tools, Macro. This menu lists the last nine edited macros. 2.
In the dialog box, select a macro file (.swp) and click Open. You can also edit .swb files. When you run or edit an .swb file, it is automatically converted to a .swp file.
3.
Edit the macro. (For details, use the help in the macro editor.)
Run Macro Opens a dialog box that lets you select the macro you want to run. To run a macro:
1.
Click Run Macro
on the Macro toolbar, or click Tools, Macro, Run.
The Run Macro dialog box appears. 2.
Locate the macro (.swp) file you want to run and click Open. NOTE: You can also open .swb files.
Stop Macro Stops recording the macro and opens a dialog box so you can save the macro. To stop recording a macro:
1.
While you are recording a macro, click Stop Macro
or Tools, Macro, Stop.
The Save As dialog box appears. 2.
Type a name for the macro and click Save to save it. (The .swp extension is automatically added to the filename.) - or Press Cancel to cancel the macro.
Assign a Macro to a Shortcut Key or Menu You can assign your own macros to shortcut keys or create new menu items for them. When you assign a macro to a shortcut key or to a menu, you can specify which method (a procedure that operates on an object) within the macro you want to run. NOTE: Before you assign a macro to a shortcut key or to a menu item, you must create a macro folder and record a macro in your SolidWorks installation directory.
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To create a macro folder and record a macro:
1.
Create a folder named \Macros in your SolidWorks installation directory (in the same folder as SOLIDWORKS.exe). This \Macros folder is where you must keep the all the macros that you access from a key or a menu.
2.
Record a macro and make sure it has a .swp extension.
3.
Save the macro in the \Macros folder.
To assign a macro to a shortcut key:
1.
With a document open, click Tools, Customize, Keyboard.
2.
Select Macros in Categories. If Macros is not listed, you must create a macro folder and record a macro in your SolidWorks installation directory, as described in the first procedure.
3.
Select the name of the macro in Commands. The macro is in the form: <macro_name>:<module_name>.<method_name>. The macro description appears in Description.
4.
Type a value for Press new shortcut key to assign a shortcut key to the macro, and click Assign. The shortcut key name appears in Current keys.
5.
Click OK.
To assign a macro to a new menu item:
1.
With a document open, click Tools, Customize, Menus.
2.
Select Macros in Categories. If Macros is not listed, you must create a macro folder and record a macro in your SolidWorks installation directory, as described in the first procedure.
3.
Select the name of the macro in Commands. The macro is in the form: <macro_name>:<module_name>.<method_name>. The macro description appears in Description.
4.
Select the menu and sub-menu, if necessary, where you want to add the new menu item for your macro in Change what menu.
5.
Select a position for the new menu item in Position on menu.
6.
Type a command name for Name of command.
7.
Click Add, then click OK.
VBA Visual Basic for Applications (VBA) is the engine that records, runs, or edits macros in SolidWorks. Recorded macros are saved as .swp VBA project files. You can read and edit .swb and .swp (VBA) files with the VBA editor. When you edit an existing .swb file, the file automatically converts into a .swp file. You can export a module to a file that you can use in other VB projects. You can use VBA to create forms and to provide more user interaction with your recorded macros. For more information on VBA, look to the Help menu in the VBA editor.
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Object Linking and Embedding - OLE Object Linking vs. Embedding When using OLE, you can link or embed files. •
Linking files. When you link a file: o
The file remains in its original location.
o
Anything you change in the original file affects all the files to which it is linked.
o
If you double-click a SolidWorks image in a Microsoft Word document, the SolidWorks software launches for you to edit the original file (if you have SolidWorks installed on your PC).
For example, if you edit a SolidWorks assembly document that is linked to several Word documents, the changes you make are reflected in both the original SolidWorks file and all of the Word documents. •
Embedding files. When you embed one file in another: o
The original file becomes part of the file in which you embedded it.
o
Any changes you make to the embedded SolidWorks document affect only that document.
o
o
Any changes you make to the original SolidWorks file do not affect the document embedded in the Word file. If you double-click a SolidWorks image in a Word document, the SolidWorks software launches for you to edit the file (if you have SolidWorks installed on your PC).
Embedding is useful if you want discrete control over the data.
Object You can embed an OLE object from another program into the active SolidWorks document. You can either open another program from within SolidWorks and create a new object, or you can insert an existing file. To create a new OLE Object:
1.
Click Insert, Object. The Insert Object dialog box appears.
2.
Click Create New.
3.
In the Object Type box, click the type of document you want to create (for example, Microsoft Excel Worksheet.) Only documents from OLE-compliant applications that are installed on your computer appear in the list.
4.
Select the Display As Icon check box if you want the new object to appear as an icon in your document.
5.
Click OK. A new document appears inside your active document. The toolbars and menus for this new document appear in place of the SolidWorks toolbars and menus. If you chose Display As Icon, an icon appears in your SolidWorks document, and the parent application opens in another window.
6.
Edit the object as though you were working in the parent application.
7.
When you finish editing, click in the SolidWorks document window anywhere outside the embedded object. The SolidWorks toolbars and menus become available again. If you chose Display As Icon, click File, Exit or File, Close & Return to <part name> in the parent application.
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To insert an existing file as an OLE object:
1.
Click Insert, Object. The Insert Object dialog box appears.
2.
Click Create from File.
3.
Click Browse, locate the file you want to insert, and click Open.
4.
Select from the following check boxes: •
Link. Displays a picture of the file contents in the SolidWorks document. The picture is linked to the original document, and changes made to the original document are reflected in the SolidWorks document.
•
Display As Icon. Displays the new object as an icon in the SolidWorks document.
NOTE: If you select both of these check boxes, the new object is displayed as an icon, and the SolidWorks software creates a shortcut to the original document. If you select neither of these check boxes, the new object is displayed in the SolidWorks document, but it is not linked. 5.
Click OK to insert the file. NOTE: To change the display of the OLE object, click Edit, Object, Display Content, Display as Icon, or Reset Size.
To edit an OLE object with its application:
1.
Right-click the OLE object and select Edit with
2.
Edit the OLE object as desired, then close it and return to the SolidWorks document. The OLE object displays your edits.
To delete an OLE object:
Select the object and click Delete
, click Edit, Delete, or press the Delete key.
TIP: You can undo the deletion of any OLE object that is inserted into a SolidWorks drawing, assembly, or part document. Click Undo
or Edit, Undo Delete.
Display Content Displays the contents of an OLE object embedded in your SolidWorks document. To display the contents an OLE object:
1.
Select the OLE object.
2.
Click Edit, Object, Display Content. If the Object menu item is not displayed in the Edit menu, you may need to add it to the menu.
Display as Icon Displays an embedded OLE object as an icon. To display an OLE object as an icon:
1.
Select the OLE object.
2.
Click Edit, Object, Display as Icon. If the Object menu item is not displayed in the Edit menu, you may need to add it to the menu.
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Reset Size Restores an embedded OLE object to its original height and width. To reset an OLE object to its original size:
1.
Select the OLE object.
2.
Click Edit, Object, Reset Size. - or Right-click the OLE object and select Reset Size.
Inserting SolidWorks Data in Other Applications Using OLE, you can link or embed the SolidWorks document with any other OLE-compliant application. For example, you can place a part in a product data sheet you created with Microsoft Word. To use a SolidWorks document in another application:
1.
In the desired application, click Insert, Object. A dialog box appears that allows you to insert an existing object or to dynamically create and insert a new object. The dialog box that appears depends on the application you are using.
2.
Select the desired options, including whether you want to link the SolidWorks document to this document and whether you want the SolidWorks document to appear as an icon in this document. The SolidWorks document or its icon appears.
OLE Object Property Lets you specify the size and scale of the OLE object inserted in a SolidWorks document. To set the size or scale of an OLE object:
1.
Right-click the OLE object in the document and select Properties. The OLE Object Property dialog box appears.
2.
Type a decimal value for the Width, Height, or Scale into the corresponding boxes.
3.
Click OK.
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Chapter 2 SolidWorks Fundamentals
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3 Sketching
Sketching in SolidWorks Most SolidWorks features begin with a 2D sketch. For information about using sketches to create solid model geometry, see Features Overview. You can also create 3D sketches with SolidWorks. In a 3D sketch, the entities exist in 3D space; they are not related to specific sketch planes. The sketch topics include: •
Starting a new 2D sketch
•
Accessing and using the sketching tools
•
Taking advantage of inferencing
•
Deriving a new sketch from another
•
Dimensioning the sketch and adding and deleting geometric relations
•
Fully defining sketches
•
Sketching on the face of a part
•
Selecting a starting plane for a sketch
•
Deciding how complex the sketch should be
•
Creating a 3D sketch
You can toggle the display of sketches. The sketch entities in the graphics area are hidden or shown when you click View, Sketches. (All sketches must be closed.)
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Chapter 3 Sketching
Sketch Create a 2D sketch to build a 3D model. To create a 2D sketch in a new part:
1.
In a new part document, click a sketch tool on the Sketch toolbar, such as Rectangle
.
- or Click Sketch 2.
on the Sketch toolbar, or click Insert, Sketch.
Click a plane on which to create the sketch: Front Plane, Top Plane, or Right Plane. When you move the pointer to the edge of a plane, the edges are highlighted in red, and you can select the plane. You can also select a plane from the flyout FeatureManager design tree. The message Editing Sketch appears in the status bar at the bottom of the SolidWorks window. If you turned on the sketch grid, the grid appears in the graphics area.
3.
If you clicked Sketch
in step 1, click a tool on the Sketch toolbar to create the sketch.
4.
Create the sketch, and dimension the sketch entities.
5.
Click Exit Sketch
on the Sketch toolbar, click Insert, Exit Sketch, or click a sketch-based feature on
the Features toolbar (Extruded Boss/Base
, for example) to create a feature from the sketch.
To edit an existing sketch:
•
Click Sketch
on the Sketch toolbar, or click Insert, Sketch. Select an existing sketch to edit.
- or •
Right-click a sketch in the FeatureManager design tree, or right-click a sketch entity in the graphics area, and select Edit Sketch.
To create a new 2D sketch in a part with existing sketches:
1.
Click a sketch tool on the Sketch toolbar, such as Rectangle - or Click Sketch
on the Sketch toolbar, or click Insert, Sketch.
2.
Click a plane, face, or edge to add a new sketch.
3.
If you clicked Sketch
4.
Create the sketch, and dimension the sketch entities.
5.
Click Exit Sketch
in step 1, click a tool on the Sketch toolbar to create the sketch.
on the Sketch toolbar, click Insert, Exit Sketch, or click a sketch-based feature on
the Features toolbar (Extruded Boss/Base
3-2
.
, for example) to create a feature from the sketch.
Sketch on the Face of a Part To create new features on a part, you sketch on the face of the part where you want to locate the feature. To sketch on model faces:
1.
Select the planar model face on which you want to sketch.
2.
Click a sketch tool on the Sketch toolbar, click Sketch
, or click Insert, Sketch.
The following happens: •
•
A grid appears on the face that you selected (if you selected Display grid in Tools, Options, Document Properties, Grid/Snap). The message Editing Sketch appears in the status bar at the bottom of the SolidWorks window.
To sketch on a different face, exit the current sketch, select the new face, and open a new sketch.
Starting a New 2D Sketch When you open a new part document, first you create a sketch. You can start by selecting: •
A sketch entity tool (line, circle, and so on) or the Sketch tool
•
A plane
To start a sketch with a sketch entity tool or with the Sketch tool:
1.
Click a sketch entity tool (line, circle, and so on) on the Sketch toolbar. - or Click Sketch
on the Sketch toolbar, or click Insert, Sketch.
You are prompted to select a plane, and the three planes (Front Plane, Top Plane, and Right Plane) are displayed.
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Chapter 3 Sketching
2.
Select a plane. The plane rotates to the Normal to orientation.
3.
Create a sketch with the sketch entity tool, or select a tool on the Sketch toolbar and create a sketch.
To start a sketch with a plane:
Select a plane in the FeatureManager design tree and click a sketch entity tool on the Sketch toolbar. - or Select a plane in the FeatureManager design tree and click Sketch
on the Sketch toolbar.
The plane is displayed in Normal to orientation.
Starting the Sketch Does it matter where I start sketching? When you create a new part or assembly, the three default planes are aligned with specific views. The plane you select for your first sketch determines the orientation of your part. For example, if you choose *Front in the Orientation dialog box (or add a front view to a drawing), the view is normal to the Front Plane. If you open a new part and select a sketch tool, you are prompted to select a plane. If your first sketch is a top view, select the Top Plane.
3-4
•
If your first sketch is a left or right view, select the Right Plane.
•
You do not have to use one of the default planes for your first sketch; you can create a new plane at any angle. The orientation of views is still determined by the default planes, however.
•
You can reorient the part (to change Front to Top for example) with Update Standard Views Orientation dialog box.
in the
Starting the Sketch How complex should sketches be? In many cases, you can produce the same result by creating an extruded feature with a complex profile, or an extruded feature with a simpler profile and some additional features. (You often face this choice when planning the base feature for a part.) For example, if the edges of an extrusion need to be rounded, you can draw a complex sketch that contains sketch fillets (A), or draw a simple sketch and add the fillets as separate features later (B)
A Complex sketch
B Simple sketch Add fillet features Here are some things to consider: •
Complex sketches rebuild faster. Sketch fillets can be recalculated much faster than fillet features, but complex sketches can be harder to create and edit.
•
Simple sketches are more flexible and easier to manage. Individual features can be reordered and suppressed, if necessary.
Working in a Sketch In an open sketch, the SolidWorks window displays: •
The CommandManager with the Sketch toolbar active
•
Information about the sketch in the status bar
•
A sketch origin
•
A sketch grid
Status Bar The following information is in the status bar at the bottom of the sketch window: •
The coordinates of the pointer’s location when sketching an entity.
•
The state of the sketch: Over Defined, Under Defined, or Fully Defined. See Sketch Geometry Status.
•
The text, "Editing Sketch." This makes it obvious that you are in sketch mode if the sketch grid is off while you are working.
•
A description of a menu item or button when the pointer is over an item. This description is on the left side of the status bar.
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Chapter 3 Sketching
To display or hide the status bar:
Click View, Status Bar. Sketch Origin The sketch origin is displayed in red in an open sketch. Use the sketch origin to help you understand the coordinates of the sketch. Every sketch in the part has its own origin, so there usually are multiple sketch origins in a part. When a sketch is open, you cannot turn off the display of its origin.
Opening a New Sketch You must select a plane on which to create a new sketch. You can create a sketch on any of the default planes (Front Plane, Top Plane, or Right Plane), a created plane, a flat surface, or a face of a solid object. To open a new sketch on the Front Plane:
1.
Click Front Plane in the FeatureManager design tree.
2.
Click Sketch
to open a 2D sketch.
- or Click 3D Sketch
to open a 3D sketch.
To insert an alternate plane on which to sketch, see Creating a Construction Plane. You can also create a new sketch by extracting entities from an existing sketch.
Inferencing Pointers and Lines While sketching, notice that the appearance of the pointer changes to provide feedback about the pointer’s current task, position, and the geometric relations that are automatically applied. •
When you move the pointer along the length of any sketched curve, it first appears as an endpoint pointer, changes to the on-curve pointer, and then to a midpoint pointer, and so on.
•
When two lines intersect, the pointer changes to indicate the intersection.
•
When you sketch an arc, the pointer changes as it moves around the arc. The pointer provides information about dimensions as you sketch lines or arcs, such as the length, angle, or radius of the sketch entity.
•
3-6
•
When you select the various sketch or dimension tools, the pointer carries an appropriate symbol with it. Shown are the Rectangle, Circle, Spline, Point, Trim, Extend, and Dimension pointers, but there are many others.
As you sketch, the SolidWorks software monitors your activity and provides inferencing lines to help you work more efficiently. While sketching, notice that dashed inferencing lines align the pointer with lines or points that you have already sketched and with existing model geometry. •
When the endpoint of any line you are creating aligns with another point that you have already sketched, a dashed inferencing line indicates this alignment. This helps you align endpoints with each other so you can sketch without using a grid.
•
When you sketch arcs, inferencing lines and dimensions guide you to create the size and shape arc that you want.
TIP: Brown inference lines indicate that a relation is added automatically; blue inference lines indicate that no relation is added. However, if the inference line is blue and the pointer for a sketch entity (such as a line) includes the H (horizontal) or V (vertical) symbol, a relation is created.
Sketch Modes There are two modes for sketching in 2D: click-drag or click-click. SolidWorks responds to your cues to determine the mode as follows: •
If you click the first point and drag, you are in click-drag mode.
•
If you click the first point and release the pointer, you are in click-click mode. When you sketch entities in click-click mode and end a line or arc on the endpoint of an existing sketch entity, the tool stays active but does not show a preview from the last location.
Only click-drag mode is available for 3D sketching. When the Line and Arc tools are in click-click mode, they create a chain of segments as you click. To terminate a sketch chain, do one of the following: •
Double-click to terminate the chain of entities and leave the tool active.
•
Right-click and select End chain, which is the same as double-clicking.
•
Press Esc to terminate the chain and release the tool.
•
Move the pointer outside the view window to stop dragging. You can then choose another tool, which also terminates the chain.
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Chapter 3 Sketching
Autotransitioning You can transition from sketching a line to sketching a tangent arc, and vice versa, without selecting the arc tool. You can also toggle between line and arc with the A key. To autotransition between line and arc:
1.
Click Line
on the Sketch toolbar, or click Tools, Sketch Entities, Line and sketch a line.
2.
Click the endpoint of the line, then move the pointer away. The preview shows another line.
3.
Move the pointer back to the endpoint, then away again. The preview shows a tangent arc.
4.
Click to place the arc.
5.
Move the pointer away from the arc endpoint. The preview shows a line. You can draw a line or change to an arc as in Step 3. To toggle between line and arc without returning to the endpoint, press A.
Silhouettes You can select the silhouette edge of a rounded surface, such as a cylinder. Use the silhouette edge with the Convert Entities, Offset Entities, Smart Dimensions, or Add Relations tools. You can also select and reference silhouette vertices to add dimensions or relations. Silhouette edges are included in box-select operations. To select a silhouette edge:
1.
In an open sketch on a model face or plane (or in an active drawing view), move the pointer over a cylindrical face until the pointer changes to
.
To set silhouette edge visibility, click Tools, Options, System Options, Display/Selection, and select Dynamic highlight from graphics view. 2.
Select the highlighted edge.
Cutting, Copying, and Pasting in Sketches Cutting, Copying, and Pasting Sketch Entities You can cut and paste, or copy and paste, one or more sketch entities from one sketch to another or within the same sketch. In an open sketch, you can: •
Copy the sketch within the same document or to different documents. Hold down Ctrl while dragging the sketch. To copy one or more sketch entities, select the entities, then click Edit, Copy, or press Ctrl+C. Click in the graphics area, then click Edit, Paste or press Ctrl+V. The center of the sketch entities is placed where you clicked.
3-8
•
Move a sketch within the same sketch. Hold down Shift while dragging the sketch.
•
Move a sketch between different documents (the second document must have an open sketch). Hold down Ctrl and drag the sketch into the second document. Release Ctrl, hold down Shift, and drop the sketch.
Copying and Pasting Entire Sketches You can copy an entire sketch and paste it on a face in the current part, or you can paste it into a different sketch, or into a part, assembly, or drawing document. The target document must be open. When you copy a sketch, the relations are not copied. To copy and paste a sketch:
1.
Select the closed sketch in the FeatureManager design tree.
2.
Click Edit, Copy, or press Ctrl+C.
3.
Click in the sketch or document where you want to paste the center of the sketch.
4.
Click Edit, Paste, or press Ctrl+V.
Modify Sketch Use the Modify Sketch tool to move, rotate, or scale an entire sketch. To move, rotate, scale, or copy individual sketch entities, use the Move or Copy Entities, Rotate or Copy Entities, or Scale or Copy Entities tools. To move a sketch:
1.
Open a sketch or select a sketch in the FeatureManager design tree, and click Modify Sketch Sketch toolbar, or click Tools, Sketch Tools, Modify.
2.
In the dialog box:
on the
•
To move the sketch geometry incrementally, under Translate, type a value for X value and Y value and press Enter.
•
To move a specified point of the sketch to a specific location, under Translate, select Position selected point and click a point in the sketch. Type a value for X value and Y value and press Enter. The Modify Sketch tool translates the entire sketch geometry in relation to the model (including the sketch origin). The sketch geometry does not move relative to the origin of the sketch. - or -
•
To move a sketch in the graphics area, use the pointer: o o
3.
Press the left-mouse button
to move the sketch.
Point at the end points or center of the black origin to display one of three flip symbols. Right-click to flip the sketch on the X axis, the Y axis, or both.
Click Close.
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Chapter 3 Sketching
To rotate a sketch:
1.
Open a sketch or select a sketch in the FeatureManager design tree, and click Modify Sketch Sketch toolbar, or click Tools, Sketch Tools, Modify.
2.
In the dialog box: •
on the
Type a value for Rotate to set the rotation value and press Enter. - or -
•
Rotate a sketch in the graphics area with the pointer: o o
Press the right-mouse button
to rotate the s ketch around the black origin.
Point at the center point of the black origin to display a point symbol . Click and drag the center of rotation independently of the sketch, then rotate the sketch around the black origin.
You cannot move a sketch that has multiple external references. When a sketch has multiple external references, the pointer has a ? on the left button. 3.
Click Close.
To scale a sketch:
1.
Open a sketch or select a sketch in the FeatureManager design tree, and click Modify Sketch Sketch toolbar, or click Tools, Sketch Tools, Modify.
2.
In the dialog box, under Scale About, select: •
on the
Sketch origin. Applies a uniform scale about the origin of the sketch. - or -
• 3.
Moveable origin. Scales the sketch about the moveable origin.
Type a value for Factor, and press Enter. You cannot scale a sketch that has external references.
4.
Click Close.
Edit Sketch Edit Sketch opens an existing sketch so you can edit it. To edit a sketch:
1.
Right-click one of the following: •
the sketch in the FeatureManager design tree
•
a feature built from the sketch, either in the graphics area or in the FeatureManager design tree
•
a sketch entity in the graphics area For features built from multiple sketches (such as lofts and sweeps), right-click the sketch in the FeatureManager design tree.
2.
Select Edit Sketch.
3.
To close the sketch when you are finished editing, right-click in the sketch and select Exit Sketch. You can also edit an existing sketch by clicking Sketch
3-10
, then selecting the sketch to edit.
Exit Sketch You exit a sketch when you: •
Create a feature from a sketched profile. For example, when you extrude a base, boss, or a cut from a sketch.
•
Click Rebuild
•
Click Exit Sketch
•
Click Insert, Exit Sketch.
•
Select Exit Sketch from the shortcut menu.
•
Click Exit Sketch
•
Click Edit, Exit Sketch without Saving Changes.
on the Standard toolbar, or click Edit, Rebuild. on the Sketch toolbar.
or Cancel
in the Confirmation Corner.
Derived Sketch Derives a sketch from another sketch that belongs to the same part, or derives a sketch from another sketch in the same assembly. When you derive a sketch from an existing sketch, you are assured that the two sketches will retain the characteristics that they share in common. Changes that you make to the original sketch are reflected in the derived sketch. To derive a sketch from a sketch in the same part:
1.
Select the sketch from which you want to derive a new sketch.
2.
Hold the Ctrl key and click the face on which you want to place the new sketch.
3.
Click Insert, Derived Sketch. The sketch appears on the plane of the selected face, and the status line indicates that you are editing the sketch.
4.
Position the derived sketch by dragging and dimensioning it to the selected face. (The derived sketch is rigid and drags as a whole entity.)
To derive a sketch from a sketch in the same assembly:
1.
Right-click the part on which you want to place a derived sketch.
2.
Select Edit Part.
3.
Select the sketch (in the same assembly) from which you want to derive a new sketch.
4.
Hold the Ctrl key and click the face on which you want to place the new sketch.
5.
Click Insert, Derived Sketch. The sketch appears on the plane of the selected face, and you are editing the sketch.
6.
Position the derived sketch by dragging and dimensioning it to the selected face. (The derived sketch is rigid and drags as a whole entity.)
Note the following: •
If you delete a sketch from which a new sketch was derived, you are prompted that all derived sketches will automatically be underived. Click Yes or No.
•
You cannot add or delete sketch entities in a derived sketch. However, you can re-orient it with dimensions and geometric relations.
•
When you make changes to the original sketch, the derived sketch updates automatically.
•
To break the link between the derived sketch and its parent sketch, right-click the derived sketch in the FeatureManager design tree and select Underive. (After the link is broken, the derived sketch no longer updates when you change the original sketch.)
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Chapter 3 Sketching
Sketch Plane References When you delete a parent feature that has child features built from sketches, you have the option to keep the child features and have the sketch plane references dangle. You can dangle a sketch plane reference by editing the sketch plane definition and removing the plane definition. To create dangling sketch plane references:
1.
Select a parent feature that has a child feature. The child must be a sketch-based child, and the sketch must be dependent on the parent.
2.
Press the Delete key.
3.
In the dialog box, clear Also delete all child features, then click Yes. The dialog box warns that the plane is missing for the sketch used to create the child feature.
4.
Click Close. In the FeatureManager design tree, the part icon, the child feature, and the sketch used to create the child feature display warning icons that indicate the sketch plane is dangling. You can use the Edit Sketch Plane command to replace the reference plane.
Edit Sketch Plane Changes the sketch plane. To change the plane of a sketch:
1.
Select the sketch in the FeatureManager design tree, and click Edit, Sketch Plane. - or Right-click the sketch in the FeatureManager design tree, and select Edit Sketch Plane.
2.
Select a new plane in the FeatureManager design tree or select a new planar face in the model for Sketch Plane/Face
3.
Click OK
. .
Shaded Sketch Plane When you are editing a sketch in Shaded With Edges or Shaded mode, you can display the sketch plane as a shaded plane. To turn the shaded sketch plane on or off:
Click Tools, Options, System Options, Sketch. Select Display plane when shaded. If the display is slow due to the shaded plane, it may be because of the Transparency options. With some graphics cards, the display speed improves if you use low transparency. To set a low transparency, click Tools, Options, System Options, Performance and clear High quality for normal view mode and High quality for dynamic view mode.
3-12
Reference Plane Normal to Edge You can sketch on a reference plane, created automatically, normal to an edge. To sketch on a reference plane normal to an edge:
1.
In a part, select an edge and click Sketch
.
A reference plane normal to the selected edge is created at the end point of the edge closest to the selected area. The origin for the new plane appears at the edge's end point. 2.
Sketch an entity such as a rectangle or circle on the plane.
3.
Create a feature such as a boss or a cut.
Example using a reference plane normal to an edge: Select edge
Plane with origin at endpoint of edge
Sketch on plane
Extruded cut normal to plane
Sketch Tools Align Grid Aligns the sketch grid with the model edge that you select. To align the grid to a model edge:
1.
Open a sketch on a model face.
2.
Click Tools, Sketch Tools, Align, Grid.
3.
Click the model edge to which you want to align the grid.
4.
In the dialog box, click Apply to apply the change. The grid shifts to align with the edge you selected and the origin is placed at the end of the edge closest to where you clicked.
5.
Click OK to accept the change. - or Click Close to close the dialog box. If you previously clicked Apply, the change is saved; if you did not click Apply, the dialog box closes without change.
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Chapter 3 Sketching
Automatic Inferencing Lines You can turn off automatic inferencing lines while editing a sketch or while sketching in a drawing document. If automatic inferencing lines are turned off, you no longer automatically infer to all model edges, active sketch entities, or non-active sketch entities. Turning off inferencing lines in a complex sketch or drawing may improve sketching performance and reduce the chance of unwanted relations. NOTE: To inference to temporary axes, make the temporary axes visible. Click View, Temporary Axes. To turn off the automatic inferencing lines:
Click Tools, Sketch Settings, Automatic Inferencing Lines to turn on or off the automatic inferencing lines. In drawings, you must activate the inferencing lines for current sketch entities. You have to activate the inferencing lines for each new entity that you sketch. To activate the inferencing lines for an entity in a drawing:
1.
Click a sketch entity tool, such as Line
.
2.
Move the pointer over the entity you want to infer to. The color of the pointer changes to orange
once the inferencing lines are active for the entity.
To wake up the edges of a model to use inferencing:
1.
Open a sketch on the planar face of the model.
2.
Click a sketch entity tool, such as Line
3.
Move the pointer over the model edge to activate it.
.
If the model is cylindrical, the center point appears as a black cross. Example: To infer to the center of a cylinder, select a sketch entity tool and wake up the edges of the cylinder. Then you can infer to the center point.
Automatic Solve Specifies whether SolidWorks should automatically do the computation to solve the sketch geometry of your part as you create it. To turn automatic computation on or off:
Click Tools, Sketch Settings, Automatic Solve. A check mark next to the menu item means that computations are solved automatically. NOTE: When you are in the process of changing many dimensions in an active sketch, you may want to turn off the Automatic Solve option temporarily.
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No Solve Move No Solve Move
lets you move sketch entities without solving the dimensions or relations in the sketch.
If dimensions or relations exist between the selected entities and other sketch entities or model geometry, a warning message appears. The message asks if you want to delete the constraints caused by the dimensions or relations: •
If you click Yes, the constraints are deleted, and the entities are moved.
•
If you click No, the constraints are not deleted, and the selected entities are copied to the location to which you moved them.
To use No Solve Move:
•
Click No Solve Move
on the Sketch toolbar.
•
Click Tools, Sketch Settings, No Solve Move.
Move or Copy PropertyManager Move, rotate, and scale items (or copies of items) in sketches and drawings. These operations do not create relations. Operation Move, Rotate, or Scale. Determines the operation you want to perform. This is pre-selected depending on which tool you clicked. For example, if you clicked Move or Copy Entities , then Move is selected. Sketch items or annotations
. Select from the following:
•
In sketches: sketch entities and some annotations (those that can be cut, copied, and pasted)
•
In drawings: sketch entities and all annotations
Copy. Copies the entities in Sketch items or annotations. Number of Copies (available when Copy is selected). Specifies the number of times to copy the entities in Sketch items or annotations. Click in the graphics area to create the number of instances specified. Keep relations (available when Move or Rotate is selected). Maintains relations between sketch entities. When cleared, relations are broken only between selected entities and those that are not selected; relations among the selected entities are maintained. Scale Factor (available when Scale is selected). Specifies the scale factor for the selected entities. The scale factor increases arithmetically (not geometrically). Base Point Base point . Defines the point from which the items are moved, scaled, or rotated. Click in the graphics area or specify coordinates to define the base point. Start X coordinate
. Displays the base point X coordinate.
Start Y coordinate
. Displays the base point Y coordinate.
Destination (available when Move is selected) Relative offset. Sets all geometry to move by the same relative amount. Delta X
(available when Relative offset is selected). Determines the X destination coordinate.
Delta Y
(available when Relative offset is selected). Determines the Y destination coordinate.
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Chapter 3 Sketching
Destination . Defines the point to which the items are moved. Click in the graphics area or specify coordinates to define the destination point. End X coordinate
. Determines the X destination coordinate.
End Y coordinate
. Determines the Y destination coordinate.
Rotate (available when Rotate is selected) Angle
. Specifies the angle of rotation.
Check Sketch for Feature Usage Check a sketch for errors that might prevent it from creating a feature. For each Feature usage type, its required sketch Contour type is displayed. If you select a new Feature usage type from the list, the corresponding Contour type changes. Each Contour type forces a different set of checks on the sketch in addition to the general checks that are common to all contour types. To check a sketch for feature usage:
1.
In an open sketch, click Tools, Sketch Tools, Check Sketch For Feature. In the dialog box, Feature usage lists all of the ways to use the sketch in a feature:
2.
•
If the sketch was used to create a feature, the feature type is displayed in Feature usage.
•
If the sketch was not used to create a feature, <none> is displayed in Feature usage and the contour is checked for errors that are common to all contour types.
Click Check. The sketch is checked according to the contour type required by the feature type listed in the Feature usage box. If the sketch passes the checks, a No problems found message appears. If there is an error, a message describes the error and, if appropriate, the error is highlighted. It finds one error for each check.
3.
To check your sketch for possible use in other feature types, select another type in Feature usage and click Check.
4.
Click Reset to return to the original Feature usage type.
5.
Click Close. Alternatively, the dialog box closes automatically when you exit the sketch, rebuild, change to a new document, and so on.
Allowed Contour Types Contour type:
Features that use the contour type:
Single Open
Base Extrude Thin, Base Revolve Thin, Boss Extrude Thin, Boss Revolve Thin, Cut Extrude, Cut Extrude Thin, Cut Revolve Thin, Loft Guide, SheetMetal Base Flange, Surface Loft Section, Sweep Path Or Guide, Sweep Section
Single Closed
Cut Extrude Thin, Loft Guide, Loft Section, Surface Loft Section, Sweep Path Or Guide
Multiple Disjoint Closed
Base Extrude, Base Extrude Thin, Base Revolve, Base Revolve Thin, Boss Extrude, Boss Extrude Thin, Boss Revolve, Boss Revolve Thin, Cut Extrude, Cut Revolve, Cut Revolve Thin, SheetMetal Base Flange, Sweep Section
General
Mold Parting Surface, Rib, SheetMetal 3D Bend, Surface Extrude, Surface Revolve, Surface Sweep Section, <none> (The contour is checked for errors that are common to all contour types.)
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Sketch Contour Single Open Single open contours can be used for extrudes, revolves, sections, paths, guides, and sheet metal. Typical open contours are sketched with lines or splines.
Sketch Contour Single Closed Single closed contours can be used for extrudes, revolves, sections, paths, guides, and sheet metal. Typical closed contours are sketched with circles, squares, closed splines, and other closed geometric shapes.
Sketch Contour Multiple Contained Closed Multiple contained closed contours can be used for extrudes, revolves, and sheet metal. If there is more than one contour, one contour must contain the rest. Typical multiple contained closed contours are sketched with circles, rectangles, and other closed geometric shapes.
Sketch Contour Multiple Disjoint Closed Multiple disjoint closed contours can be used for extrudes, revolves, and sheet metal; for example, to cut several holes on the face of a part. Typical multiple disjoint closed contours are sketched with circles, rectangles, and other closed geometric shapes.
Circular Sketch Step and Repeat Use the Circular Sketch Step and Repeat tool to create a circular pattern of sketch entities. To create a circular pattern of sketch entities:
1.
Open a sketch on a model face and sketch an item to repeat.
2.
With the sketch entities selected, click Circular Sketch Step and Repeat click Tools, Sketch Tools, Circular Step and Repeat.
on the Sketch toolbar, or
You can also select the entities after you click Circular Sketch Step and Repeat. The names of the selected sketch entities appear under Items to repeat. 3.
Under Arc, set: •
Radius. Measures the distance from the center of the pattern to a center point or vertex on the selected entities. If you select Fixed, the Radius is displayed as an explicit value when the pattern is complete.
•
Angle. Measures the angle from the center of the selected entities to the center point or vertex of the pattern.
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Chapter 3 Sketching
4.
Under Center, either: •
Set values for the X and Y coordinates to position the center point or vertex of the pattern. - or -
• 5.
6.
Drag the center point or vertex of the pattern in the graphics area. The X and Y coordinates update accordingly.
Under Step, set: •
Number. Specifies the number of pattern instances, including the original sketch entity.
•
Total angle (available when Equal is selected). Specifies the angle between the first and last instance in the pattern.
•
Spacing (available when Equal is cleared). Specifies the angle between the pattern instances.
•
Reverse Rotation
•
Equal. Sets an equal distance between each pattern instance.
•
Constrain spacing (available when Equal is cleared). Constrains the Total angle between pattern instances in the pattern.
. Reverses the pattern rotation.
If you type values for Radius, Angle, X or Y, Number, Spacing, or Total Angle, (instead of clicking the buttons) you must click Preview to see a preview of the pattern. You can then adjust any of the values and click Preview again. You can drag one of the selection points to set the radius and angle and the spacing between instances.
7.
Select a number in Instances and press Delete to delete that instance in the pattern. The number then appears in Instances deleted. To return the instance to the pattern, select the number in Instances deleted and press Delete.
8.
Click OK.
To edit a circular sketch step and repeat pattern feature:
1.
Right-click the pattern sketch and select Edit Sketch.
2.
Select an instance and click Tools, Sketch Tools, Edit Circular Step and Repeat. - or Right-click an instance and select Edit Circular Step and Repeat.
3.
Set the Number of pattern instances, then click OK. Additionally, you can modify the pattern in the following ways:
4.
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•
Double-click the angle dimension and change the angle in the Modify dialog box (available only if you cleared Equal and selected Constrain spacing when you created the pattern).
•
Drag the center point of the pattern to a new location (available only if you cleared Equal when you created the pattern).
•
Change the rotation of the pattern by dragging the center point of the pattern or by selecting a pattern instance and dragging it.
•
Change the radius of the pattern arc by dragging the first instance of the pattern by its center point or vertex (available only if you cleared Equal when you created the pattern).
•
Select and delete individual pattern instances.
Exit the sketch.
Constrain Spacing and Fixed Options Circular Sketch Step and Repeat Pattern •
Select the Constrain spacing check box to constrain the Total Angle between pattern instances in the circular pattern. After the pattern is created, you can change the angle (or spacing) by double-clicking the dimension and using the Modify dialog box. (This option is only available if the Equal check box is not selected.)
•
The Fixed option is related to the Radius value. If you select the Fixed check box, the result is as follows: o
The radius is displayed as an explicit dimension.
o
You can control the radius by double-clicking the dimension and using the Modify dialog box.
Return to Circular Sketch Step and Repeat.
Constrain All Sets constraints on the sketch entities of an unconstrained imported .DXF or .DWG drawing. To solve relations in an imported drawing:
1.
Import a sketch from a .DXF or .DWG drawing.
2.
Click Tools, Relations, Constrain All. The command tries to solve all the apparent relations in the sketch and reports the number of constraints that were added to the sketch.
Contour Selection Select sketch contours and model edges, and apply features to them. This allows you to use a partial sketch to create features. To select and extrude contours:
1.
In an active sketch, right-click in the graphics area and select Contour Select Tool. The pointer changes to
2.
.
Select a contour. The contour can include model edges. To select multiple contours, hold down Ctrl.
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Chapter 3 Sketching
3.
Click a feature to apply to the selected contours; Extruded Boss/Base, for example.
A tooltip appears when a contour cannot be selected for one of the following reasons: •
The part has too many edges.
•
Edges are created on offset planes.
•
Edges are chamfered.
•
Edges are filleted.
Contour selection is also restricted as follows: •
•
When reusing a sketch, you can select only on the original face. If, for example, part of the face has been extruded, the tool does not recognize the new face. You can select contours only on the face with the sketch. If, for example, the face with the sketch is cut by a solid object (as shown at right), the tool can select the part of the face still visible but does not recognize the solid object.
Example of Sketch Reuse
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Sketch used for revolve surface
Same sketch reused for surface extrude
Sketch used for sweep thin feature
Same sketch used for boss extrude thin feature
Close Sketch to Model Closes a sketch with an open profile, using existing model edges. To use an open profile sketch to extrude using existing model edges:
1.
Open a sketch on a model face.
2.
Sketch an open profile with endpoints that are coincident with model edges on the same face boundary.
3.
Click Tools, Sketch Tools, Close Sketch to Model. An arrow points in the direction in which the sketch will close. (The extruded boss will either be within the sketch lines or outside of the sketch lines.)
4.
In the dialog box, select Reverse direction to close the sketch, if necessary.
5.
Click Yes when the arrow points in the correct direction.
6.
Click Extruded Boss/Base
or Insert, Boss, Extrude,
or Extruded Cut or Insert, Cut, Extrude, and specify the End Condition in the PropertyManager. 7.
Click OK
.
Construction Geometry You can convert sketch entities in a sketch or drawing to construction geometry. Construction geometry is used only to assist in creating the sketch entities and geometry that are ultimately incorporated into the part. Construction geometry is ignored when the sketch is used to create a feature. Construction geometry uses the same line style as centerlines. To convert sketch entities to construction geometry:
In an open sketch, select one or more sketch entities and do one of the following: •
Select For construction in the PropertyManager.
•
Click Construction Geometry
•
Click Tools, Sketch Tools, Construction Geometry.
•
Right-click a sketch entity and select Construction Geometry (drawings only).
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on the Sketch toolbar.
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Chapter 3 Sketching
Convert Entities You can create one or more curves in a sketch by projecting an edge, loop, face, curve, or external sketch contour, set of edges, or set of sketch curves onto the sketch plane. To convert an entity:
1.
In an open sketch, click a model edge, loop, face, curve, external sketch contour, set of edges, or set of curves.
2.
Click Convert Entities
on the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities.
The following relations are created: o
o
On Edge. Created between the new sketch curve and the entity, which causes the curve to update if the entity changes. Fixed. Created internally on the endpoints of the sketch entity so the sketch remains in a "fully defined" state. This internal relation is not displayed when you use Display/Delete Relations. Remove the Fixed relation by dragging the endpoints.
Detach Segment on Drag You can detach a segment (line, arc, ellipse, or spline) from the other entities it is attached to in a sketch, if dimensions or relations do not prevent dragging. Detach Segment on Drag is not available in 3D sketches. To detach a sketch segment:
1.
In an open part, click Tools, Sketch Settings, Detach Segment on Drag.
2.
Select the entity that you want to detach from another sketch entity and drag it to a new location. Detach Segment On Drag does not delete relations. Delete relations before you drag an entity to detach. See Sketch Relations PropertyManager.
Extend Entities You can add to the length of a sketch entity (line, centerline, or arc). Typically, you use Extend Entities to extend a sketch entity to meet another sketch entity. To extend a sketch entity:
1.
In an open sketch, click Extend Entities The pointer changes to
2.
on the Sketch toolbar, or click Tools, Sketch Tools, Extend.
.
Move the pointer over the sketch entity to extend. The selected entity appears in aqua, and a preview appears in pink in the direction to extend the entity.
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3.
If the preview extends in the wrong direction, move the pointer to the other half of the line or arc.
4.
Click the sketch entity to accept the preview.
Face Curves You can extract iso-parametric (UV) curves from a face or surface. Applications of this functionality include extracting the curves for imported surfaces and then performing localized cleanup using the face curves. You can specify a mesh of evenly spaced curves or a position that creates two orthogonal curves.
Mesh
Position
Each curve created by this process becomes a separate 3D sketch. However, if you are editing a 3D sketch when you invoke the Face Curves tool, all extracted curves are added to the active 3D sketch. To extract iso-parametric curves:
1.
Click Face Curves
or Tools, Sketch Tools, Face Curves, then select a face or surface.
- or Select a face or surface, then click Face Curves
or Tools, Sketch Tools, Face Curves.
A preview of the curves appears on the face. The curves are one color in one direction and another color in the other direction. The colors correspond to the colors in the Face Curves PropertyManager. The name of the face appears in the Face 2.
Under Selections, choose either: o o
3.
Mesh - evenly spaced curves. Specify an integer number of curves for Direction 1 and Direction 2. Position - the intersection of two orthogonal curves. Drag the position in the graphics area or specify the percentage distance from the bottom for Direction 1 and from the right for Direction 2. •
Direction 1 On/Off or Direction 2 On/Off check box - clear if the curve is not required.
•
Position Vertex - select a vertex or point to specify the intersection of the two curves. This vertex cannot be dragged.
Under Options, select or clear: o o
4.
box.
Constrain to model - when selected, the curves are updated if the model changes. Ignore holes - useful for imported surfaces with internal gaps or loops. When selected, the curves are generated across holes as though the surface were intact. When cleared, the curves stop at the edges of holes.
Click OK
.
The curves appear as 3D sketches in the FeatureManager design tree. NOTE: If surface edge information cannot be matched, edge curves cannot be generated. The error message states: "Failed to create X out of X face curves. Please consider using convert entities." You can generate the missing curves by opening a 3D sketch and using the Convert Entities
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sketch tool.
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Chapter 3 Sketching
Intersection Curve Intersection Curve
opens a sketch and creates a sketched curve at the following kinds of intersections:
•
A plane and a surface or a model face
•
Two surfaces
•
A surface and a model face
•
A plane and the entire part
•
A surface and the entire part
You can use the resulting sketched intersection curve in the same way that you use any sketched curve, including the following tasks: •
Measure thickness at various cross sections of a part. (See steps below.)
•
Create sweep paths that represent the intersection of a plane and the part.
•
Make sections out of imported solids to create parametric parts.
To use the sketched curve to extrude a feature, the sketch that opens must be a 2D sketch. Other tasks can be performed using a 3D sketch. •
To open a 2D sketch, select the plane first then click Intersection Curve.
•
To open a 3D sketch, click Intersection Curve first then select the plane.
To measure the thickness of a cross section of a part:
1.
With a part open, click Intersection Curve Curve. A 3D sketch opens (because you clicked
2.
on the Sketch toolbar, or Tools, Sketch Tools, Intersection
before selecting a plane).
Select the intersecting items: •
Select a plane that intersects a face of the part.
•
Click the face of the part. A sketched spline appears at the intersection of the plane and the top face.
3.
Rotate the part, then click the opposite (inside) face of the part. Another sketched spline appears on the inside face.
You can also select the part in the FeatureManager design tree. A sketched spline appears on every face where the plane intersects.
3-24
4.
Click Tools, Measure and measure the distance between the two sketched splines.
Linear Sketch Step and Repeat Use the Linear Sketch Step and Repeat tool to create a linear pattern of sketch entities. To create a linear pattern of sketch entities:
1.
Open a sketch on a model face and sketch one or more items to repeat.
2.
With the sketch entities selected, click Linear Sketch Step and Repeat Tools, Sketch Tools, Linear Step and Repeat.
on the Sketch toolbar, or click
You can also select the sketch entities after you click Linear Sketch Step and Repeat. The names of the selected sketch entities appear in Items to repeat. 3.
4.
Under Direction 1, set: •
Number. Total number of pattern instances, including the original sketch.
•
Spacing. Distance between pattern instances. If you select Fixed, the Spacing value is displayed as an explicit value when the pattern is complete.
•
Angle. Angle of rotation for the pattern.
•
Reverse Direction 1
. Reverses the direction of the pattern.
If you type values for Number, Spacing, or Angle, (instead of clicking the buttons) you must click Preview to see a preview of the pattern. You can then adjust any of the values and click Preview again. You can also change the Spacing and Angle by dragging the selection point in the pattern preview.
5.
To create a pattern in two directions, repeat step 3 and set values for Direction 2. In two-directional patterns, you can select Constrain angle between axes.
6.
Select a position (column, row) in Instances and press Delete to delete that instance in the pattern. The position appears in Instances deleted. To return the instance to the pattern, select the position in Instances deleted and press Delete.
7.
Click OK.
To edit the linear sketch step and repeat pattern feature:
1.
Right-click the pattern sketch and select Edit Sketch.
2.
Select an instance and click Tools, Sketch Tools, Edit Linear Step and Repeat. - or Right-click an instance and select Edit Linear Step and Repeat.
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Chapter 3 Sketching
3.
Change the Number of instances in one or both directions, and click OK. Additionally, you can modify the pattern in the following ways:
4.
•
Drag a point or vertex on one of the pattern instances.
•
Change the angle of the pattern by double-clicking the angle and changing its value in the Modify dialog box.
•
Add dimensions and change their values using the Modify dialog box.
•
Add relations to the pattern instances.
•
Select and delete individual pattern instances.
Exit the sketch to complete the new pattern feature.
Fixed Spacing in Linear Sketch Step and Repeat The Fixed check box in the Linear Sketch Step and Repeat dialog box applies to the Spacing value for each linear direction. If you select the Fixed check box before creating the linear array, the result is as follows: •
Corresponding points on the first and second instance are joined with a construction line, and this line is dimensioned.
•
The resulting dimension is displayed as an explicit sketch dimension.
•
You can control the spacing by double-clicking the dimension and using the Modify dialog box.
Constrain Angle in Linear Sketch Step and Repeat The Constrain angle between axes check box is available if you define two pattern directions. If you select Constrain angle between axes, the result is as follows: •
The angle between the two directions is defined by a construction line through corresponding points on the first and second instance, in each direction.
•
After the pattern is created, by clicking OK, you can change this angle by double-clicking the dimension and using the Modify dialog box.
Return to Linear Sketch Step and Repeat.
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Mirror Entities You can mirror sketch entities around a centerline. When you create mirrored entities, the SolidWorks software applies a symmetric relation between each corresponding pair of sketch points (the ends of mirrored lines, the centers of arcs, and so on). If you change a mirrored entity, its mirror image also changes. Mirror Entities is not available in 3D sketches. To mirror existing sketch entities:
1.
In an open sketch, click Centerline
on the Sketch toolbar and sketch a centerline.
2.
Select the centerline and the items you want to mirror.
3.
Click Mirror Entities
on the Sketch toolbar, or click Tools, Sketch Tools, Mirror.
To mirror sketch entities as you sketch them:
1.
Click Centerline
2.
Click Mirror Entities
on the Sketch toolbar and sketch a centerline. on the Sketch toolbar, or click Tools, Sketch Tools, Mirror. Symmetry symbols
appear at both ends of the centerline. 3.
Create the sketch entities that you want to mirror. The entities are mirrored as you sketch them.
4.
To turn mirroring off, click Mirror Entities
again.
Move, Rotate, Scale, or Copy Move, rotate, scale, or copy items in sketches and drawings with the Move or Copy PropertyManager. The Move or Copy operations do not create relations. To create relations, you must add relations. To move or copy sketch entities:
1.
In an open sketch, click Move or Copy Entities Move or Copy.
2.
To copy the sketch entities, in the PropertyManager, under Operation, select Copy, and set the Number of Copies
3.
on the Sketch toolbar, or click Tools, Sketch Tools,
to create.
Select the sketch entities or annotations to move. In parts and assemblies, you can select any annotations that can be cut, copied, and pasted. In drawings, you can select all annotations. The pointer changes to , which indicates that the entities are ready to move. If you selected the entities before you clicked Move or Copy Entities, this pointer does not appear; go to step 5.
4.
In the graphics area, right-click. The pointer changes to
5.
.
Click to set the base point.
The pointer changes to
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Chapter 3 Sketching
6.
Click to set the destination point.
7.
The sketch entities are set and the PropertyManager closes. If Keep Visible
is selected, the pointer changes to
(if Copy is selected) or
(if Copy is
cleared). With the •
pointer, you can: Right-click to accept the move and close the PropertyManager. - or -
•
With the
Move the pointer away from the destination point. The pointer changes to additional sketch entities.
, and you can move
pointer, you can:
•
Click to place additional copies of the sketch entities.
•
Click OK
to close the PropertyManager.
To rotate or copy sketch entities:
1.
In an open sketch, click Rotate or Copy Entities Rotate or Copy.
on the Sketch toolbar, or click Tools, Sketch Tools,
2.
To copy the sketch entities, in the PropertyManager, under Operation, select Copy, and set the Number of
3.
Copies to create. Select the sketch entities or annotations to rotate. In parts and assemblies, you can select any annotations that can be cut, copied, and pasted. In drawings, you can select all annotations. The pointer changes to , which indicates that the entities are ready to rotate. If you selected the entities before you clicked Rotate or Copy Entities, this pointer does not appear; go to step 4.
4.
In the graphics area, right-click. The pointer changes to
5.
Click to set the base point. This is the point about which to rotate the entities. The pointer changes to
6.
.
.
Move the pointer to set the rotation angle, then click and drag the pointer to rotate the sketch entities. When you drag the pointer, angle snap increments vary depending on the distance of the pointer from the base point. Exact angle values are displayed when you inference to model geometry.
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7.
Right-click to accept the rotation and to close the PropertyManager. - or If Keep Visible
is selected, click and drag the pointer to rotate the same sketch entities or to rotate
additional copies of the sketch entities. When you right-click to accept the rotation, Angle Click OK
is set to 0.
, or right-click again to close the PropertyManager.
To scale or copy sketch entities:
1.
In an open sketch, click Scale or Copy Entities Scale or Copy.
2.
To copy the sketch entities, in the PropertyManager, under Operation, select Copy, and set the Number of Copies
on the Sketch toolbar, or click Tools, Sketch Tools,
to create.
If you select Copy, and:
3.
•
the scale of the copied sketch entity is too large or too small, the number of copies is reduced.
•
set the Scale Factor , then change the Number of Copies accommodate the copies specified.
, the Scale Factor updates to
Select the sketch entities or annotations to scale. In parts and assemblies, you can select any annotations that can be cut, copied, and pasted. In drawings, you can select all annotations. The pointer changes to , which indicates that the entities are ready to scale. If you selected the entities before you clicked Scale or Copy Entities, this pointer does not appear; go to step 5.
4.
In the graphics area, right-click. The pointer changes to
5.
.
Click to set the base point. This is the point about which to scale the entities. The pointer changes to
6.
Set the Scale Factor
. .
The Scale Factor increases arithmetically (not geometrically). The example shows a sketch entity with copies at scale factors of 2, 3, and 4.
7.
Right-click to accept the scaled entity and close the PropertyManager. If Keep Visible
is selected, Scale Factor
is set to 1.0, and you can continue to scale sketch
entities. Click OK to close the PropertyManager. (If Scale Factor is not set to 1.0, click OK to close the PropertyManager.)
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Chapter 3 Sketching
Offset Entities Use the Offset Entities tool to create sketch curves offset from one or more selected sketch entities, edges, loops, faces, curves, set of edges, or set of curves by a specified distance. The selected sketch entity can be construction geometry. The offset entities can be bidirectional. The SolidWorks software creates an on-edge relation between each original entity and the corresponding sketch curve. If the original entity changes, then the offset curve also changes when you rebuild the model. To create a sketch curve offset from a model edge:
1.
In an open sketch, select one or more sketch entities, a model face, a model edge, or external sketch curves.
2.
Click Offset Entities
3.
In the PropertyManager, under Parameters, set:
on the Sketch toolbar, or click Tools, Sketch Tools, Offset Entities.
When you click in the graphics area, the Offset Entity is complete. Set the Parameters before you click in the graphics area.
4.
•
Offset Distance . Set a value to offset the sketch curve by a specified distance. You can also hold down the mouse button and drag the pointer in the graphics area to see a dynamic preview. When you release the mouse button, the Offset Entity is complete.
•
Reverse. Changes the direction of a one-directional offset.
•
Select chain. Creates an offset of all contiguous sketch entities.
•
Bi-directional. Creates offset entities in two directions.
Click OK
or click in the graphics area.
To change the size of a sketch curve offset:
Double-click the offset’s dimension and change the value. In a bi-directional offset, change the dimensions of the two offsets individually.
Override Dims on Drag/Move You can override dimensions by dragging sketch entities. The sketch dimensions update at the end of the drag. They remain driving dimensions and update in the part, assembly, and drawing. You can set an option to enable this functionality in all documents, or you can enable it for the active document only. To set the option for all documents:
1.
Click Tools, Options, System Options, Sketch.
2.
Select Override Dims on Drag/Move and click OK.
To enable the functionality in the active document:
Click Tools, Sketch Settings, Override Dims on Drag/Move. To move a dimensioned sketch entity:
1.
Select Override Dims on Drag/Move by one of the above methods.
2.
In an open sketch, select a sketch entity.
3.
Drag the sketch entity. - or Click Tools, Sketch Tools, Move or Copy, and set the values in the Move or Copy PropertyManager.
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Sketch Chamfer The Sketch Chamfer tool applies a chamfer to adjacent sketch entities in 2D and 3D sketches. This tool is available for both 2D and 3D sketches. The Chamfer tool on the Features toolbar chamfers entities such as edges in parts. To create a sketch chamfer:
1.
In an open sketch, click Sketch Chamfer Chamfer.
on the Sketch toolbar, or click Tools, Sketch Tools,
2.
In the PropertyManager, set the Chamfer Parameters as necessary.
3.
In the graphics area, select the two sketch entities to chamfer. To select the sketch entities, you can: •
Hold Ctrl and select two sketch entities.
•
Select a vertex.
The chamfer is applied immediately. 4.
Click OK to accept the chamfer, or click Undo to remove the chamfer. You can undo a sequence of chamfers in reverse order.
Sketch Chamfer Parameters •
•
Angle-distance o
Distance 1
is applied to the first sketch entity selected.
o
Direction 1 Angle
is applied from the first sketch entity toward the second.
Distance-distance o
Equal distance check box selected. Distance 1
o
Equal distance check box cleared. Distance 1 Distance 2
Angle-distance
is applied to both sketch entities. is applied to the first sketch entity selected.
is applied to the second sketch entity selected. Distance-distance
Equal distance
Sketch Fillet The Sketch Fillet tool trims away the corner at the intersection of two sketch entities to create a tangent arc. This tool is available for both 2D and 3D sketches. The Fillet tool on the Features toolbar fillets entities such as edges in parts. Example of Sketch Fillets The four corners of the rectangle are filleted with the same radius and with Keep constrained corners selected.
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Chapter 3 Sketching
To create a fillet in a sketch:
1.
In an open sketch, click Sketch Fillet
2.
Set the properties in the Sketch Fillet PropertyManager.
3.
Select the sketch entities to fillet. (You can select non-intersecting entities. The entities are extended, and the corner is filleted.) To select the sketch entities, you can:
4.
on the Sketch toolbar, or Tools, Sketch Tools, Fillet.
•
Hold Ctrl and select two sketch entities.
•
Select a corner.
Click OK to accept the fillet, or click Undo to remove the fillet. You can undo a sequence of fillets in reverse order.
Sketch Fillet PropertyManager The Sketch Fillet PropertyManager controls the following properties during creation of a sketch fillet. The Fillet tool on the Features toolbar fillets entities such as edges in parts. Fillet Parameters •
Radius
. Controls the fillet radius.
Consecutive fillets with the same radius are not dimensioned individually; they have an automatic Equal relation with the first fillet in the series. •
Keep constrained corners. Maintains the virtual intersection point if the vertex has dimensions or relations. When cleared, and if the vertex has dimensions or relations, you are asked if you want to delete those geometric relations when the fillet is created.
•
Undo. Undoes the last fillet. You can undo a sequence of fillets in reverse order.
Split Entities You can split a sketch entity to create two sketch entities. Conversely, you can delete a split point to combine two sketch entities into a single sketch entity. Use two split points to split a circle, full ellipse, or a closed spline. You can dimension to a split point. Also, you can insert parts at split points in a routing assembly. To split a sketch entity:
1.
In an open sketch, click Split Entities Entities. The pointer changes to
2.
on the Sketch toolbar, or click Tools, Sketch Tools, Split
.
Click the sketch entity at the location where you want the split to occur. The sketch entity splits into two entities, and a split point is added between the two sketch entities.
To combine two split sketch entities into one:
In an open sketch, click the split point and press Delete.
Trim Entities Use Trim Entities to:
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•
Trim a line, arc, circle, ellipse, spline, or centerline to its intersection with a line, arc, circle, ellipse, spline, or centerline.
•
Delete a line, arc, circle, ellipse, spline, or centerline.
•
Extend a sketch segment until it is coincident with another entity.
To delete a sketch entity:
1.
In an open sketch, click Trim Entities
2.
Move the pointer red, then click.
on the Sketch toolbar, or click Tools, Sketch Tools, Trim.
over a sketch until the sketch segment that you want to trim (delete) is highlighted in
The segment is deleted up to its intersection with another sketch segment (line, arc, circle, ellipse, spline, or centerline) or model edge. The entire sketch segment is deleted if it does not intersect with any another sketch segment. To extend a sketch entity:
Drag the endpoint of a sketch entity until it is coincident with another entity. You cannot use Trim Entities to extend a sketch segment unless there is another entity to which you can extend the segment.
Dimensions and Relations Dimensions You dimension sketch entities and other objects with the Smart Dimension tool. The type of dimension is determined by the items you click. For some types of dimensions (point-to-point, angular, circular), where you place the dimension also affects the type of dimension that is added. You can drag or delete a dimension while the Smart Dimension tool is active. To add a dimension to a sketch or drawing:
1.
Click Smart Dimension on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart. The default dimension type is Parallel. Optionally, you can choose a different dimension type from the shortcut menu. Right-click the sketch, and select More Dimensions. Choose from Horizontal, Vertical, Ordinate, Horizontal Ordinate, or Vertical Ordinate. If you are editing a drawing view, you have additional choices of Baseline and Chamfer.
2.
Select the items to dimension, as shown in the table below. As you move the pointer, the dimension snaps to the closest orientation.
3.
Click to place the dimension.
To dimension the...
Click...
•
Length of a line or edge
The line.
•
Angle between two lines
Two lines, or a line and a model edge.
Note: Placement of the dimension affects the way the angle is measured. Example
•
Distance between two lines
Two parallel lines or a line and a parallel model edge.
•
Perpendicular distance from a point to a line
The point and the line or model edge.
•
Distance between two points
Two points.
•
Radius of an arc
The arc.
•
True length of an arc
The arc, then the two end points
SolidWorks 2004 Reference Guide
One of the points can be a model vertex. Example Example
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Chapter 3 Sketching
•
Diameter of a circle
The circumference.
Displayed as linear or diameter, depending on placement. Example
•
Distance when one or both entities is an arc or a circle
The centerpoint or the circumference of the arc or circle, and the other entity (line, edge, point, and so on).
By default, distance is measured to the centerpoint of the arc or circle, even when you select the circumference. Example
The dimension shortcut menu provides Display Options. The choices available depend on the type of dimension and other factors and may include the following: •
Center between witness lines
•
Offset Text
•
Show Parentheses
•
Show as Inspection
Horizontal Dimension You can specify a horizontal dimension between two entities. The horizontal direction is defined by the orientation of the current sketch. To specify a horizontal dimension:
1.
In an open sketch, click Horizontal Dimension Dimensions, Horizontal. The pointer changes to
on the Dimensions/Relations toolbar, or click Tools,
.
2.
Select the two entities to dimension.
3.
Click a location to place the dimension.
Vertical Dimension You can create a vertical dimension between two points. The vertical direction is defined by the orientation of the current sketch. To create a vertical dimension:
1.
Click Vertical Dimension
on the Dimensions/Relations toolbar, or click Tools, Dimensions, Vertical.
2.
Click the two points to dimension.
3.
Click a location to place the dimension.
Lock Dimensions When you create a dimension, the dimension snaps to the closest orientation as you move the pointer. When the preview indicates the dimension type you want, right-click to accept the dimension. You can then move the pointer to place the dimension in another location without changing the dimension type. To lock a dimension:
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1.
In an open sketch, click Smart Dimension Dimension, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Click the items to dimension.
3.
Move the pointer around until the preview indicates the dimension type you want.
4.
Right-click to lock the dimension type.
5.
Move the pointer around until the dimension is in the location you want.
6.
Click to place the dimension.
Point-to-Point Dimensions You can place a horizontal, vertical, or linear dimension between two sketch points, sketch segment endpoints, or model vertices. The model origin can also be one of the two points. Select the two points, then move the pointer around to observe the dimension preview. To create a dimension between two points:
1.
Click Smart Dimension
on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart.
2.
Click one point.
3.
Click the other point.
4.
Move the pointer to show the dimension preview.
5.
Click to place the desired dimension.
Point-to-Point Dimensions These distance dimensions were all created by selecting the same two points, then selecting a different location for each dimension.
Arc Dimensions The default dimension type for an arc is radius. You only need to select the arc for this dimension type. You can dimension the true length of the arc. To dimension the true length of an arc:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Click the arc.
3.
Click the two endpoints of the arc.
4.
Move the pointer to show the dimension preview.
5.
Click to place the dimension.
Arc Dimensions When you dimension an arc, the default dimension type is radius.
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Chapter 3 Sketching
To dimension the true length of an arc, select the arc and the two endpoints of the arc.
Circular Dimensions You can create a circular dimension as a diametrical dimension or as a linear dimension. By placing the dimension at an angle, the dimension is displayed as a diameter. By placing the dimension vertically or horizontally, it is displayed as a linear dimension. To create a circular dimension and then rotate the dimension around the circle:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Select the circle.
3.
Drag the dimension and click to place it.
4.
In the Modify box, set a value if necessary and click
.
If the Modify box does not appear, either double-click the dimension or select Input dimension value in Tools, Options, System Options, General. 5.
If the dmension is a diametrical dimension, select the dimension drag handle and drag to rotate the dimension to reposition it.
Circular Dimensions By placing the dimension at an angle, the dimension is displayed as a diameter.
By placing the dimension vertically or horizontally, it is displayed as a linear dimension. To modify the angle of a linear dimension, click the dimension, then drag the handle on the text. The dimension snaps to 15 degree increments.
To change the display of a circular dimension from linear to radial, right-click the dimension, select Properties, then clear the Display as linear dimension check box.
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Angular Dimensions Between Two Lines You can place an angular dimension between two lines or a line and a model edge. Select the two entities, then move the pointer to observe the dimension preview. The angle to be dimensioned changes based on the pointer position. To create an angular dimension between two lines:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
on the Dimensions/Relations toolbar, or click Tools,
2.
Click one line.
3.
Click the second line.
4.
Move the pointer to show the angular dimension preview.
5.
Click to place the dimension.
Angular Dimensions These angular dimensions were all created by selecting the two sketch lines, then selecting a different location for each dimension.
Angular Dimensions Between Three Points You can place an angular dimension between three sketch points, sketch segment endpoints, or model vertices. The model origin can also be used as one of the three points. Select the point for the vertex of the angle, then select the other two points. To create an angular dimension between three points:
1.
In an open sketch, click Smart Dimension Dimensions, Smart.
2.
Click a point to be the vertex of the angle.
3.
Click the other two points.
4.
Move the pointer to show the angular dimension preview.
5.
Click to place the angular dimension.
SolidWorks 2004 Reference Guide
on the Dimensions/Relations toolbar, or click Tools,
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Chapter 3 Sketching
Dimensions Between Arcs or Circles By default, distances are measured to the center of an arc or circle. You can also dimension between concentric circles and use extension lines. To change the way the distance is measured:
1.
Right-click the dimension, and select Properties.
2.
Set First arc condition and Second arc condition, then click OK. In these examples, First arc condition is set to Center, and Second arc condition is set as shown.
Center
Min
Max
You can drag the extension lines to new attachment points in circles and arcs. The dimensions update automatically. In the following example, the extension line of the right circle is dragged from the Min attachment point to the Center. Attachment at Min
Attachment dragged to Center
You can drag an arc radial dimension, and the dimension moves automatically between outside and inside. Arc dimension inside
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Arc dimension outside
To dimension between concentric circles and display extension lines:
1.
In an open sketch, click Smart Dimension on the Dimensions/Relations toolbar, or click Tools, Dimensions, Smart.
2.
Click one concentric circle, then click the second concentric circle.
3.
To display extension lines, right-click. Extension lines
4.
Click to place the dimension. To display extension lines after placing the dimension, click the Select right-click the dimension and select Display Options, Show extension lines.
tool, then
Autodimension Use the Autodimension tool to automatically insert dimensions in a sketch. You can also autodimension a sketch to model entities. The Autodimension PropertyManager controls: Entities to Dimension •
All entities in sketch. Dimensions all entites in the sketch.
•
Selected entities. Dimensions only the selected entities.
Horizontal Dimensions •
Scheme. Sets the horizontal dimension scheme and sets the entity as the vertical point of origination for the dimensions.
•
Dimension placement o
Above sketch. Places dimensions above the sketch.
o
Below sketch. Places dimensions below the sketch.
Vertical Dimensions •
Scheme. Sets the vertical dimension scheme and sets the entity as the horizontal point of origination for the dimensions.
•
Dimension placement o
Left of sketch. Places dimensions to the left of the sketch.
o
Right of sketch. Places dimensions to the right of the sketch.
To autodimension a sketch:
1.
In an open sketch, click Autodimension Dimensions, Autodimension.
2.
Set the properties in the Autodimension PropertyManager.
3.
Click OK
SolidWorks 2004 Reference Guide
on the Dimensions/Relations toolbar, or click Tools,
.
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Chapter 3 Sketching
To autodimension a sketch to model entities:
1.
Create a sketch on a model face.
2.
In the open sketch, click Autodimension Dimensions, Autodimension.
on the Dimensions/Relations toolbar, or click Tools,
The color of the entities autodimensioned in the graphics area correspond to the colors shown in the PropertyManager. 3.
Click OK
.
Geometric Relations Click Add Relations on the Dimensions/Relations toolbar, or click Tools, Relations, Add to create geometric relations (such as tangent or perpendicular) between sketch entities, or between sketch entities and planes, axes, edges, or vertices. You can also add relations while you create individual sketch entities, or when you select two exisitng entities. Existing Relations and Add Relations sections appear in all sketch entity PropertyManagers. When you create relations, at least one of the items must be a sketch entity. The other item (or items) can be either a sketch entity or an edge, face, vertex, origin, plane, axis, or curve from another sketch that forms a line or arc when projected on the sketch plane. Geometric relations can also be created automatically. See Automatic Relations.
Automatic Relations You can choose whether geometric relations are automatically created as you create sketch entities. To turn automatic relations on or off:
Click Tools, Sketch Settings, Automatic Relations, or click Tools, Options, System Options, Sketch, and select Automatic Relations. As you sketch, the pointer changes shape to show you which relations can be created. When Automatic Relations is turned on, the relations are added.
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Horizontal
Vertical
Coincident
Midpoint
Intersection
Tangent
Perpendicular
Brown inference lines indicate that a relation is added automatically; blue inference lines indicate that no relation is added.
Add Relations/Properties PropertyManager The Add Relations PropertyManager appears when you click Add Relation on the Dimensions/Relations toolbar. The Properties PropertyManager appears when you select multiple sketch entities in the graphics area. You can create geometric relations between sketch entities, or between sketch entities and planes, axes, edges, or vertices. Selected Entities Displays the names of selected sketch entities. Add entities to the list by selecting them in the graphics area. Existing Relations •
Relations
•
Information on).
. Displays relations that exist for the selected sketch entity. . Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations •
You can add relations to the selected entities from the list. The list includes only relations that are possible for the selected entities. Equal
and Midpoint
relations are not available in 3D sketches.
When you add relations to entities, at least one item must be a sketch entity. Other items can include additional sketch entities, edges, faces, vertices, origins, planes, or axes. You can also include sketch curves from other sketches that form lines or arcs when projected onto the sketch plane. Options For construction. Converts the entities to construction geometry (not available in Add Relations PropertyManager).
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Chapter 3 Sketching
Sketch Relations The following table describes the entities that you can select for a relation and the characteristics of the resulting relation. Relation
Entities to select
Resulting relations
Horizontal or Vertical
One or more lines or two or more points.
The lines become horizontal or vertical (as defined by the current sketch space). Points are aligned horizontally or vertically.
Collinear
Two or more lines.
The items lie on the same infinite line.
Coradial
Two or more arcs.
The items share the same centerpoint and radius.
Perpendicular
Two lines.
The two items are perpendicular to each other.
Parallel
Two or more lines.
The items are parallel to each other.
A line and a plane (or a planar face) in a 3D sketch.
The line is parallel to the selected plane.
ParallelYZ
A line and a plane (or a planar face) in a 3D sketch.
The line is parallel to the YZ plane with respect to the selected plane.
ParallelZX
A line and a plane (or a planar face) in a 3D sketch.
The line is parallel to the ZX plane with respect to the selected plane.
AlongZ
A line and a plane (or a planar face) in a 3D sketch.
The line is normal to the face of the selected plane.
Tangent
An arc, ellipse, or spline, and The two items remain tangent. a line or arc.
Concentric
Two or more arcs, or a point The arcs share the same centerpoint. and an arc.
Midpoint
A point and a line.
The point remains at the midpoint of the line.
Intersection
Two lines and one point.
The point remains at the intersection of the lines.
Coincident
A point and a line, arc, or ellipse.
The point lies on the line, arc, or ellipse.
Equal
Two or more lines or two or more arcs.
The line lengths or radii remain equal.
Symmetric
A centerline and two points, lines, arcs, or ellipses.
The items remain equidistant from the centerline, on a line perpendicular to the centerline.
Fix
Any entity.
The entity’s size and location are fixed. However, the end points of a fixed line are free to move along the infinite line that underlies it. Also, the endpoints of an arc or elliptical segment are free to move along the underlying full circle or ellipse.
Pierce
A sketch point and an axis, edge, line, or spline.
The sketch point is coincident to where the axis, edge, or curve pierces the sketch plane. The pierce relation is used in Sweeps with Guide Curves.
Merge Points
Two sketch points or endpoints.
The two points are merged into a single point.
NOTES:
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•
When you create a relation to a line, the relation is to the infinite line, not just the sketched line segment or the physical edge. As a result, some items may not touch when you expect them to.
•
When you create a relation to an arc segment or elliptical segment, the relation is actually to the full circle or ellipse.
•
If you create a relation to an item that does not lie on the sketch plane, the resulting relation applies to the projection of that item as it appears on the sketch plane.
•
Additional relations are created automatically when you use Offset Entities and Convert Entities.
Sketch Relations Callouts In an open sketch, when you double-click a sketch entity in the graphics area, the PropertyManager opens and callouts appear for all the relations of the selected entity. Alternatively, when you select a relation under Relations graphics area.
in the PropertyManager, a callout appears in the
The callouts display the relations applied to the selected sketch entity and the names of the related sketch entities. The color of the callout specifies the status of the entity (under defined, over defined, dangling, and so on). The default system color for fully defined status is black. In the callouts, fully defined status is blue, the same as for under defined. The other colors in the callouts follow the system defaults. The status also appears next to Information
in the PropertyManager.
To delete a relation, select the relation under Relations, or select the callout in the graphics area, and press Delete. To open the Display/Delete Relations PropertyManager, double-click the callout .
Sketch Geometry Status Sketch geometry can be in any of the following states. The color in parenthesis indicates the color of the sketch state. •
Dangling (brown). The sketch geometry can no longer be resolved (for example, a dimension to a deleted entity).
•
Over Defined (red). The sketch geometry is either in conflict or is redundant.
•
Fully Defined (black). The sketch geometry fully describes all of the sketch entities.
•
Under Defined (blue). The sketch geometry is not defined and is free to change.
•
Not Solved (pink). The sketch geometry cannot determine the position of one or more sketch entities.
•
Driven (gray). The dimension’s value is driven by solving the sketch.
•
Invalid (yellow). This sketch geometry would be geometrically invalid if the sketch were solved.
Sketch Status Conventions Sketches can be in any of five states described below. The state of the sketch is displayed in the status bar at the bottom of the SolidWorks window. •
Fully Defined. All the lines and curves in the sketch, and their positions, are described by dimensions or relations, or both.
•
Over Defined. Some dimensions or relations, or both, are either in conflict or are redundant. To view and remove conflicting relations, see Display/Delete Relations PropertyManager.
•
Under Defined. Some of the dimensions or relations in the sketch are not defined and are free to change. You can drag endpoints, lines, or curves until the sketch entity changes shape.
•
No Solution Found. The sketch is not solved. The geometry, relations, and dimensions that prevent the solution of the sketch are displayed.
•
Invalid Solution Found. The sketch is solved but results in invalid geometry, such as a zero length line, zero radius arc, or self-intersecting spline.
With the SolidWorks software, it is not necessary to fully dimension or define sketches before you use them to create features. However, you should fully define sketches before you consider the part complete. To always use fully defined sketches to create features, click Tools, Options, System Options, Sketch, and select Use fully defined sketches.
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Chapter 3 Sketching
Display/Delete Relations PropertyManager The Display/Delete Relations PropertyManager appears when you click Display/Delete Relations Dimensions/Relations toolbar.
on the
Relations •
Filter. Specifies which relations to display, such as All in this sketch, Selected Entities, or any of the following: o
Dangling
o
Over Defined/Not Solved
o
External
o
Defined In Context
o
Locked
o
Broken
•
Selected Entities (available when Filter is set to Seleted Entities). Displays the names of entities you select in the sketch.
•
Relations . Displays existing relations based on the selected Filter. When you select a relation from the list, the names of the related entities are displayed under Entities and the sketch entity is highlighted in the graphics area. The status of external references is displayed the same as in the FeatureManager design tree.
•
Information . Displays the status of the selected sketch entity. If the relation was created within the context of an assembly, the status can be Broken or Locked.
•
Suppressed. Suppresses the relation for the current configuration. The name of the relation turns gray and the Information status changes (from Satisfied to Driven, for example).
• •
Undo last relation change . Deletes or replaces the last action. Delete and Delete All. Deletes the selected relations or deletes all the relations.
Entities •
Entities used in the selected relation: o o
o
Entity. Lists each selected sketch entity in Relations. Status. Displays the status of the selected sketch entity, such as Fully Defined, Under Defined, and so on. Defined In. Displays the location where the entity is defined, such as Current Sketch, Same Model, or External Model.
Information for external entities in assemblies: o
Entity. Displays the entity name for sketch entities in the Same Model or External Model.
o
Owner. Displays the part to which the sketch entity belongs
o
•
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Owner and Assembly. Displays the name of the top-level assembly where the relation was created for sketch entities in an External Model.
Replace. Replaces the selected entity with another entity. In the graphics area, select an entity for Entity to replace the one selected above, and click Replace. If the replacement is not appropriate, the status is Invalid. o
Undo last relation change
. Undoes the last Replace action.
o
Replace in all relations. Replaces the sketch entity in all relations.
Configurations For models with multiple configurations, you can apply the selected relations to This configuration, All configurations, or Specify configurations. If you select Specify configurations, select configurations in the Configurations list. Click All to select all the configurations in the list. Click Reset to reset the selections to the original settings.
Scan Equal Use the Scan Equal tool to scan a sketch for entities with equal lengths or radii, and set an Equal relation between sketch entities that are the same length or radius. To locate sketch entities with equal radii or line lengths:
1.
In an open sketch, click Scan Equal Scan Equal.
on the Dimensions/Relations toolbar, or click Tools, Relations,
If equal sketch entities exist, the appropriate selections are available: • Length. Two or more lines are equal.
2.
3.
4.
•
Radii. Two or more arcs have equal radii.
•
Both. An arc has a radii equal to a line length.
To see the equal sketch entities, select one of the available selections. The following occurs: •
The entities are highlighted in the sketch.
•
Value. Displays the length or radii.
•
Line Count and Arc Count. Displays the number of equal entities.
Click for additional options: •
Find Next. Available if additional sets of equal entities exist.
•
Set Equal. Creates an Equal relation between the highlighted entities.
Click Close.
External vs. Defined in Context External - A relation that is "External" is a relation between a sketch entity and something outside of that sketch. This thing can be an edge or vertex within the same model or it can be an edge or vertex within a different model within an assembly. Defined in Context - A relation that is "Defined in Context" is a relation between a sketch entity in one part and some entity in another part. This relation occurs within the context of the assembly. Entities that are "Defined in Context" are listed as "External" because they have relations outside of the sketch. However, not all "External" relations are "Defined in Context" because they may be relations within the same part file.
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Chapter 3 Sketching
Splines Splines You can create spline curves. Splines can have as few as two points, and you can specify tangency at the end points. You can create spline curves in 3D sketches. To create a spline:
1.
Click Spline
on the Sketch toolbar, or Tools, Sketch Entities, Spline.
The pointer changes to
.
2.
Click to place the first point and drag out the first segment.
3.
Click the endpoint and drag out the second segment.
4.
Repeat until the spline is complete. Alternatively, you can click on each through point to create the spline, then double-click when the spline is complete.
To add relations to the spline points:
Select points and use Add Relations in the active PropertyManager to specify relations between spline points or endpoints. To reshape a spline:
1.
In an open sketch, select the spline. Handles appear on the through points and the segment end points.
2.
You can modify the spline using the following techniques: •
Drag the handles.
•
Remove through spline points.
•
Right-click and select Spline Point, Moving Frame, or Simplify Spline.
To change the properties of a spline:
In an open sketch, select a spline and edit its properties in the Spline PropertyManager. You can specify the spline to be Proportional. To create a two-point spline with tangency:
1.
In an open sketch, click Spline points.
on the Sketch toolbar and sketch a spline with three or more spline
2.
Right-click the spline and select Simplify Spline.
3.
In the dialog box, click Smooth until the spline contains only two points, then click OK. The endpoints of the spline retain their slope. You can also add tangency to a two-point spline by adding a relation as described above.
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Add tangent relation between spline and line
Simplify spline to two points with slope retained
Proportional Splines A newly created spline is non-proportional by default. You can change its shape by dragging a spline point or endpoint. A proportional spline retains its shape when you drag the endpoints; the entire spline resizes proportionally. You can add dimensions and relations to internal points of proportional splines.
Spline PropertyManager The Spline PropertyManager controls the following properties of a sketched Spline: Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You cannot add relations to splines. You can add relations to the spline points. Click a point on the spline to add a relation. Options For construction. Converts the entity to construction geometry. Parameters Specify any appropriate combination of the following parameters to define the spline if the spline is not constrained by relations. Spline Point Number. Highlights the selected spline point in the graphics area. X Coordinate. Specifies the x coordinate of the spline point. Y Coordinate. Specifies the y coordinate of the spline point. Proportional.Retains the spline shape when you drag an endpoint; the entire spline resizes proportionally.
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Chapter 3 Sketching
Fit Spline Use the Fit Spline tool to fit sketch segments to a spline. Fit splines are parametrically linked to underlying geometry so that changes to the geometry update the spline. Fit spline chooses the most logical fit to the geometry you select, but you can modify the fit. If you select an entity that has been fit, the entity is no longer part of the spline. If you select an entity that is not part of the spline, the spline adjusts to include the selected entity. You can also include model edges in a fit spline. However, you cannot constrain other geometry to the splines.
Sketch has four entities
Fit Spline tool converts the geometry to a single spline
The Fit Spline PropertyManager controls: Parameters •
Delete geometry. Deletes the original sketch segments from the sketch. Otherwise, the segments remain as construction geometry separate from the spline. When cleared, you can select the Constrained, Unconstrained, or Fixed options.
•
Closed spline. Creates a closed contour spline.
•
Constrained. Parametrically links the fitted spline to the defining geometry.
•
Unconstrained. Creates the fitted spline as the same shape as the original defining geometry but with no constraints. You can dimension, constrain, and drag the spline.
•
Fixed. Creates the fitted spline as the same shape as defining geometry but it is fixed in space.
•
Edit Chaining. Allows you to edit the chain of splines created. Editing applies only to the order of the noncontiguous spline elements, not the sketch entities. Click
or
to undo or redo the edits.
Tolerance •
Tolerance
. Specifies the maximum deviation allowed from the original sketch segments.
•
Actual Deviation. Updates based on the Tolerance value and the geometry selected. This is automatically calculated.
To fit sketch segments to a spline:
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1.
In an open sketch, click Tools, Spline Tools, Fit Spline.
2.
In the graphics area, click the sketch entities to fit to the spline.
3.
Set the properties in the Fit Spline PropertyManager.
4.
Click OK
.
Simplify Spline Use the Simplify Spline tool to reduce the number of points in a spline and to increase system performance in models with complex spline curves. You can also simplify splines that were created from imported models or from tools such as Convert Entities, Offset Entities, Intersection Curve, and Face Curves. To simplify a spline:
1.
In an open sketch, select the spline in the graphics area, then click Simplify Spline toolbar, or click Tools, Spline Tools, Simplify Spline.
on the Spline Tools
2.
In the dialog box, set a value for Tolerance and press Enter, or click Smooth. (You can continue to click Smooth until only two spline points remain). The SolidWorks software: •
Adjusts the tolerance and calculates a new curve with fewer spline points. The original spline is displayed in the graphics area along with a preview of the smoothed curve.
•
Displays the Number of spline points in In original curve and In simplified curve.
•
Displays the simplified Tolerance, which measures the intended deviation of the simplified curve from the original curve. Click Previous to return through the sequence as far as the original curve.
3.
Click OK.
Insert Spline Point The Insert Spline Point command adds one or more points to the spline. With spline points, you can: •
Use spline points as handles to pull the spline into the shape you want
•
Add dimensions between spline points or between spline points and other entities
•
Add relations to spline points
To insert spline points:
1.
In an open sketch, right-click the spline and select Insert Spline Point, or click Tools, Spline Tools, Insert Spline Point. The pointer changes to
2.
. If the pointer is not on the spline, the pointer changes to
.
Click one or more places on the spline where you want to insert a point.
To delete spline points:
In an open sketch, select a point and press Delete.
Moving Frame The moving frame is a way to manipulate a spline without adding points. You can use the moving frame in a part or drawing document. The moving frame is available for both 2D or 3D splines. NOTE: The moving frame can be used with splines created in SolidWorks that you are able to modify. It cannot be used with imported or converted splines.
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To add a moving frame to a spline:
Right-click the sketched spline and select Moving Frame. You can use the moving frame in the following ways:
•
Drag the moving frame by the frame point to move it along the spline to wherever you want to place it.
•
Pull the frame handles to change the shape of the spline curve. Select the frame and modify the X and Y coordinates of the frame point by entering new values in the Frame Point Properties PropertyManager.
•
•
Add multiple moving frames to a spline, making it possible to control the curve of the spline where there are no spline points. Only the active frame is fully displayed. Other frames are displayed as small triangles on the outside of the curve.
•
When used in conjunction with Curvature Comb, the center handle of each moving frame joins with the curvature comb.
Frame Point PropertyManager The Frame Point Properties PropertyManager controls the following properties of a spline Moving Frame: Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity.
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Parameters You can specify any appropriate combination of the following parameters to define the frame point if the frame point is not constrained by relations. When you change one or more parameters, the other parameters update automatically. X Coordinate Y Coordinate Curvature - of the spline at the frame point Tangency - of the moving frame at the frame point
3D Frame Point PropertyManager The 3D Frame Point PropertyManager controls the following properties of a spline Moving Frame: Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined and so on) is
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Parameters You can specify any appropriate combination of the following parameters to define the frame point if the frame point is not constrained by relations. When you change one or more parameters, the other parameters update automatically. X Coordinate Y Coordinate Z Coordinate Curvature - of the spline at the frame point Tangency - in the XY plane Tangency - in the XZ plane Tangency - in the YZ plane
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Curvature Combs Curvature combs provide visual enhancement of the slope and curvature of most sketch entities in part, assembly, and drawing documents.
To show the curvature combs of a sketch entity:
1.
In an open sketch, right-click a sketch entity and select Show Curvature Combs. A comb appears that displays the curvature of the entity. For splines, the comb crosses the spline at inflection points. The comb changes shape dynamically as you drag the sketch entity and its curvature changes.
2.
In the PropertyManager, move the Scale slider to adjust the size of the curvature comb.
3.
Click OK
.
The comb remains visible when you close the sketch (unless the sketch is made into a feature). To change the scale of all curvature combs in a sketch:
1.
In an open sketch, right-click a sketch entity with curvature combs displayed and select Modify Curvature Scale.
2.
In the PropertyManager, move the Scale slider to adjust the size of the curvature comb.
3.
Click OK
.
To hide the curvature comb of a sketch entity:
In an open sketch, right-click the sketch entity and select Show Curvature Combs.
Curvature Scale The Scale slider adjusts the size of all the curvature combs in the active sketch.
Inflection Points The Show Inflection Points tool displays all points where the concavity of a spline changes. The inflection point symbol appears at the point where the spline changes from concave to convex. To display inflection points of a spline:
In an active spline sketch, select a spline, right-click, and select Show Inflection Points. The inflection points appear.
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Minimum Radius The Show Minimum Radius tool displays the radial measurement of the curve with the smallest radius of a spline. To display the minimum radius of a spline:
In an active spline sketch, select a spline, right-click, and select Show Minimum Radius. The minimum radius curve appears with the radial measurement.
2D Sketching Line Creates a sketched line. To sketch a line:
1.
Click Line
on the Sketch toolbar, or click Tools, Sketch Entities, Line.
The pointer changes to
.
2.
Click in the graphics area to start the line.
3.
Complete the line in one of the following ways: •
Drag the pointer to the end of the line and release.
•
Release the pointer, move the pointer to the end of the line, and click again. A horizontal or vertical line automatically snaps to the grid points if grid snap is on.
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To modify the line by dragging:
In an open sketch, do one of the following: •
To change the length of the line, select one of the endpoints and drag to lengthen or shorten the line.
•
To move the line, select the line and drag the line to another position.
•
To change the angle of a line, select an endpoint and drag to a different angle. If the line has a vertical or horizontal relation, delete the vertical or horizontal relation in the Line PropertyManager before dragging to a new angle.
To change the line properties:
In an open sketch, select a line and edit its properties in the Line PropertyManager.
Line PropertyManager The Line PropertyManager controls the following properties of a sketched Line. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the line if the line is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Start X Coordinate Start Y Coordinate End X Coordinate End Y Coordinate Length Angle. Relative to the grid, with horizontal 180°, vertical 90°, and the positive direction counterclockwise. Delta X. Difference between the start and end X coordinates. Delta Y. Difference between the start and end Y coordinates.
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Points You can insert points into sketches and drawings. To create sketch points:
1.
Click Point
on the Sketch toolbar, or Tools, Sketch Entities, Point.
The pointer changes to 2.
.
Click in the graphics area to place the point. The Point tool remains active so you can continue to insert points.
To change the properties of a point:
In an open sketch, select a point and edit its properties in the Point PropertyManager.
Point PropertyManager The Point PropertyManager controls the following properties of a sketched Point. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Parameters You can specify the following parameters to define the point if the point is not constrained by relations. X Coordinate Y Coordinate
Circle You can create a sketched circle. To create a circle:
1.
Click Circle on the Sketch toolbar, or click Tools, Sketch Entities, Circle. The pointer changes to
.
2.
Click in the graphics area to place the center of the circle.
3.
Move the pointer and click to set the radius.
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To modify a circle by dragging:
In an open sketch: • • •
Enlarge the circle by dragging its edge away from its center point. Make the circle smaller by dragging its edge toward its center point. Move the circle by dragging its center point.
To change the properties of a circle:
In an open sketch, select the circle and edit its properties in the Circle PropertyManager.
Circle PropertyManager The Circle PropertyManager controls the following properties of a sketched Circle. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the circle if the circle is not constrained by relations. Center X Coordinate Center Y Coordinate Radius
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Ellipse Use the Ellipse tool to create a complete ellipse. Use the Partial Ellipse tool to create an elliptical arc. To create an ellipse:
1.
Click Ellipse
on the Sketch toolbar, or Tools, Sketch Entities, Ellipse.
The pointer changes to
.
2.
Click in the graphics area to place the center of the ellipse.
3.
Drag and click to set the major axis of the ellipse.
4.
Drag and click again to set the minor axis of the ellipse.
To change the properties of an ellipse:
In an open sketch, select the ellipse and edit the properties in the Ellipse PropertyManager.
Partial Ellipse You can create a partial ellipse (an elliptical arc) from a centerpoint, a start point, and an end point, similar to creating a Centerpoint Arc. To create a partial ellipse:
1.
In an open sketch, click Partial Ellipse Ellipse. The pointer changes to
on the Sketch toolbar, or click Tools, Sketch Entities, Partial
.
2.
Click in the graphics area to place the center of the ellipse.
3.
Drag and click to define one axis of the ellipse.
4.
Drag and click to define the second axis. The circumference guideline remains.
5.
Drag the pointer around the circumference to define the extent of the ellipse, then click to complete the ellipse.
To change the partial ellipse properties:
In an open sketch, select the ellipse and edit its properties in the Ellipse PropertyManager.
Ellipse PropertyManager The Ellipse PropertyManager controls the following properties of a sketched Ellipse or Partial Ellipse. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity.
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Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the ellipse if the ellipse is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Some parameters are available only for a Partial Ellipse. Center X Coordinate Center Y Coordinate Start X Coordinate (Partial Ellipse only) Start Y Coordinate (Partial Ellipse only) End X Coordinate (Partial Ellipse only) End Y Coordinate (Partial Ellipse only) Radius 1 Radius 2 Angle (Partial Ellipse only)
Centerlines Use centerlines to create symmetrical sketch elements (see Mirror Entities) and revolved features (see Revolve), or as construction geometry. To create a centerline:
1.
Click Centerline
on the Sketch toolbar, or click Tools, Sketch Entities, Centerline.
The pointer changes to
.
2.
Click to start the centerline.
3.
Drag, or move the pointer and click, to set the end of the centerline.
To change the centerline properties:
In an open sketch, select a centerline and edit its properties in the Line PropertyManager.
Virtual Sharp A virtual sharp creates a sketch point at the virtual intersection point of two sketch entities. Dimensions and relations to the virtual intersection point are retained even if the actual intersection no longer exists, such as when a corner is removed by a fillet or chamfer. To create a virtual sharp:
1.
In an open sketch, hold down Ctrl and select two sketch entities.
2.
Click Point
on the Sketch toolbar, or click Tools, Sketch Entities, Point.
A virtual sharp appears at the point where the sketch entities would intersect. Set the virtual sharp display style in Tools, Options, Document Properties, Virtual Sharps.
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Centerpoint Arc Use the Centerpoint Arc tool to create an arc from a centerpoint, a start point, and an end point. To create a centerpoint arc:
1.
In an open sketch, click Centerpoint Arc Centerpoint Arc. The pointer changes to
on the Sketch toolbar, or click Tools, Sketch Entities,
.
2.
Click in the graphics area to place the start point of the arc, then click where you want to place the end point of the arc.
3.
Drag to set the angle and the radius of the arc.
4.
Click to place the arc.
5.
Set the properties in the Arc PropertyManager.
6.
Click OK
.
To change the properties of the arc:
In an open sketch, select the arc and edit the properties in the Arc PropertyManager.
Tangent Arcs Creates an arc, tangent to a sketch entity. You can transition from sketching a line to sketching a tangent arc without selecting the Tangent Arc tool by autotransitioning. To create a tangent arc:
1.
Click Tangent Arc
on the Sketch Tools toolbar, or Tools, Sketch Entity, Tangent Arc.
2.
Click the pointer on the end point of a line, arc, ellipse, or spline. The Arc PropertyManager appears and the pointer changes to
3.
.
Drag the arc to the desired shape. NOTE: SolidWorks infers from the pointer motion whether you want a tangent or normal arc. There are four intent zones, with eight possible results as shown. Moving the pointer in a tangent direction creates a tangent arc. Moving the pointer in a normal direction creates a normal arc. You can toggle between tangent and normal arcs by returning to the end point and moving away in a new direction.
4.
Release the mouse button.
To change the properties of the arc, select the arc to open the Arc PropertyManager.
3 Point Arc You can create an arc by specifying three points (start, end, and midpoint). To create a 3 point arc:
1.
Click 3 Point Arc
on the Sketch toolbar, or click Tools, Sketch Entities, 3 Point Arc.
The Arc PropertyManager appears and the pointer changes to
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2.
Click where you want the arc to start.
3.
Drag to where you want the arc to end.
4.
Release the pointer.
5.
Drag the arc to set the radius and to reverse the arc, if necessary.
6.
Release the pointer.
7.
Make any necessary changes in the PropertyManager and click OK
.
To change the properties of the arc:
Select the arc and edit the properties in the Arc PropertyManager.
Arc PropertyManager The Arc PropertyManager controls the following properties of a sketched Centerpoint Arc, Tangent Arc, or 3 Point Arc. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entities to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the arc if the arc is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Center X Coordinate Center Y Coordinate Start X Coordinate Start Y Coordinate End X Coordinate End Y Coordinate Radius Angle. Subtended by the arc.
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Parabolas You can create a parabolic curve. To create a parabola:
1.
Click Parabola
on the Sketch toolbar, or Tools, Sketch Entities, Parabola.
The pointer changes to 2.
.
Click to place the focus of the parabola and drag to enlarge the parabola. The parabola is outlined.
3.
Click on the parabola and drag to define the extent of the curve.
To modify the parabola:
1.
In an open sketch, select a parabola. (The pointer changes to
2.
Drag the vertex to shape the curve. The pointer changes to • •
when it is over a parabola.) when you select the vertex.
To flatten the curve, drag the vertex away from the focus. To make a sharper curve, drag the vertex closer to the focus. A move icon appears next to the pointer when you move the vertex.
•
To change the length of a side of the parabola without modifying the curve of the parabola, select an endpoint and drag.
•
To move the parabola to a new location, select the curve of the parabola and drag.
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•
To modify the length of both sides of the parabola without changing the arc of the parabola, drag the parabola away from its endpoints.
To change the properties of a parabola:
In an open sketch, select a parabola and edit its properties in the Parabola PropertyManager.
Parabola PropertyManager The Parabola PropertyManager controls the following properties of a sketched Parabola. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the parabola if the parabola is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Start X Coordinate Start Y Coordinate End X Coordinate End Y Coordinate Center X Coordinate Center Y Coordinate Apex X Coordinate Apex Y Coordinate
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Polygons You can create equilateral polygons with any number of sides between 3 and 40. To create a polygon:
1.
Click Polygon
on the Sketch toolbar, or click Tools, Sketch Entities, Polygon.
The pointer changes to
.
2.
Set the properties in the Polygon PropertyManager as necessary.
3.
Click in the graphics area to place the center of the polygon, and drag out the polygon.
4.
To sketch another polygon, click New Polygon and repeat steps 2 through 5.
5.
Click OK
.
The Polygon tool is still active. You can create additional polygons, although the PropertyManager does not open. To release the tool, click the tool on the Sketch toolbar, click another tool, or press Esc. To modify the polygon by dragging:
In an open sketch: •
Resize the polygon by dragging it by one of its sides. - or -
•
Move the polygon by dragging one of its vertices or its center point.
To edit a polygon:
1.
In an open sketch, select one of the sides of the polygon and click Tools, Sketch Tools, Edit Polygon. - or Right-click a side of the polygon and select Edit polygon.
2.
Modify the polygon in the Polygon PropertyManager.
Polygon PropertyManager The Polygon PropertyManager controls the following properties during creation of a sketched Polygon. Existing Relations No relations exist for polygons. Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You cannot add relations to polygons. However, you can add relations to the points and lines of polygons. Options For construction. Converts the entity to construction geometry.
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Parameters You can specify any appropriate combination of the following parameters to define the polygon. When you change one or more parameters, the other parameters update automatically. •
Number of Sides
. Sets the number of sides in the polygon. A polygon can have 3 to 40 sides.
•
Inscribed circle. Displays an inscribed circle inside the polygon to define the size of the polygon. The circle is construction geometry.
•
Circumscribed circle. Displays a circumscribed circle outside of the polygon to define the size of the polygon. The circle is construction geometry.
•
Center X Coordinate
. Displays the X coordinate for the center of the polygon.
•
Center Y Coordinate
. Displays the Y coordinate for the center of the polygon.
•
Circle Diameter
•
Angle
•
New Polygon. Lets you to create another polygon.
. Displays the diameter of the inscribed or circumscribed circle.
. Displays the angle of rotation.
Rectangles You can create rectangles whose sides are horizontal or vertical with respect to the sketch grid. For rectangles whose sides are at a different orientation, create a Parallelogram. To create a rectangle:
1.
Click Rectangle
on the Sketch toolbar, or Tools, Sketch Entities, Rectangle.
The pointer changes to 2.
.
Click to place the first corner of the rectangle, drag, and release when the rectangle is the correct size and shape. Instead of dragging, you can move the pointer and click again (click-click mode).
While dragging, the dimensions of the rectangle are dynamically displayed.
To change the size or shape of a rectangle:
In an open sketch, drag a side or vertex. You can force sketch segments to detach when you drag them. Click Tools, Sketch Settings, Detach Segment on Drag. To change the properties of an individual line in the rectangle:
In an open sketch, select the line and edit the properties in the Line PropertyManager.
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Parallelograms You can create a parallelogram and also create a rectangle whose sides are not horizontal or vertical with respect to the sketch grid. To create a parallelogram:
1.
2.
Click Parallelogram
on the Sketch toolbar, or click Tools, Sketch Entities, Parallelogram.
The pointer changes to
.
Click to place the first corner of the parallelogram, drag, and release when one edge of the parallelogram is the correct length. Instead of dragging, you can move the pointer and click again (click-click mode).
3.
Click again and drag until the parallelogram is the correct size and shape. •
Press Ctrl while dragging to create a parallelogram at any angle. You can reshape and resize the parallelogram by dragging its corners and sides.
•
Drag without pressing Ctrl to create a rectangle at an angle. You can resize the rectangle by dragging its corners and sides. You cannot change the angle of the rectangle by dragging.
Text You can sketch text on the face of a part and extrude or cut the text. The text can be inserted on any set of continuous curves or edges, including circles or profiles made up of lines, arcs, or splines. Example of Sketch Text The text is sketched along the outside edge of the face of the part, formatted, then cut.
A sketched spline creates an offset edge. A second sketch places the text on the offset line. The text is formatted, then extruded.
If the curve is a sketch entity, or a set of sketch entities, and the sketch text is in the same sketch as the curve, convert the sketch entities to construction geometry.
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To sketch text on a part:
1.
Click a face of a part. Click Text
on the Sketch toolbar, or click Tools, Sketch Entities, Text.
To create a profile for placing the text, sketch a circle or a continuous profile from lines, arcs, or splines in a sketch, close the sketch, then open another sketch for the text. 2.
In the graphics area, select an edge, curve, sketch, or sketch segment. The selected item appears under Curves
3.
.
In the PropertyManager, under Text, type the text to display. The text appears in the graphics area as you type.
4.
Set the properties in the Sketch Text PropertyManager as necessary.
5.
Click OK
6.
With the sketch still open, Extrude or Cut the text.
.
To edit sketch text:
1.
In an open sketch, right-click the text (the pointer changes to Properties.
when it is over the sketch text) and select
2.
Edit the text and its properties in the Sketch Text PropertyManager as necessary.
Sketch Text PropertyManager You can sketch text on the face of a part and extrude or cut the text. The text can be inserted on any set of continuous curves or edges, including circles or profiles made up of lines, arcs, or splines. You can specify the following properties in the Sketch Text PropertyManager. Curves Select edges, curves, sketches, or sketch segments. The name of the selected entity appears in the box, and the text appears along the entity. Text •
Text. Type text in the Text box. The text appears along the selected entity in the graphics area. If no entity is selected, the text appears horizonally starting at the origin.
•
Style. You can select individual characters, or groups of characters, to apply Bold Rotate
or Italic
or to
.
Click Rotate to rotate the selected text 30 degrees counterclockwise. For other rotation angles, click Rotate and then edit the code in the Text box. For example, for an angle of 10 degrees clockwise, replace
Alignment. Justify the text Left Align , Center Align , Right Align Alignment is available only for text along a curve, edge, or sketch segment.
•
Flip. Flip the text in the Flip Vertical
•
and back . Flip Vertical is available only for text along a curve, edge, or sketch segment. Width Factor . Widen each character evenly by the specified percentage. Width Factor is not available when Use document's font is selected
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direction and back
, or Full Justify
, or in the Flip Horizontal
.
direction
•
Spacing . Change the spacing between each character by the specified percentage. Spacing is not available when the text is fully justified or when Use document's font is selected.
•
Use document's font. Clear to choose another font.
•
Font. Click to open the Font dialog box and choose a font style and size.
Sketch Picture You can insert a picture (.bmp, .gif, .jpg, .jpeg, .tif, and .wmf) on a sketch plane. Pictures can be used as an underlay for creating 2D sketches. The Sketch Picture PropertyManager controls the picture's position, size, angle, orientation, and aspect ratio setting. •
The picture is inserted with its (0, 0) coordinate at the sketch origin, an initial size of 1 pixel per 1 mm, and locked aspect ratio.
•
The picture is embedded in the document (not linked). If you change the original image, the sketch picture does not update.
•
If you sketch on top of the picture, there is no snap to picture, inferencing, or autotracing capability. If the image is moved, or deleted and replaced, the sketch does not update.
•
If you hide the sketch, the picture is also hidden.
•
Pictures can be inserted into assemblies when editing a part in context, but they cannot be inserted into assembly sketches.
Example of Sketch Picture A sketch picture is inserted with its (0, 0) coordinate at the sketch origin.
To insert a picture on a sketch plane:
1.
In an open sketch, click Sketch Picture Picture.
on the Sketch toolbar, or click Tools, Sketch Tools, Sketch
2.
In the dialog box, browse to the picture file and click Open. The picture is inserted.
3.
Set the properties in the Sketch Picture PropertyManager as necessary. You can resize the picture in the graphics area by dragging its handles. You can drag the picture without changing its size when the pointer changes to
4.
Click OK
.
.
To edit the picture after you have inserted it, double-click the picture.
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Sketch Picture PropertyManager You can insert a sketch picture onto either side of a sketch plane. The Sketch Picture PropertyManager controls the following properties. Origin X Position. Enter an X coordinate value for the origin of the picture. Origin Y Position. Enter a Y coordinate value for the origin of the picture. Angle. Enter a value in degrees. A positive angle rotates the picture counterclockwise. Width. Enter a value for the picture width. If Lock Aspect Ratio is selected, the height adjusts automatically. Height. Enter a value for the picture height. If Lock Aspect Ratio is selected, the width adjusts automatically. Lock Aspect Ratio. Select to keep a fixed width and height aspect ratio. Flip Horizontally. Click to flip the picture horizontally within its borders. Flip Vertically. Click to flip the picture vertically within its borders. NOTE: Values in the Sketch Picture PropertyManager update automatically when you change the size or position of the picture in the graphics area.
3D Sketching 3D Sketching A 3D sketch consists of lines and arcs in series, and splines. You can use a 3D sketch as a sweep path, as a guide curve for a loft or sweep, a centerline for a loft, or as one of the key entities in a routing system. (The routing functionality is an add-in application.) To begin a 3D sketch, click 3D Sketch on the Sketch toolbar, or click Insert, 3D Sketch. A space handle helps you maintain orientation while sketching on several planes. By default, you sketch relative to the default coordinate system in the model. To switch to one of the other two default planes, click the sketch tool and press Tab. The origin of the current sketch plane is displayed. Before you begin a 3D sketch, change the view orientation to Isometric. It is easier to create a 3D sketch in an isometric orientation because the X, Y, and Z directions are visible. The sketch tools available in 3D sketching are: Line creates 3D lines. Spline creates 3D splines. Point creates 3D points. Centerline creates construction geometry. Convert Entities creates one or more entities in a 3D sketch by projecting an edge, loop, face, external curve, external sketch contour, set of edges, or set of external curves onto the sketch plane. Face Curves extracts 3D iso-parametric curves from faces or surfaces.
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Sketch Fillet rounds the intersections of sketched lines. Sketch Chamfer bevels the intersections of sketched lines. Intersection Curve creates a sketched curve at intersections. Trim Entities trims or extends a sketch entity in a 3D sketch. Extend Entities extends a sketch entity in a 3D sketch. Construction Geometry converts sketched curves in a 3D sketch to construction geometry. As you sketch a line, the line snaps to one of the major directions, X, Y, or Z, if applicable, and is constrained as Horizontal, Vertical, or Along Z, respectively. The relations are added with respect to the current coordinate system for the 3D sketch. See Dimensioning a 3D Sketch. You are not restricted to drawing lines along one of the three major directions. You can sketch in the current sketch plane at an angle to one of the major directions, or you can sketch out-of-plane if the endpoint of the line snaps to existing model geometry.
To create an arc in a 3D sketch:
1.
Click Sketch Fillet
on the Sketch toolbar, or click Tools, Sketch Tools, Fillet.
2.
In the PropertyManager, under Fillet Parameters, set the Radius
3.
Select two intersecting line segments, or select their intersection. Selecting an intersection
.
Three intersections filleted
Line Snap While you create a line in a 3D sketch, you can snap the line to geometry that already exists in the part, such as model surfaces or vertices, and sketch points. •
Snap is not enabled if you are sketching in one of the major coordinate directions.
•
If you are sketching on a plane, and the SolidWorks software infers a snap to a non-planar point, a temporary 3D graphics box is displayed to indicate an off-planar snap.
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3D Lines You can create lines in 3D sketches. To create a line in a 3D sketch:
1.
Click 3D Sketch
on the Sketch toolbar, or click Insert, 3D Sketch.
2.
Click Standard Views directions.
3.
Click Line
4.
Click in the graphics area to start the line.
, then select Isometric
on the View toolbar so you can view all three
on the Sketch toolbar, or click Tools, Sketch Entities, Line.
The 3D Line PropertyManager appears and the pointer changes to
.
Each time you click, the space handle appears to help you sketch on the different planes.
5.
If you want to change planes, press Tab.
6.
Drag to where you want the line segment to end.
7.
To continue the line, select the end point and press Tab to change to another plane if necessary.
8.
Drag the second segment and release the pointer.
To modify the line by dragging:
•
To change the length of the line, select one of the endpoints and drag to lengthen or shorten the line.
•
To move the line, select the line and drag the line to another position.
To change the line properties:
In a 3D sketch, select a line and edit its properties in the Line PropertyManager.
3D Line PropertyManager The 3D Line PropertyManager controls the following properties of a sketched 3D Line. Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry.
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Parameters You can specify any appropriate combination of the following parameters to define the line if the line is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Start X Coordinate Start Y Coordinate Start Z Coordinate End X Coordinate End Y Coordinate End Z Coordinate Length Angle. Relative to the grid, with horizontal 180°, vertical 90°, and the positive direction counterclockwise. Delta X. Difference between the start and end X coordinates. Delta Y. Difference between the start and end Y coordinates. Delta Z. Difference between the start and end Z coordinates.
3D Splines You can create splines in 3D sketches. To create a spline in a 3D sketch:
1.
Click 3D Sketch
on the Sketch toolbar, or Insert, 3D Sketch to open a 3D sketch.
2.
Click Standard Views directions.
3.
Click Spline
4.
Click in the graphics area to place the first point and drag the first segment.
, then select Isometric
on the View toolbar so you can see all three
on the Sketch toolbar, or Tools, Sketch Entities, Spline.
The Spline PropertyManager appears. Each time you click, the space handle appears to help you sketch on the different planes.
5.
If you want to change planes, press Tab.
6.
Select the endpoint and drag the second segment.
7.
Repeat until the spline is complete. Alternatively, you can click to place each through point, then double-click to place the endpoint and complete the spline.
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To add relations to the spline points:
Select points and add relations between points or endpoints, or between the spline points and other sketch entities in the Point PropertyManager. To reshape a spline:
1.
In a 3D sketch, select the spline. Handles appear on the through points and endpoints.
2.
You can modify the spline using the following techniques. •
Drag the handles to reshape the spline.
•
Add or remove through spline points to aid in shaping the spline. Right-click the spline and select Spline Point, or select a spline point and press Delete.
•
Insert a moving frame along the curve of the spline to manipulate the spline shape. Right-click the spline and select Moving Frame.
•
Smooth the spline. Right-click the spline and select Simplify Spline.
To change the properties of a spline:
In a 3D sketch, select a spline and edit its properties in the Spline PropertyManager.
3D Spline PropertyManager The 3D Spline PropertyManager controls the following properties of a sketched 3D Spline: Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined, and so on) is
Add Relations You cannot add relations to splines. NOTE: You can add relations to the spline points. Click a point on the spline to add a relation. Options Select the For construction check box to convert the entity to construction geometry. Parameters Specify any appropriate combination of the following parameters to define the spline if the spline is not constrained by relations. Spline Point Number. When you scroll through the points, the corresponding coordinates appear below X Coordinate. The x coordinate of the spline point. Y Coordinate. The y coordinate of the spline point. Z Coordinate. The z coordinate of the spline point. Proportional. A proportional spline retains its shape when you drag the endpoints; the entire spline resizes proportionally. You can add dimensions and relations to internal points of proportional splines.
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3D Points You can insert points into 3D sketches. To create sketch points in a 3D sketch:
1.
Click 3D Sketch
on the Sketch toolbar, or Insert, 3D Sketch to open a 3D sketch.
2.
Click Standard Views directions.
3.
Click Point
4.
Click in the graphics area to place the point.
, then select Isometric
on the View toolbar so you can view all three
on the Sketch toolbar, or Tools, Sketch Entities, Point.
The Point PropertyManager appears. The Point tool stays active so you can continue to insert points. To change the properties of a point:
In a 3D sketch, select the point and edit its properties in the Point PropertyManager.
3D Point PropertyManager The 3D Point PropertyManager controls the following properties of a sketched 3D Point. Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area. NOTE: When you sketch a 3D point on a face or surface, the point automatically has a coincident relation with the face or surface.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined and so on) is
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Parameters You can specify the following parameters to define the point if the point is not constrained by relations. X Coordinate Y Coordinate Z Coordinate
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3D Circle PropertyManager The 3D Circle PropertyManager controls the following properties of a 3D Circle. To create a circle in a 3D sketch, open a 3D Sketch on a circular face of a part, click Convert Entities
, and select the circular edge.
Existing Relations •
Relations . Relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information displayed.
. The status of the selected sketch entity (Fully Defined, Under Defined and so on) is
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options Select the For construction check box to convert the entity to construction geometry. Parameters You can specify any appropriate combination of the following parameters to define the circle if the circle is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Center X Coordinate Center Y Coordinate Center Z Coordinate Radius
Coordinate System - 3D Sketching When creating a 3D sketch, by default, you sketch relative to the default coordinate system in the model. To switch to one of the other two default planes, click the desired sketch tool, and press the Tab key. The origin of the current sketch plane is displayed.
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•
To change the coordinate system for your 3D sketch, click the desired sketch tool, hold down the Ctrl key, and click a plane, a planar face, or a user-defined coordinate system.
•
If you select a plane or a planar face, the 3D sketch planes rotate so that the XY sketch plane is aligned with the selected item.
•
If you select a coordinate system, the 3D sketch planes rotate so that the XY sketch plane is parallel to the XY plane of the coordinate system.
Space Handle When working in a 3D sketch, a graphical assistant is provided to help you maintain your orientation while you sketch on several planes. This assistant is called a space handle. The space handle appears when the first point of a line or spline is defined on a selected plane. Using the space handle, you can select the axis along which you want to sketch. By default, you sketch relative to the default coordinate system in the model. To switch to one of the other two default planes, click the sketch tool and press Tab. The origin of the current sketch plane is displayed.
Dimensioning a 3D Sketch When working in a 3D sketch, you can sketch lines to the approximate length, and then dimension them. •
You can add a length dimension by selecting two points, a line, or two parallel lines.
•
You can add an angular dimension by selecting either three points or two lines.
Virtual Sharps - 3D Sketch A virtual sharp represents a sketch point at the virtual intersection of two sketch entities. Virtual sharps appear automatically in 3D sketches for: •
Fillets
•
Sketch Chamfers
You can delete the automatic virtual sharps. To insert a virtual sharp between two sketch entities:
1.
Select the sketch entities.
2.
Click Point
or Tools, Sketch Entity, Point.
A virtual sharp appears at the point where the entities would intersect. You can add dimensions and relations to virtual sharps in 3D sketches.
3D Arc PropertyManager The Arc PropertyManager controls the following properties of an arc in a 3D sketch. To create an arc in a 3D sketch, use Sketch Fillet
on the Sketch toolbar to fillet two lines.
Existing Relations •
Relations . Displays relations inferenced automatically during sketching or created manually with Add Relations. When you select a relation in the list, a callout is highlighted in the graphics area.
•
Information on).
. Displays the status of the selected sketch entity (Fully Defined, Under Defined, and so
Add Relations You can add relations to the selected entity. The list includes only relations that are possible for the selected entity. Options For construction. Converts the entity to construction geometry.
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Parameters You can specify any appropriate combination of the following parameters to define the arc if the arc is not constrained by relations. When you change one or more parameters, the other parameters update automatically. Center X Coordinate Center Y Coordinate Center Z Coordinate Start X Coordinate Start Y Coordinate Start Z Coordinate End X Coordinate End Y Coordinate End Z Coordinate Radius Angle. Subtended by the arc.
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4 2D to 3D Conversion
2D to 3D Conversion Overview You can convert 2D sketches into 3D models. Example of 2D to 3D Conversion: The original drawing is imported into a part document as Sketch1. The sketch entites in the lower left corner become the Front view. The top left becomes the Top view. The lower right becomes the Right view. The upper right is an Auxiliary view.
The Front view is at the lower left. The Top, Right, and Auxiliary views are folded perpendicular to the Front view.
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Chapter 4 2D to 3D Conversion
An isometric view displays the orientation of the sketches.
Align the left edges of the Auxiliary and Top sketches, then the Right and Auxiliary sketches.
Extrude the base feature.
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Cut or extrude other features. In this example, a round hole, a rectangular hole, and a rectangular notch are cut to complete the part.
The 2D sketch can be an imported drawing, or it can be a sketch constructed in SolidWorks. In either case, it must be a single sketch in a part document. NOTE: Even though the sketch can be an imported drawing, it must be imported into a sketch in a part document. You can copy and paste the drawing from a drawing document, or you can import the drawing directly into a 2D sketch in a part document. The conversion procedure is generally as follows: 1.
In a part document, import a drawing into a sketch or construct a new sketch.
2.
Edit the sketch.
3.
Extract sketches for views from the Front, Top, and so on. The sketches fold up into the appropriate orientation.
4.
Align the sketches.
5.
Extrude the base feature.
6.
Cut or extrude other features.
The tools for the conversion process are on the 2D To 3D Toolbar.
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Chapter 4 2D to 3D Conversion
2D to 3D Toolbar The 2D to 3D tools help you convert a 2D drawing to a 3D part. Some of the tools can be used in any sketches. Front. The selected sketch entities become the front view in converting to a 3D part. Top. The selected sketch entities become the top view in converting to a 3D part. Right. The selected sketch entities become the right view in converting to a 3D part. Left. The selected sketch entities become the left view in converting to a 3D part. Bottom. The selected sketch entities become the bottom view in converting to a 3D part. Back. The selected sketch entities become the back view in converting to a 3D part. Auxiliary. The selected sketch entities become an auxiliary view in converting to a 3D part. You must select a line in another view to specify the angle of the auxiliary view. Create Sketch from Selections. The selected sketch entities become a new sketch. You can extract a sketch, for example, and then modify it before creating a feature. Repair Sketch. You can fix errors in a sketch so that the sketch can be used to extrude or cut a feature. Typical errors can be overlapping geometry, small gaps, or many small segments that are collected into a single entity. Align Sketch. Select an edge in one view to align to the edge selected in a second view. The order of selection is important. Extrude. Extrude a feature from the selected sketch entities. You do not have to select a complete sketch. Cut. Cut a feature from the selected sketch entities. You do not have to select a complete sketch.
Importing Drawings into Part Documents You can import a 2D drawing directly into a sketch in a part document for conversion into a 3D model. To import a drawing into a part document:
1.
Open the drawing (.dwg or .dxf file) in SolidWorks. The DXF/DWG Import dialog box appears.
2.
Select Import to a new part and click Next.
3.
Select Import to a 2D sketch. NOTE: It is recommended that you select Skip CrossHatch Import when importing for conversion.
4.
Click Finish. The drawing appears as Sketch1 in the FeatureManager design tree. To continue with the conversion, edit the sketch and extract new sketches.
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Extracting Sketches To create a base feature from a 2D drawing, extract sketches to specify the appropriate views. The sketches fold up automatically into the correct orientation as though the drawing were a piece of paper. Specify which portions of the drawing are the sketches for the front view, the right view, and so on. You can also create auxiliary sketches that are not parallel to the principal view planes. To extract a sketch for the front view:
1.
While editing a sketch, select the sketch entities that make up the front view. NOTE: You must define a Front view before defining any of the other views. You can box select, chain select, or hold Ctrl and select entities individually.
2.
Click Front
on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Front.
A new sketch appears in the FeatureManager design tree. To extract other orthogonal sketches:
1.
While still editing the original sketch, select the sketch entities that make up one of the orthogonal views, such as the top, right, left, bottom, or back.
2.
Click the corresponding icon on the 2D to 3D toolbar or on the Tools, Sketch Tools, 2D to 3D menu. A new sketch appears in the FeatureManager design tree. The sketch folds into the correct orientation to the Front view.
To extract auxiliary sketches:
1.
While editing a sketch, select the sketch entities that make up the auxiliary view.
2.
Hold Ctrl and select a line in another view to specify the angle of the auxiliary view.
3.
Click Auxiliary
on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Auxiliary.
Example of Auxiliary View: Sketch entities for auxiliary view Line defines angle of auxiliary view
Next, align the sketches.
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Chapter 4 2D to 3D Conversion
Aligning Sketches After extracting sketches for conversion to a 3D part, you can align the sketches before creating the base feature. The sketch selected first moves to align with the sketch selected second. To align sketches:
1.
Select a line or a point in a sketch to be aligned with another sketch.
2.
Hold Ctrl and select a line or a point in the second sketch to which the first sketch is to be aligned.
3.
Click Align Sketch
on the 2D to 3D toolbar, or click Tools, Sketch Tools, Align, Sketch.
Example of Aligning Sketches: Two sketchs, Top and Auxiliary, are not aligned. The Top sketch is to remain stationary while the Auxiliary sketch moves into alignment.
Top sketch Select the line indicated in the Auxiliary sketch, then hold Ctrl and select the line indicated in the Top sketch.
Click Align Sketch . The Auxiliary sketch moves into alignment with the Top sketch.
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Auxiliary sketch
Extruding in 2D to 3D You can extrude base features and other features using Extrude
on the 2D to 3D toolbar with partial sketches.
NOTE: Extruded Boss/Base on the Features toolbar accepts only complete sketches. To extrude a feature:
1.
Edit a sketch.
2.
Select the sketch entities required for the feature. NOTE: It is not necessary to select a complete sketch.
3.
Hold Ctrl and select a point (in any sketch) to be the starting point for the extrusion. NOTE: If you do not select a starting point, or if you select a point in the edited sketch, the plane of the sketch is considered to be the starting point.
4.
Click Extrude on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Extrude, and click in the graphics area to establish the direction of the extrusion. The Base-Extrude PropertyManager appears.
5.
Edit the properties in the Base Extrude PropertyManager. NOTE: For 2D to 3D conversion, you can specify the depth of a blind extrusion by selecting a sketch entity. Click Depth
6.
Click OK
and select an entity in a sketch. .
Example of Extruding in 2D to 3D Conversion: Select the sketch entities (in the Front sketch at the lower left) as the basis for the base extrusion. Hold Ctrl and select a starting point (upper left vertex in the Top sketch).
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Click in the graphics area to establish the direction of the extrusion.
In the Base-Extrude PropertyManager, click Depth and select the line shown to specify the depth of the extrusion.
Cutting in 2D to 3D You can cut features using Cut
on the 2D to 3D toolbar with partial sketches.
NOTE: Extruded Cut on the Features toolbar accepts only complete sketches. To cut a feature:
1.
Edit a sketch.
2.
Select the sketch entities required for the feature. NOTE: It is not necessary to select a complete sketch.
3.
Hold Ctrl and select a face to be the starting point for the cut.
4.
Click Cut on the 2D to 3D toolbar, or click Tools, Sketch Tools, 2D to 3D, Cut, and click in the graphics area to establish the direction of the cut. The Cut-Extrude PropertyManager appears.
5.
Edit the properties in the Base Extrude PropertyManager. NOTE: For 2D to 3D conversion, you can specify the depth of a blind cut by selecting a sketch entity. Click Depth
6.
4-8
Click OK
and select an entity in a sketch. .
Example of Cutting in 2D to 3D Conversion: Select the sketch entities shown in the auxiliary view to define the cut. Hold Ctrl and select the face shown on the base feature as the starting point.
Click Cut on the 2D to 3D toolbar and click in the graphics area to establish the direction of the cut.
In the Cut-Extrude PropertyManager, click Depth and select the line shown in the front view to specify the depth of the cut. Click OK
.
Click Hidden Lines Visible View toolbar to see the cut.
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Chapter 4 2D to 3D Conversion
Additional Conversion Tools Repair Sketch Repair Sketch can often fix errors in a sketch so that the sketch can be used to create a feature. Some tools (Extrude and Cut, for example) repair sketches automatically when they detect errors they can fix. You can also repair sketches manually. Repair Sketch is particularly useful for sketches created by importing DXF/DWG files. Repair Sketch proceeds automatically as follows: •
Delete zero length line and arc segments (zero length is a segment less than ±1.0e-8 meters)
•
Merge colinear lines that overlap
•
Eliminate gaps of less than ±1.0e-8 meters in colinear lines
•
Collect small segments in colinear lines with no gaps greater than ±1.0e-8 meters
•
Merge coincident lines (separated by less than ±1.0e-8 meters) into one line
To repair a sketch automatically:
1.
Select a sketch in the FeatureManager design tree.
2.
Click Extrude
or Cut
on the 2D to 3D toolbar, or click Extruded Base/Boss
or Extruded
Cut on the Features toolbar. A warning message states the error and offers to repair the sketch. 3.
Click OK to attempt the repair and continue to create the feature.
To repair a sketch manually:
1.
Select a sketch in the FeatureManager design tree.
2.
Click Repair Sketch
on the 2D to 3D toolbar, or click Tools, Sketch Tools, Repair Sketch.
Create Sketch from Selections With Create Sketch from Selections , you can extract only those elements of a sketch (usually in an imported drawing) that you require to create a feature. You can extract a sketch, for example, and then modify it before creating a feature. To create a sketch from selections:
1.
Edit a sketch.
2.
Select the sketch entities you want in the new sketch.
3.
Click Create Sketch from Selections
, or click Tools, Sketch Tools, Create Sketch from Selections.
A new sketch appears in the FeatureManager design tree.
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5 Reference Geometry
Reference Geometry Overview Reference geometry defines the shape or form of a surface or a solid. Reference geometry includes planes, axes, coordinate systems, points, and 3D curves. You can use reference geometry in the creation of several kinds of features: •
planes are used in lofts and sweeps
•
split lines are used in some drafts and chamfers
•
an axis is used in a circular pattern
This chapter includes: •
Creating and using planes
•
Creating and using axes
•
Creating local coordinate systems
•
Converting sketch lines to construction geometry
•
Creating 3D curves
•
Creating reference points
Updating Reference Geometry in Document Templates You control the visibility of reference geometry and the names of the default planes in the document templates. To update the document templates:
1.
Click Open
2.
Select Template Files (*.prtdot, *.asmdot, *.drwdot) from the Files of type list.
3.
Browse to the desired file, and click Open.
4.
Make the necessary changes to the document template including the following:
5.
or File, Open.
•
Rename the planes
•
Toggle the visibility of the reference geometry (for example, click View, Origins.)
Click Save or File, Save to update the existing document template. Click File, Save As to update the name of the document template as well.
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Chapter 5 Reference Geometry
Planes Creating Planes You can create planes in part or assembly documents. You can use planes to sketch, to create a section view of a model, for a neutral plane in a draft feature, and so on. You can preselect items before you click Plane . If you preselect items, SolidWorks attempts to select the appropriate type of plane. You can always select a different type of plane. You can right-click in the graphics area and select a plane type from the shortcut menu. When you have selected enough entities to create a plane, the OK
pointer appears. Right-click to create the plane.
NOTE: The created plane is 5% larger than the geometry on which the plane is created, or 5% larger than the bounding box. This helps reduce selection problems when planes are created directly on faces or from orthogonal geometry. To create a construction plane:
1.
Click Plane
on the Reference Geometry toolbar, or click Insert, Reference Geometry, Plane.
The Plane PropertyManager appears. 2.
Under Selections, select the type of plane you want to create and the items to create the plane: •
Through Lines/Points. Create a plane through an edge, axis, or sketch line, and a point, or through three points.
Select three points. Parallel Plane at Point. Create a plane through a point parallel to a plane or face. •
Select a face or planar face.
5-2
Then select a midpoint.
The new plane is parallel to the selected face through the chosen midpoint.
At Angle. Create a plane through an edge, axis, or sketch line at an angle to a face or plane.
• a.
Select a plane or planar face, and then select an edge, axis, or sketch line.
b.
Enter the angle between the planes in the Angle box.
c.
Select the Reverse direction check box, if necessary. The behavior of the plane is as follows:
If the selected line is in the same plane as the selected plane, the new plane rotates around the selected line.
If the selected line is parallel to the selected plane, the new plane moves to the parallel line and rotates around the line.
If the selected line is skewed with respect to the selected plane, the selected line is projected onto the selected plane and then the plane rotates around the projected line. In this sample, use Plane 1 and Axis 1 to create a new plane at an angle. Sketch the extrusion profile on Plane 4. Create the Y-shaped pipe. Offset. Create a plane parallel to a plane or face, offset by a specified distance. This is the default plane created.
• a.
Select a plane or planar face.
b.
Enter the offset distance in the Distance box.
c.
Select the Reverse direction check box, if necessary.
d.
To create multiple planes offset the same Distance from the selected plane, enter the number of planes in the Number of Planes to Create
Single offset plane
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Multiple offset planes
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Chapter 5 Reference Geometry
Normal to Curve. Create a plane through a point and perpendicular to an edge or curve.
• a.
Select an edge or curve, and a vertex or point.
b.
Select the Set origin on curve check box to place the origin on the curve; the default is to place the origin on the vertex or point.
In this example, you select just the helix to create the new plane. Plane 4 is perpendicular to the end of the tapered helix.
A circle is swept along the helix to create a spring.
The helical spring is used in a battery contact terminal.
On Surface. Create a plane on a non-planar face or angular surface. See Plane On Surface Examples.
• a.
Select a surface.
b.
Select a sketch point on the surface.
• a.
Drag and Drop. You can also drag and drop to create a plane. Select an existing plane border.
b.
Hold down the Ctrl key and drag the plane. The Plane PropertyManager appears with Offset Distance new plane appears in the graphics area.
c.
Drop the new plane in the new location.
d.
Adjust the values in the PropertyManager.
The selected items appear in the Reference Entities appears in the graphics area. 3.
Click OK
selected. A preview of the
box. A preview of the new plane
to create the plane.
The new plane appears in the graphics area and is listed in the FeatureManager design tree. NOTES:
5-4
•
To cancel the transaction, click Cancel
.
•
To display the Planes online help topic, click Help
•
To create multiple planes, click Keep Visible
. to keep the Plane PropertyManager displayed.
Plane On Surface Examples You can create the following types of planes using the On Surface •
tool in the Plane PropertyManager:
Any surface and a point that is not on that surface, using a projected sketch or the closest point 1.
Select the sketch point and the model surface.
Two options appear in the Plane PropertyManager: Project to nearest location on surface and Project onto surface along normal. 2.
Select one of these options. A preview of the new plane appears.
Project to nearest location on surface is selected. The new plane is created at the point on the surface closest to the selected sketch point.
SolidWorks 2004 Reference Guide
Project onto surface along sketch normal is selected. The new plane is created at the point on the surface obtained by projecting the sketch point normal to the plane on which the sketch point is located. Select the Reverse check box if the plane preview does not appear.
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Chapter 5 Reference Geometry
•
A cylindrical face and a plane 1.
Select the cylindrical face.
2.
Select a plane that intersects the axis of the cylinder.
The preview of the new plane is created tangent to the selected face, along the line where the plane intersects the surface. 3.
Select the Normal plane check box (optional).
A preview of the new plane appears with an Offset angle of 45 degrees. You can adjust the offset angle, as needed. The new plane intersects the axis of the cylinder.
5-6
•
A conical face and a plane 1.
Select the conical face.
2.
Select a plane that intersects the selected face.
The preview of the new plane is created tangent to the selected surface, along the line where the plane intersects the surface. 3.
Select the Normal plane check box (optional).
The plane preview changes. The axis of the selected face is used for an at-angle plane relative to the selected plane, creating a new plane normal to the selected surface. 4.
Adjust the angle of the new plane in the Offset
box.
The new plane
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Chapter 5 Reference Geometry
•
A surface, a plane, and an edge 1.
Select a surface.
2.
Select a plane that cuts through the surface.
3.
Select an edge on the surface. A preview of the new plane appears.
The plane is created tangent to the selected surface at the point where the selected plane intersects the selected edge.
Plane tangency
The new plane
Changing Plane Names To change the names for construction planes in the current document:
1.
Click-pause-click the plane’s name in the FeatureManager design tree.
2.
Type a new name. TIP: As you create additional construction planes, it is a good idea to change their names to indicate their purpose.
To change the default names used for planes:
You can create new default plane names to replace the existing plane names. You save this information in a document template.
Plane Display You can set the following plane display options for part and assembly documents: •
Face color
•
Transparency
•
Intersection display and color
NOTE: You must enable the Display shaded planes option to display shaded planes. To set the plane display:
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1.
Open a part or assembly document.
2.
Click Tools, Options. On the Document Properties tab, click Plane Display.
3.
Under Faces, set the following options:
•
Front Face Color. Displays the Color dialog box that you use to set the front face color of planes.
Front face color
Back face color
•
Back Face Color. Displays the Color dialog box that you use to set the back face color of planes.
•
Transparency. Controls the plane transparency (0% displays a solid face color; 100% displays no face color).
0% transparency
75% transparency
100% transparency
NOTE: Edges take the same color as the front and back faces, are not transparent, and are always displayed. 4.
Under Intersections, set the following options: •
Show intersections. Select or clear the Show intersections check box to display or hide the intersection of planes.
Plane intersection lines displayed • 5.
Plane intersection lines hidden
Line Color. Displays the Color dialog box that you use to set the plane intersection line color.
Click OK to accept the changes, or Cancel to discard the changes and exit the dialog box.
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Chapter 5 Reference Geometry
Hiding or Showing Planes You can turn the display of planes on or off. To toggle the display of planes:
Click View, Planes. A check mark next to the menu item means planes are visible (except for planes you have hidden individually). To hide or show individual planes:
1.
Right-click the plane in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show. NOTE: Individual planes always are highlighted when you select them, even when hidden.
Moving, Resizing, and Copying Planes You can move, resize, and copy planes using the plane handles and edges. To display the plane’s handles:
•
Click the plane’s name in the FeatureManager design tree or in the graphics area, - or -
•
Click the edge of the plane.
Using the plane’s handles and edges, you can do the following: •
Resize the plane by dragging a corner or edge handle.
•
Move the plane by dragging the edge of the plane.
•
Copy the plane by selecting a plane in the graphics area. Then hold down the Ctrl key and, using the edge, drag to a new location. An offset plane is created.
To modify the offset distance, angle, or distance between planes:
1.
Double-click the plane to display the offset distance or angle.
2.
Double-click the dimension or angle and type a new value in the Modify dialog box. - or -
1.
Right-click the name of the plane in the FeatureManager design tree.
2.
Select Edit Feature.
3.
In the PropertyManager, enter new values to define the plane, then click OK
.
Automatic Sizing of Planes and Axes Planes and axes that you create are automatically sized to either the geometry on which they are created, or to the bounding box of the model geometry. As the geometry changes size, the planes and axes update accordingly. You can override the automatic sizing by manually changing the plane or axis size, which disables future autosizing for that entity. You can re-enable autosizing by selecting Autosize from the shortcut menu. NOTE: The created plane is 5% larger than the geometry on which the plane is created, or 5% larger than the bounding box. This helps reduce selection problems when planes are created directly on faces or from orthogonal geometry.
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To see an example of automatic sizing of planes:
1.
Select a planar face and create an offset plane. Offset plane 1 appears and is automatically sized to the geometry of the face from which it was created.
2.
Click View, Planes.
3.
Edit the sketch to double the dimension of the bottom edge of the model, then exit the sketch. The plane 1 size updates automatically when you change the geometry of the face on which it was created.
4.
Drag upwards to manually resize the top edge of plane 1. Autosizing becomes disabled.
5.
Edit the sketch again to change the bottom edge dimension back to the original size, then exit the sketch. Plane 1 does not resize automatically because autosizing is disabled.
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Chapter 5 Reference Geometry
6.
Right-click plane 1 in the graphics area and select Autosize. Autosizing is re-enabled. Plane 1 automatically resizes to the updated model geometry.
Axis Overview You can use an axis in creating sketch geometry or in a circular pattern. Every cylindrical and conical face has an axis. Temporary axes are those created implicitly by cones and cylinders in the model. You can set the default to either hide or show all temporary axes. To display temporary axes:
Click View, Temporary Axes. A check mark next to the menu item means temporary axes are visible.
To turn the display of axes on or off:
Click View, Axes. A check mark next to the menu item means axes are visible (except for axes you have hidden individually). To hide or show an individual axis:
1.
Right-click the axis in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show.
Reference Axis You can create a reference axis, also called a construction axis. To create a reference axis:
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1.
Click Axis
on the Reference Geometry toolbar, or click Insert, Reference Geometry, Axis.
2.
Select the axis type in the Axis PropertyManager, then select the required entities for that type.
3.
Verify that the items listed in Reference Entities
4.
Click OK
5.
Click View, Axes to see the new axis.
.
correspond to your selections.
Reference Axis The Axis PropertyManager appears when you create a new axis or edit an existing axis. The PropertyManager controls the following properties: Reference Entities. Displays the selected entities. One Line/Edge/Axis. Select a sketch line, an edge, or select View, Temporary Axes and then select the axis that is displayed. Two Planes. Select two planar faces, or select View, Planes, and then select two planes. Two Points/Vertices. Select two vertices, points, or midpoints. Cylindrical/Conical Surface. Select a cylindrical or conical face. Point and Surface. Select a surface or plane and a vertex point, or midpoint. The resultant axis is normal to the selected surface or plane through the selected vertex, point, or midpoint. If the surface is non-planar, the point must be on the surface.
Coordinate System You can define a coordinate system for a part or assembly. Use this coordinate system with the Measure and Mass Properties tools, and for exporting SolidWorks documents to IGES, STL, ACIS, STEP, Parasolid, VRML, and VDA. To create a coordinate system:
1.
Click Coordinate System Coordinate System.
on the Reference Geometry toolbar, or click Insert, Reference Geometry,
2.
Use the Coordinate System PropertyManager to create the coordinate system. You can amend your selections:
3.
•
To change your selections, right-click in the graphics area and select Clear Selections.
•
To reverse the direction of an axis, click its Reverse Axis Direction PropertyManager.
Click OK
button in the
.
You may need to locate a coordinate system where there are insufficient entities available to define the coordinate system. In this case, you can define a coordinate system someplace on the part that does provide the entities you need. Then you can move the new origin to the desired location. The new location must contain at least one point or vertex. To translate a coordinate system to a new location:
1.
Click Coordinate System
or Insert, Reference Geometry, Coordinate System.
2.
Define the coordinate system at a location on the part that provides the entities you need to control the angle and direction of each axis.
3.
Click in Origin, then select the point or vertex to which you want to translate the origin.
4.
Click OK. The origin moves to the location that you selected. When you create a coordinate system, it is a good idea to give it a meaningful name to explain its purpose. Click-pause-click the coordinate system’s name in the FeatureManager design tree and enter a new name.
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Chapter 5 Reference Geometry
To toggle the display of coordinate systems:
Click View, Coordinate Systems. A check mark next to the menu item means coordinate systems are visible. To hide or show individual coordinate systems:
1.
Right-click the coordinate system in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show. Individual coordinate systems always are highlighted when you select them, even when hidden.
Coordinate System PropertyManager The Coordinate System PropertyManager appears when you add a new coordinate system to a part or assembly or edit an existing coordinate system. The PropertyManager controls the following properties: Origin. Select a vertex, point, midpoint, or the default point of origin on a part or assembly for the coordinate system origin. X axis, Y axis, and Z axis. Select one of the following for the Axis Direction Reference: •
Vertex, point, or midpoint. Aligns the axis toward the selected point.
•
Linear edge or sketch line. Aligns the axis parallel to the selected edge or line.
•
Non-linear edge or sketch entity. Aligns the axis toward the selected location on the selected entity.
•
Planar face. Aligns the axis in the normal direction of the selected face. Reverse Axis Direction. Reverses the direction of an axis.
Origin The model origin appears in blue and represents the (0,0,0) coordinate of the model. When a sketch is active, a sketch origin appears in red and represents the (0,0,0) coordinate of the sketch. Dimensions and relations can be added to the model origin, but not to a sketch origin. To toggle the origin display:
Click View, Origins. A check mark next to the menu item means origins are visible (except for origins you have hidden individually).
Centroid If you select centroid as the reference point for a table-driven or sketch-driven pattern, the system determines the centroid based on the type of seed feature.
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•
For cylindrical, conical, or revolved features, the centroid is the intersection of the axis of revolution with the X-Y plane of the pattern.
•
If the sketch consists of lines and arcs, such as rectangles or oval shapes, and if the sketch plane is parallel to the X-Y plane, the centroid is defined as the centroid of the sketch.
•
For any other condition, the centroid is the centroid of the face of the seed feature.
•
If there is more than one seed feature, the centroid of the first seed feature is used.
•
If the seed feature is generated from a sketch that includes multiple contours, the centroid of the largest closed contour is used.
Converting Sketch Lines to Construction Geometry You can convert sketched entities into construction geometry to use in creating model geometry. To convert one or more sketch entities to construction geometry:
1.
In an open sketch, select the sketch entities to convert.
2.
Do one of the following: •
Click Construction Geometry
on the Sketch toolbar.
•
Select the For construction check box in the PropertyManager.
To convert sketch entities in a drawing to construction geometry:
Select the sketch entities that you want to convert and use one of the following methods: •
Click Construction Geometry
on the Sketch toolbar.
•
Click Tools, Sketch Tools, Construction Geometry.
•
Select the For construction check box in the PropertyManager.
•
Right-click any selected sketch entity and select Construction Geometry.
Curve Overview You can create several types of 3D curves by using these methods: •
Projected Curve - from a sketch projected to a model face or surface, or from sketched lines on intersecting planes
•
Composite Curve - from a combination of curves, sketch geometry, and model edges
•
Helix and Spiral - by specifying a circular sketch, pitch, number of revolutions, and height
•
Split Line - from a sketch projected to planar or curved (silhouette) faces
•
Curve Through Reference Points - from user-defined points or existing vertices
•
Curve Through XYZ Points - from a list of X,Y, Z coordinates for points
You can then use the curves to create solid model features. For example, you can use a curve as the path or guide curve for a sweep feature, as the guide curve for a loft feature, as a parting line for a draft feature, and so on. You can turn the display of curves on or off. To toggle the display of curves:
Click View, Curves. A check mark next to the menu item means curves are visible (except for curves you have hidden individually). To hide or show individual curves:
1.
Right-click the curve in the graphics area or in the FeatureManager design tree.
2.
Select Hide or Show. Individual curves always are highlighted when you select them, even when hidden.
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Chapter 5 Reference Geometry
Curve Through XYZ Points 1.
Click Curve Through XYZ Points XYZ Points.
on the Curves toolbar, or click Insert, Curve, Curve Through
2.
Create new sets of coordinates by double-clicking cells in the X, Y, and Z columns and entering a point coordinate in each one. (Created outside of a sketch, the X, Y, and Z coordinates are interpreted with respect to the Front plane coordinate system.) The numbers in the Point column define the order in which the points are connected.
3.
Click OK to display the curve. The Curve Through XYZ Points tree.
icon appears next to the curve name in the FeatureManager design
Tips for working with this tool:
•
Open an existing curve file. Click Browse and navigate to a curve file to open. You can open .sldcrv files or .txt files that use the same format as .sldcrv files. You can also create 3D curves in Excel for example, save them as .txt files, then open them in SolidWorks. To be able to open text files, they must contain only coordinate data (not the X, Y, or Z labels , or other extraneous data).
•
Change coordinates. Double-click in a cell and enter a new value. (As you enter values, notice the preview of the curve is displayed in the graphics area.)
•
Add a row. Double-click in a cell in the row below the last numbered row.
•
Insert a row. Drag the cursor across a row to select it, then click Insert. A new row is inserted above the selected row.
•
Delete a row. Drag the cursor across a row to select it, then press the Delete key.
•
Save the curve file. Click Save or Save As, navigate to the desired location, and specify the filename. If you do not specify an extension, the SolidWorks application adds the extension .sldcrv.
Curve Through Reference Points Creates a curve through points located on one or more planes. 1.
Click Curve Through Reference Points Through Reference Points.
on the Curves toolbar, or click Insert, Curve, Curve
The Curve Through Reference Points PropertyManager appears. 2.
Select the sketch points or vertices, or both, in the order in which you want to create the curve. As you select, the entities are listed in the Through Points box.
3.
If you want to close the curve, select the Closed Curve check box.
4.
Click OK
.
The Curve Through Reference Points design tree.
Create curves to connect sketch points between two loft profiles.
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icon appears next to the curve name in the FeatureManager
Create the propellers for the fan using a loft feature and a circular pattern.
Here is the completed fan assembly.
Curve from File To create a curve from an existing file containing coordinate values:
1.
Create a file containing coordinate values for curve points using a text editor or worksheet application. The file format must be a three-column, tab or space-delimited list of only X, Y, and Z coordinates. Do not include any column headings, such as X, Y, and Z.
2.
Save the file as a text file.
3.
Click Curve Through XYZ Points XYZ Points.
4.
Click Browse to locate the file, then click Open.
on the Curves toolbar, or click Insert, Curve, Curve Through
The coordinates from the file are displayed in the Curve File dialog box. Notice the numbers in the Point column, indicating the order in which the points will be connected. 5.
Examine the preview of the curve, and edit the coordinates if necessary, until you are satisfied with the result. (Double-click in any cell, then edit the value.)
6.
Click OK.
Helix and Spiral You can create a helix or spiral curve in a part. The helix can be used as a path or guide curve for a swept feature, or a guide curve for a lofted feature. To create a helix or spiral:
1.
Open a sketch and sketch a circle. The diameter of this circle controls the diameter of the helix.
2.
Click Helix and Spiral
3.
Set values in the Helix/Spiral PropertyManager.
on the Curves toolbar, or click Insert, Curve, Helix/Spiral.
To define a helix, you specify two values, and the third value is automatically calculated. 4.
Click OK
.
The helix and the sweep profile are on the neck of the bottle.
A boss-sweep feature (shown in blue) creates the threads on the neck of the bottle.
Spiral spring
Spiral spring in the internal mechanism of a clock
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Chapter 5 Reference Geometry
Helix/Spiral PropertyManager The Helix/Spiral PropertyManager appears when you create a new helix or spiral in a sketch or edit an existing helix or spiral. The PropertyManager controls the following properties: Defined By •
Pitch and Revolution. Creates a helix defined by Pitch and Revolutions.
•
Height and Revolution. Creates a helix defined by Height and Revolutions.
•
Height and Pitch. Creates a helix defined by Height and Pitch.
•
Spiral. Creates a spiral defined by Pitch and Revolutions.
Parameters •
Height (Helix only). Sets the height.
•
Pitch. Sets the rate of change of radius for each revolution. The Pitch value must be at least 0.001 and not greater than 200000.
•
Revolutions. Sets the number of turns.
•
Reverse direction. Extends the helix backwards from the point of origin, or creates an inward spiral.
•
Start angle. Sets where to start the first turn on the sketched circle.
•
Clockwise. Sets the direction of the turns to clockwise.
•
Counterclockwise. Sets the direction of the turns to counterclockwise.
Taper Helix •
Taper Helix. Creates a tapered helix.
•
Taper Angle. Sets the angle of the taper.
•
Taper outward. Tapers the helix outward.
Projecting Sketched Curves You can project a sketched curve onto a model face to create a 3D curve. You can also create a 3D curve that represents the intersection of two extruded surfaces generated by creating sketches on two intersecting planes. You can preselect items before you click Projection appropriate type of projection. •
. If you preselect items, SolidWorks attempts to select the
If you preselect two sketches, the Sketch onto Sketch option is activated with the two sketches shown under Sketches to Project
.
•
If you preselect a sketch and one or more faces, the Sketch onto Face(s) option is activated with the selected items shown in the correct boxes.
•
If you preselect one or more faces, the Sketch onto Face(s) option is activated.
You can right-click in the graphics area and select a projection type from the shortcut menu. When you have selected enough entities to create a projected curve, the OK
pointer appears. Right-click to create the projected curve.
To project a curve:
1.
Click Projection
on the Curves toolbar, or Insert, Curve, Projected.
The Projected Curve PropertyManager appears. 2.
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Under Selections, set Projection Type to one of the following:
Sketch onto Face(s)
Use this selection to project a sketched curve onto a model face. •
Under Sketch to Project design tree.
, select the curve in the graphics area or from the flyout FeatureManager
•
Under Projection Faces
•
Select the Reverse Projection check box, or click the handle in the graphics area, if necessary.
, select the cylindrical face on the model where you want to project the sketch.
Original sketch to project onto a face
Projected curve
Projected curve used as a sweep path
Sketch onto Sketch
Use this selection to create a curve that represents the intersection of sketches from two intersecting planes. •
Create a sketch on each of two intersecting planes, closing each sketch when you are done.
•
Align the sketch profiles such that when they are projected normal to their sketch plane; the implied surfaces will intersect, creating the desired result.
•
Under Sketches to Project graphics area.
, select both sketches in the flyout FeatureManager design tree or the
The two sketches (gray) project onto each other to form the 3D curve (green).
The curve is used as a path for a sweep.
The swept geometry is used to create this power adapter.
A preview of the projected curve appears. 3.
Click OK
to create the projected curve, or Cancel
to cancel the transaction.
Replacing a Sketch of a Projected Curve You can replace one or more of the sketches that make up a projected curve of two sketches projected onto one another. To replace a sketch in a projected curve:
1.
Right-click the Curve feature in the FeatureManager design tree, or right-click the curve in the graphics area, and select Edit Feature. The Curve PropertyManager appears.
2.
3.
Choose one of the following methods to clear the unwanted sketch from the Sketch to Project box: •
Click the sketch in the flyout FeatureManager design tree.
•
Click the sketch in the graphics area.
• Select the sketch in the Sketches to Project box under Selections, and press Delete. Select the replacement sketch in either the flyout FeatureManager design tree or in the graphics area, then click OK
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Chapter 5 Reference Geometry
Split Lines The Split Line tool on the Curves toolbar projects a sketch to curved or planar faces. It divides a selected face into multiple separate faces, enabling you to select each face. You can also project a sketch onto a surface body. You can use this tool to create two types of split lines: •
Projection. Projects a sketch line on a surface.
•
Silhouette. Creates a split line on a cylindrical part.
To create a projection split line:
1.
Sketch a line to project as a split line.
2.
Click Split Line
on the Curves toolbar, or click Insert, Curve, Split Line.
The Split Line PropertyManager appears. 3.
Under Type of Split, select Projection.
4.
Under Selections, do the following:
5.
•
If necessary, click the Sketch to Project box and select the sketched line in the flyout FeatureManager design tree or in the graphics area.
•
Click the Faces to Split box and select the faces around the perimeter of the part that you want the split line to pass through.
•
Select the Single Direction check box to project the split line in only one direction.
•
Select the Reverse Direction check box, if necessary, to project the split line in the opposite direction.
Click OK
.
The sketch line is projected onto the faces you selected. In this example, the four sides were selected. The split line appears on each face, dividing each face into two sections. Example of a projected split line on a surface:
Before
5-20
After
To create a silhouette split line:
1.
Click Split Line
on the Curves toolbar, or click Insert, Curve, Split Line.
The Split Line PropertyManager appears. 2.
Under Type of Split, click Silhouette.
3.
Under Selections, do the following:
4.
•
Under Direction of Pull , in the flyout FeatureManager design tree or graphics area, select a plane to project through the model's silhouette (outer edges).
•
Under Faces to Split
Click OK
, select one or more faces to split. The faces cannot be planar.
.
The plane is projected through the model, creating silhouette split lines where the plane intersects the outer edges of the selected faces.
The selected plane is projected through the model in the direction of pull.
A silhouette split line is created on the model where the selected plane projected through the outer model edges.
Composite Curve You can create composite curves by combining curves, sketch geometry, and model edges into a single curve. Use a composite curve as a guide curve when creating a loft or a sweep. To create a composite curve:
1.
Click Composite Curve
on the Curves toolbar, or click Insert, Curve, Composite.
2.
Click the items (sketch entities, edges, and so on) that you want to join. The selected items appear in the Composite Curve Property Manager, under Entities to Join in the Sketches, Edges, and Curves to Join
3.
Click OK
to create the composite curve.
Select the edges on the model for the curve.
SolidWorks 2004 Reference Guide
box.
Create the sweep profile sketch, then use the composite curve as the sweep path.
Here is the completed sweep cut.
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Chapter 5 Reference Geometry
Reference Points You can create several types of reference points to use as construction objects. You can also create multiple reference points that are a specified distance apart on curves. Click View, Points to toggle the display of reference points. When you select items, the SolidWorks software attempts to select the appropriate point construction method. For example, if you select a face, SolidWorks selects the Center of Face construction method in the PropertyManager. You can always select a different type of point construction method. To create a single reference point:
1.
Click Point
on the Reference Geometry toolbar, or click Insert, Reference Geometry, Point.
2.
In the PropertyManager, select the type of reference point to create.
3.
In the graphics area, select the entities to use to create the reference point.
4.
Click OK
.
To create multiple reference points along a curve:
1.
In a model with a curve, click Point Geometry, Point.
2.
In the PropertyManager:
3.
on the Reference Geometry toolbar, or click Insert, Reference
•
Select Along curve distance or multiple reference point
•
Select a curve along which you want to create the reference points.
•
Select a distribution type: Distance, Percentage, or Evenly Distribute.
•
Set values for Number of specified points according to distance.
Click OK
.
and for Enter the distance/percentage value
.
Point PropertyManager The Point PropertyManager appears when you create a new reference point or edit an existing reference point. When you select items, the SolidWorks software attempts to select the appropriate point construction method. For example, if you select a face, SolidWorks selects the Center of Face construction method in the PropertyManager. You can always select a different type of point construction method. The PropertyManager controls the following properties: Reference Entities. Displays the selected entities used to create a reference point. Arc Center. Creates a reference point at the center of the selected arc or circle. Center Of Face. Creates a reference point at the center of gravity of the selected face. You can select planar or non-planar faces. Intersection. Creates a reference point at the intersection of the two selected entities. You can select edges, curves, sketch segments, and reference axes. Projection. Creates a reference point from one entity projected onto another. Select two entities: the entity to project and the entity onto which to project. You can project points, endpoints of curves and sketch segments, and vertices of solids and surfaces onto planes and faces (planar or non-planar). The point is projected normal to the plane or face.
5-22
Along curve distance or multiple reference point. Creates a set of reference points along edges, curves, or sketch segments. Select the entity and create the reference points using these options: •
Enter the distance/percentage value according to distance. Set a distance or percentage value to create the reference points. If the value is too large to create the specified number of reference points, a message warns you to set a smaller value.
•
Distance. Creates the number of reference points spaced at the distance you set, starting from the closest endpoint. The first reference point is created at this distance from the endpoint, not on the endpoint.
•
Percentage. Creates the number of reference points spaced at the percentage you set, starting from the closest endpoint. Percentage means percentage of the length of the selected entity. For example, select a 100mm-long entity. If you set the number of reference points to 5 and the percentage to 10, the 5 reference points are spaced 10 percent of the total entity length (or 10mm) apart from each other.
•
Evenly Distribute. Evenly distributes the number of reference points on the entity. If you edit the number of reference points, the reference points update their position relative to the starting endpoint.
•
Number of reference points. Set the number of reference points to create along the selected entity. The reference points are created using the selected Distance, Percentage, or Evenly Distribute option.
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Chapter 5 Reference Geometry
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6 Features
Features Overview Features are the individual shapes that, when combined, make up the part. You can also add some types of features to assemblies. Features include multibody part capability. You can include separate extrude, revolve, loft, or sweep features, within the same part document. Features include: •
Base/Boss, and Cut
•
Extrude, Revolve, Sweep, and Loft
•
Fillet/Round, Chamfer, and Draft
•
Hole - Simple and Hole Wizard
•
Scale
•
Shell
•
Rib
•
Dome
•
Shape
•
Pattern and Mirror
Some features originate as sketches; other features, such as shells or fillets, are created when you select the appropriate tool or menu command and define the dimensions or characteristics that you want. Surfaces Surfaces are another type of feature. You can use surfaces to create or modify solid features. Other ways you can use surfaces include the following: •
Import from other applications
•
Thicken to create solid geometry
•
Extrude, revolve, sweep, loft, knit, or offset from a model face or surface
•
Extend, fillet, or trim a surface
•
Create a mid surface
•
Fill surface
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Chapter 6 Features
Features Toolbar The Features toolbar provides tools for creating model features. The set of features icons is very extensive so not all of them are included on the default Features toolbar. You can customize this toolbar by adding and removing icons to suit your working style and frequent tasks. See Customize Toolbars for more information. Extruded Boss/Base Revolved Boss/Base Sweep Loft Thicken Extruded Cut Revolved Cut Swept Cut Lofted Cut Thickened Cut Cut with Surface Fillet Chamfer Rib Scale Shell Draft Simple Hole Hole Wizard Dome Shape Deform
6-2
Wrap Move/Size Features Suppress Unsuppress Unsuppress with Dependents Linear Pattern Circular Pattern Mirror Feature Curve Driven Pattern Sketch Driven Pattern Table Driven Pattern Split Combine Join Delete Solid/Surface Imported Geometry Insert Part Move/Copy Bodies Library Feature
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Chapter 6 Features
Feature Previews You can display detailed previews and control what displays with the Detailed Preview PropertyManager. You can access the Detailed Preview PropertyManager from the PropertyManager in the following features: •
Extrudes
•
Ribs
•
Drafts
In the Detailed Preview PropertyManager you can select: •
Highlight new or modified faces. Display new extrude, rib, or draft features, or the faces that were affected by the previous edit. If you check this option, new or modified faces are highlighted in a different color, as opposed to appearing shaded as they do in the standard PropertyManager. All separate bodies appear in the preview.
•
Show only new or modified bodies. Display only new or modified bodies. All separate bodies are hidden in the preview. Only separate bodies are affected.
Detailed Preview - Extrudes
6-4
Extruded Cut. Standard preview from PropertyManager
Detailed View PropertyManager. Neither Highlight new or modified faces nor Show only new or modified faces are checked.
Detailed View PropertyManager. Highlight new or modified faces is checked.
Detailed View PropertyManager. Both Highlight new or modified faces and Show only new or modified faces are checked. All separate bodies are hidden in the preview.
Detailed Preview - Ribs
Ribs. Normal PropertyManager preview
Detailed View. Neither Highlight new or modified faces nor Show only new or modified faces are checked.
Detailed View. Highlight new or modified faces is checked.
Ribs applied to feature.
Detailed Preview - Draft
Draft. Normal PropertyManager preview.
Detailed View PropertyManager. Neither Highlight new or modified faces nor Show only new or modified faces are checked.
Detailed View PropertyManager. Highlight new or modified faces is checked.
Detailed View PropertyManager. Both Highlight new or modified faces and Show only new or modified faces are checked. All separate bodies are hidden in the preview.
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Chapter 6 Features
To use detailed preview:
1.
Create a model with an extrude, a rib, or a draft. You can also use an existing model, and add an extrude, a rib, or a draft, or click Edit Feature and review the most recent extrude, rib, or draft.
2.
Click Detailed Preview in the PropertyManager for the extrude, the rib, or the draft.
3.
In the Detailed Preview PropertyManager, select one of the following: • •
Highlight new or modified faces Show only new or modified faces
Highlight new or modified faces 4.
Click Detailed Preview to return to the normal PropertyManager. - or Click OK
6-6
to apply the new feature.
If you leave both check boxes clear, the preview is identical to the preview in the normal PropertyManager.
Show only new or modified faces
Chamfers Creates a beveled feature on selected edges or a vertex. To create a chamfer:
1.
Click Chamfer
on the Features toolbar, or click Insert, Features, Chamfer.
2.
Under Chamfer Parameters, do the following: •
Click Edges and Faces or Vertex
•
Select one of the following from the PropertyManager (or right-click to use the shortcut menu): o
Distance-distance
o
Angle-distance
o
Vertex
•
Select the Equal Distance check box to specify a single value for distance or vertex.
•
Select the Keep features check box if you want to retain features such as cuts or extrudes that would otherwise be removed when you apply the chamfer.
Original part
3.
, then select an entity in the graphics area.
Click OK
Keep features cleared
Keep features checked
.
Chamfer Distance-distance
Enter values for both distances on either side of the selected chamfer edges, or click Equal Distance and specify a single value.
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Chapter 6 Features
Chamfer Angle-distance Enter values for distance and angle in the Chamfer PropertyManager or in the graphics area. An arrow appears that points in the direction in which the distance is measured. If necessary, click Flip direction.
Chamfer Vertex
Chamfer-vertex Enter values for the distances on each side of the selected vertex, or click Equal Distance and specify a single value.
Deform Deform The deform feature allows you to alter the shape of a model locally or globally. You can apply the deform feature to both SolidWorks and imported models. There are two deform types: Curve to curve and Point. With each type, dynamic options control which faces or bodies are deformed, and the resulting geometry of the model. The curve to curve and point descriptions are an overview. For complete options: •
Curve to curve options
•
Point options
For examples on how to apply the deform feature: •
To deform a model using Curve to curve
•
To deform a model using Point
Curve to Curve Overview With Curve to curve deform, you select connected Initial curves , and connected Target curves under Deform curves. The curves you select can be part of the model, or separate sketches. The curves can be curved or linear entities.
6-8
Under Deform Region, you can specify the Bodies to be deformed: •
With Fixed edges selected, you can specify Fixed curves/edges/faces deform
•
, and Additional faces to
.
With Fixed edges cleared, you can control the area to deform by specifying a Deform radius
.
You can create different shapes when you select or clear the Uniform option. With Shape Options, you can also control the shape of the deformation by specifying a level of stiffness. Point Overview With Point deform, you select a point on a body or a point in space. A point on a body can be: •
point on an edge
•
point on a face
•
vertex
The point you select is the center of the deformation. You can control the deformation by specifying: •
Deform distance
. The length of the pull of the center of the deformation.
•
Deform radius
•
Bodies to be deformed not belong to a body.
. . Specify in a multibody part environment, or when the point you select does
You can also control the area of the deformation with the Deform region. When the Deform region check box is selected, additional controls appear: •
Fixed curves/edges/faces
•
Additional faces to deform
. Entities not affected by the deformation. .
If items selected as fixed entities contradict with deform entities, the latest item overrides any previous, contradictory item. For example, if you first specified a face to deform, and then specified the same face as fixed, the face would be fixed. •
Deform region check box. Clear the Deform region check box to control the shape of the deformation by selecting an edge or a sketch line, and then specifying a Deform radius creates a bending-type deformation, though not an exact bending.
. The Deform axis
option
With Shape Options, you can also control the shape of the deformation by specifying a level of stiffness.
Deform Curve to Curve Deform Feature Using Curve to Curve You can use Curve to curve deformations to: •
Modify the shape of complex models. deformation on a complex model
•
Change dimensions in an imported model. deformation on an imported model
•
Fill the gaps between surfaces. deformation to fill surfaces
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Chapter 6 Features
There are many options in Curve to curve deformations. Some options are only available with specific selections. However, you can combine options. The procedure below only uses some of these options. See curve to curve options for details and models that display how these options interact. To deform a model using curve to curve:
This procedure uses a multibody part. You select the curves on one body as the Initial curves, and the curves along the second body as the Target curves. 1.
Click Deform
2.
Under Deform Type, select Curve to curve.
3.
Under Deform curves:
a.
on the Features toolbar, or click Insert, Features, Deform.
Select each of the top edges of the block as Initial curves
.
The selected edges, as shown in this example, are outlined in green.
b.
Click in Target curves , and select the bottom circular edge of the round extrude feature, as shown. The selected edge, as shown in this example, are outlined in purple.
6-10
c.
Align the connector along the profiles. A connector is made up of a point along each curve, and the connecting entity between the two points. You can drag the points along each of the curves to synchronize the alignment.
d.
Click either of the connector handles.
e.
Click the arrow on the connector handle - the pointer changes to - to align the direction vectors so that they point in the same direction.
f.
Right-click and select Add Connector.
g.
Repeat Add Connector, and add a connector for each corner of the bottom rectangular profile.
h.
Right-click and select Show Connection Lines.
Align connector
The connection lines should be evenly distributed along the entire perimeter. If they are not, align the connectors. Uneven distribution of the connection lines can cause twisted geometry. i.
Align direction vectors
Align the connectors by dragging the handles on each curve. The connectors should be evenly distributed along the perimeter of the circle, and at the center of each rounded corner. Aligning the Connectors
Add connectors and Show Connection Lines
Note how the perimeter of the rectangular model (green), and the perimeter of the deform preview are parallel along the four sides. 4.
Under Deform Region, click Fixed edges. Fixed curves/edges/faces
and Additional faces to be deformed
appear.
These options are only available when you click Fixed edges. Both of these options are optional. The geometry of your model, and the intended deformation dictate their usage.
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Chapter 6 Features
5.
Click in Fixed curves/edges/faces
, then select the bottom of the base.
6.
Under Shape Options, click Stiffness - medium
7.
Click OK
.
.
If you encounter problems, such as the error message Could not replace geometries, under Shape Options, move the Shape accuracy slider. Other solutions include adding additional connectors, and re-aligning existing connectors. You can also select Ignore warning when a warning message appears. The system attempts to complete the process and provides additional information on what options to modify to maximize success. Deform Feature Curve to Curve Options This type of deformation is based on initial curves and target curves. Deform Curves Under Deform curves, select one or more connected curves as the Initial curves curves as the Target curves
. The curves can be curved or linear, and be part of the model or separate sketches.
Initial curves
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, and one or more connected
Target curves
curve to curve deformation with fixed curve
Fixed curve Deform Region Under Deform Region, you can specify the following options: •
Fixed Edges
•
Uniform
•
Fixed curves/edges/faces
•
Additional faces to deform
•
Bodies to be deformed
Fixed Edges Select Fixed edges to display additional deformation options: •
Fixed curves/edges/faces
•
Additional faces to deform
. Select entities that are unaffected by the deformation. . Select multiple faces to deform.
Clear Fixed edges and specify a Deform radius to create a bending-type deformation, though not an exact bending, with a specified radius. Uniform Select Uniform to create different shape options. Example of deform with Uniform selected and cleared: Uniform is independent of other options under Deform Region. Fixed Curves, Edges and Faces When you specify Fixed curves/edges/faces
, the selected entities are not deformed.
With closed contours of fixed edges, the deformation depends on the position of the Initial curves
:
•
If the Initial curves
are within the closed contour, the deformation is confined to the contour.
•
If the Initial curves
are outside of the closed contour, no point inside the contour is deformed.
Example of the fixed edges option
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Chapter 6 Features
Additional Faces to be Deformed You can select Additional faces to deform
to include additional faces in the deformation.
Example of the additional faces option Bodies to be Deformed Specifying Bodies to be deformed
is geometry-dependent:
•
Required. If the Initial curves
are sketch curves, you must select Bodies to be deformed
.
•
Optional. If you have a multibody part, you can select Bodies to be deformed , after you specify the initial body to deform by selecting the initial and target curves under Deform Curves. Example of the bodies to be deformed option You can use the options Fixed curves/edges/faces , Bodies to be deformed , and Additional faces to deform in any combination, dependent on the geometry of the model and the desired results. If the selected options are conflicting, the latest item overrides any previous, contradictory item. For example, if you first specified a face to deform, and then specified the same face as fixed, the face would be fixed.
Shape Options You can also control the shape of curve to curve deformations by modifying the degree of stiffness, the Shape accuracy
, and the Weight
.
Stiffness There are three levels of stiffness: •
Stiffness - minimum
•
Stiffness - medium
•
Stiffness - maximum
You can combine any stiffness level with the options under Deform Region. Example of shape stiffness levels Shape Accuracy Shape accuracy . The shape accuracy slider controls the surface quality. The default quality can be inadequate in high curvature areas. When you increase the accuracy by moving the slider to the right, you can increase the success rate of the deform feature. Move the slider only as needed; increasing surface accuracy decreases performance.
Minimum Example of shape accuracy
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Maximum
Weight Weight . If you clear Uniform and select Fixed edges, the weight slider appears. The weight slider controls the degree of influence between two options: •
Fixed edges. The entities you specify under Fixed curves/edges/faces
•
Moving curves. The edges and curves you specify under Deform Curves as Initial curves Target curves
. , and
.
Fixed
Moving
Example of weight value Ignore Warning If an error message appears: • Verify your input. In curve to curve deformations, add new connectors or realign existing connectors. •
Verify the preview.
•
Improve the surface quality using Shape accuracy
•
Clear the Uniform check box under Deform Region.
•
Select Ignore warning under Shape Options. The system attempts to complete the deformation process by ignoring small errors. For example, short edges may be merged or the body check may be skipped.
•
If you select Ignore warning, inspect whether the results are topologically and geometrically correct.
•
Read the warning
•
Click Check on the Tools toolbar, or click Tools, Check to check the part. If you get additional, system-generated warnings from HOOPS routines, such as
under Shape Options.
following the build.
Normal vector is of zero or nearly zero length the problematic area is highlighted. Example of Deform with Uniform Selected
Uniform cleared
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Uniform selected
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Chapter 6 Features
Example of Deform Curve to Curve with Fixed Edges
Model with no deformation
Deformation with no fixed edges selected
Fixed curves/edges/faces selected, as shown
Example of Deform Curve to Curve with Additional Faces
(1) Initial curve
, (2) Target curve
Top face selected for Additional faces to be deformed
6-16
.
and Fixed edges/curves/faces
selected
No face selected. The bottom face is affected by the deformation of the body.
Example of Deform Curve to Curve Bodies to be Deformed
Select one body to deform
Select multiple bodies to deform
Example of Deform Curve to Curve Stiffness
No deformation applied Stiffness - minimum
Stiffness - medium
SolidWorks 2004 Reference Guide
Stiffness - maximum
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Chapter 6 Features
Example of Deform Shape Accuracy
Accuracy slider - Minimum
Accuracy slider - Maximum
Example of Deform Curve to Curve Weight
Fixed curves/edges/faces
Fixed
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Moving
Fixed
Moving
Fixed
Moving
Deform Point Deform Feature Using Point There are many options in Point deformations. Some options are only available with specific selections. However, you can combine options. The procedure below only includes some only of these options. See point options for details and models that display how these options interact. Point deformation that affects a small area may not display using default image quality settings. Click Tools, Options, Document Properties, Image Quality. To increase the quality, move the Shaded and draft quality HLR/ HLV resolution slider to the right, or select Optimize edge length. To deform a model using point:
1.
Click Deform
2.
Under Deform Type, select Point.
3.
Under Deform point, select these items: •
on the Features toolbar, or click Insert, Features, Deform.
Face. When you select a point on a face, the default Deform direction is perpendicular to the face (Normal to picked is selected). If you clear Normal to picked, select a Deform direction using a linear edge, a sketch line, a planar face, or a plane. If necessary, click to reverse the direction.
a.
•
Edge. When you select a point on an edge, the default Deform direction is an average between the normals to the two adjacent faces (Normal to picked is selected). The location of the edge on the model determines the center of the deformation.
•
Vertex. When you select a vertex, the default Deform direction is an average between the normals to all adjacent faces (Normal to picked is selected).
•
Point. When you select a point in space, there is no default deform direction (Normal to picked is cleared). You must specify the Deform direction, and under Deform Region, you must select one or more bodies to deform.
Select a point on an edge, a point on a face, a vertex, or a point in space as the Deform point
Select a point on an edge
SolidWorks 2004 Reference Guide
Select a point on a face
.
Select a point in space and a Deform direction
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Chapter 6 Features
4.
b.
Click Reverse deform direction
to reverse the direction.
c.
With a point in space as the Deform point , select a linear edge, a face, or a plane as the Deform direction. With a point on an edge, a point on a face, or a vertex, you can keep Normal to picked selected.
d.
Type a value for Deform distance
.
Under Deform Region, select these items: a.
Set a value for Deform radius
.
b.
Select Deform region to confine the deformation to the area enclosed by the perimeter of the face selected. With Deform region you can also select Fixed curves/edges/faces to be deformed
and Additional faces
.
When you select a point on a face, and select Deform region, you can confine the deformation to the area enclosed by the perimeter of the face selected. When you select a point on an edge, a vertex, or a point in space, the deformation is not directly affected by this option. c. 5.
Select Bodies to be deformed
when the model includes multiple bodies.
Under Shape Options: •
Select a level of stiffness. Deform region selected
Deform region cleared
Stiffness - minimum
Stiffness - medium
Stiffness - maximum
6-20
•
Deform axis . When the Deform region check box is clear, you can control the shape of the deformation by selecting a linear edge, a sketch line, a planar face or a plane as a deform axis.
Shape accuracy . Move the slider to control surface quality. Increasing the quality also increases the success rate of the deform feature. For example, if you get an error message Could not replace geometries, move the slider towards the right. Move the slider only as needed; increasing surface accuracy decreases performance. 6.
Click OK
.
Deform Feature Point Options This type of deformation is based on a point and its pull direction vector. Deform Point Point to deform. Under Deform point, you can select a point to deform on a face, an edge,a vertex, or a point in model space. •
Face. Select a point on a face, and the default Deform direction is perpendicular to the face (Normal to picked is selected). If you clear Normal to picked, select a Deform direction by specifying an edge, a sketch line, or a planar face, or a plane. If necessary, click
to reverse the deform direction.
o
Linear edge or sketch line. Deform direction is parallel to the specified entity.
o
Planar face or plane. Deform direction is perpendicular to the planar face or plane.
The location of the point on the face determines the center of the deformation. Example of a point on a face •
Edge. Select a point on an edge, and the default Deform direction is an average between the normals to the two adjacent faces (Normal to picked is selected). If you clear Normal to picked, select a Deform direction in the manner described in the section above. The location of the point on the edge determines the center of the deformation. Example of a point on an edge
•
Vertex. Select a vertex, and the default Deform direction is an average between the normals to the three adjacent faces (Normal to picked is selected). If you clear Normal to picked, select a Deform direction in the manner described in the section above.
•
Point. When you select a point in space, there is no default deform direction (Normal to picked is cleared). You must specify the deform direction. Under Deform Region, you must also select one or several bodies to deform. Example of a point in space
Deform Region The interaction between the options under Deform Point and selecting the Deform region check box independently are as follows: Under Deform Point:
Under Deform Region:
Point on an edge
Deform region check box
Results •
Vertex Point in space Point on a face
• Deform region check box
•
•
SolidWorks 2004 Reference Guide
The area of the deformation is not affected by selecting the Deform region check box independently. Other options are enabled The area of the deformation is affected by selecting the Deform region check box independently. Other options are enabled
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Chapter 6 Features
The Deform region check box enables the following options: •
Fixed/curves/edges/faces
•
Additional faces to deform
. Select entities that are unaffected by the deformation. . Select multiple faces to deform.
When the Deform region check box is cleared, it enables an additional option under Shape Options: Deform axis
.
Example of a point on a face and Deform region Deform distance and deform radius. Two of the parameters that control the deformation are distance and radius. •
Under Deform point, specify a Deform distance
.
•
Under Deform Region, specify a Deform radius checkbox to change the Deform radius.
. You do not need to select the Deform region
Example of Deform distance and Deform radius Fixed/curves/edges/faces . Besides Deform distance and Deform radius , you can control the shape of the deformation by selecting one of several curves, an edges, or faces. The selected entities are not deformed. With closed contours, deformation behavior depends on the following: •
If the center of the deformation is within the closed contour, the deformation is confined to the contour.
•
If the center of the deformation does not belong to the closed contour, no point inside the contour is deformed. Example of a fixed curve, edge, or face
If items selected as fixed entities contradict, the latest item overrides any previous, contradictory item. For example, if you first specified a face to deform, and then specified the same face as fixed, the face would be fixed. Additional faces to deform
. You can also select more than one face on the model to deform.
Example of multiple faces Bodies to be deformed
. You can deform more than one body in a multibody part environment.
Example of multiple bodies
Under Deform Region: •
Specify Fixed/curves/edges/faces , and Additional faces to deform select the Deform region check box.
, only when you
•
Select Bodies to be deformed
•
Select each option individually, or combine all three options in the same model.
, with Deform region selected or cleared.
Shape Options You can also control the shape of point deformations by modifying the degree of stiffness, specifying a deform axis, and modifying the Shape accuracy
6-22
.
Stiffness There are three levels of stiffness: •
Stiffness - minimum
•
Stiffness - medium
•
Stiffness - maximum
You can combine the stiffness level with other controls. Example of shape stiffness levels Deform Axis With the Deform region check box cleared, you can control the shape of the deformation by selecting a linear edge or a sketch line as a deform axis. •
The Deform axis
•
The Deform radius specified radius.
determines the shape of the deformation using the Deform radius
.
option creates a bending-type deformation, though not an exact bending, with a
Example of the deform radius axis You can combine the deform axis with stiffness levels. Shape Accuracy Shape accuracy . The shape accuracy slider controls the surface quality. When you increase the accuracy by moving the slider to the right, you can increase the success rate of the deform feature. Move the slider only as needed; increasing surface accuracy decreases performance.
Minimum
Maximum
Point deformation that affects a small area may not display using default image quality settings. Click Tools, Options, Document Properties, Image Quality. To increase the quality, move the Shaded and draft quality HLR/ HLV resolution slider to the right, or select Optimize edge length. Ignore Warning If an error message appears: •
Verify your input.
•
Verify the preview.
•
Improve the surface quality using Shape accuracy
•
Clear the Uniform check box under Deform Region.
•
Select Ignore warning under Shape Options. The system attempts to complete the deformation process by ignoring small errors. For example, short edges may be merged or the body check may be skipped.
•
If you select Ignore warning, inspect whether the results are topologically and geometrically correct.
•
Read the warning
•
Click Check on the Tools toolbar, or click Insert, Tools, Check to check the part. If you get additional, system-generated warnings from HOOPS routines, such as
under Shape Options.
following the build.
Normal vector is of zero or nearly zero length, the problematic area is highlighted.
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Chapter 6 Features
Maintain Boundary Maintain boundary appears only when you select the Deform region check box. Clear Maintain Boundary to reduce the deform region, create new edges and move the boundaries. Additional Faces Only Additional faces only appears when: •
You select the Deform region check box
•
Clear Maintain boundary
When you include the Fixed/curves/edges/faces option, all entities are deformed except the fixed edges. To deform only the top face of the model while fixing one of the edges, select Additional faces only. Example of Deform Select Different Points on Face
Point. Different points selected on the same face. Example of Deform Select Point on an Edge
Point. Different points selected on the same edge.
6-24
Example of Deform Select Point Point. With a point in space, you must always select the Deform direction, and under Deform region, specify the Body to be deformed.
Deform direction. Parallel to the edge of the extrude with draft feature, circled in red.
Deform direction. Perpendicular to the face of the main extrude feature,circled in red.
Example of Deform Region - 1 Both examples use the same initial face to deform, with Deform distance - 60, and Deform radius - 100.
Deform region selected
Deform region cleared
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Chapter 6 Features
Example of Deform Distance and Deform Radius
Deform distance: 20 - Deform radius: 80
Deform distance: 50 - Deform radius: 80
Deform distance: 50 - Deform radius: 40
Deform distance: 80 - Deform radius: 40
Example of Deform Select Curve-Edge-Face
6-26
All examples use the same Deform distance
and Deform radius
Before deform
Deform with no fixed entities selected
Preview of fixed edges
Deform with fixed edges selected
Example of Deform Point with Additional Faces All examples use the same initial face to deform, with Deform distance - 60, and Deform radius - 100.
Single face selected to deform under Deform point
One additional face selected under Additional faces to deform
Two additional faces selected under Additional faces to deform Example of Deform with Multiple Bodies Point on edge selected as Deform point , and face selected as the Deform direction. All examples use Deform distance - 60, and Deform radius - 100.
No additional body selected as Bodies to be deformed
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.
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Chapter 6 Features
One additional body selected as Bodies to be deformed
Two additional bodies selected as Bodies to be deformed
.
.
Example of Deform Point Shape Stiffness All examples use the same options except for the stiffness.
Stiffness - minimum
Stiffness - medium
Stiffness - maximum
Example of Deform with Deform Axis
No deformation
6-28
No Deform axis selected
Edge selected as Deform axis
Example of Deform Maintain Boundary
Maintain Boundary checked
Maintain Boundary cleared
Example of Deform Region - 2 Deform region cleared
Deform region selected
With point on a face selected, clearing or selecting the Deform region check box affects the deformation.
With point on an edge selected, clearing or selecting the Deform region check box does not affect the deformation.
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Chapter 6 Features
Example of Deform Axis
No Deform axis
Edge selected as the Deform axis
Domes You can create one or more dome features simultaneously on the same model. The Parameters in the dome PropertyManager include: •
Faces to Dome
. Select one or more planar or non-planar faces.
you can apply domes to faces whose centroid lies outside the face. This allows you to apply domes to irregularly shaped contours. •
Distance. Set a value for the distance by which the dome expands.
•
Reverse Direction
•
Constraint Point or Sketch . Control the dome feature by selecting a sketch to constrain the shape of the sketch. When you use a sketch as a constraint, the Distance is disabled.
•
Direction. Click Direction , and select a direction vector from the graphics area to extrude the dome in a direction other than normal to the face. As a direction vector, you can use a linear edge or the vector created by two sketch points.
•
Elliptical dome. Specify an elliptical dome for cylindrical or conical models. An elliptical dome's shape is a half ellipsoid, with a height equal to one of the ellipsoid radii.
•
Continuous dome. Specify a continuous dome for polygonal models. A continuous dome's shape slopes upwards, evenly on all sides. If you clear Continuous dome, the shape rises normal to the edges of the polygon.
. Click to create a concave dome (default is convex).
Continuous dome is not available when you use a Constraint Point or Sketch
or a Direction
vector. •
Show preview. Check for a preview. On cylindrical and conical models, you can set Distance to 0. The software calculates the distance using the radius of the arc as a basis for the dome. It creates a dome that is tangent to the adjacent cylindrical or conical face.
6-30
To create a dome:
1.
Click Dome
on the Features toolbar, or click Insert, Features, Dome.
2.
In the PropertyManager, under Parameters, follow the guidelines listed above.
3.
Click OK
.
Example of Dome on Irregular non-Planar Faces
Irregular-shaped, non-planar faces
Dome applied to non-planar faces
Example of Dome with Elliptical Option
Elliptical dome checked
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Elliptical dome cleared
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Chapter 6 Features
Example of Continuous Dome Continuous dome option
Checked
Cleared
Example of Dome with Zero Distance
Conical and elliptical dome features with a Distance of zero.
Drafts Draft Overview Draft tapers faces using a specified angle to selected faces in the model. One application is to make a molded part easier to remove from the mold. You can insert a draft in an existing part or draft while extruding a feature. You can apply draft to solid or surface models. When creating a draft using a parting line with step draft, you can select Perpendicular steps to prevent tapering of the slanted faces. Using the draft feature, you can specify the following: •
Neutral plane
•
Parting line
•
Step draft
Draft Feature Creates a feature that tapers selected model faces by a specified angle, using either a Neutral Plane or a Parting Line. You can apply draft to either solid or surface models. You can also apply a draft angle as a part of an extruded base, boss, or cut.
6-32
To draft a model face to a neutral plane: Example
1.
Click Draft
2.
Under Type of Draft, select Neutral Plane.
3.
Under Draft Angle
4.
Under Neutral plane, do the following:
5.
6.
on the Features toolbar, or Insert, Features, Draft.
, enter the number of degrees.
•
Select either a face or a plane to serve as the neutral plane. The draft angle is measured perpendicular to this plane.
•
Select Reverse direction
to slant the draft to slant in the opposite direction.
Under Faces to draft , select the faces to draft in the graphics area, and choose an item from the Face propagation list if you want to propagate across additional faces: •
Along Tangent. Extend the draft to all faces that are tangent to the selected face.
•
All Faces. Draft all faces extruded from the neutral plane.
•
Inner Faces. Draft all faces extruded from the neutral plane.
•
Outer Faces. Draft all faces next to the neutral plane.
Click OK
.
Example of Draft on Surface
No draft to surface model
Neutral Plane draft applied
Draft with Neutral Plane Using Neutral Plane as the Type of Draft, you can draft some of the outer faces, all the outer faces, some of the inner faces, all of the inner faces, faces that are tangent, or a combination of both the inner and outer faces. Face Propagation
Selection in Graphics Area
Draft Results
None. Only the selected face is drafted. The top face is used as the Neutral Plane in all the examples.
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Chapter 6 Features
Along Tangent. Extend the draft to all faces that are tangent to the selected face. (The faces meet with filleted corners). The outer faces include any of the faces you select on the bass-extrude. All Faces. Draft all faces next to the neutral plane and extruded from the neutral plane. The inner faces include any faces on the three boss-extrudes.
Inner Faces. Draft all inner faces extruded from the neutral plane.
Outer Faces. Draft all outer faces next to the neutral plane.
Neutral Plane The Neutral Plane is the plane or face that you choose to determine the pull direction when creating a mold. The Z axis direction of this chosen plane is the direction in which the part ejects from the mold. Reverse direction changes the direction of the draft, not the direction of the pull. In the example below, Plane 1 is the Neutral Plane, with the arrow indicating the pull direction.
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Parting Line Draft The parting line option lets you draft surfaces around a parting line. The parting line can be non-planar. In a draft using a parting line, you can also include a Step draft. To draft on a parting line, you can first divide the faces to be drafted by inserting a split line, or you can use an existing model edge. Then you specify the direction of pull, or the side of the parting line from which material is removed. You can check the draft angles on your model using the draft analysis tool. Draft analysis creates a color-coded rendition of the model faces based on the angle and the direction of pull criteria that you specify. To insert a draft angle parting line:
1.
Sketch the part to be drafted.
2.
Insert a split line curve, if desired.
3.
Click Draft
4.
Under Type of Draft, select Parting Line.
on the Features toolbar or click Insert, Features, Draft.
Under some conditions, select the Allow reduced angle check box. 5.
Under Draft Angle, enter the Draft angle
.
6.
Under Direction of Pull, select an edge or face in the graphics area to indicate the direction of pull. Note the arrow direction, and click Reverse Direction
7.
Under Parting Lines
if desired.
, select the parting lines in the graphics area.
Note the arrow direction. To specify a different draft direction for each segment of the parting line, click the name of the edge in the Parting Lines box, and click Other Face.
First draft direction
Other Face selected
NOTE: In this example, all parting lines were selected, using the same face. 8.
9.
Choose the Face propagation type: •
None. Draft only the selected face.
•
Along Tangent. Extend the draft to all faces that are tangent to the selected face.
Click OK
.
Draft applied with first direction
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Draft applied with Other Face
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Chapter 6 Features
Allow Reduced Angle Option The Allow reduced angle check box is available only with Parting Line draft. NOTE: When you select this option, the draft angle on some portions of the drafted face may be smaller than the specified draft angle.
Use the Allow reduced angle check box under the following condition: The normal of one or more side faces adjacent to the edge and the faces being drafted is nearly perpendicular to the Direction of Pull. With this model type and condition, select the Allow reduced angle check box when the maximum angle between the pull direction and the normal of the steep face, plus the draft angle, is greater than or equal to 90°. The vertical blue arrow represents the Direction of Pull (Top plane). The red arrow represents the surface normal at its maximum angle to the pull direction. When the sum of the angle produced by the maximum angle and the Draft Angle is 90° or greater, select the Allow reduced angle check box to create the draft.
Draft applied (Draft Angle
is 25°).
The image above displays the same 25° draft applied. However, it is enhanced by applying an offset face and displaying curvature on the offset face.
In this example, the draft angle towards the narrow ends of the drafted face is reduced below the specified 25° to create the draft.
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Parting Line with Step Draft A step draft is a variation of a parting line draft. The step draft creates one face rotated about the plane used as the Direction of Pull. This results in small faces, reperesenting the steps (highlighted in blue in the example below).
Model with parting line
Parting line draft
Parting line with step draft
You can check the draft angles on your model using the draft analysis tool. Draft analysis creates a color-coded rendition of the model faces based on the angle and the direction of pull criteria that you specify. To insert a draft angle using parting line with step draft:
1.
Sketch the part to be drafted.
2.
Create a plane.
3.
Create desired parting line. Make sure that: •
4.
At least one parting line segment is coincident to the parting plane on each draft face. • All other parting line segments are in the pull direction of the plane. • None of the parting line segments are perpendicular to the plane. Insert a split line curve.
5.
Click Draft on the Features toolbar or click Insert, Features, Draft.
6.
Under Type of draft, select Step Draft. •
•
Select Tapered steps if you want the surfaces to generate in the same manner as the tapered surfaces. Select Perpendicular steps if you want the surfaces perpendicular to the original main face.
7.
Under Draft Angle
8.
Under Direction of Pull, do the following: • •
, enter the number of degrees.
Select a plane to indicate the direction of the pull. Select Reverse direction to slant the draft in the opposite direction.
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Chapter 6 Features
9.
Under Parting Lines • • •
, do the following:
Select the parting line segments in the graphics area. Note the direction of the preview arrow. Click Other Face to specify a different draft direction for each segment of the parting line. Select the Face propagation type: None. Draft only the selected face. Along Tangent. Extend the draft to all faces that are tangent to the selected face (faces that meet with fillets or rounds.)
10. Click OK
.
Tapered and Perpendicular Draft Steps
Model with no draft applied
Tapered steps applied
Perpendicular steps applied
Extrudes Extrude Feature An extrude operation can either add material to a part (in a base or boss) or remove material from a part (in a cut or hole). Extrude extends a sketched profile in one or two directions as either a thin feature or a solid feature.
A circle extruded as a solid feature
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A circle extruded as a thin feature
A rectangle extruded as a solid feature
A rectangle extruded as a thin feature (with draft)
You can also extrude in a direction other than normal to the profile of the sketch by selecting a direction vector.
Extrude Feature Overview When you extrude a feature you specify an extrusion End Condition. Depending on the type of extrusion you select, additional options are available. Extrude Direction •
Observe the preview to verify the direction and depth of the feature.
•
Select the parameters under Direction 1 to extrude the feature in one direction from the sketch plane.
•
Select Direction of Extrusion
•
Select the parameters under Direction 2 to extrude the feature in both directions from the sketch plane.
to extrude in a direction other than normal to the profile of the sketch.
End Condition •
If you choose Blind or Mid Plane, you must specify the Depth
•
If you choose Offset From Surface, you must specify the Offset.
.
When you choose Offset from Surface, you can specify Translate Surface. When you specify the Translate Surface option, the end of the extrusion is a translation of the reference surface, rather than a true offset. •
If necessary, select the Reverse offset check box. If the End Condition you specified relies on the selection of a surface or vertex, click that item in the graphics area. The selection is listed in the Face/Plane
•
box.
Up To Body. Specify the body you want to extrude up to in the graphics area. The selection is listed in the Solid/Surface Body box. TIP: You can use Up To Body when making extrusions in an assembly. Up To Body extends the sketch only up to the selected body. If the sketch that you extrude extends outside of the selected face or surface body, Up To Body can do some automatic extension of one analytic face to terminate the extrusion. The Up To Body option is also useful with mold parts, if the body you extrude to has an uneven surface.
Depth Depth
specifies the depth of the extrusion.
Reverse Direction Click Reverse Direction graphics area.
SolidWorks 2004 Reference Guide
to extend the feature in the opposite direction from that shown in the preview in the
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Chapter 6 Features
Link to Thickness Link to Thickness is used on sheet metal parts. Selecting this option automatically links the depth of an extruded boss to the thickness of the base feature. Flip Side Flip Side to Cut appears only when you are extruding a cut. By default, material is removed from the inside of the profile. Selecting Flip Side to Cut removes all material from the outside of the profile.
Default cut
Flip side cut
Draft Click Draft On/Off outward check box.
to add a draft to the feature. Enter a Draft Angle
No draft
10° draft angle inward
. If necessary, select the Draft
10° draft angle outward
Thin Feature Thin Feature adds (or removes) thin-walled volumes to the model. A Thin Feature base can also be used as a basis for a sheet metal part.
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•
Select One-Direction, Two-Direction, or Mid-Plane
•
Enter a Thickness
•
If you selected Two-Direction, enter a Thickness
•
If necessary, select the Cap ends check box and enter a Cap Thickness
for the thin feature. for the second direction. .
Extrude Direction Along Vector You can extrude 2D and 3D sketches normal to the face, or you can select a Direction of Extrusion
.
You can also select a Direction with the Dome feature.
Use any of the following for Direction of Extrusion Cylindrical faces
Linear edges
Conical faces
Linear sketch entities
Planar faces
Reference axes
Sketch points
References planes
Vertices
Points in reference geometry
Example of Translate Surface
Translate Surface cleared
Translate Surface selected
Offset from Surface 7mm
Offset from Surface 27mm
Select the Translate Surface check box when a larger offset is required.
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Chapter 6 Features
End Condition Extrude When you extrude a profile, you need to select a Type from the Extrude Feature dialog box. Isometric View
Top View
Function Blind. Extends the feature from the sketch plane for a specified distance.
Through All. Extends the feature from the sketch plane through all existing geometry.
Up To Next. Extends the feature from the sketch plane to the next surface that intercepts the entire profile. (The intercepting surface must be on the same part.)
Up To Vertex. Extends the feature from the sketch plane to a plane that is parallel to the sketch plane and passing through the specified vertex. Sketch vertices are now valid selections for Up To Vertex extrusions.
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Up To Surface. Extends the feature from the sketch plane to the selected surface.
Offset From Surface. Extends the feature from the sketch plane to a specified distance from the selected surface.
Up To Body. Extends the feature from the sketch plane to a specified body. You can use Up To Body with assemblies, mold parts, or multibody parts.
Mid Plane. Extends the feature from the sketch plane equally in both directions.
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Chapter 6 Features
Extruded Boss/Base Listed below are the steps you follow to create an extruded boss/base feature. For related information about the extrude feature, see the following: •
Extrude feature overview
•
Extrude thin feature
•
Examples of thin features
To create an extruded base or boss:
1.
With a sketch active, click Extruded Boss/Base Extrude.
2.
Under Direction 1, do the following:
on the Features toolbar or Insert, Boss/Base,
•
Select an End Condition.
•
Examine the preview and if necessary, click Reverse Direction direction.
•
To extrude in a direction other than normal to the profile of the sketch, select Direction of Extrusion
to extrude in the opposite
.
•
Enter a Depth
.
•
If necessary, click Draft On/Off
•
Enter a Draft Angle.
•
If necessary, select the Draft outward check box.
to add a draft to the feature.
3.
If necessary, select the Direction 2 check box to apply the extrusion in a second direction. Follow the procedure listed under step 2.
4.
To create a thin-walled feature, select the Thin Feature check box and do the following: •
Select a Type: One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and if necessary, click Reverse Direction the opposite side.
•
Enter a Direction 1 Thickness
• •
If you selected Two-Direction as the Type, enter a Direction 2 Thickness . Click the Cap ends check box to cap the ends of a closed profile base feature and create a hollow part. Enter a Cap Thickness
•
.
.
Click the Auto fillet corners check box to round-off the corners. This applies only to open profile thin based features. Enter a Fillet Radius
5.
to create the thin feature on
Click OK
.
.
For bosses on sheet metal parts, click Link to Thickness tab to link the depth of the boss to the thickness of the base feature.
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Boss/Base-Extrude The Extrude PropertyManager defines the characteristics of extruded features. You can create either solid features or thin features. To create a solid feature:
1.
In the PropertyManager under Direction 1, set the End ConditionType to determine how the feature extends. •
If you choose Blind or Mid-Plane, specify the Depth
.
•
If you choose Up To Vertex, select a Vertex
•
If you choose Up To Surface, specify the the Face/Plane
•
If you choose Offset From Surface, specify the Face/Plane
in the graphics area. in the graphics area. , and enter the Offset Distance
. Click the Reverse Direction check box, if appropriate. TIP: To select a plane, use the flyout FeatureManager design tree. •
If you choose Up To Body, specify the body you want to extrude up to in the graphics area. TIP: You can use Up To Body when making extrusions in an assembly. Up To Body extends the sketch only up to the selected body. If the sketch that you extrude extends outside of the selected face or surface body, Up To Body can do some automatic extension of one analytic face to terminate the extrusion. The Up To Body option is also useful with mold parts, if the body you extrude to has an uneven surface.
2.
If you extrude a cut, you can select Flip side to cut. By default, material is removed from the inside of the profile. Flip Side to Cut lets you sketch the portion that you want to remain, and remove the material surrounding the profile. NOTE: When you extrude a cut, you can create multibody parts, as well as select which bodies are affected by the cut.
3.
If necessary, click Reverse Direction the preview.
to extend the feature in the opposite direction from that shown in
4.
If necessary, click Draft On/Off to add a draft to a feature while you extrude it. Set the Draft Angle, and check the Draft outward check box, if necessary.
5.
To create an extrusion in the other direction, click Direction 2, and follow the same steps.
6.
Click OK
.
To create a thin feature:
1.
In the Extrude PropertyManager, under Direction 1, set the End Condition Type to determine how the feature extends.
2. 3.
Click Thin Feature. For Type, select One-Direction, Mid Plane, or Two-Direction. •
If you choose One-Direction or Mid Plane, set the Thickness
•
If you choose Two-Direction, set the Direction 1 Thickness
. and the Direction 2 Thickness
. 4.
If necessary, select the Cap ends check box and enter the Cap Thickness
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.
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Chapter 6 Features
5.
6.
If you created an open profile you can select the following options: •
Click the Auto fillet corners check box to automatically create a round at each edge where lines meet at an angle.
•
Enter a Fillet Radius
Click OK
to specify the inside radius of the round.
.
Extrude Thin Feature Whenever you sketch an open profile, you can select Thin Feature in the PropertyManager. Type The Type specifies whether to extrude the thin feature in One-Direction, Mid-Plane, or Two-Direction. •
One-Direction extrudes the sketch in one direction using the specified wall thickness.
•
Mid-Plane extrudes the sketch in both directions, dividing the specified wall thickness equally on both sides of the sketch geometry.
•
Two-Direction extrudes the sketch in both directions, using a different wall thickness on each side of the sketch geometry (as specified for Direction 1 Thickness
and Direction 2 Thickness
).
Wall Thickness The wall thickness specifies the thickness of the thin feature wall. Reverse Reverse Direction allows you to add the wall thickness to the inside of the sketched profile. The default is to add the wall thickness to the outside of the sketched profile. Additional Options For thin feature base extrusions only, you can specify the following additional options: •
Cap Ends - If you create a closed profile sketch, you can use the Cap Ends option. This option covers (caps) the ends of the feature, creating a hollow part. If you select this option, you must also specify the Cap Thickness
•
.
Auto Fillet corners - If you create an open profile sketch, you can use the Auto Fillet corners option. This option creates a round at each edge where lines meet at an angle. If you select this option, you must also specify the Fillet Radius
(the inside radius of the round).
Examples of Thin Feature Extrude
Direction 1 and Direction 2 extude
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Direction 1 and Direction 2 thickness
Cap ends applied to thin feature
Auto fillet corners applied to thin feature
Cut Feature A cut is a feature that removes material from a part or an assembly. With multibody parts, you can use cuts to create disjoint parts. You can control which parts to keep and which parts are affected by the cut. You can create a cut by using any of the following: •
Extrude
•
Revolve
•
Sweep
•
Loft (from one or more sketches)
•
Thicken feature (from a surface)
Cutting Tools You can use features to cut a solid model. The model can be a single part or a multibody part. To cut a solid model with any of these tools:
1.
Display the base model you want to cut.
2.
Create the sketches, based on the feature to use as the cutting tool. The feature you select depends on your base model and the shape you want the cut to produce. Cutting tools include: •
Extruded Cut
•
Revolved Cut
•
Swept Cut
•
Lofted Cut
•
Thickened Cut
•
Cut with Surface
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Chapter 6 Features
3.
Use the feature to cut the base model.
Extruded Cut
Revolved Cut
Swept Cut
Lofted Cut
Thickened Cut
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Cut with Surface
Surface Cut With multibody parts, you can select which bodies to keep when you use a surface to cut multiple parts. You can cut a solid body with a plane, as well as with a surface.
To cut a solid body with a surface or a plane:
1.
Click Insert, Cut, With Surface. The SurfaceCut PropertyManager appears.
2.
Select the surface or the plane to use for the cut.
The surface or the plane appears under Surface Cut Parameters. 3.
Examine the preview, and if necessary, click
Flip cut to reverse the direction of the cut.
The arrow points in the direction of the solid to discard.
4.
With multibody parts, under Feature Scope, select one of the following: •
All bodies. The surface cuts all bodies every time the feature regenerates. If you add new bodies to the model that are intersected by the cutting surface, these new bodies are also regenerated to include the cut.
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Chapter 6 Features
•
Selected bodies. The surface cuts only the bodies you select using the pointer . If you add new bodies to the model that are intersected by the cutting surface, you need to use Edit Definition to select those bodies, and to add them to the list of selected bodies. If you do not add the new bodies to the list of selected bodies, they remain intact.
•
Auto-select. The option is selected by default, and is only available if you click Selected bodies. When you first create a model with multibody parts, the cutting surface automatically processes all the relevant intersecting parts. The Auto-select option is faster than the All bodies option, since it processes only the bodies on the initial list, and does not regenerate the entire model. If you click Selected bodies, and clear Auto-select, you must select the bodies you want to cut from the graphics area. The solid bodies you select are highlighted in the graphics area, and listed in the Feature Scope box. In the example below, only the yellow body (third from the right), was not selected.
5.
Click OK , right-click the surface in the FeatureManager design tree, and select Hide Surface Body to hide the cutting surface.
The bodies are cut and the cutting surface is hidden.
Extruded Cut When you use the Extruded Cut Preview
tool, you can display an additional PropertyManager by selecting Detailed
to enhance details and choose entities to display.
To create an extruded cut:
1.
With a sketch active, click Extruded Cut
2.
Under Direction 1: •
Select an End Condition.
•
Click in Direction of Extrusion, other than normal to the sketch.
on the Features toolbar or click Insert, Cut, Extrude.
then select an entity to extrude the feature in a direction
Example of extrude along direction vector • •
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Examine the preview and if necessary, click Reverse Direction direction. If necessary, select Flip side to cut.
to extrude in the opposite
•
Click Draft On/Off
to add a draft to the feature.
•
Enter a Draft Angle.
•
Select Draft outward to change the draft direction.
3.
If necessary, select Direction 2 to apply the cut extrude in a second direction. Follow the procedure listed under step 2 above.
4.
To create a thin-walled feature, select Thin Feature and do the following:
5.
6.
7.
•
Select a Type: One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and if necessary, click Reverse Direction the opposite side.
•
Enter a Direction 1 Thickness
•
If you selected Two-Direction as the Type, enter a Direction 2 Thickness
to create the thin feature on
.
With multiple sketch entities, click Selected Contours
.
:
•
In the graphics area choose the sketches you want as the cutting tools.
•
In the PropertyManager, the selections appear in Selected Contours
.
With multibody parts, click Feature Scope: a.
In the graphics area, select the bodies you want cut for Solid Bodies to Affect
b.
In the PropertyManager, select the scope of the operation.
c.
Click OK
d.
Click OK to exit the PropertyManager.
Click OK
, and in the Bodies to Keep dialog box, select which bodies to keep after the cut.
.
Cut extrude
Flip side to cut selected
Cut extrude with Draft
Cut extrude with Thin Feature
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Chapter 6 Features
Example of Extrude - Direction of Extrusion You can specify extrude direction with 2D and with 3D sketches by specifying a direction vector as the Direction of Extrusion. Direction vectors include: Cynlindrical faces
Linear edges
Reference axes
Vertices
Points in reference geometry
Conical faces
Sketch points
Linear sketch entities
Reference planes
Planar faces
Preview - normal extrude Sketch entity used for Direction of Extrusion
Extrude applied Using sketch for Direction of Extrusion Example of Cut Extrude Selected Contours
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Example of Cut Extrude Feature Scope
Select body to cut
Keep all bodies after cut
Select bodies to keep after cut
Fillets Fillet You can create different types of fillets. The PropertyManager dynamically displays the appropriate options, based on the type of fillet you create. Fillets include previews for all fillet types. You can select a Partial preview, a Full preview, or No preview in the Fillet PropertyManager. If you choose a face or more than one edge on the model and select Partial preview, you can cycle through all the filleted edge previews. To view each fillet preview in turn, press A (the default toggle key). Example You can select an edge or you can apply a fillet to a feature. Using Select Feature or Select Loop on the shortcut menu applies the same radius fillet to all edges that make up the feature. Example
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Chapter 6 Features
To create a constant radius fillet or round:
1.
Click Fillet
on the Features toolbar, or Insert, Features, Fillet/Round.
2.
Select the edges, loops, and faces you want to fillet in the graphics area - or right-click on the feature and choose Select feature to fillet all the edges on the feature.
3.
Under Fillet Type, select Constant radius.
4.
Under Items to Fillet, do the following: •
Specify the Radius
•
Verify that the edges you want to fillet are displayed in the Edges
•
If necessary, select the Multiple radius fillet check box. Then highlight each Edge, and specify the Radius
5.
box.
for that edge.
•
The default setting is Tangent propagation. It extends the fillet to all faces that are tangent to the selected face. Click to clear the Tangent propagation check box, if necessary.
•
Select Partial preview to see only the first edge preview in a series, Full preview to see a fillet preview of all the edges, or No preview to prevent any preview. No preview improves rebuild time with complex models.
If your model includes cut or boss features, use Keep features under Fillet Options when you apply a fillet radius large enough to absorb the cut or boss feature. Clear the check box if you want the features absorbed by the fillet. Example If the feature you want to fillet is an attachment, you can omit the fillet from the attachment edges. Under Fillet Options, Feature attachment, click the Omit attach edges check box. Example
6.
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Click OK
.
Other fillet topics: Fillet Overview
Full Round Fillet
Constant Radius Fillet
Round Corner Fillet
Variable Radius Fillet
Multiple Radius Fillet
Setback Fillet
Face Blend Fillet
Example of Fillet Selections
Click on face
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Use Select Feature on the shortcut menu
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Chapter 6 Features
Fillet Keep Features Options
Model with no fillets
Model with Keep features applied to fillets for front boss and right cut features
Model with Keep features applied to all fillets
Example of Fillet Omit Attach Edges
Omit attach edges check box checked: attachment edge without the fillet
Omit attach edges check box cleared: fillet included on the attachment edge
Example of Fillet by Feature
Select one or more features
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Fillet applied to all features
Fillet Overview Fillet/Round creates a rounded internal or external face on the part. You can fillet all edges of a face, selected sets of faces, selected edges, or edge loops. Select a Partial preview, a Full preview, or No preview in the Fillet PropertyManager. Fillets now include previews with all fillet types except face fillets and full round fillets. If you choose a face or more than one edge on the model and select Partial preview in the Fillet PropertyManger, you can cycle through all the filleted edges. To view each fillet preview in turn, press A (the default toggle key). Example Fillets include the following types: Full round fillet. With full round fillets, you can select three adjacent face sets (two or more tangent faces), and apply a fillet that is tangent to the three face sets.
Full Round Fillet
Constant Radius Fillet
Multiple Radius Fillet
Round Corner Fillet
Setback Fillet
Variable Radius Fillet
Face Fillet
Recommendations for Fillets In general, it is best to follow these rules when making fillets: •
Add larger fillets before smaller ones. When several fillets converge at a vertex, create the larger fillets first.
•
Add drafts before fillets. If you are creating a molded or cast part with many filleted edges and drafted surfaces, in most cases you should add the draft features before the fillets.
•
Save cosmetic fillets for last. Try to add cosmetic fillets after most other geometry is in place. If you add them earlier, it takes longer to rebuild the part.
•
To enable a part to rebuild more rapidly, use a single Fillet operation to treat several edges that require equal radius fillets. Be aware, however, that when you change the radius of that fillet, all the fillets created in the same operation change.
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Chapter 6 Features
Example of Fillet Previews
Constant radius fillet using Partial preview
Constant radius fillet using Full preview
Variable radius fillet
Constant Radius Fillet To fillet multiple model edges or faces:
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1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, click Constant radius.
3.
Under Items to Fillet, do the following: •
Enter a Radius
.
•
In the graphics area, select Edges, Faces, Features and Loops
•
Clear the Tangent propagation check box if you do not want the fillet to extend to all faces that are tangent to the selected face or edge.
•
Select Full preview, Partial preview, or No preview.
to fillet.
Tangent Propagation Tangent edges
Starting with a block, apply a fillet to the edge, as shown.
Edge selected to fillet
Result: Example of fillet with Tangent propagation check box checked
Result: Example of fillet with Tangent propagation check box cleared
4.
5.
Under Fillet Options, do the following: •
If necessary, clear the Keep features check box. Example
•
If necessary, click the Round corners check box.
•
Select the Overflow Type.
Click OK
.
Overflow Type •
Default. The system chooses one of the following options, depending on the geometry conditions (convexity of edges being filleted and the adjacent edges, and so on).
•
Keep edge. Maintains the integrity of adjacent linear edges. However, the fillet surface is broken into separate surfaces, and in many cases the top edge of the fillet may have a dip in it.
•
Keep surface. Uses the adjacent surface to trim the fillet. As a result, the fillet edge is continuous and smooth, but the adjacent edge is disturbed.
Keep edge
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Keep surface
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Chapter 6 Features
Multiple Radius Fillet Using multiple radius fillets, you can create fillets with the following features: •
Select a different radius value for each selected edge.
•
Create corners using three edges with different radii that meet at a common vertex.
•
Select surfaces as well as edges. However, you cannot assign multiple radii to faces with common edges.
•
Select a Full preview, a Partial preview, or No preview in the Fillet PropertyManager.
To create multiple radius fillets:
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, select Constant radius.
3.
Under Items to Fillet, do the following: •
Select the Multiple radius fillet check box.
•
Enter the Radius
•
In the graphics area, highlight the Edges, Faces, Features and Loops
for the first edge or loop. to fillet.
The edge or loop and the radius is listed in the Edges, Faces and Loops box. •
Enter the Radius
for the next edge or loop to fillet, and in the graphics area, select the next
Edges, Faces and Loops
.
Repeat until you have selected all the edges to fillet.
4.
•
The default setting is Tangent propagation. It extends the fillet to all faces that are tangent to the selected face. Clear the Tangent propagation check box, if necessary.
•
Select Full preview, Partial preview, or No preview.
If necessary, under Fillet Options, clear the default Keep features check box. Example
5.
Click OK
.
Dimensions for multi radius fillet
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Multi radius fillets applied
Round Corner Fillet Fillets with round corners allow you to control the transition between edges at the corners. A rounded fillet blends the adjoining edges, eliminating or smoothing the sharp juncture where the two edges meet. To create round corner fillets:
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, keep the default Constant radius.
3.
Under Items to fillet, do the following: •
Clear the Tangent propagation check box.
•
Enter a Radius
•
In the graphics area, select two or more adjacent Edges, Faces, Features and Loops
. to fillet.
- or right-click on the feature and choose Select feature to fillet all the edges on the feature. • 4.
Select Full preview, Partial preview, or No preview.
Under Fillet Options, click Round corners. If necessary clear the Keep features check box.
5.
Click OK
.
Fillets applied without Round corners
Fillets applied with Round corners
Example of Full Round Fillet
Two instances of a full round fillet applied to tangent face sets
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Chapter 6 Features
Single instance of a full round fillet applied to tangent face set
Setback Fillet With setback fillets, you can create a smooth transition between the blended surface, along the edge of the part, into the fillet corner. You select a vertex and a radius, and then assign the same or different setback distances for each edge. The setback distance is the point along each edge at which the fillet starts to blend into the three faces that meet at the common vertex. Example of Setback Fillet Preview
Setback fillet shown with Full preview, and
Setback fillet shown with Full preview, and
with the same setback Distance applied to all three edges.
with a different setback Distance to all three edges.
Setback Distance (12mm)
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of 12mm
uniform for all edges
applied
Setback Distance different for all edges (4mm, 8mm, and 12mm)
To create setback fillets:
1.
Create a part that includes edges, meeting at a vertex, that you want to blend together.
2.
Click Fillet
3.
Under Fillet Type, keep the default Constant radius.
4.
Under Items to Fillet, do the following:
on the Features toolbar or click Insert, Features, Fillet/Round.
•
Select the Multiple radius fillet check box.
•
Clear the Tangent propagation check box.
•
In the graphics area, select three or more edges with a common vertex. You must select all the edges that meet at the common vertex.
The edges are listed in the Edge, Faces, Features and Loops • 5.
Select Full preview, Partial preview, or No preview.
If you want to apply the same setback distance to all edges, do the following: •
Under Setback Parameters, enter a Distance
•
Select one or more vertices for the Setback Vertices
•
Click Set All to apply equal setback distances to all edges on each vertex.
The values are displayed in the Setback Distances box 6.
box.
. box.
and on the callouts in the graphics area.
If you want to apply a different setback distance to each edge, do the following: •
Select one or more vertices for the Setback Vertices
•
Select Vertex <1> in the Setback Vertices box
•
Select the first edge (E1) in the Setback Distances box
•
Enter a Distance
•
Select the next edge (E2) belonging to Vertex <1>, and enter a Distance
•
Repeat the process for all edges belonging to Vertex <1>.
•
To apply the same Setback Distances Set Unassigned. The current Distance
•
box. . .
for the first edge (E1).
to all unspecified edges in the remaining vertices, click
is applied to all remaining vertices.
To apply different Setback Distances
to the remaining vertices, repeat the process for each
vertex (Vertex <2>, Vertex <3>, and so on) in the Setback Vertices box 7.
Click OK
SolidWorks 2004 Reference Guide
for that edge.
.
.
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Chapter 6 Features
Example of Setback Fillets
Model with no setback fillets applied
Model with preview of selected edges
Model with preview of setback callouts
Model with setback fillets applied
Variable Radius Fillet You can create variable radius fillets by specifying a different radius for each vertex of the edges you want to fillet. Variable radius fillets work on both solid and surface models. Between the two vertices in a sketch entity, there are variable radius control points that operate as follows: •
You can assign a radius value to each control point, or just assign values to one or both enclosing vertices.
•
The system defaults to three control points located at equidistant increments of 25%, 50%, and 75% along the edge.
•
You can change the relative position of each control point.
•
You can add or subtract control points along the edge you select to fillet. Adding or subtracting control points along the edge positions the control points in equidistant increments along the edge you select. Example of variable radius control points and tips on how to use them with a part.
To insert variable radius fillets:
1.
Click Fillet
2.
Under Fillet Type, select Variable Radius.
3.
Under Items to Fillet, do the following: o
on the Features toolbar or click Insert, Features, Fillet/Round.
Select the edges to fillet in the graphics area. NOTE: If you want to position and assign radii to the control points between the vertices, select a single edge, assign a value to the vertices first, and then manipulate the control points for that sketch segment. Once the first sketch segment is complete, select the second sketch segment, and repeat the process. The edges are listed in the Edges, Faces, Features, and Loops
box.
Under Variable Radius Parameters, the vertices are listed in the Attached Radii
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o
Clear Tangent propagation if necessary.
o
Select Full preview, Partial preview, or No preview.
box.
4.
5.
If you want to apply the same radius to all unassigned vertices in the Attached Radii following: a.
Under Variable Radius Parameters, enter a Radius
b.
Click Set All to apply equal radii to all vertices.
box, do the
.
To apply a different radius to all unassigned radii, do as follows: o
Under Variable Radius Parameters, select V1 in the Attached Radii radius to V1.
o
Enter a Radius
o
Select V2 in the Attached Radii
o
o
box to assign the
for the first vertex. box, and enter a Radius
for the second vertex.
To apply the same radius to all remaining vertices (and still retain the value assigned to V1), click Set unassigned. To keep applying different radii to the remaining vertices, select the remaining unassigned vertices in the Attached Radii
box, and enter a Radius
for each.
NOTE: You do not have to assign radius values to all the vertices in the Vertex list. However, you must assign a radius value to at least one vertex for each chain of edges. The software calculates the radii of the unassigned vertices, based on the following:
6.
o
the values of the adjacent vertices to which you have assigned radius values
o
the length of edges that connect the vertices
To apply radius values and manipulate control points, do the following: o
Select the first unassigned control point in the graphics area, located by default at 25%. NOTE: You can leave one or all control points unassigned.
o
Changing control point position: If necessary, drag the control point to a new position. The pointer changes to
o
.
Enter a radius value in the callout, or select P1 in the Attached Radii
box, and enter a Radius
. o
o o
To apply the same radius to all remaining control points (and still retain the value assigned to P1), select the remaining control points (P2 and P3), and click Set unassigned. If necessary, repeat the process for the remaining control points, P2 and P3. Add control points: If necessary, you can add additional control points by selecting the control point, pressing Ctrl and dragging the new control point into position. Or, from the PropertyManager, you can increment the value in the control points box . Adding new control points through the PropertyManager places the points at default positions. If necessary, you can then drag the control points to a new position.
o
Subtract control points: You can remove specific control points by right-clicking, and selecting Delete from the shortcut menu. Or, from the PropertyManager, you can decrement the value in the control points box . Deleting new control points through the PropertyManager removes the points from the default positions. NOTE: You can edit radius values for vertices or control points, but you cannot add new control points after you first build the part.
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Chapter 6 Features
7.
8.
Select a transition type. •
Smooth transition creates a fillet that changes smoothly from one radius to another when matching a fillet edge to the adjacent face.
•
Straight transition creates a fillet that changes from one radius to another linearly without matching edge tangency with an adjacent fillet.
Click OK
.
NOTE: You can remove an assigned radius value by selecting the vertex in the Attached Radii
box,
and pressing Delete. Radius values calculated by the software are not shown in the Attached Radii box or in the Radius
box.
Example of Variable Radius Fillet
Model with tangent faces
Edges to fillet
Variable radius fillets applied
To change radius values after they are inserted:
1.
Double-click the VarFillet feature in the FeatureManager design tree.
2.
Double-click and modify the dimensions displayed on the vertices in the graphics area. Radius values calculated by the software are not shown in the graphics area.
3.
4.
You can modify the value and position of control points: •
Select the control point in the Attached Radii in the graphics area.
box, or double-click and modify the dimension
•
Select the control point, the pointer changes to
, and drag the control point to the new position.
Click OK
.
Example of Variable Radius Fillet on Surface
No fillet applied to revolved surface
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Variable radius fillets applied to revolved surface
Example of Variable Radius Control Points
No control points
Variable radius control points
With control points
Using Variable Radius Control Points You can manipulate and assign radius values to the control points between the vertices of a variable radius fillet. Variable radius fillets now include previews. You can select a Full preview, a Partial preview, or No preview in the Fillet PropertyManager. TIPS: Here are some some tips on how to use variable radius fillet control points: •
You can assign a radius value to each control point, or just assign values to one or both enclosing vertices.
•
The system defaults to three control points located at equidistant increments of 25%, 50%, and 75% along the edge between the two variable radii.
•
You can change the relative position of each control point using the following methods:
•
o
Change the percentage of the control point in the callout
o
Select the control point and drag it to a new location
You can add or subtract control points along the edge you select to fillet, either as you create the fillet, or after you create the fillet by using Edit Definition. Adding or subtracting control points along the edge positions the control points in equidistant increments along the edge you select. o
Add control points: You can select a control point and Ctrl-drag to create an additional control point at a new location. Or, from the PropertyManager, you can increment the value in the control points box positions.
o
. Adding new control points through the PropertyManager adds points in the default
Subtract control points: You can remove specific control points by right-clicking, and selecting Delete from the shortcut menu. Or, from the PropertyManager, you can decrement the value in the control points box . Deleting new control points through the PropertyManager removes the points from the default positions.
•
You can select more than one sketch entity to fillet. Complete each entity before selecting any additional entities under Items to Fillet
, in the following manner:
o
Apply a radius to each vertex first
o
Apply radius values to one or all control points
o
Change the position of a control point before or after you apply a radius value
o
Add new control points, if necessary
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Chapter 6 Features
Model with single sketch entity selected and three default, unassigned control points.
Model with radii assigned to control points in default locations. NOTE: If you want to select two sketch segments, assign radii to the vertices and to the control points of the first sketch entity, before selecting any additional sketch entities.
Model with two sketch segments selected, and radius assigned to vertex from the second entity. NOTE: Before assigning radii to the control points, you should assign a radius to the vertex.
Model with two sketch segments selected, and all control points with assigned radii. NOTE: Both the old and new control point position are displayed, but only the new position includes the callout.
You can assign radius values to any number of control points, or leave them as unassigned.
Variable radius fillet applied
Return to Variable Radius Fillet
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Full Round Fillet With full round fillets, you can select three adjacent face sets (one or more tangent faces), and apply a fillet that is tangent to the three face sets. To create a full round fillet:
1.
Open the part to which you want to apply the fillet. Detail on the model
2.
Click Fillet on the Features toolbar, or Insert, Features, Fillet/ Round.
3.
Under Fillet Type, select Full round fillet.
4.
Under Items to Fillet, do the following:
5.
•
For Side Face Set 1 , select the top face, as shown on the right.
•
For Center Face Set , select the side face of the model, as shown on the right.
•
For Side Face Set 2 , select the face opposite Side Face Set 1, as shown. Note: Make sure that the Tangent Propagation check box is selected.
Click OK
.
The full round fillet is applied to one side of the model. Note: You can apply a full round fillet to the other side of the model. However, you need to create the second full round fillet as a separate feature.
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Chapter 6 Features
Full Round Fillet Details Note the following about the sketch used for the sample part on the right:
•
The three sketch entities indicated by the arrows are tangent to each other, as shown above.
•
Vertical relations are applied to the endpoints of the tangent sketch entities, as shown above.
Face Fillet You can blend non-adjacent faces with a face fillet. To insert a face fillet:
1.
Create a part with two or more adjacent, non continuous faces.
2.
Click Fillet
3.
Under Fillet Type, click Face fillet.
4.
Under Item to Fillet, do the following:
on the Features toolbar or Insert, Features, Fillet/Round.
•
Enter a Radius
•
In the graphics area, select first face or set of faces to blend. The selections are listed in the Face Set 1
•
.
box.
Click the Face Set 2
box and select the faces in the graphics area to blend with Face Set 1.
NOTE: If you select more than one face for either Face Set 1 or Face Set 2, each set of faces must be smoothly connected for the face fillet to properly propagate to all faces. • 5.
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces.
Under Fillet Options, you can do either of the following: •
Click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross section as opposed to a circular cross section. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary.
•
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Click the Help point check box to resolve an ambiguous selection. Then click a vertex close to the location where you want to insert the fillet.
6.
Click OK
.
Face Set 1 and Face Set 2 selected
Face fillet applied
Example of Curvature Continuous Fillet
No face fillet
Curvature continuous cleared
Curvature continuous checked
Using Help Point with Face Fillets When creating a face fillet between two faces, it may not be clear where the face blend should occur. Use Help point to define the desired location. Create a Help point by clicking a vertex on the side where you want the face fillet. The fillet is created at the location closer to the Help point.
Face Fillet with Hold Line You can determine the radius and shape of a face fillet by setting a boundary, or hold line, for the fillet. The hold line can be an edge on the part or a split line projected on a face to be filleted. In a face fillet with hold line, the radius of the fillet is driven by the distance between the hold line and the edge to be filleted. To insert a face fillet using an edge:
1.
Click Fillet
on the Features toolbar or Insert, Features, Fillet/Round.
2.
Under Fillet Type, click Face fillet.
3.
Under Item to Fillet, do the following: •
Do not enter a Radius determines the radius.
•
In the graphics area, select first face or set of faces to blend. The selections are listed in the Face Set 1
•
box.
Click the Face Set 2
SolidWorks 2004 Reference Guide
. The distance between the hold line and the edge that is filleted
box, and select the faces in the graphics area to blend with Face Set 1.
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Chapter 6 Features
•
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces. For Face Set 1, select a model face to fillet. For Face Set 2, select an adjacent face from the model to fillet. In this instance, include the additional model face for Face Set 2, to fillet along the entire edge of the model
The Hold line determines where the fillet ends. In this model, the lower edge of the faces selected for Face Set 2. 4.
Under Fillet Options, click the model edge or edges that mark the end of the fillet. The names are listed in the Hold lines box. If necessary, click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross section as opposed to a circular cross section. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary. When you use Hold lines and the Curvature continuous options together, you can select a hold line for each face.
5.
Click OK
.
The faces that share an edge with the hold lines are removed by the fillet. Example of Face Fillet Hold Lines
Faces to fillet
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Hold lines
Face fillet applied
Face Fillet with Split Line A split line is another way of creating a face fillet with a hold line. Instead of selecting an edge as the hold line, you use a split line. To create a face fillet with split line:
1.
Create a split line on a model face.
2.
Click Fillet
3.
Under Item to Fillet, do the following:
on the Features toolbar or Insert, Features, Fillet/Round.
•
Do not enter a Radius the model face).
•
In the graphics area, select first face or set of faces to blend. The selections are listed in the Face Set 1
4.
. The radius is determined by the hold line (the split line you created on
box.
•
Click the Face Set 2
box, and select the faces in the graphics area to blend with Face Set 1.
•
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces.
Under Fillet Options, click the model edge or edges that mark the end of the fillet. The names are listed in the Hold lines box. If necessary, click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes. You can also analyze the curvature using the curvature tool. Curvature continuous fillets differ from standard fillets in the following ways. They have a spline cross section as opposed to a circular cross section. Curvature continuous fillets are smoother than standard fillets because there is no jump in curvature at the boundary. Standard fillets include a jump at the boundary because they are tangent continuous at the boundary.
5.
Click OK
SolidWorks 2004 Reference Guide
.
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Chapter 6 Features
Holes Simple Hole Hole creates various types of hole features in the model. You place a hole and set a depth on a planar face. You can specify its location by dimensioning it afterwards. Recommendations In general, it is best to create holes near the end of the design process. This helps you avoid inadvertently adding material inside an existing hole. Also, if you are creating a simple hole which does not require additional parameters, use Simple Hole. The second option, using Hole Wizard introduces additional parameters that are not required with simple holes. Simple Hole provides better performance than Hole Wizard for simple holes. Hole Wizard
creates holes with complex profiles, such as Counterbore or Countersunk.
To insert a simple hole:
1.
Select a planar face on which to create the hole.
2.
Click Simple Hole
3.
Under Direction 1, do the following to select an End Condition:
or click Insert, Features, Hole, Simple.
•
If you choose Blind, specify the Depth
.
•
If you choose Up to Vertex, select a Vertex
•
If you choose Up to Surface, specify the the Face/Plane
•
If you choose Offset from Surface, specify the Face/Plane
in the graphics area. in the graphics area. , and enter the Offset distance
. Select the Reverse offset check box, if appropriate. To select a plane, use the flyout FeatureManager design tree. 4.
To extrude in a direction other than normal to the profile of the sketch, select Direction of Extrusion
5.
Type in a Hole Diameter
6.
If necessary, click Draft On/Off outward check box, if necessary.
7.
Click OK
to add a draft to the hole. Set the Draft Angle, and select the Draft
.
Normal to sketch extrusion
6-74
.
Direction vector extrusion
.
To position the hole:
1.
Right-click the hole feature in the model or the FeatureManager design tree, and select Edit Sketch.
2.
Add dimensions to position the hole. You can also modify the hole diameter in the sketch.
3.
Exit the sketch or click Rebuild
.
To change the diameter, depth, or type of the hole, right-click the hole feature in the model or the FeatureManager design tree, and select Edit Definition. Make the necessary changes, and click OK. Example of Hole Offset
True offset - Translate surface check box cleared
SolidWorks 2004 Reference Guide
Translated surface - Translate surface check box selected
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Chapter 6 Features
Creating a Simple Hole To create a simple hole:
1.
Select an End Condition to determine how far the feature extends. •
If you choose Blind, specify the Depth
.
•
If you choose Up to Vertex, select a Vertex
•
If you choose Up to Surface, specify the the Face/Plane
•
If you choose Offset from Surface, specify the Face/Plane
in the graphics area. in the graphics area. , and enter the Offset distance
. Select the Reverse offset check box, if appropriate. Select the Translate surface check box if you want to use an offset relative to the surface or the plane selected. If you want to use a true offset, clear the Translate surface check box. TIP: To select a plane, use the flyout FeatureManager design tree. 2.
Type in a Hole Diameter
.
3.
If necessary, click Draft On/Off outward check box, if necessary.
4.
Click OK
to add a draft to the hole. Set the Draft Angle, and select the Draft
.
End Condition Types The Type determines how far the hole extends.
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Blind
Extends the feature from the sketch plane for a specified distance.
Through All
Extends the feature from the sketch plane through all existing geometry.
Up to Next
Extends the feature from the sketch plane to the next surface that intercepts the entire profile. (The intercepting surface must be on the same part.)
Up to Surface
Extends the feature from the sketch plane to the selected surface. Click on a face to specify the surface.
Offset from Surface
Extends the feature from the sketch plane to a specified distance from the selected surface. Click on a face to specify the surface. Specify an Offset.
Up to Vertex
Extends the feature from the sketch plane to a plane that is parallel to the sketch plane and passing through the specified vertex. Click on a Vertex.
Hole Wizard Hole Wizard Overview The Hole Wizard user interface includes the following capabilities: Dynamic Updating The hole type you select determines the capabilities, available selections, and graphic previews. After you select a hole type, you determine the appropriate fastener. The fastener dynamically updates the appropriate parameters. The interface uses a three column format (Property, Parameter 1, Parameter 2), along with an overall graphic preview based on end condition and depth. Parameters may include one or two values. You can adjust the width of each parameters column. In addition to the dynamic graphic preview based on end condition and depth, graphics in the parameter columns show specific details, as they apply to the type of hole you select. Capabilities Functionality includes tabs for the following hole types: •
Counterbore
•
Countersink
•
Hole
•
Tap
•
PipeTap
•
Legacy
When you create a hole using the Hole Wizard, the type and size of the hole, based on the Description, appears in the FeatureManager design tree. You can create holes on a plane with the Hole Wizard, as well as holes on planar faces. Holes on a plane allows you to create holes at an angle to the feature. You can edit the plane you create to use with the Hole Wizard. Pre-Selection and Post-Selection Note the following regarding pre-selection and post-selection of a face when using the Hole Wizard hole: •
When you pre-select a planar face, and click Hole Wizard is a 2D sketch.
on the Features toolbar, the resulting sketch
•
If you first click Hole Wizard 3D sketch.
•
Unlike a 2D sketch, you cannot constrain a 3D sketch to a line. However, you can constrain a 3D sketch to a face.
, and select either a planar or a non-planar face, the resulting sketch is a
Favorite Name For each hole type (except Legacy), you can create, save, update, or delete hole types to include your favorite properties parameters. This allows you to apply any saved hole types to a SolidWorks document.
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Chapter 6 Features
Hole Wizard Holes as Assembly Features You can add any hole wizard hole as an assembly feature that extends through more than one component. Functionality includes display of cosemetic threads on assembly feature holes. Using the Hole Series tab, you can create hole features in the components of the assembly. Unlike other assembly features, the holes are contained in individual parts as externally referenced features. To access hole wizard:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the appropriate tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
Hole Wizard on a Plane
Example of Non-Planar Hole Wizard Hole
NOTE: On models with multiple features, you can add hole wizard holes to any of the features in the model.
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Hole Wizard Hole Placement You can position a single hole created with Hole Wizard. You can also create and position multiple holes, using the initial instance as the seed. To position a single Hole Wizard hole:
1.
Click Hole Wizard to create the Hole Wizard hole, and enter the information in the Parameters column for each Property that you want to customize.
2.
Click Next to display the Hole Placement dialog box.
3.
Drag the hole to its approximate position by clearing the Point
The pointer changes from 4.
Use Dimension hole.
5.
Click Finish.
to
or Add Relations
tool on the Sketch Tools toolbar.
. on the Sketch Relations toolbar to position and fully define the
To create and position multiple Hole Wizard holes:
1.
Create the Hole Wizard hole, selecting the hole type and the parameters.
2.
Click Next to display the Hole Placement dialog box.
3.
Using the Point
4.
Click Dimension
5.
Click Finish.
SolidWorks 2004 Reference Guide
tool, click where you want to create each hole. and add the appropriate dimensions for each hole to fully define.
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Chapter 6 Features
Favorite Hole Types When you select either the Countersink, Counterbore, Hole, Tap, or Pipe Tap tabs, you can create favorite hole types. Favorite hole types can include any of the characteristics that are relevant to that hole type. Once you create a favorite hole type using the appropriate information from the Property and Parameters columns, you add the hole to the files. You can later select the favorite hole type by scrolling down the list, and apply it to the part. You can update (change values, but retain the same favorite name), or delete a favorite hole type. Property Each tab in the Hole Definition dialog box represents a hole type. Select a hole type, and the appropriate changes display in the Property column. For example, the Property column includes a listing for Standard as well as Screw type. For each item listed in the Property column, the appropriate items are displayed in the Parameters column. Return to overview Parameters Each tab in the Hole Definition dialog box represents a hole type. Select a hole type, and the appropriate changes display in the Parameters column, where you enter information to customize each hole type. The listings and previews in the Parameters column vary, depending on which hole type you select. For example, all hole types include, as a Property, a Standard recognized by the industry. The Standard includes definitions such as ISO and JIS. Other descriptions and values, however, depend on which tab (hole type) you select. The different and appropriate parameters are displayed in the Property and Parameters columns. The system also updates dynamically, reacting to the information that you enter in the Parameters column. For example, with a countersink type, you can adjust the Hole Fit & Diameter to be either: Close, Normal, or Loose. As you select each of these values, the diameter changes, based on dimensions you have set in other areas. Close Normal Loose NOTE: Some values do not use the document’s units. Instead, they adopt units based on the selected fastener type. Return to overview
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Delete Favorite Hole To delete a favorite hole type:
1.
Select the appropriate tab from the Hole Definition dialog box.
2.
Scroll down the list of Favorites to select.
3.
Click Delete.
Retrieve Favorite Hole To retrieve a favorite hole type:
1.
Select the appropriate tab from the Hole Definition dialog box.
2.
Scroll down the list of Favorites to select.
Update Favorite Hole To update a favorite hole type:
1.
Select the appropriate tab from the Hole Definition dialog box.
2.
Scroll down the list of Favorites to select.
3.
Enter the information in the Parameters column for each Property that you want to update.
4.
Click Update and click Yes to the prompt to apply the new values to the same favorite hole type.
New Favorite Name Use the New Favorite Name dialog box to add a specific hole wizard configuration to your list. The favorite hole type is available for future holes you create. To add a new favorite name:
1.
Click Hole Wizard want to customize.
, and enter the information in the Parameters column for each Property that you
2.
Under Favorites, click Add to display the New Favorite Name dialog box.
3.
Accept the default name retrieved from the Description, or type in the name of your choice.
4.
Click OK.
Hole Series You can use Hole Series to create a series of holes through the individual parts of an assembly.
The Hole Series is an assembly feature which creates hole features in the components of the assembly. A Hole Series extends through each unsuppressed component in the assembly that intersects the axis of the hole (the components do not have to touch). Unlike other assembly features, the holes are contained in the individual parts as externally referenced features. If you edit a Hole Series within an assembly, the individual parts are modified.
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To create a Hole Series:
1.
Suppress the components in your assembly that you do not want to be cut by the hole.
2.
Select a plane or planar face in your assembly, and click Hole Wizard Hole, Wizard.
, or Insert, Assembly Feature,
The Hole Definition dialog box appears. 3.
Click the Hole Series tab. The Hole Series is divided into First Part, Middle Parts, and Last Part.
4.
•
The First Part is the part whose face you selected. The counterbored or countersunk hole, if any, is in the First Part.
•
The Last Part is the last part through which the hole passes. The Last Part contains the tap, or the bottom of the hole if it is a blind hole.
•
The Middle Parts are all the other parts through which the hole passes.
If you want all parts of the hole series to be the same diameter if you change the Size property, select the Automatically select middle and end hole sizes based on first hole size check box. This sets the diameters for the middle and last parts by choosing the closest available hole size to the diameter of the first part. The available hole sizes depend on the selected screw type. Select this check box before you set a diameter for the hole in the first part.
5.
Enter parameters for the hole series: a.
b.
c.
On the First Part tab: •
Choose a Standard, Style, Screw type, and Size.
•
If you select a Screw type of C'Bore or C'Sink, choose a Hole Fit.
•
The parameters of the hole appear in the box. You can change the parameters.
On the Middle Parts tab: •
Select a size, or accept the default.
•
Choose a Screw type.
On the Last Part tab: •
Select a Style (Hole or Tap). If you select Tap, choose Bottoming Tapped hole, or Tapped hole. Select from the cosmetic thread display options. If you select Hole, choose a Screw type.
•
For a tapped hole, select a Tap Drill Type. If you select Blind, choose a depth. This is the depth from the front face of the Last Part in the hole series. If you select Up To Next, choose a Thread Type.
• 6.
The parameters of the hole appear in the box. You can change these parameters.
Click Next. The Hole Placement dialog box appears.
7.
Add dimensions to locate the center of the hole, or add sketch points to create multiple holes.
8.
Click Finish to add the holes to your assembly and close the dialog box.
NOTES: •
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You cannot use Hole Series on assembly components which are multiple instances of the same part, unless each instance is a separate configuration of the part.
•
You cannot edit the parameters of a Hole Series hole in an individual part (unless you underive the feature), although you can delete or suppress the hole. To edit the parameters of the hole in context of the assembly, go to the assembly and edit the Hole Series. If you underive the Hole Series hole in an individual part it becomes a Hole Wizard hole with no reference to the assembly.
Hole Wizard Holes Hole Wizard Custom Standards Click Tools, Options, System Options, Data Options, Edit Standards Data to display the Configure Data dialog box. Create Standards To create new hole wizard standards:
1.
On the Standards tab, type a name for Create new standard name.
2.
Select an industrial or national standard in Create from to specify the type of standard.
3.
Click Create. The new standard name appears in the Derived Standards list. The new standard includes data from the selected industrial or national standard.
4.
Click Apply to save your changes and continue editing, or click OK to save your changes and close the Configure Data dialog box.
Delete Standards You can delete derived hole wizard standards. To delete one of your standards:
1.
Select any standard you created from the Derived Standards list.
2.
Click Delete.
3.
Click Apply to save your changes and continue editing, or click OK to save your changes and close the Configure Data dialog box.
Edit Hole Wizard Standards You can edit derived hole wizard standards. To edit the data:
1.
Click Tools, Options, System Options, Data Options.
2.
Click Edit Standards Data.
3.
On the Edit Data tab, select a catalog from the tree.
4.
Expand the catalog, then the chapters and the pages beneath the catalog to select the Hole Wizard hole to edit. Each row in the table refers to a Hole Wizard configuration.
5.
Editing values: •
Change: To change a value, click in the table and edit the value.
For example, under Bolts and Screws , Machine Screws change the Size name, the Pitch, the Diameter, and so on.
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, Hex Screw - Ansi
, you can
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6.
•
Add. To add a new row of data, scroll to the bottom of the table and type values in the row with the asterisk.
•
Delete. To delete a row of data, click the button at the beginning of the row and press Delete.
Click Apply to save your changes and continue editing, or click OK to save your changes and close the Configure Data dialog box.
Hole Wizard - Edit Standards Data You can create your own standards for Hole Wizard holes by deriving new standards from an existing standard. To customize existing standards, Hole Wizard uses the same database used by the SolidWorks Toolbox add-in. You do not need to have SolidWorks Toolbox installed on your system to create new standards for Hole Wizard holes. To create your own Hole Wizard standards:
1.
Click Tools, Options, System Options, Data Options.
2.
Click Edit Standards Data. The Configure Data dialog box appears.
Counterbore When you select the Counterbore tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The preview also updates, depending on your selections. To access hole wizard and use counterbore type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Counterbore tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a counterbore hole:
1.
Determine what type of fastener you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Metric or JIS. Screw type, select for example Button or Hex Screw. Size, select a size for your fastener. The Description updates.
Preview with the Counterbore tab
NOTE: Once you have selected a type of fastener, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameters for the hole you want to create on your part. •
•
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End Condition & Depth, select an end condition from the list and enter a depth. Note how the preview for the end condition updates and items in the Parameters column change appropriately. Hole Fit & Diameter, select a fit and enter a diameter. Note that when you change the hole fit, the value updates, increasing or decreasing as appropriate.
Preview of Up to Vertex Example of dynamic counterbore values
3.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Note: Setting a Head Clearance value other than 0.00 adds that value to the Counterbore value above it.
Dynamic Changes with Counterbore Holes For example, if you select Up To Vertex: •
The preview updates to show a vertex.
•
In the End Condition & Depth box, the depth becomes unavailable.
•
In the Selected Item & Offset box, the vertex becomes available so you can select a vertex from the graphics area. The offset box becomes unavailable.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Countersink When you select the Countersink tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The preview also updates, depending on your selections. To access hole wizard and use countersink type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Countersink tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a countersink hole:
1.
Determine what type of fastener you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Metric or BSI. Screw type, select for example Flat Head or Oval Head. Size, select a size for your fastener. The Description updates.
Preview with the Countersink tab
NOTE: Once you have selected a type of fastener, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameters for the hole you want to create on your part. •
•
3.
End Condition & Depth, select an end condition from the list and enter a depth. Note how the preview for the end condition updates and items in the Parameters column, change appropriately. Hole Fit & Diameter, select a fit and enter a diameter. Note that when you change the hole fit, the value updates, increasing or decreasing as appropriate.
Preview of Offset From Surface Example of dynamic countersink values
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
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4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Dynamic Changes with Countersink Holes For example, if you select Offset From Surface: •
The preview updates to show an offset.
•
In the End Condition & Depth box, depth becomes unavailable.
•
The Selected Item & Offset box becomes available so you can select an item in the graphics area from which to offset, and enter an offset value.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Hole When you select the Hole tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The graphic preview also displays only information that applies to holes that do not fall into the other identified categories. To access hole wizard and use hole type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Hole tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a hole:
1.
Determine what type of fastener you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Inch or DIN. Screw type, select for example Screw Clearances or Fractional Drill Sizes. Size, select a size for your fastener. The Description updates properly.
Preview with the Hole tab
NOTE: Once you have selected a type of fastener, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameters for the hole you want to create on your part. •
•
3.
Hole Type & Depth, select an end condition from the list and enter a depth. Note how the preview for the end condition updates and items in the Parameters column update appropriately. Hole Diameter & Fit, select a fit and enter a diameter. Note that when you change the hole fit, the value updates, increasing or decreasing as appropriate.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
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4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Preview of Up to Surface Example of dynamic hole values
Dynamic Changes with Regular Holes For example, if you select Up To Surface: •
The preview updates to show a reference surface at which the hole stops. Note that the reference surface does not need to be flat.
•
The Hole Type & Depth box becomes unavailable.
•
The Selected Item & Offset box becomes available so you can select a reference surface in the graphics area at which the hole stops.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Tap When you select the Tap tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The graphic preview also displays only information that applies to tap holes. To access hole wizard and use tap type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Tap tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a tap hole:
1.
Determine what type of tap you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ISO or DIN. Screw type, select a Bottoming Tapped Hole or a Tapped hole. Size, select a size for your tap. The Description updates.
Preview with the Tap tab
NOTE: Once you have selected a tap type, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameter for the hole you want to create on your part. •
3.
Tap Drill Type & Depth, select an end condition from the list and enter a depth if appropriate. Note how the preview for the end condition updates and opens the appropriate items in the Parameters column.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
SolidWorks 2004 Reference Guide
Preview of Through All Example of dynamic tap values NOTE: You can click the Add Cosmetic Thread arrow to display the options. For tapped holes with cosmetic threads created in the Hole Wizard, the hole diameter is the diameter of the tap drill. For tapped holes without cosmetic threads, the hole diameter is the basic major diameter of the thread: the cylinder is at nominal thread diameter. NOTE: To create a hole at the tap drill size for the thread: Make a plain hole with the screw type set to Tap Drills, and choose the appropriate thread size.
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4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Dynamic Changes with Tap Holes For example, if you select Through All: •
The preview updates to show a hole that extends through all of the part.
•
The Tap Drill Type & Depth and the Selected Item & Offset boxes become unavailable.
•
The Tap Drill Diameter & Angle box is displayed. The diameter is available, but the angle is not.
•
The Thread Type & Depth box, available with Tap holes, displays the most likely calculated values, along with the option to change both the thread type and the depth.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
NOTE: For tapped holes with cosmetic threads created in the Hole Wizard, the hole diameter is the diameter of the tap drill. For tapped holes without cosmetic threads, the hole diameter is the outer diameter of the thread. Pipe Tap When you select the Pipe Tap tab in the Hole Definition dialog box, all the information in the Property and Parameters columns update to retrieve only information that applies to this hole type. The graphic preview also displays only information that applies to pipe tap holes. To access hole wizard and use pipe tap type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Pipe Tap tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To create a pipe tap hole:
1.
Determine what type of pipe tap you need. For each of the following items in the Property column, select the corresponding item from the Parameters column. • • •
Standard, select for example ANSI Inch or DIN. Screw type: select Tapered Pipe Tap. Size, select a size for your pipe tap. The Description updates properly.
Preview with the Pipe Tap tab
NOTE: Once you have selected a pipe tap type, the Hole Wizard updates items in the Parameters column. 2.
Determine the following parameter for the hole you want to create on your part. •
3.
Tap Drill Type & Depth, select an end condition from the list and enter a depth if appropriate. Note how the preview for the end condition updates and opens the appropriate items in the Parameters column.
Determine which (if any) of the remaining parameters you need to change. Enter the values, using the illustrations as a guide to what each item in the Property column represents.
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Preview of Through All Example of dynamic pipe tap values NOTE: You can click the Add Cosmetic Thread arrow to display the options.
4.
To save these settings and use them for future holes, save as a favorite.
5.
Click Next to position the hole on your model.
Dynamic Changes with Pipe Tap Holes For example, if you select Through All: •
The preview updates to show a hole that extends through all of the part.
•
The Tap Drill Type & Depth and the Selected Item & Offset boxes become unavailable.
•
The Tap Drill Diameter & Angle box is displayed. The diameter is available but the angle is not.
•
The Thread Depth box, available with Pipe Tap holes, displays the most likely calculated value, along with the option to change the depth.
•
The system calculates the most likely remaining values. You can accept or enter appropriate new values.
Legacy Use the Legacy tab to edit any holes that you created prior to the SolidWorks 2000 release. When you select the Legacy tab in the Hole Definition dialog box, all the information including the graphic preview, displays in the same format as when you originally created the hole, prior to the SolidWorks 2000 release. NOTE: If you scroll through the list, the Hole type list now includes all the new hole types that are part of the Hole Wizard. To access hole wizard legacy type:
1.
Create a part and select a planar surface.
2.
Click Hole Wizard
3.
Click the Legacy tab in the Hole Definition dialog box.
on the Features toolbar or Insert, Features, Hole, Wizard.
To edit a hole created prior to SolidWorks 2000:
1.
With the part open, right-click the hole in FeatureManager design tree and select Edit Definition. The hole type you created is displayed, along with existing dimensions and a preview.
2.
To change a dimension in the Section dimensions box, click-pause-click, then enter a new dimension value.
3.
If necessary, select the End condition from the list.
4.
Specify the Face, Vertex, or Offset, if the end condition requires it.
5.
Click Next.
6.
Drag the hole center to the desired location or dimension the center point as required.
7.
Click Finish.
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Lofts Loft Overview Loft creates a feature by making transitions between profiles. A loft can be a base, boss, cut, or surface. You can manipulate a loft in the following ways: •
Create a loft as a thin feature.
•
Synchronize loft profiles.
•
Control the magnitude and direction of a tangency in a loft.
•
Add, position, and edit new loft sections.
•
Add side tangency to lofts that use guide curves.
•
View the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. When you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. You create a loft using two or more profiles. Only the first, last, or first and last profiles can be points. For a solid loft, the first and last profiles must be model faces or faces created by split lines, planar profiles, or surfaces.
Other loft topics:
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Loft: split line
Loft: guide curve and planar profile
Loft: centerline
Loft: guide curve and non-planar profile
Loft: thin feature
Loft: tangency control
Loft: add sections
Loft: side tangency
Loft Features You can create a loft by connecting profiles. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. To create a loft:
1.
Click Loft
, or Insert, Boss, Loft. Select the profile sketches in order in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. TIP: For each profile, select the point from which you want the path of the loft to travel. In the PropertyManager, the sketches are listed under Profiles
.
2.
Examine the path preview. If necessary, click Move Up or Move Down profiles, or re-select the sketches to connect different points on the profiles.
to adjust the order of the
3.
Under Start/End Tangency: If you want to select a different option for Start tangency type or End tangency type, click Start/End Tangency. •
Select the start and end tangency type.
•
To control tangency, enter a start and an end tangent length in the PropertyManager, or drag the arrows in the graphics area. If necessary, click Reverse Tangent Direction
4.
5.
Under Options, select the following check boxes if necessary: •
Maintain tangency causes the surfaces in the resulting loft to be tangent if the corresponding segments are tangent.
•
Advanced smoothing obtains smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs.
•
Close loft creates a closed body along the loft direction. This connects the last sketch and the first sketch automatically.
•
Show preview displays shaded previews by default. Click to clear the Show preview check box to view the path and the guide curves.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
If you are using guide curves, click Guide Curves as guide curves. If necessary, click Move Up
6.
.
, then select the sketches in the graphics area to use or Move Down
to reorder multiple guide curves.
You can add side tangency between adjacent faces that lie along the path of a guide curve. This creates a smoother transition between the adjacent faces. Select All Faces in the Guide tangency type list. NOTE: For best results when using side tangency, the profiles should also be tangent to the tangency faces at the point where each profile meets the guide curve. Ideal tolerance is 2 degrees or less. Avoid profiles with connection points greater than 2 degrees off tangency.
7.
Under Centerline Parameters: If you are using a centerline parameter as opposed to a guide curve, click
8.
Centerline Parameters , then select the sketch in the graphics area to use as the centerline. Click the Thin Feature check box to create a thin feature. •
Set the Type, and click Reverse Direction
•
Click the Direction 1 Thickness
SolidWorks 2004 Reference Guide
if necessary.
, and if necessary the Direction 2 Thickness
.
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9.
Click OK
to create the loft.
NOTE: After you create a loft, you can add and edit additional loft sections. Other loft topics:
Loft: split line
Loft: guide curve and planar profile
Loft: centerline
Loft: guide curve and non-planar profile
Loft: thin feature
Loft: tangency control
Loft: add sections
Loft: side tangency
Example of Shaded Loft Preview
Loft shaded preview
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Loft feature applied
Example of Loft Control Tangency
Loft with no control tangency
Loft with control tangency
Example of Loft Using Maintain Tangency
Sketch profile with preview
Loft without using Maintain tangency option
Loft using Maintain tangency option
Click Maintain tangency to cause the corresponding surfaces in the resulting loft to be tangent if the corresponding lofting segments are tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs may be converted to splines. Example of Using Close Loft
Shaded loft preview with Close loft cleared.
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Loft with Close loft cleared
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Shaded loft preview with Close loft selected.
Loft with Close loft selected
Click Close loft under Options to create a closed body along the loft direction. This connects the last sketch and the first sketch automatically. Example of Loft with Side Tangency
Loft with side tangency not applied
Loft with side tangency applied
Loft with Thin Feature You can create a Thin Feature loft. To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness .
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, if necessary.
and if using Two-Direction as the Type, a Direction 2 Thickness
Loft Thin Feature Samples
Loft
Loft with thin features
Loft with Non-Planar Profile You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles. The guide curves help you control the intermediate profiles that are generated. View the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. After you create a loft, you can add and edit additional loft sections. To create a loft using non-planar profiles:
1.
Create at least one non-planar profile. The non-planar profile can be a model face or a model edge.
2.
Set up the planes needed for the profile sketches. Use existing planes, or create new planes. The planes do not have to be parallel.
3.
Sketch the profiles.
4.
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Lofted Cut Cut, Loft
on the Features toolbar, or Insert,
•
Lofted Surface on the Surfaces toolbar or Insert, Surface, Loft The non-planar profile is represented by the boss-extrude with rounded top. The planar profiles are sketched on planes 4 and 5.
5.
Under Profile: a.
Select the Profiles to loft in the graphics area. Select the face of the non-planar profile and the other profiles in order, by clicking a corresponding point on each profile. You do not have to select the vertices precisely; the vertex closest to the selection point is used. A shaded preview connecting the selected entities appears in the graphics area.
6.
b.
You can change the synchronization between the profiles by manipulating the connectors.
c.
Examine the preview, and click Move Up
or Move Down
to reorder the profiles.
To control tangency at the start and end of the loft, click Start/End Tangency.
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7.
Under Options, select Maintain tangency, Advanced smoothing, or Close loft, if needed. •
Clear Show preview to display only the profiles and the path.
•
Merge result merges all the loft elements.
8.
To create a loft with thin walls, select the Thin Feature check box.
9.
Click OK
.
Loft with Split Line You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. To create a loft using a split line:
1.
Use a split line to create a non-planar profile on a model face.
2.
Set up the planes needed for the profile sketches. Use existing planes, or create new planes. The planes do not have to be parallel.
3.
Sketch the profiles.
4.
Click one of the following: • •
Loft on the Features toolbar or Insert, Boss, Loft Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar or Insert, Surface, Loft
The planar profile is a circle created on plane 4.
5.
The face created by the split line is projected onto a non-planar face.
Under Profile, do the following: •
Select the Profiles
to loft in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. •
Click Move Up
or Move Down
6.
To control tangency, click Start/End Tangency.
7.
Under Guide Curves
to reorder the profiles.
select guide curves from the graphics area, if needed.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type.
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8.
9.
Under Options, select Maintain tangency, Advanced smoothing, or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
To create a loft with thin walls, click Thin Feature.
10. Click OK
.
Loft with Guide Curve and Planar Profile You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles. The profiles can be either planar or non-planar. The guide curves help you control the intermediate profiles that are generated. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. After you create a loft, you can add and edit additional loft sections. To create a loft using guide curves and planar profiles:
1.
Sketch one or more guide curves.
2.
Sketch the profiles. See recommendations for using guide curves with a loft.
3.
Add relations between the guide curves and the profiles. You can use a combination of: •
•
•
4.
5.
Pierce relations between the guide curves and vertices, user-defined sketch points, or both, on the profile. Coincident relations between vertices, userdefined sketch points, or both, of the guide curves and the profiles. Add these relations to the profile sketches.
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar or Insert, Surface, Loft
Under Profile, do the following: •
Select the Profiles
to loft in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. •
Click Move Up
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or Move Down
to reorder the profiles.
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6.
You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. To control Start/End Tangency, do the following: •
For Start tangency type select either Normal to Profile, Direction Vector, or All Faces. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
.
•
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
•
Examine the preview and click Reverse Tangent Direction tangent.
•
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
to reverse the direction of the
.
Examine the preview and click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options Example of controlling the tangency magnitude and direction: 7.
Under Guide Curves, do the following: •
Select the Guide Curves
•
Click Move Up
in the graphics area.
or Move Down
to change the order in which to use the guide curves.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type. 8.
9.
Under Options, select Maintain tangency, Advanced smoothing or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness Thickness
10. Click OK
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.
.
, if necessary.
and if using Two-Direction as the Type, a Direction 2
Loft with Guide Curve and non-Planar Profile You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles. The profiles can be either planar or non-planar. The guide curves help you control the intermediate profiles that are generated. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. After you create a loft, you can add and edit additional loft sections. To create a loft using guide curves and non-planar profiles:
1.
Use a split line to create a non-planar profile on a model face.
2.
Sketch one or more guide curves. See recommendations for using guide curves with a loft.
3.
Add a Pierce relation between the guide curves and an edge or vertex on the non-planar face.
4.
Sketch the remaining profiles needed to create the loft. Add Pierce relations between the profiles and the guide curves. The relations should be added to the profile sketches.
Non-planar profile with split line and guide curve 5.
6.
Non-planar profile with split line and guide curve leading to planar profile
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar or Insert, Surface, Loft
Under Profile, do the following: •
In the graphics area, select the split line face and the planar Profiles
in order.
In the graphics area, a shaded preview connecting the selected entities appears. • 7.
Click Move Up
or Move Down
to reorder the profiles.
Under Start/End Tangency: You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. To control Start/End Tangency, do the following: •
For Start tangency type select either Normal to Profile, Direction Vector, or All Faces. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
.
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
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•
Examine the preview and click Reverse Tangent Direction tangent.
•
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
to reverse the direction of the
.
Examine the preview and click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options Example of controlling the tangency magnitude and direction 8.
Under Guide Curves, do the following: •
Select the Guide Curves
•
Click Move Up
in the graphics area.
or Move Down
to change the order in which to use the guide curves.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type. 9.
Under Options, select Maintain tangency, Advanced smoothing or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
10. To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness Thickness
11. Click OK
, if necessary.
and if using Two-Direction as the Type, a Direction 2
.
.
Example of Using Control Tangency in Lofts
Loft between adjacent edges of two surfaces
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Loft preview using zero Start tangency and End tangency
Loft using Normal to profile for both Start tangency and End tangency
Recommendations for Lofts with Guide Curves Consider the following when creating lofts with guide curves. •
Guide curves must intersect all the profiles.
•
There is no limit to the number of guide curves you may use.
•
Guide curves can intersect at points.
•
You can use any of the following items as a guide curve: sketched curves, model edges, or curves of any kind.
•
If a loft fails or twists: o
o
Use loft synchronization to modify the synchronization between loft profiles. You adjust the synchronization by changing the alignment between the profiles. To adjust the alignment, you manipulate the handles which appear in the graphics area as part of the connector. The connector is the poly line connecting corresponding points in both directions. Add a Curve Through Reference Points as a guide curve, selecting corresponding vertices of the profiles to create the curve.
•
Guide curves can be longer than the resulting loft. The loft stops at the end of the smallest guide curve.
•
You can further control the behavior of the loft by creating the same number of segments on all the guide curves. The endpoints of each segment mark corresponding points for transition of the profiles.
Loft Side Tangency You can add side tangency between adjacent faces that lie along the path of a guide curve. This creates a smoother transition between the adjacent faces. NOTE: For best results when using side tangency, the profiles should also be tangent to the tangency faces at the point where each profile meets the guide curve. The ideal tolerance is 2 degrees or less. You can use profiles with connection points up to 30 degrees off tangency before the loft fails. To add side tangency:
1.
Under Profiles
2.
Under Guide Curves
3.
, select the loft profiles in the graphics area. , do the following:
•
Select the guide curves in the graphics area.
•
Select All Faces from the Guide tangency type list.
Click OK
.
Loft with Centerline You can create a loft that uses a variation of a guide curve that acts as a centerline. The sketch planes of all the intermediate sections are normal to the centerline. The centerline may be a sketched curve, a model edge, or a curve. After you create a loft, you can add and edit additional loft sections. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. To use a center line to guide a loft:
1.
Create the profiles.
2.
Sketch a curve, or create a curve. The curve must intersect the area inside each closed profile and any split line faces.
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3.
4.
Click one of the following: •
Loft
on the Features toolbar or Insert, Boss, Loft
•
Insert, Cut, Loft
•
Lofted Surface
on the Surfaces toolbar, or Insert, Surface, Loft
Under Profile, do the following: •
Select the Profiles
to loft in the graphics area.
In the graphics area, a shaded preview connecting the selected entities appears. • 5.
Click Move Up
or Move Down
to reorder the profiles.
Under Start/End Tangency: You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. To control Start/End Tangency, do the following: •
For Start tangency type select either Normal to Profile, Direction Vector, or All Faces. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
.
•
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
•
Examine the preview and click Reverse Tangent Direction tangent.
•
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
•
to reverse the direction of the
.
Examine the preview and click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options Example of controlling the tangency magnitude and direction 6.
When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type.
7.
Under Options, select Maintain tangency, Advanced smoothing, or Close loft, if needed. •
You can also clear the Show preview check box to display only the profiles and the path.
•
Merge result is the default value. Clear the check box if you do not want to merge all the loft elements.
8.
Under Centerline Parameters, select the Centerline
sketch in the graphics area.
9.
You can preview the effect of the centerline. Click Number of Sections and adjust the slider to change the number of previews to display in the graphics area. Then click Show Sections
to display the previews
by using the arrows . NOTE: The number of sections you specify affects the shape of the loft. You may need to increase, or decrease, the number of sections to get the desired shape.
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10. To apply a Thin Feature, do the following: •
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
•
Examine the preview and click Reverse Direction
•
Enter a Direction 1 Thickness Thickness
11. Click OK
, if necessary.
and if using Two-Direction as the Type, a Direction 2
.
.
Loft with Start and End Tangency Control You can control the tangency magnitude and direction of a loft between sketches, faces, or edges of surfaces. When using guide curves, you can also control side tangency by selecting All Faces under Guide tangency type. You can view the loft using zebra stripes as you create it. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra stripes preview. To control Start/End Tangency, do the following:
1.
Under Start/End tangency type select either Normal to Profile, Direction Vector. NOTE: If you use Direction Vector as the Start tangency type, select a plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
.
2.
Set the Start Tangent Length. Use the handles in the graphics area and drag to change the value, or enter the values directly in the PropertyManager.
3.
Examine the preview and if necessary, click Reverse Tangent Direction tangent.
4.
Select an End tangency type, and set an End Tangent Length. If you use Direction Vector as the End tangency type, select a different plane (using the flyout FeatureManager design tree) or a linear edge or axis to define the Direction Vector
5.
to reverse the direction of the
.
Examine the preview and if necessary, click Reverse Tangent Direction tangent.
to reverse the direction of the
Example of loft tangency options
Loft preview using no Start tangency and End tangency
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Loft using All Faces for both Start tangency and End tangency
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Chapter 6 Features
Add Loft Section You can add one or more loft sections to an existing loft. When you add a section, it creates a loft section and a temporary plane. You can drag the plane to position the new loft section along the axis of the path. You can also use a pre-existing plane (created before the loft feature) to position the new loft section. Once you position the new loft section, you can use the shortcut menu to edit the new loft section. Edit the loft section as you would any other sketch element (dimension, add relations, modify shape, and so on). You can view the loft using zebra stripes as you add the new loft section. Place the pointer on the loft, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear Zebra stripes preview. To add a loft section:
1.
Right-click along the path of the existing loft where you want to add the new loft section, and select Add Loft Section. The Add Loft Section PropertyManager appears with the current loft sections listed. In the graphics area, a temporary plane appears with the new loft section. NOTE: You can click OK in the PropertyManager after adding the new loft section if you do not need to specify a different plane, reposition the loft section, or use the edit functions.
2.
If you want to use the temporary plane, position the plane along the path of the existing loft by doing one of the following: •
Drag the plane along the axis of the path of the existing loft.
•
Place the pointer at one of edges of the plane. The pointer changes to . This allows you to change the angle of the plane and modify the shape of the new loft section.
Drag plane 3.
Rotate plane
If you want to use another previously created plane, click the Use selected plane check box, and select a plane
.
NOTE: The plane you use to add a new loft section must appear before the loft section in the FeatureManager design tree. 4.
Once you position the new loft section, you can do either of the following: •
Click OK
in the PropertyManager to create the loft section.
•
Use the shortcut menu and select Edit Loft Section to add relations, dimension, and so on
If you select Edit Loft Section, a dialog box appears, allowing you to go Back (to reposition the plane), Cancel (the add section process), or Finish.
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5.
Once you define the new loft section, click Finish. The sketch used to add the new loft section appears in the loft feature.
You can delete any sketch you added using Add Loft Section. To delete a new loft section from a loft:
1.
Right click the loft icon in the FeatureManager design tree and select Edit Definition.
2.
In the Loft PropertyManager, select the new sketch in the Profiles box, and press Delete.
3.
Click OK
.
This removes the loft sketch from the loft section, and places it above the loft feature in the FeatureManager design tree. It does not remove the loft section. 4.
To permanently remove the loft section and the sketch from the model, do the following: •
Select the sketch from the FeatureManager design tree.
•
Press Delete.
Example of Loft Add Sections
Add a loft section
Position a loft section
Modify a loft section
Finish a loft section
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Loft Synchronization This capability allows you to modify the synchronization between loft profiles. You adjust the synchronization by changing the alignment between the profiles. To adjust the alignment, you manipulate the handles which appear in the graphics area as part of the connector. The connector is the poly line connecting corresponding points in both directions. Loft synchronization is available with new or legacy models. The type of control you can apply to connectors depends on: •
Selection sequence. Whether it is the first connector you modify, or whether you modify connectors added to the profile.
•
Type of profile. Connectors in smooth contour profiles react differently than connectors on profiles with non-tangent edges.
•
Guide curves. With guide curves and closed contour profiles, the guide curve defines the start point for the profiles.
Connector control is either global or local: •
Global twist control. The first connector on a profile with non-tangent edges moves from vertex to vertex along an edge. When you select a handle, it moves the connector to the next vertex.
•
Local twist control. When you add connectors to profiles with vertices, those connectors have local twist control. Local twist control means that you can select the handle and drag it along the profile to modify the synchronization between the profiles.
To control connectors using global twist control:
1.
Click a handle
on one of the profiles.
The handle changes color
.
Regardless of the profile you select, the behavior is identical. However, the shape of the loft varies accordingly. 2.
Start to drag towards the vertex on which you want to relocate the connector. The connector moves to the next vertex along the edge you specified. The loft preview updates with the new synchronization.
To add a connector:
1.
Select and edge.
2.
Right-click and chose Add Connector. Once you add connectors to profiles, you can reposition each of these connectors. The number of connectors you can add is based on the number of vertices in the profile.
Once you add new connectors to profiles with vertices, or with smooth contour profiles, you can drag the handles to reposition the connector.
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To control connectors using local twist control:
1.
Click a handle
on one of the profiles.
The handle changes color
.
2.
Drag the connector along the edge to the location you want.
3.
Release the handle. The loft preview updates with the new synchronization.
To move additional connectors:
1.
Select a handle on the new connector.
2.
Drag the connector along the edge in between the vertices.
If you have coincident vertices, you need to select the corresponding vertex to move the initial handle. To move connectors with coincident vertices:
Press Shift and select the handle to twist the corresponding connector. You can also right-click to manipulate connectors using the following techniques: •
Show All Connectors.
•
Reset Connectors. Removes all changes implemented by moving connectors.
•
Hide Connector. Select a handle to remove a connector from the profiles, without deleting it.
•
Hide All Connectors. Hides all connectors, but does not delete them.
Show All Connectors
Hide All Connectors
Hide Connector
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Example of Loft Synchronization Handles
Loft synchronization handles: The Connector includes two handles linked by poly line.
Patterns and Mirroring Pattern and Mirror Overview Pattern repeats the selected features in an array based on a seed feature. You can create a linear pattern, a circular pattern, a curve driven pattern, or use sketch points or table coordinates to create the pattern. Mirror copies the selected features or all features, mirroring them about the selected plane or face. With multibody parts, you can use the pattern or the mirror feature to pattern or mirror multiple bodies within the same document.
Mirror multibody parts about a plane
Linear pattern in two directions with multibody parts
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•
For a Linear Pattern, select the features, then specify the direction, the linear spacing, and the total number of instances.
•
For a Circular Pattern, select the features and an edge or axis as the center of rotation, then specify: The total number of instances and the angular spacing between instances. – or – The total number of instances and the total angle in which to create the pattern.
•
For a Curve Driven Pattern, select the features and an edge or sketch segment on which to pattern the feature. Then you can specify the type of curve, the curve method, and the alignment method.
•
For a Sketch Pattern, select where to populate a seed feature by sketching points on model face.
•
For a Table Pattern, add or retrieve previously created X-Y coordinates to populate a seed feature on the face of the model.
•
For a Mirror Feature, select the features to copy and a plane about which to mirror them. If you select a planar face on the model, you mirror the entire model about the selected face.
You can also create patterns of patterns, and mirrored copies of patterns, as well as control and modify patterns. For information about using a pattern of components in an assembly, see adding a component pattern.
Patterns of Patterns With multibody parts, you can create a pattern that includes some or all of the multibody parts that you used to create the original multibody part pattern. You can use any of the patterns such as linear, circular, sketch driven, and so on. You have the same options with patterns of patterns in the multibody part environment as you have in the single body environment. For example, you can use more than one direction, skip instances, and so on.
Pattern from existing linear pattern. Some bodies and a single direction selected.
Pattern from existing linear pattern. Some bodies, single direction, and instance to skip selected.
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To create a pattern of patterns:
1.
Click Mirror on the Features toolbar, or click Insert, Pattern/Mirror. Then select either linear, circular, or curve driven pattern. You can also use a pattern you created using X-Y coordinates (table pattern) or sketch points.
2.
Do one of the following:
3.
•
For a single body pattern, select the pattern feature in the FeatureManager design tree, or select a face on a pattern instance in the model.
•
For a multibody part pattern, under Bodies to Pattern , select the individual instances from the existing pattern that you want to include in the new pattern.
Proceed as described in Linear Pattern, Circular Pattern, or curve driven pattern.
Curve Driven Pattern Overview The Curve Driven Pattern tool on the Features toolbar allows you to create patterns along a planar curve. To define the pattern, you can use any sketch segment, or the edge of a face (solid or surface), that lies along the plane. Like other pattern types, such as linear or circular, you can skip pattern instances, and pattern in one or two directions. Elements specific to curve driven patterns include the following: •
Type of curve. The type of curve you use to create your pattern determines how you specify the number of instances to pattern for both directions. You can base your pattern on an open curve or a closed curve (such as a circle). o
o
o
Direction 1. You can equally space the pattern instances by applying the Equal spacing option. Alternatively, you can specify a distance along the curve between each pattern instance. The distance between the curve or sketch segment and the Feature to Pattern is measured normal to the curve. Direction 2. For Direction 2, you can also apply the Equal spacing option or specify step distances. If you use a closed curve, you can create patterns of concentric rings or rows of identically patterned features. Implicit Direction 2. If you select the Direction 2 check box without specifying a sketch element or edge, an implicit pattern is created. The implicit Direction 2 is based on what you specified for Direction 1.
•
Curve method. You can define the direction of the pattern by transforming how you use the reference curve (an edge, sketch, or curve) on which your pattern is based. The default method is Transform curve, in which the feature you pattern follows the shape of the reference curve. Using Offset curve, the feature you pattern is offset from the reference curve.
•
Alignment method. You can align the features to the original alignment of the seed feature. Alternatively, you can align the features tangent to the direction reference.
Curve Driven Pattern You can create patterns based on a curve. Although curve driven patterns have similarities to linear and circular patterns, they include unique options. Bodies to Pattern. For multibody parts, select a separate body to create a curve driven pattern. You can use all functions such as Direction 2 or Instances to Skip with Bodies to Pattern. Example
6-110
To create a curve driven pattern:
1.
Create a part that includes a feature you want to pattern along a curve.
2.
Click Curve Driven Pattern Pattern.
3.
Under Direction 1, do the following: •
on the Features toolbar, or Insert, Pattern/Mirror, Curve Driven
In the graphics area, click a curve, edge, or a sketch entity, or select a sketch from the FeatureManager to use as the pattern. If necessary, click Reverse Direction to change the direction of the pattern. The examples below use the upper edge of the model as Direction 1.
•
Specify the Number of Instances
•
Specify the Spacing
.
between pattern instances.
- or Select the Equal spacing check box. With equal spacing, the separation between each pattern instance depends on the the curve you select as the pattern, and the Curve method.
Equal spacing check box cleared
Equal spacing check box selected
•
Under Curve method, click either Transform curve or Offset curve.
•
Under Alignment method, click either Tangent to curve or Align to seed.
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Curve: Transform curve Alignment: Align to seed
Curve: Offset curve Alignment: Align to seed
Curve: Offset curve Alignment: Tangent to curve
Curve: Transform curve Alignment: Tangent to curve
4.
If you want to skip pattern instances, click Instances to Skip, and in the graphics area, select each of the pattern instances to skip. The pointer changes to when you mouse over each pattern instance. Click to select a pattern instance. The coordinates of the pattern instance appear. To restore a pattern instance, click the instance again, or delete the pattern instance from the Instances to Skip box. If you want to pattern only the geometry (faces and edges) of the features, rather than patterning and solving each instance of the feature, under Options, click to clear Geometry Pattern. NOTE: In some cases, the geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.
5.
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
NOTE: If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern , select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself. NOTE: When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
•
6.
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To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
Click OK
to create the curve driven pattern.
, select the the body to
To create a curve pattern in two directions: Example
1.
Follow steps 1-5 above to create a linear pattern in Direction 1. NOTE: You can select the Features to Pattern, Faces to Pattern, or Bodies to Pattern, and the Options before or after you select Direction 2.
2.
Under Direction 2, do the following: •
In the graphics area, click a curve or an edge to use as the pattern direction. In the example below, the right edge is selected. If necessary, click Reverse Direction pattern.
to change the direction of the
•
Set the Spacing
between pattern instances.
•
Set the Number of Instances
•
Select the Pattern seed only check box to replicate only the seed pattern. Selecting the Pattern seed only check box, creates a curve pattern under Direction 2, without replicating the curve pattern created under Direction 1.
.
TIP: The Pattern seed only option is especially useful when creating patterns in two opposite directions. Use Pattern seed only to prevent duplicate copies of the feature in the same location. 3.
4.
If you want to include specific pattern instances to skip, do the following: •
Click Instances to Skip
•
In the graphics area, select each pattern instance you want to skip. The pattern instances along with their coordinates are listed in the Instances to Skip box.
Click OK
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.
.
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Chapter 6 Features
Example of Multibody Part with Curve Driven Patterns
Multibody part with Body to Pattern
Curve driven pattern applied
Example of Curve Pattern in Two Directions
Pattern seed only
Pattern all instances
Linear Pattern Creates multiple instances of selected features along one or two linear paths. You can specify the following with linear patterns: •
Bodies to Pattern. For multibody parts, select a separate body to create a linear pattern. You can use all functions such as Direction 2 or Instances to Skip with Bodies to Pattern. Example
•
Direction of the pattern.
•
Number of pattern instances in each direction.
•
Distance between pattern instances.
•
Pattern instances to skip.
•
Pattern only the seed feature. If you modify the original feature (seed feature), all instances in the pattern are updated to reflect the changes.
•
Faces to Pattern. You can select the faces that make up a feature to create the pattern. This is useful with models that import only the faces that make up the feature, and not the feature itself. When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
•
Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
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To create a linear pattern in one direction: Example
1.
Create a base part and on the base part, create one or more cut, hole, or boss features that you want to repeat.
2.
Click Linear Pattern
3.
Under Direction 1, do the following:
4.
on the Features toolbar or click Insert, Pattern/Mirror, Linear Pattern.
•
Click a model edge or a dimension to indicate the first direction for the pattern. The name of the edge or dimension appears in the Direction 1 box.
•
Click Reverse Direction
•
Set the Spacing
•
Set the Number of Instances
if the arrow on the model points in the wrong direction.
between pattern instances. .
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern select all the faces in the graphics area.
•
To create a feature pattern on multibody parts:
• 5.
6.
,
a.
Under Features to Pattern design tree.
, select the feature to pattern from the FeatureManager
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
, select the body to
If you want to include specific pattern instances to skip, do the following: Example •
Click Instances to Skip
.
•
In the graphics area, select each pattern instance you want to skip. The pattern instances along with their coordinates are listed in the Instances to Skip box.
•
To restore pattern instances, select the pattern instances again, or select the coordinates in the Instances to Skip box and press Delete.
Under Options, do the following: •
Click Vary sketch if you want the pattern to change as it is repeated. Click Geometry Pattern if you want to pattern only the geometry (faces and edges) of the features, rather than solving each instance of the feature. In some cases, the geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.
7.
Click OK
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to create a linear pattern in Direction 1.
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To create a linear pattern in two directions: Example
1.
Follow steps 1-6 above to create a linear pattern in Direction 1. NOTE: You can select the Features to Pattern and the Options before or after you select Direction 2.
2.
Under Direction 2, do the following: •
Click a model edge or a dimension to indicate the second direction for the pattern. The name of the edge or dimension appears in the Pattern Direction box.
•
Click Reverse Direction
•
Set the Spacing
•
Set the Number of Instances
•
Select the Pattern seed only check box to replicate only the seed pattern. Selecting the Pattern seed only check box, creates a linear pattern under Direction 2, without replicating the linear pattern created under Direction 1.
if the arrow on the model points in the wrong direction.
between pattern instances. .
The Pattern seed only option is especially useful when creating patterns in two opposite directions. Use Pattern seed only, to prevent duplicate copies of the feature in the same location. • 3.
4.
• •
•
To create a feature pattern on multibody parts, follow the same steps from the procedure above.
If you want to include specific pattern instances to skip, do the following: •
Click Instances to Skip
•
In the graphics area, select each pattern instance you want to skip. The pattern instances along with their coordinates are listed in the Instances to Skip box.
Click OK
.
.
The following applies to linear patterns: When you create a pattern using a Shape feature, all pattern instances must be on the same face. Pattern instances inherit the feature color of the original feature as long as: o the pattern is based on one feature. o the color of the pattern or any faces on any pattern instances has not been changed. The feature colors are not inherited if you pattern or mirror multibody parts.
Example of Linear Patterns Single Direction
Linear pattern Direction 1 preview
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Linear pattern Direction 1 applied
Example of Linear Pattern Instances to Skip
Instances to Skip selected
Instances to Skip restored
Example of Linear Patterns Two Directions
Linear pattern both directions preview
Linear pattern both directions applied
Example of Linear Pattern Seed Feature
Linear pattern Pattern seed only not applied
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Linear pattern Pattern seed only applied
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Example of Multibody Part with Linear Patterns
Multibody part with Body to Pattern
Linear pattern applied
Example of Feature Scope Linear Pattern
Extrude and dome features applied to selected body
Extrude and dome feature applied to all bodies
Example of Boundaries and Faces to Pattern
Boundary causes pattern to fail
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Pattern suceeds without boundary
Circular Pattern Creates multiple instances of one or more features which you can space uniformly around an axis. Circular pattern includes the following: •
Bodies to Pattern. For multibody parts, select a separate body to create a circular pattern. You can use all functions such as Instances to Skip with Bodies to Pattern. Example
•
Seed feature. Modify the original feature (seed feature), and all instances in the pattern are updated to reflect the change.
•
Select pattern instances to skip as you create the circular pattern.
•
Faces to Pattern. Select the faces that make up a feature to create the pattern. This is useful with models that import only the faces that make up the feature, and not the feature itself. When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
•
Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
To create a circular pattern:
1.
Create one or more features to replicate.
2.
Create an axis around which to pattern the features. For information about how to create an axis, see Reference Axis.
3.
Click Circular Pattern
4.
Under Parameters, do the following:
on the Features toolbar, or Insert, Pattern/Mirror, Circular Pattern.
•
In the graphics area, select an axis, model edge or an angular dimension as the Pattern Axis.
•
If necessary click Reverse Direction
•
Specify the Number of instances
•
Specify the Angle
to change the direction of the circular pattern. .
between each instance.
- or Select the Equal spacing check box. With equal spacing, the Total Angle defaults to 360°. You can change the Angle the graphics area.
in which to create the pattern, using the PropertyManager or the callout in
If you change Number of instances or the Angle using the PropertyManager or the callout box, a preview of the resulting pattern is automatically displayed in the graphics area.
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5.
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern select all the faces in the graphics area.
•
To create a feature pattern on multibody parts:
• 6.
,
a.
Under Features to Pattern design tree.
, select the feature to pattern from the FeatureManager
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
, select the body to
If you want to skip circular pattern instances, click Instances to Skip, and in the graphics area, select each of the pattern instances to skip. The pointer changes to when you mouse over each pattern instance. Click to select a pattern instance. The coordinates of the pattern instance appear. To restore a pattern instance, click the instance again. If you want to pattern only the geometry (faces and edges) of the features, rather than patterning and solving each instance of the feature, under Options, click to clear Geometry Pattern. In some cases, the geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part.
7.
Click OK
.
When you create a pattern using a Shape feature, all pattern instances must be on the same face. Pattern instances inherit the feature color of the original feature as long as: • the pattern is based on one feature. • the color of the pattern or any faces on any pattern instances has not been changed. The feature colors are not inherited if you pattern or mirror multibody parts.
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Example of Multibody Part with Circular Patterns
Multibody part with Body to Pattern
Circular pattern applied
Example of Feature Scope Circular Pattern
Cut extrude feature applied to all multibody parts.
Cut extrude feature using circular pattern applied to single body
Cut extrude feature using circular pattern applied to all bodies
Sketch Driven Patterns Using sketch points within a sketch, you can specify a feature pattern. The seed feature propagates throughout the pattern to each point in the sketch. You can use sketch-driven patterns for holes or other feature instances. Bodies to Pattern. For multibody parts, select a separate body to create a sketch driven pattern. Example To build a sketch-driven pattern:
1.
Open a sketch on the face of a part.
2.
If necessary, create a seed feature on the model.
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3.
Click Point or Tools, Sketch Entity, Point and add multiple sketch points to represent the pattern you want to create, based on the seed feature.
4.
Click Sketch Driven Pattern Pattern.
5.
Under Selections, do the following:
on the Features toolbar, or click Insert, Pattern/Mirror, Sketch Driven
•
If necessary, use the flyout FeatureManager design tree to select a Reference Sketch the pattern.
to use as
•
Click either Centroid to use the centroid of the seed feature, or Selected point to use another point as the reference point.
•
If you chose Selected point as the reference point, select a Reference Vertex area.
in the graphics
NOTE: You can use the centroid of the seed feature, the sketch origin, a vertex, or another sketch point as a reference point in a sketch-driven pattern. 6.
Do one of the following: •
To create the pattern based on the feature, under Features to Pattern graphics area.
, select the feature in the
NOTE: If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features. •
To create the pattern based on the faces that make up the feature, under Faces to Pattern , select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself. NOTE: When using Faces to Pattern, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
• 7.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
Under Options, select the Geometry pattern check box (see Geometry Pattern). NOTE: The Geometry pattern is not available with Bodies to Pattern.
8.
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Click OK
to create the sketch pattern.
, select the the body to
The sketch-driven pattern is displayed.
Sketch pattern with Centroid as the reference point
Sketch pattern the Selected point as the reference point
Example of Multibody Part with Sketch Driven Patterns
Multibody part with Body to Pattern and sketch points
Sketch driven pattern applied
Reference Points for Sketch Driven Patterns Depending on what you select as your Reference point, the position of the features you propagate will change.
Origin used as the Reference point
Selected Vertex used as the Reference point
NOTE: You can also alter the relative position of the features you propagate when using a table driven pattern.
Table Driven Patterns Using X-Y coordinates, you can specify a feature pattern. Hole patterns using X-Y coordinates are a common application for table driven patterns. However, you can use other seed features, such as a boss, with table driven patterns. You can also save and load the X-Y coordinates of a feature pattern, and apply them to a new part. Bodies to copy. For multibody parts, select a separate body to create a table driven pattern. Example
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To build a table-driven pattern:
1.
Open a sketch on the face of a part or on a plane, and add a point to identify the reference point for the table pattern.
2.
Close the sketch.
3.
Create a coordinate system (see Coordinate System) based on the point in the previous sketch.
4.
If necessary, create a seed feature.
5.
Click Table Driven Pattern Pattern.
6.
In the Reference point box, select Centroid to use the centroid of the seed feature or Selected point, to use another point as the Reference point.
on the Features toolbar, or click Insert, Pattern/Mirror, Table Driven
NOTE: You can use the centroid of the seed feature, the sketch origin, a vertex, or another sketch point as a reference point in table driven pattern. See Centroid for more information on how the system determines the centroid of a seed feature. 7.
In the Coordinate system box, select the Coordinate System you created from the FeatureManager design tree.
8.
Do one of the following: •
To create the pattern based on the feature, under Features to copy, select the feature in the graphics area. NOTE: If the feature to pattern includes fillets or other additions, use the flyout FeatureManager design tree to select these features.
•
To create the pattern based on the faces that make up the feature, under Faces to copy, select all the faces in the graphics area. This is useful with models that import only the faces that make up the feature, and not the feature itself. NOTE: When using Faces to Copy, the pattern must remain within the same face or boundary. It cannot cross boundaries. For example, a cut across the entire face or different levels (such as a raised edge) would create a boundary and separate faces, preventing the pattern from propagating.
• 9.
To create a pattern based on multibody parts, under Bodies to Pattern pattern in the graphics area.
, select the the body to
Select the Geometry pattern check box (see Geometry Pattern). NOTE: The Geometry pattern is not available with Bodies to Pattern.
10. Double-click the area under Point 0 to enter the X-Y coordinates for each instance of the table pattern. Note that the X-Y coordinates of your seed feature are displayed for Point 0. NOTE: You can use positive or negative coordinates. To enter a negative coordinate, precede the value with a minus (-). 11. Click OK to create the table pattern. The table driven pattern is displayed.
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Example of Multibody Part with Table Driven Patterns
Save Table Pattern Coordinates You can also save and load (see Load Table Pattern Coordinates) the X-Y coordinates of a feature pattern, and apply them to a new part. To save a table-driven pattern instance:
1.
Create a part with a seed feature and create a table pattern.
2.
In the Table Driven Pattern dialog box, click Save. (If you use an existing set of X-Y coordinates that you modified, use Save As to rename the new pattern).
3.
Browse to the folder where you want to save the Table Pattern, and enter a name. The .sldptab extension is added automatically.
4.
Click Save to save the Table Pattern (.sldptab), and OK in the Table Driven Pattern dialog box to save the part.
Load Table Pattern Coordinates You can load the X-Y coordinates of a feature pattern that you saved (see Save Table Pattern Coordinates), and apply them to a new part. To load a table-driven pattern instance:
1.
With a part open, click Table Driven Pattern Table Driven Pattern.
on the Features toolbar, or click Insert, Pattern/Mirror,
2.
Click Browse to locate the .sldptab file, then click Open. The file name appears in the Read a file from box, along with the X-Y coordinates.
3.
Enter the appropriate Reference point and Coordinate system.
4.
Click OK to apply the Table Pattern to the part.
Mirror Pattern You can select one or more features, the faces that comprise a feature, or with multibody parts, select a body to create a mirror pattern. Multibody parts. Apply features to one or more by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
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To create a mirrored copy of a pattern:
1.
Click Mirror
on the Features toolbar or click Insert, Pattern/Mirror, Mirror.
2.
Under Mirror Face/Plane
, select a face or a plane in the graphics area.
You can select features or the faces that comprise features. •
To use features: Under Features to Mirror flyout FeatureManager design tree.
, click one or more features in the model or use the
•
To use faces: Under Faces to Mirror , in the graphics area click the faces that comprise the feature you want to mirror. Faces to Mirror is useful with imported parts where the import process included the faces of the feature, but not the feature itself.
•
To mirror a feature pattern on multibody parts: a.
Under Features to Pattern design tree.
, select the feature to pattern from the FeatureManager
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
•
To use bodies: Under Bodies to Mirror , in the graphics area select the body you want to mirror. If you select Bodies to Mirror, the following Options appear:
•
Merge solids. When you select a face on a solid part, and clear the Merge solids check box, you can create a mirrored body that is attached to the original body, but is a separate entity. If you select Merge solid, the original part and the mirrored part become a single entity.
•
Knit surfaces. If you select to mirror a surface by appending the mirror face to the original face without intersecting it, you can select Knit surfaces to knit the surfaces together. A preview of the mirrored pattern appears.
3.
Click Geometry pattern if you want to make an exact, geometric copy of the faces and edges of the original feature. Under certain conditions, when using Faces to Mirror, you may not be able to use the Geometry Pattern option. The Geometry Pattern is not available with Bodies to Mirror. To mirror a feature pattern on multibody parts, you must select Geometry Pattern.
4.
Click OK
.
Control and Modify Patterns You can control and modify feature patterns in the following ways: •
Use the Geometry pattern option to make exact patterned and mirrored copies of features, and to improve system performance when using patterned and mirrored features.
•
Use the Vary sketch option to adjust the profile of the patterned feature based on its dimensions and relations to other features.
•
Use a mathematical Equation to calculate values that define the pattern.
•
Use edit Seed Feature to modify the original feature of a pattern or mirrored feature based on a single feature.
•
Use Delete Pattern Instances to remove selected instances in a pattern.
•
Modify the Curve method and the Alignment method when applying curve-driven patterns.
Pattern instances inherit the feature color of the original feature as long as:
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•
the pattern is based on one feature.
•
the color of the pattern or any faces on any pattern instances has not been changed.
Geometry Pattern The Geometry Pattern option speeds up the creation and rebuilding of a pattern. Individual instances of the feature being copied are not solved; end conditions and calculations are ignored. Each instance is an exact copy of the faces and edges of the original feature. By default, the Geometry Pattern option is not selected except when you create a pattern using a Shape or Dome feature. In this example, the cut is extruded with the Offset from Surface end condition, and the bottom face selected.
With Geometry Pattern not selected, each instance is offset from the selected surface by the same amount (the end condition is solved).
With Geometry Pattern selected, each instance is an exact copy of the original feature (the end condition is ignored).
NOTE: You cannot create geometry patterns of features that have faces merged with the rest of the part.
Geometry Pattern must be cleared to create this pattern.
The Geometry Pattern option is available when creating any type of pattern: •
Circular Pattern
•
Linear Pattern
•
Curve-Driven Pattern
•
Table Pattern
•
Sketch Pattern
•
Mirror Feature
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Vary Sketch Use the Vary Sketch option if you want the pattern to change its dimensions as it is repeated. For example, you may want to maintain a specific distance between the edges of the base part and the patterned features. In this example, the first feature (the hole feature) is patterned three times.
When Vary Sketch is not checked, the pattern remains the same regardless of the defining geometry.
When Vary Sketch is checked, the pattern maintains its relation to the sloping edge, based on the dimensions and constraints of the first instance of the pattern.
To create a variable pattern:
1.
2.
Create a sketch for the first feature in the pattern, observing the following recommendations: •
The feature sketch must be constrained to the boundary that defines the variation of the pattern instances. For example, in the illustrated pattern, the angled top edge of the first feature is parallel and dimensioned to the angled edge on the base part.
•
The feature sketch should be fully defined.
Double-click one of the feature dimensions and click the arrows in the Modify box to change the dimension. This gives you a preview of the way this dimension will drive the feature when you create the pattern. Try a different dimension for a different result.
3.
When you are satisfied that the dimensions are correct and the pattern will repeat as you wish, click Insert, Cut, Extrude (or Insert, Boss, Extrude) to create the first feature.
4.
In the FeatureManager design tree, select the feature to repeat.
5.
From the Features toolbar, click Linear Pattern
6.
Click the dimension that you want to use to drive the pattern. Notice the preview arrow.
7.
Click the Vary Sketch check box.
8.
Specify the values for the Spacing and Total Instances of the pattern.
9.
Click OK to create the pattern.
, or click Insert, Pattern/Mirror, Linear Pattern.
Pattern Deletion To delete pattern instances:
1.
Select a face of the pattern instance that you want to delete. Edges cannot be selected because they are shared by more than one feature.
2.
Press the Delete key.
3.
In the Pattern Deletion dialog box, select one of the following:
4.
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•
Delete Pattern Instances. Only the selected instances are deleted. The instance locations are displayed in the Instances Deleted box.
•
Delete Pattern Feature. The complete pattern is deleted, not including the initial feature.
Click OK to delete, or click Cancel to exit the dialog box.
To restore deleted pattern instances:
1.
Right-click the pattern feature, and select Edit Definition.
2.
Select the coordinates of the deleted instance in the Instances to Skip box, and press Delete to restore that instance.
3.
Click OK
.
To delete a table driven pattern instance:
1.
Right-click the pattern in the FeatureManager design tree and select Edit Definition.
2.
In the Table Driven Pattern dialog box, click the number of the pattern you want to delete to highlight the X-Y coordinates.
3.
Press Delete.
4.
Click OK.
To delete a sketch driven pattern instance:
1.
Right click the sketch used by the sketch-driven pattern in the FeatureManager design tree, and select Edit Sketch.
2.
Select the sketch points you want to delete and press Delete.
3.
Click Rebuild
to close the sketch and update the pattern.
To delete a feature from a multi-feature pattern:
1.
Select the feature in the FeatureManager design tree that you want to delete.
2.
Press Delete.
3.
In the Confirm Delete dialog box, select the Also delete absorbed features check box, if available.
4.
Click Yes to delete the feature from the pattern and to close the dialog box. The feature is deleted from the pattern.
Seed Feature The original feature for any type of pattern (linear, circular, sketch driven and so on) or mirrored pattern, is called the seed feature. You can edit this feature. To edit the definition of the original feature:
1.
Right-click a pattern or mirrored instance, and select Edit Seed Feature.
2.
Change the desired parameters.
3.
Click OK.
Mirror Feature Creates a copy of a feature, (or multiple features), mirrored about a face or a plane. You can select the feature or you can select the faces that comprise the feature. •
Bodies to Mirror. Select a body in a single model or multibody part to create a mirror entity.
•
Multibody parts. Apply features to one or more multibody parts by selecting Geometry Pattern and using Feature Scope to choose which bodies should include the feature. You must create the model to which you want to add the features for multibody parts prior to adding those features.
Example If you modify the original feature (seed feature), the mirrored copy is updated to reflect the changes.
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To mirror a feature:
1.
Click Mirror
on the Features toolbar or Insert, Pattern/Mirror, Mirror.
2.
Under Mirror Face/Plane
, select a face or a plane in the graphics area.
You can select features, the faces that comprise features, or a body with multibody parts. •
To use features: Under Features to Mirror flyout in the FeatureManager design tree.
, click one or more features in the model or use the
•
To mirror the entire model: Under Bodies to Mirror
, select a model in the graphics area.
The mirrored model attaches to the face you select. •
To use faces: Under Faces to Mirror feature you want to mirror.
•
To mirror a feature pattern on multibody parts:
• 3.
, in the graphics area click the faces that comprise the
a.
Under Features to Pattern design tree.
b.
Under Options, select Geometry pattern.
c.
Under Feature Scope, select an option based on the bodies to which you want to apply the feature.
To use bodies: Under Bodies to Mirror mirror.
, select the feature to pattern from the FeatureManager
, in the graphics area select the body you want to
If you select Bodies to Mirror, the following Options appear: •
Merge solids. When you select a face on a solid part, and clear the Merge solids check box, you can create a mirrored body that is attached to the original body, but is a separate entity. If you select Merge solid, the original part and the mirrored part become a single entity.
•
Knit surfaces. If you select to mirror a surface by attaching the mirror face to the original face without intersections or gaps between the surfaces, you can select Knit surfaces to knit the two surfaces together.
Example 4.
If you want to mirror only the geometry (faces and edges) of the features, rather than solving the whole feature, select Geometry Pattern. The geometry pattern option speeds up the creation and rebuilding of the pattern. However, you cannot create geometry patterns of features that have faces merged with the rest of the part. To mirror a feature pattern on multibody parts, you must select Geometry Pattern. The geometry pattern is only available with Features to Mirror and Faces to Mirror.
5.
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Click OK
.
Example of Feature Scope Mirror Pattern
Plane used to mirror pattern
Pattern mirrored on body
Example of Multibody Part with Mirror
Select the body to mirror
Body mirrorred
Example of Multibody Surface with Knit Surface
Surface created on Front plane
Surface mirrored using Front plane. Knit surface option is available.
Surface mirrored using Top plane. Knit surface option is not available.
Surface mirrored using Right plane. Knit surface option is not available.
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Chapter 6 Features
Revolves Revolved Boss/Base Revolve creates a base or boss by revolving a sketch around a centerline. The default angle is 360°. You can also create revolved cut or revolved surface. With the Selected Contours pointer, you can choose different sketches from among intersecting or non-intersecting sketches to create the revolve. Example To create a revolve feature, use the following guidelines:
•
The sketch for a solid revolved feature can contain multiple intersecting profiles. With the Selected
•
Contours pointer, you can select one or more intersecting profiles. The sketch for a thin or surface revolved feature can contain multiple open or closed intersecting profiles.
•
Profiles cannot cross the centerline. If the sketch contains more than one centerline, select the centerline you want to use as the axis of revolution.
•
When you dimension a revolve feature inside the centerline, you produce a radius dimension for the revolve feature. If you dimension across the centerline, you produce a diameter dimension for the revolve feature.
To create a revolve feature, use one of the following tools:
•
Revolved Boss/Base
•
Revolved Cut
•
Revolved Surface
on the Features toolbar, or Insert, Boss/Base, Revolve
on the Features toolbar, or Insert, Cut, Revolve on the Surfaces toolbar, or Insert, Surface, Revolve
To define a revolve feature, specify the following parameters:
•
Revolve Type (One-Direction, Mid-Plane, or Two-Direction)
•
Angle
•
Reverse Direction
•
Thin Feature
•
Selected Contours
Revolve Features Revolve creates a feature that adds or removes material by revolving one or more profiles around a centerline. The feature can be either a solid, a thin feature, or a surface. With the Selected Contours pointer, you can choose different sketches from among intersecting or non-intersecting sketches to create the revolve. Example
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To create a revolved feature:
1.
Create a sketch containing one or more profiles and a centerline.
Sketching Tips for Revolves
•
The sketch for a solid revolved feature can contain multiple intersecting profiles. With the Selected Contours
pointer, you can select to revolve one or more intersecting profiles.
•
The sketch for a thin or surface revolved feature can contain multiple open or closed intersecting profiles.
•
Profiles cannot cross the centerline. If the sketch contains more than one centerline, select the centerline you want to use as the axis of the revolution.
•
When you dimension a revolve feature inside the centerline, you produce a radius dimension for the revolve feature. If you dimension across the centerline, you produce a diameter dimension for the revolve feature.
2.
Click one of the following:
3.
•
Revolved Boss/Base Revolve
•
Revolved Cut
•
Revolved Surface
in the Features toolbar, or Insert, Base, Revolve, or Insert, Boss,
in the Features toolbar, or Insert, Cut, Revolve in the Surfaces toolbar, Insert, Surface, Revolve
Under Revolve Parameters, do the following: •
Select a Revolve Type. Click Reverse Direction
•
The angle defaults to 360°. If necessary, change the Angle area.
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, if necessary , or drag the handles in the graphics
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4.
5.
If creating a Thin Feature, click the Thin Feature check box, and do the following: •
Select a Type. If necessary, click Reverse Direction
•
Click the Direction 1 Thickness
.
and enter a value. If necessary, click Direction 2 Thickness
and enter a value. If creating a revolve with multiple contours, click Selected Contours, and do the following: a.
Hover over the region with the pointer , and select the contours you want to revolve, You can select any combination of regions to create single or multibody parts. The selected region becomes red.
b.
Click to create a preview of the revolve. The selected region becomes yellow, and the region of the sketch appears in the Selected Contours box.
Select region 3.
Click OK
Preview contour
Create revolve
Revolve thin feature
Revolve from multiple contours
.
Revolve solid
Example of Revolve with Multiple Contours
Select top region (contour)
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Select top and mid regions (contours)
Select mid region (contour)
Select bottom region (contour)
Select bottom and mid regions (contours)
Select all regions (contours)
Ribs Rib Overview Rib is a special type of extruded feature created from an open sketched contour. It adds material of a specified thickness in a specified direction between the contour and an existing part. Elements that control the type of rib you create include: •
Specifying single open or closed sketch elements on a plane or a face
•
Selecting the type of the plane such as parallel
•
Changing the extrusion direction
•
Selecting either a linear or natural extension
•
Creating multiple open sketch elements on a plane
•
Using multiple drafts
•
Using the Detailed Preview PropertyManager with multibody parts to enhance detail and select entities to display
For additional information and examples of the rib feature, see the following topics: •
Creating a simple rib
•
Creating a rib using Normal to Sketch
•
Using multiple open sketch elements
•
Using the multiple drafts feature
•
Reversing the direction of the rib extrusion
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The examples below display some of the methods and results you can apply to create the rib feature.
Single open sketch on face. The arrow indicates the direction of the rib feature
Rib feature applied using Parallel
Rib feature applied using
Sketch on plane, parallel to the plane used for the Base-Extrude (15mm). The arrow indicates the direction of the rib feature.
Normal to Sketch Extrusion direction.
as the
Multiple open sketches on parallel plane, same distance as used for the Base-Extrude (30mm). The arrow indicates the direction of the rib feature.
to Sketch direction.
as the Extrusion
Sketch on parallel plane, same distance as used for the BaseExtrude (30mm). The arrow indicates the direction of the rib feature.
Rib feature applied using Parallel to Sketch direction.
Rib feature applied using Normal to Sketch direction.
as the Extrusion
as the Extrusion
Type: Natural Type: Linear
Example of Ribs with Open Sketches With an open sketch, you can create ribs in the following ways:
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•
Use one or multiple open sketches
•
Create sketches on intersecting, parallel, or other planes
•
Select Parallel to Sketch or Normal to Sketch model and the position of the bounding edges
as the Extrusion Direction, depending on your
Multiple open and closed contours sketched on a plane
Rib feature applied using Normal to Sketch
Single open contour sketch on a plane using
Single open contour sketch on a plane using
Parallel to Sketch Direction
Normal to Sketch Direction
as the Extrusion
as the Extrusion Direction
as the Extrusion
Single open contour sketch on a face. With an open contour sketch on a face, you can only use Parallel to Sketch
as the Extrusion Direction.
Using multiple open contour sketches on a plane, you can select only Normal to Sketch as the Extrusion Direction. However, you can select either of the following: •
Type: Natural
•
Type: Linear
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Example of Ribs and Direction of Extrusion
Flip material side Example of Rib Feature with Multiple Drafts To create a rib using multiple drafts, see rib feature.
Click Next Reference
Repeat and click Next Reference, until you have selected the contour you wish to use as the reference.
Apply a draft Angle and apply rib with multiple drafts.
Rib - Linear and Natural Type When you specify Normal to Sketch types.
under Parameters, you have the option to create Linear or Natural rib
You can use the Detailed Preview PropertyManager with multibody parts to enhance detail and select entities to display. To create a rib using Normal to Sketch:
1.
Create a plane on which to sketch. NOTE: In the example below, the base feature uses plane 2, and plane 4, which is Offset 10 mm from plane 2, is used to sketch the rib profile. You can also use other types of planes, such as Parallel Plane at Point, to achieve results.
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2.
Sketch a profile as a basis for the rib feature.
3.
Click Rib
on the Features toolbar, or click Insert, Features, Rib.
4.
Under Parameters, do the following. Select a Thickness from the following options: •
Create rib on the left of the sketch
•
Create rib on both sides of the sketch
•
Create rib on the right of the sketch
Enter a Rib Thickness
- adds material only to the left side of the sketch. - adds material equally to both sides of the sketch. - adds material only to the right side of sketch.
.
Select Normal to Sketch as the Extrusion direction, and choose either of the following: • Linear creates a rib that extends the sketch contours normal to the direction of the sketch until they meet a boundary. •
Natural creates a rib that extends the sketch contours in the same directions as the contour until they meet a boundary.
Linear
Natural
Select the Flip material side check box to change the direction of the extrusion. Click Draft On/Off 5.
Click OK
to add a draft, and enter the Draft Angle.
.
Rib Feature You can create a rib using either single or multiple open, or closed, sketches. Detailed Preview
is available from the Rib PropertyManager.
To create the rib:
1.
Using a plane that intersects the part, sketch the contour to use as the rib feature. NOTE: you can also do the following to create a rib feature: o
Use planes that are parallel or at an angle to existing planes
o
Sketch a single element, or multiple elements, using either closed or open contours
Sketch for rib feature created on an intersecting plane
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Rib applied selecting Parallel to sketch
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Sketch for rib using open sketch elements created on a parallel plane. With this type of sketch, you can either select: Normal to Sketch Parallel to Sketch
Rib using open sketch elements, selecting
Rib using open sketch elements, selecting
Normal to sketch
Parallel to sketch
2.
Click Rib
on the Features toolbar or click Insert, Features, Rib.
3.
Select a Thickness from the following choices: •
Create rib on the left of the sketch
•
Create rib on both sides of the sketch
•
Create rib on the right of the sketch
- adds material only to the left side of the sketch. - adds material equally to both sides of the sketch. - adds material only to the right side of sketch.
4.
Enter a Rib Thickness
5.
Select an Extrusion direction from the following choices: •
.
Parallel to Sketch
- creates the rib extrusion parallel to the sketch.
NOTE: If you select Parallel to Sketch as the Extrusion direction, you can select only Linear as an Extension Type.
6.
•
Normal to Sketch
•
With Normal to Sketch, select a Type, either Linear or Natural.
•
Select the Flip material side check box to change the direction of the extrusion.
Click Draft On/Off
- creates the rib extrusion normal to the sketch.
to add a draft, and enter the Draft Angle.
You can also create drafts using multiple drafts. 7.
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Click OK
.
Scaling You can scale a part or surface model about its centroid or about the model origin. The Scale feature scales only the geometry of the model, for use in data export, cavities, and so on. It does not scale dimensions, sketches, or reference geometry. With multibody parts, you can select to scale one or more models. A Scale feature is like any other feature in the FeatureManager design tree: it manipulates the geometry, but it does not change the definitions of features created before it was added. To temporarily restore the model to its unscaled size, you can roll back or suppress the Scale feature. You can select to scale a model using a uniform or non-uniform scaling by selecting X-Y-Z coordinate values. To scale a single solid or surface model:
1.
In a part document, click Scale
on the Features toolbar or click Insert, Features, Scale.
The Scale PropertyManager appears. 2.
From the Scale about list, select: Centroid, Coordinate System, or Origin.
3.
If you want uniform scaling, specify a scaling value in the Scale factor box.
4.
If you want non-uniform scaling, click to clear the Uniform scaling check box., and enter values for X, Y, and Z.
5.
Click OK
.
Solid model: uniform scaling
Solid model: non-uniform scaling
Surface: uniform scaling
Surface: non-uniform scaling
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To scale multibody parts or multiple surfaces:
1.
In a part document, click Scale
on the Features toolbar or click Insert, Features, Scale.
The Scale PropertyManager appears. 2.
Under Scale Parameters, select a solid or surface body in the graphics area.
3.
From the Scale about list, select: Centroid, Coordinate System, or Origin.
4.
If you want uniform scaling, specify a scaling value in the Scale factor box.
5.
If you want non-uniform scaling, clear the Uniform scaling check box and enter values for X, Y, and Z.
6.
Click OK
.
Multibody parts: uniform scaling
Multibody parts: non-uniform scaling
Shapes Shape Feature Creates a deformed surface on a model by expanding, constraining, and tightening the selected surface. A deformed surface is flexible, much like a membrane. It can be expanded, constrained, and tightened using the sliders on the Controls tab on the Shape Feature dialog box. To create a shape feature:
1.
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Sketch one or more entities with which to constrain the shape feature. You can create the constraining entities directly on the face or on a plane. Valid entities are as follows: •
Points (sketch points, endpoints, vertices, and so on)
•
Sketches
•
Edges
•
Curves
Example of Shape Constraints
Sketch points on face
Using Bend to change shape
Sketch rectangle on face
Using multiple controls to change shape
Sketch shape on separate plane
Using Resolution to change shape
2.
Click Shape
on the Features toolbar or click Insert, Features, Shape.
3.
Select a face on a model. (You can only select one face.)
4.
Click the Constrain to check box and select entities to constrain the shape.
5.
If desired, click to clear Maintain Boundary Tangents.
Maintain Boundary Tangents, selected
Maintain Boundary Tangents, cleared
6.
Click Preview. Rotate the part and examine the shape from different angles.
7.
Use the sliders on the Controls tab to adjust the shape.
8.
When you are satisfied with the shape, click OK. NOTE: If you constrain the shape using a vertex of a 3D sketch, you can use a feature handle to adjust the shape. See Move/Size Features with Feature Handles.
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Shape Feature Controls Tab The Shape Features Controls tab lets you adjust the shape of the deformed surface. After adjusting a slider, observe the preview. Experiment until you are satisfied with the results. Under Gains: •
Pressure. Deflates or inflates the shape.
•
Curve influence. Moves the shape away from or toward the constraining entities. The Curve influence control is grayed out if Constrain to is not selected on the Shape Feature tab.
Pressure and Curve Influence Sliders example. Under Characteristics: •
Stretch. Adjusts the degree of stretching.
•
Bend. Adjusts the degree of bending.
Stretch and Bend Sliders example. Under Advanced controls: •
Resolution. Adjusts the precision of the shape by changing how many points on the face are deformed. Higher Resolution often smooths the flat areas and sharpens the shape near the constraining entities. Lower Resolution provides better performance and a coarser shape; however, some details may be omitted.
Resolution Slider example. After making the first adjustment to the shape, the icon is displayed. Click adjustment. You can undo an unlimited number of adjustments.
to undo the previous
Pressure and Curve Influence Sliders The following illustrations show how you can get different results by adjusting the Pressure and Curve influence sliders. In each case, this same base feature and sketch are used.
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Pressure decreased
Pressure increased
Curve influence decreased
Curve influence increased
Stretch and Bend Sliders The following illustrations show how you can get different results by adjusting the Stretch and Bend sliders. Each illustration is derived from this same base feature, which was shaped by increasing Pressure on the front face.
Stretch decreased
Stretch increased
Bend decreased
Bend increased
Resolution Slider The following illustrations show how you can get different results by adjusting the Resolution slider.
Increase resolution
Shells Shell Features The shell tool hollows out the part, leaves open the faces you select, and creates thin-walled features on the remaining faces. If you do not select any face on the model, you can shell a solid part, creating a closed, hollow model. If you plan on adding fillets to the part, you should fillet the part before you shell it. If you have problems shelling a model, you can run the error diagnostics. To create a shell feature:
1.
Click Shell
on the Features toolbar or Insert, Features, Shell.
2.
To shell using uniform thickness, under Parameters, do the following: •
Enter the Thickness
•
Click on the Faces to remove one or more open faces.
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to control the thickness of the wall. , and select the faces from the graphics area to create a part with
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•
Select the Shell Outward check box if you want the shell feature to increase the outside dimensions of the part. NOTE: You also have the option to shell a model using multiple thicknesses.
3.
Click OK
.
Example of Shell Hollow Model
Shelled model with no faces removed
Shell with Multi-Thickness Faces To set a different shell thickness for each face:
1.
Click Shell
on the Features toolbar or click Insert, Features, Shell.
2.
Click the faces you want to remove in the graphics area. - or Click Multi-thickness Settings, and under Multi-thickness Faces remove in the graphics area. The faces are listed in the Multi-thickness Faces
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box.
, select the faces you want to
3.
Select Face <1> in the Multi-thickness Faces thickness(es)
4.
box, and enter a wall thickness in the Multi-
box.
Select each remaining Face <> in the the Multi-thickness Faces Multi-thickness (es)
box, and enter a wall thickness in the
box for that Face <>.
NOTE: You can add additional faces to the Multi-thickness Faces
box.
5.
Under Parameters, select the Shell outward check box if you want the shell thickness added to the outside.
6.
Click OK
.
Shell with variable thickness and face removed
Shell with variable thickness and model hollow (no faces removed)
Shell Feature Diagnostics The shell feature displays error messages and includes tools to help you identify why the shell feature failed. The diagnostic tool Error Diagnostics is available in the Shell PropertyManager. To run error diagnostics:
1.
Under Error Diagnostics: •
Select Entire body to diagnose all areas of the model - or -
• 2.
Select Failing faces to diagnose and identify the faces that failed to shell.
Click Check body/faces to run the diagnostic tool. The results display in the graphics area, using a callout to pinpoint the specific area on the model that needs correction.
For example, the shell feature can fail because the Thickness at a point is too large relative to one of the selected faces. A message that displays the minimum radius of curvature indicates that the shelling thickness is too large at that point. You can also select Display mesh or Display curvature. •
Display mesh shows a uv mesh. This mesh operates in the same manner as the Preview mesh option in Filled Surface.
•
Display curvature shows a curvature plot for the bodies.
Because problems related to surface gaps and curvature often relate to surface inconsistencies, you can click Go to offset surface. This opens the Offset Surface PropertyManager where the offset surfaces in the model are displayed. Return to Shell feature.
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Surfaces Surfaces Overview Surfaces are a type of geometry that can be used to create solid features. Surface tools are available on the Surfaces toolbar. You can create surfaces by these methods: •
Insert a planar surface from a sketch or from a set of closed edges that lie on a plane
•
Extrude, revolve, sweep, or loft from sketches
•
Offset from existing faces or surfaces
•
Import a file
•
Create mid-surfaces
You can modify surfaces in the following ways: •
Extend
•
Trim existing surfaces
•
Untrim surfaces
•
Fillet surfaces
•
Repair surfaces using Fill Surface
•
Move/Copy surfaces
•
Delete and patch a face
You can use surfaces in the following ways: •
Select surface edges and vertices to use as a sweep guide curve and path.
•
Create a solid or cut feature by thickening a surface.
•
Extrude a solid or cut feature with the end condition Up to Surface or Offset from Surface.
•
Create a solid feature by thickening surfaces that have been knit into a closed volume.
•
Replace a face with a surface
Surfaces Toolbar The Surfaces toolbar provides tools for creating and modifying surfaces. Extruded Surface Revolved Surface Swept Surface Lofted Surface Offset Surface Radiate Surface Knit Surface Planar Surface
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Extended Surface Trimmed Surface Filled Surface Mid-Surface Replace Face Delete Face Untrim Surface
Surface Bodies Surface body is a general term that describes connected zero-thickness geometries such as single surfaces, knit surfaces, trimmed and filleted surfaces, and so on. You can have multiple surface bodies in a single part. You can select a surface body from the graphics area using Filter Surface Bodies You can select all types of surfaces with Filter Surface Bodies. The cursor changes to
on the Selection Filter toolbar.
, indicating when the pointer is over a surface body. Surface bodies can include:
•
Single face surfaces
•
Multiple face surfaces
•
Knit surfaces
•
Filleted surfaces
•
Trimmed and extended surfaces
•
Imported surfaces
•
Planar surfaces and mid surfaces
•
Surfaces made by extrude, revolve, loft, sweep, offset, radiate, or fill
To select a single face in a complex surface body, use Filter Faces
on the Selection Filter toolbar.
Surface Features Planar Surface To create a bounded planar surface from a sketch:
1.
Create a non-intersecting, single contour, closed sketch.
2.
Click Planar Surface
on the Surfaces toolbar, or Insert, Surface, Planar.
The Planar Surface PropertyManager appears. 3.
Select the sketch in the FeatureManager design tree or in the graphics area. The sketch name appears under Bounding Entities
4.
Click OK
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To create a planar surface bounded by a set of closed edges in a part or assembly:
1.
Click Planar Surface
on the Surfaces toolbar, or Insert, Surface, Planar.
2.
Select a set of closed edges in a part or assembly. (All edges in the set must be on the same plane.)
The names of the edges appear under Bounding Entities 3.
Click OK
.
.
To edit the planar surface:
•
If the planar surface is created from a sketch, you can edit the sketch.
•
If the planar surface is created from a set of closed edges, right-click the surface and select Edit Definition.
Extruded Surface To extrude a surface:
1.
Sketch the profile of the surface.
2.
Click Extruded Surface
3.
Under Direction 1, do the following:
on the Surfaces toolbar or Insert, Surface, Extrude.
•
Select an End Condition.
•
If necessary, click Reverse Direction
•
If using Offset from surface, select a Face/Plane in the graphics area. Examine the preview. If the offset is in the wrong direction, click the Reverse offset check box.
•
Enter a Depth
to extrude the surface in the opposite direction.
.
Extruded surface using Mid Plane from sketched spline
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4.
If necessary, click Direction 2 and repeat the same process you followed under Direction 1.
5.
Click OK
.
Resulting extruded surface Revolved Surface Choose different sketches from intersecting or non-intersecting sketches to create the revolve with the Selected Contours pointer
.
Example To revolve a surface:
1.
Sketch a profile and a centerline around which to revolve the profile.
2.
Click Revolved Surface
3.
Under Revolve Parameters, do the following:
4.
5.
on the Surfaces toolbar or click Insert, Surface, Revolve.
•
Select a Revolve type: One-Direction, Two-Direction, or Mid-Plane.
•
Click Reverse Direction
•
Enter an Angle
to change the direction of the revolve.
.
When creating a revolve with multiple contours do the following: a.
Hover over the region with the pointer , and select the contours you want to revolve, You can select any combination of regions to create single or multiple revolved surfaces. The selected region becomes red.
b.
As you drag the pointer over the contours, the color of the contours changes to pink, then yellow when you select them. The region of the sketch appears in the Selected Contours box.
Click OK
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Example of Surface Revolves with Selected Contours
Non-intersecting profiles
Selected Contours
Intersecting profiles
Selected Contours
Swept Surface To sweep a surface:
1.
Create planes as needed for sketching the sweep profile, sweep path, and the guide curves (if any are needed).
2.
Sketch the sweep profile and path on the planes that you created. NOTE: You can also sketch the sweep path on a model face or use a model edge for the path.
Profile sketch
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Profile sketch with path sketch
Preview of sweep
3.
If you are using one or more guide curves, create coincident or pierce relations between the guide curves and the profile.
4.
Click Swept Surface
5.
Under Profile and Path, do the following:
on the Surfaces toolbar or click Insert, Surface, Sweep.
•
Click Profile
and select the profile sketch in the graphics area.
•
Click Path and select the path sketch in the graphics area. NOTE: If you preselect either the profile sketch or the path sketch, the sketch appears in the appropriate box of the PropertyManager.
6.
Apply Options if needed. NOTE: Some of these Options apply only to sweeps using a guide curve.
7.
Under Guide Curves, do the following: •
Select the Guide Curves
in the graphics area.
• •
Click Move Up or Move Down to change the order in which to use the guide curves. If necessary, clear the Merge smooth faces check box. Example
•
Click Show Sections Section Number.
, and click the arrows
8.
Apply Start/End Tangency if necessary.
9.
Click OK
to view and troubleshoot the profile by
.
Lofted Surface To loft a surface:
1.
Create a plane for each profile section of the loft. (The planes do not need to be parallel.)
2.
Sketch the section profiles on the planes. You need a separate sketch for each profile.
3.
Create guide curves, if needed. You need a separate sketch for each guide curve.
Profiles
Profiles with Guide Curves
4.
Click Lofted Surface
5.
Click Profiles , then in the graphics area select the profiles in the order you want to connect them. Select corresponding segments on each profile; the vertex closest to the selection point is used to connect the profiles. Examine the preview curve.
6.
on the Surfaces toolbar or Insert, Surface, Loft.
•
If the preview curve looks wrong, you may have selected the sketches in the wrong order. Use
•
Move Up or Move Down to rearrange the profiles. If the preview curve indicates that the wrong vertices will be connected, click the profile with the wrong vertex connected to clear it, then click again to select a different point on the profile.
•
To clear all selections and start over, right-click in the graphics area, select Clear Selections, and try again.
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7.
Under Options, select from the following as needed: •
Maintain tangency
•
Advanced smoothing obtains smoother surfaces. This option is available only if the loft sections have circular or elliptical arcs. The sections are approximated, and sketch arcs can be converted to splines.
•
Close loft
•
Show preview
8.
If you are using guide curves, select the Guide Curves
9.
Move Down to change the order in which to use the guide curves. To control tangency, click Start/End Tangency.
Simple loft 10. Click OK
in the graphics area. Click Move Up
Loft using guide curve
.
Offset Surface 1.
Click Offset Surface
or Insert, Surface, Offset.
The Offset Surface PropertyManager appears. 2.
Select the surfaces or faces to offset. The name of the surfaces appear under Offset Parameters
.
NOTE: If you select multiple faces, they must be contiguous. 3.
Enter an offset distance in the Offset Distance box. NOTE: You can create an offset surface with a distance of zero.
The selected faces are listed under Offset parameters, and a preview of the offset is displayed.
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4.
Click Flip Offset Direction
5.
Click OK
.
to change the direction of the offset.
or
Radiating a Surface from a Parting Line You can create surfaces by radiating a parting line, an edge, or a set of contiguous edges inwards or outwards, and parallel to a selected plane. To create a surface by radiating a parting line:
1.
Sketch a curve on the face of a part.
2.
Project the curve as a Split Line.
3.
Click Radiate Surface
4.
Under Radiate Parameters, do the following: •
on the Surfaces toolbar or Insert, Surface, Radiate.
Select a plane that is parallel to the direction in which you want the surface to radiate. The name of the plane appears in the Radiate Direction Reference box.
•
Select the split line in the graphics area to place it in the Edges to radiate box. Note the arrow
•
direction. If necessary, click the Reverse direction check box. Set the width of the surface in the Radiate distance box.
• 5.
Click Propagate along tangent faces if you want the surface to continue around the tangent faces of the part.
Click OK
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Surface Face Blend Fillet To create a face blend fillet between surfaces:
1.
Create two surfaces (the surfaces need not be adjacent).
2.
Click Fillet
3.
Under Fillet Type, click Face Fillet.
4.
Under Items to Fillet, enter the Radius
5.
In the graphics area, select the first face to fillet.
6.
on the Features toolbar or click Insert, Surface, Fillet/Round.
•
The face you selected appears in the Face Set 1 box. The preview arrow indicates the direction of the face blend.
•
If the preview arrow points away from the second face, click Reverse Face Set direction of the face blend.
to change the
In the graphics area, select the second face to fillet. •
The face you selected appears in the Face Set 2 box.
•
Click Reverse Face Set
, if necessary, so that the arrows point towards each other.
7.
Tangent Propagation is the default. Click to clear the check box if you do not want the fillet to apply to tangent faces.
8.
Under Fillet Options, you can do the following: •
Click under Hold line then click an edge on one of the faces to define the size of the fillet. You cannot pick a laminar edge as a hold line. (A laminar edge is an edge with only one attached face.)
•
Click Curvature continuous to resolve discontinuity problems and create a smoother curvature between adjacent surfaces. To verify the effect of the curvature continuity, you can display Zebra Stripes.
•
Click the Help point check box to resolve an ambiguous selection. Then click a vertex close to the location where you want to insert the fillet.
•
Under Trim surfaces, select one of the following: o
o
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.
Trim and attach. Trim the filleted faces and knit the surfaces into one surface body. This is the default. Don't trim or attach. Add a new fillet surface, but do not trim the faces or knit the surfaces.
9.
Click OK
.
The face blend fillet combines the two separate surface bodies into a single surface body.
Surface Controls Extend Surface You can extend a surface by either selecting an edge, multiple edges, or a face. To extend a surface:
1.
Click Extended Surface
on the Surfaces toolbar or click Insert, Surface, Extend.
2.
In the graphics area, select one or more edges (to extend those edges), or a face (to extend the entire surface an equal amount on all edges). The edge or face you select displays in the Edges/Faces to Extend box.
3.
4.
Select an End Condition. •
Distance. Enter a value under Distance to extend the surface that distance. Use the handles or enter the Distance in the PropertyManager.
•
Up to point. Select a Vertex
•
Up to surface. Select a Surface/face surface ends.
in the graphics area where the extended surface ends. (or a plane) in the graphics area where the extended
Select an Extension Type. •
Same surface extends the surface along the geometry of the surface.
•
Linear extends the surface tangent to the original surface along the edges.
Extend edge using Same surface as the Extension Type.
Extend edge using Linear as the Extension Type.
Extend surface using the face as the Edges/Faces to Extend and Same surface as the Extension Type.
TIP: To extend a surface up to another surface or reference plane, click FeatureManager design tree to select the surface or plane.
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5.
Click OK
.
To extend one or more tangent surfaces:
1.
Create a surface composed of multiple tangent surfaces.
2.
Select to extend individual adjacent tangent surfaces, non-adjacent tangent surfaces, or all tangent surfaces (see tangent surfaces sample). •
To extend individual or multiple (adjacent or non-adjacent) tangent surfaces, select any edge or face.
•
To extend all tangent surfaces, select an edge, and click Propagate tangent edges. Propagate
•
to highlight and extend all
changes color, indicating that you can extend all tangent edges.
Click Propagate again
to cancel the extension of all additional tangent edges.
NOTE: Propagate only displays when you select an edge. If you select the face, the surface extends in all directions. 3.
Select an Extension Type and End Condition.
4.
Click OK
.
Example of Extend Tangent Surfaces
Extend tangent surfaces selecting a single edge
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Click Propagate to highlight and extend all tangent surfaces
Extend tangent surfaces selecting multiple adjacent edges
Extend tangent surfaces selecting multiple non-adjacent edges
Fillet Surface You can use a fillet to smooth the edge between two adjacent faces in a surface body that meet at an angle. Select a Partial preview, a Full preview, or No preview in the Fillet PropertyManager. Fillets now include previews with all fillet types except face fillets and full round illets.
Constant radius surface fillet with Full preview
Constant radius surface fillet applied
Multiple radius surface fillet with Partial preview
Multiple radius surface fillet applied
Surface filleting works as it does for solid bodies with a few exceptions. You can do the following: •
Fillet the edges of a surface body.
•
Make multiple radius surface fillets.
•
Make fillets between two surfaces, or face blend fillets.
•
Add setback parameters to the surface fillets.
•
Make surface fillets with hold lines.
•
Trim or keep the filleted surfaces in a face blend fillet.
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You can not do the following: •
Make a variable radius fillet on a surface.
•
Preserve a cut in a surface body with the Keep features option.
•
Select a surface to fillet by feature.
To fillet edges on a surface body:
1.
Click Fillet
on the Features toolbar or Insert, Surface, Fillet/Round.
2.
Under Fillet Type, select Constant radius.
3.
Under Items to Fillet, enter the Radius
4.
In the graphics area, highlight the edges to fillet. The edge or loop and the radius is listed in the Edges, Faces, Features and Loops
.
box.
NOTE: Make sure that the edges you select have two attached faces. You should knit adjacent surfaces prior to filleting. 5.
Choose options such as Multiple radius fillets, Setback parameters, Keep features, Round corners, and Overflow type, as you would for a fillet on a solid body.
6.
Click OK
.
Example of Keep Features in Surface Fillet The Keep Features option in surface filleting works differently than it does in solid filleting. In a solid part, if you have a boss or cut feature in the area of a fillet, you can preserve the features when filleting. In a surface body, you can preserve a boss, but not a cut.
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Knit Surface Use the Knit Surface function to combine two or more faces and surfaces into one. Note the following about knit surfaces: Edges of the surfaces must be adjacent and not overlapping. Surfaces do not need to be on the same plane. Select the entire surface body, or select one or more adjacent surface bodies. •
Knit surfaces do not absorb the surfaces you used to create them.
•
Create a solid body when the knit surfaces form a closed volume, or leave as a surface body.
To knit surfaces:
1.
Click Knit Surface
or Insert, Surface, Knit.
In the PropertyManager, under Selections: a.
Select the faces and surfaces to knit in the graphics area or in the FeatureManager design tree. The result is a single surface listed in the FeatureManager design tree as SurfaceKnit
Create adjacent, non-intersecting surfaces
There is no difference in the appearance of the faces and surfaces after knitting. b.
Select Try to form solid if you want to create a solid model from the enclosed surfaces. Select the faces to knit
2.
Click OK
.
The surfaces are knit.
To use the Seed face option:
To knit surfaces with the Seed option, you must use Radiate Surface. 1.
Create a radiated surface.
2.
Click Knit Surface
3.
In the Faces and surfaces box, select the radiated surface.
4.
Click the Seed face box, and click any face on the model you want to knit with the radiated surface.
5.
Click OK
or Insert, Surface, Knit.
.
The seed face and all adjacent faces are knitted to the radiated surface.
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Mid Surface The Mid Surface tool enables you to create mid surfaces between suitable selected face pairs. Suitable face pairs should be offset from each other. Examples of suitable face pairs include two parallel planes, or two concentric cylindrical faces. Mid surface is useful for generating meshes of two-dimensional elements in finite element modeling.
You can create any of the following mid surfaces: •
Single. Select a single pair of offset faces from the graphics area.
•
Multiple. Select multiple pairs of offset faces from the graphics area.
•
All. Click Find Face Pairs to have the system select all suitable offset faces on the model .
The resulting surface includes all the same attributes as any surface created in SolidWorks. To create a mid surface:
1.
Click Mid-Surface
on the Surfaces toolbar, or click Insert, Surface, Mid Surface.
2.
Under Selections, choose one of the following: from the graphics area an individual set of face pairs, multiple sets of face pairs - or from the PropertyManager, click Find Face Pairs to have the system scan the model for all suitable face pairs. Find Face Pairs automatically filters out any unsuitable face pairs.
Individual face pair selected
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All face pairs selected (Find Face Pairs)
3.
Use Position to place the mid surface between the face pair. The default is 50%. The position is the distance between the faces that appear in the Face 1 and Face 2 boxes, starting from Face 1. mid surface face 1 face 2 face 3 Position 50%
face 4 4.
Position 75%
When you use Find Face Pairs, you can specify a Recognition threshold to filter the results. The Recognition threshold is based on combining the following: •
The Threshold Operator function (= equal, < less than, <= less than or equal to, > greater than, >= greater than or equal to), is the mathematical operative.
•
The Threshold Thickness is the wall thickness. For example, you can set the system to recognize all suitable face pairs that have a wall thickness of less than or equal to (<=) 3 millimeters. Any face pair not meeting this criteria is not included in the results.
5.
If necessary, under Options, click the Knit surfaces check box to clear the default which creates a knit surface.
6.
Click OK
.
You can either add new face pairs, delete existing ones, or update face pairs. To delete face pairs:
1.
Select a set in Face Pairs and press Delete.
2.
Click OK
.
To add face pairs:
1.
Select Face 1 in the PropertyManager, and choose a face in the graphics area.
2.
Choose an offset face as Face 2. The selected faces are highlighted in the graphics area, and listed under Face Pairs.
3.
Click OK
.
To update face pairs:
1.
Select a set in Face Pairs. The face pair is displayed in Face 1 and Face 2.
2.
Select another pair of offset faces in the graphics area. NOTE: You can also amend one selection of the offset pair, provided the new face you select is offset to the first face.
3.
Click Update Pair to update Face pairs with the new set of faces.
4.
Click OK
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Fill Surface The Fill Surface feature constructs a surface patch with any number of sides, within a boundary defined by existing model edges, sketches, or curves. You can use this feature to construct a surface to fill a gap in a model. You can apply Fill Surface in one or more of the following cases: •
Correct a part that does not import correctly into SolidWorks (where there are missing faces).
•
Fill the holes in a part used for core and cavity molding.
•
Construct a surface for industrial design applications.
•
Create a solid.
•
Include features as separate entities, or merge those features.
Fill Surface includes the following capabilities in the PropertyManager. Patch Boundary Patch Boundary capabilities.
defines the edges of the patch you apply. Boundaries include the following properties and
•
You can use surfaces or solid edges, as well as 2D or 3D sketches as boundaries for the patch.
•
For all sketch boundaries, you can select only a Contact patch as the type of Curvature Control.
Alternate Face Example With Alternate Face, you can flip the boundary face for the curvature control of the patch. Alternate Face is used only when creating a patch on a solid model. Curvature Control Curvature Control defines the type of control you want to exert on the patch you create. The types of Curvature Control include: •
Contact. Creates a surface within the selected boundary.
•
Tangent. Creates a surface within the selected boundary, but maintains the tangency of the patch edges.
You can apply different types of Curvature Control in the same patch. Example Apply to all edges The Apply to all edges check box enables you to apply the same curvature control to all edges. If you select the function after applying both Contact and Tangent to different edges, it applies the current selection to all edges. Optimize surface Select the Optimize surface option with two, three, or four-sided surfaces. The Optimize surface option applies a simplified surface patch that is similar to a lofted surface. Potential advantages of the optimized surface patch include faster build times, and increased stability when used in conjunction with other features in the model. Show preview Display a shaded preview of the surface fill. Preview mesh Display a grid on the patch to help you visualize the curvature. The Preview mesh is available only when you select Show preview.
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Reverse Surface Change the direction of the surface patch. The Reverse Surface button is dynamic, and only displays under these conditions: •
All boundary curves are coplanar
•
No constraint points exist
•
No interior constraints
•
Fill surface is non-planar Example
Constraint Curves Constraint Curves allow you to add slope control to the patch. They are used primarily with industrial design applications. You can create a constraint curve using sketch elements such as sketch points or splines. Click on the images below to see examples of applying Fill Surface
Imported surface example
Industrial design example
Resolution Control If your fill surface is not smooth, you can improve its quality by adjusting the Resolution Control
slider.
The Resolution Control is available only when the Optimize Surface check box is cleared. The resolution is set to 1 by default. Change the setting to 2 or 4 to increase the number of patches defining the surface. A higher setting improves the quality of the surface profile. Changing the resolution increases the model size and processing time. You should not change the default setting if your surface is satisfactory.
Quality set to 1
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Options You can create a solid model with the Filled Surface tool. Options include: •
Merge result
•
Try to form solid
•
Reverse direction
Merge result The behavior for this option depends on the boundaries. When all the boundaries belong to the same solid body, you can use the surface fill to patch the solid. If at least one of the edges is an open sheet edge and you select Merge result, then the Surface Fill knits with the surfaces to which the edges belong. If all the boundary entities are open edges, then a solid may optionally be created.
Model without Filled Surface applied. Note the features inside.
Model with Filled Surface applied and Merge result selected. The surface fill joins the solid, removing the features inside.
Model with Filled Surface applied and Merge result cleared. The surface fill creates a new surface, and the features inside remain. Merge result option allows: •
Streamline operation, eliminating Replace face.
•
Hide solid details within the model.
Try to form solid Forming a solid is possible if all the boundary entities are open surface edges. The option Try to form solid is cleared by default. Reverse direction When patching a solid with a fill surface there are often two possible results. Click Reverse direction to correct if the fill surface displays in an unwanted direction.
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Example of Using Alternate Face Example of a solid model, using Contact as the Curvature Control. The fill surface feature automatically selects a direction when you pick a boundary. In some cases, there is more than one possible direction option. To choose other directions, select Alternate Face.
Example of Multiple Curvature Control This example of an imported surface has a gap along the front face. To patch the surface correctly, you must apply a different curvature control type to the different boundary edges. 1.
Import model and click Filled Surface on the Surfaces toolbar, or Insert, Surface, Fill.
2.
In the graphics area, under Patch Boundary, select the boundary edges. •
Apply Contact patch to the two curved edges.
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•
3.
Apply Tangent patch to the two horizontal edges.
Click OK
to apply Fill Surface.
Example of Surface Fill with Reverse Surface
Left image: You select the top profile for the tangent surface fill (orange arrow), but the surface is attached to the bottom profile (black arrow). Correction is required. NOTE: The red section is the top of the fill surface extruding from the bottom profile through the top (blue).
Right image: You select the top profile for the tangent surface fill (orange arrow), and click Reverse Surface. Correction is applied. NOTE: The tangent fill surface (green), is correctly attached to the top profile.
Fill Surface Imported Surface Example This example of a casing is an imported surface. One of the faces in this example has failed. You can repair it by using fill surface. Creating a fill surface from an imported part:
1.
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Import the part.
2.
Click Filled Surface
on the Surfaces toolbar, or Insert, Surface, Fill.
3.
In the graphics area, under Patch Boundary, select each of the tangent edges around the hole.
The edges, along with the curvature type are listed in the Patch Boundaries
box.
NOTE: In this case use Tangent to apply constraints to the patch. 4.
Click OK
.
Fill Surface Industrial Design Example This model uses sketches as patch boundaries for the fill surface. To help shape the patch, it also uses sketch points and a spline as constraint curves. Creating a fill surface using constraint curves:
1.
Sketch1 - Sketch an arc on Plane1 (Front) and dimension.
2.
Sketch2 - Sketch an arc on Plane3 (Right), dimension, and add the necessary relations.
Sketch1
Sketch2
3.
Sketch3 - Sketch an arc to connect Sketch1 and Sketch2 on Plane2 (Top). Dimension and add the necessary relations.
4.
Create Plane4 (at angle to Plane1) and add sketch points (Sketch4), as shown, to use as constraint curves.
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5.
Create Plane5 (offset from Plane2) and sketch spline (Sketch5), as shown, to use as a constraint curve.
Sketch3
Sketch4
Sketch5
6.
Click Filled Surface
on the Surfaces toolbar, or Insert, Surface, Fill.
7.
In the graphics area, under Patch Boundary, select the edges created by Sketch1, Sketch2, and Sketch3. The edges, along with the curvature type are listed in the Patch Boundaries
box.
NOTE: The curvature control defaults to Contact, since only contact surfaces are eligible with sketch boundaries. 8.
Under Constraint Curves, select Sketch4 and Sketch5 in the graphics area. Sketch4 and Sketch5 are listed in Constraint Curves box
9.
Click OK
.
.
Three views of the industrial design example with fill surface applied Trim Surface You can use a surface, plane, or sketch as a trim tool to trim other surfaces where they intersect. You can also use a surface in conjunction with additional surfaces, as mutual trim tools. Trim surface includes the following options:
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•
Trim type: Standard or Mutual.
•
Keep selections Retains trimmed surfaces.
•
Remove selections. Discards trimmed surfaces.
•
Natural. Trims and forces the boundary edges to follow the shape of the surface.
•
Linear. Trims and forces the boundary edges to follow a linear direction from the trim point.
•
Split All. Displays all possible splits on the surface.
To trim a surface:
1.
Create two surfaces which intersect at one or more points.
2.
Click Trimmed Surface
3.
Under Trim Type, select Standard.
4.
Under Selections:
5.
6.
on the Surfaces toolbar or Insert, Surface, Trim.
•
In the graphics area, select a surface, plane, or sketch as the Trim tool
•
In the graphics area, select a surface as the Pieces to keep based on the following:
.
, or as the Pieces to remove
,
o
Keep selections. Select to retain the surface bodies listed under Pieces to keep.
o
Remove selections. Select to discard the surface bodies listed under Pieces to remove.
Under Surface Split Options, select an item: •
Natural. Boundary edges follow shape of the surface.
•
Linear. Boundary edges follow linear direction from trim point.
•
Split All. Display all splits in the surface.
Click OK
.
Trim tool
Pieces to keep
Trimmed surface
To trim a surface using mutual trim:
1.
Create two or more surfaces which intersect at one or more points.
2.
Click Trimmed Surface on the Surfaces toolbar or Insert, Surface, Trim.
3.
Under Trim type, select Mutual.
4.
Under Selections, do the following: •
In the graphics area, select at least two intersecting surfaces you want to use as the Trimming surfaces
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•
In the graphics area, select the areas you want as the Pieces to keep
, or as the
Pieces to remove , based on the following: o Keep selections. Select to retain the surface bodies listed under Pieces to keep. o Remove selections. Select to discard the surface bodies listed under Pieces to remove.
You can select one or more areas to keep, depending on the intersecting surfaces. 5.
Under Surface Split Options, select an item: • • •
6.
Natural. Boundary edges follow shape of the surface. Linear. Boundary edges follow linear direction from trim point. Split All. Display all splits in the surface.
Click OK
.
Two different sets of results.
Untrim Surface With Untrim Surface, you can patch surface holes and external edges by extending an existing surface along its natural boundaries. You can also extend the natural boundaries of the surface by a given percentage, or connect the end points to fill the surface. Use the Untrim Surface tool with any imported surface or surfaces that you create. Note: Untrim Surface extends an existing surface, whereas Surface Fill creates different surfaces, applies a patch between multiple faces, uses constraint curves, and so on.
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Example of Untrim Surface
Select the edges as shown and under Options, choose Extend edges
Select the edges as shown, and under Options, choose Extend edges.
Select edges as shown, and under Options, choose Connect endpoints.
Select the edge as shown, keep the
Select the edge as shown, change the Distance
Distance at the default 0%. Under Options, choose Extend edges.
to 30%. Under Options, choose Extend edges.
Select the face, and under Options, choose Internal edges.
Select the face, and under Options, choose External edges. You can also select All edges to untrim both internal and external edges.
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To use Untrim Surface:
1.
Open the surface part that you want to untrim.
2.
Click Untrim Surface on the Surfaces toolbar, or Insert, Surface, Untrim.
3.
Under Selections , choose the face or the edges you want to untrim. Note: Depending on the edge you select, the surface can extend to its natural boundary. To constrain the edge, select the adjacent edge, as show below.
Extend edges. If you select the edge as shown, the surface extends to its natural boundaries. 4.
To constrain the surface extension, select both edges, as shown above.
Under Options, as the Edge untrim type, you can accept the default Extend edges to extend all edges to their natural boundaries. Or you can select both edges and choose Connect endpoints, as shown at right. To create a surface extension that merges with the original surface, select the Merge with original check box (default). To create a new, separate surface body, clear the Merge with original check box. Both the original and the new surface body appear in the FeatureManager design tree.
5.
Click OK
to untrim the surface.
Surface untrim, select both left edges and the inner edge. Under Options, select Connect endpoints.
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Surface untrim, select the face. Under Options, select All edges. All edges are extended to their natural boundaries.
Radiate Surface Radiate surface works on edges, parting lines, or planar and non-planar curves. To radiate a surface:
1.
Click Radiate Surface
or Insert, Surface, Radiate.
The Radiate Surface PropertyManager appears. 2.
Select a reference plane that is parallel to the direction in which you want the surface to radiate.
3.
Click the Edges To Radiate box
4.
Note the arrow direction. To specify the opposite direction, click Flip Radiate Direction
5.
Select Propagate along tangent faces if the part has tangent faces and you want the surface to continue around the part.
6.
Specify the width of the surface in the Radiate Distance
7.
Click OK
, then click a parting line, an edge, or a set of contiguous edges. .
box.
.
Hide and Show Bodies With multibody parts, the solid bodies can be independent of other solid bodies or surfaces. You can hide or show surface (or solid) bodies, using View, Hide/Show Bodies. In the PropertyManager, you can select one or more surface bodies or a solid body from the graphics area. To hide bodies:
1.
Open a document containing multiple surface or solid bodies.
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2.
Click View, Hide/Show Bodies. The Hide/Show Bodies PropertyManager appears.
3.
Select one or more entities in the graphics area. Your selections appear under Hidden Bodies. When you select a solid body or a surface body, it becomes translucent in the graphics area.
4.
Click OK
.
The entities you selected remain hidden.
To show hidden bodies:
1.
Click View, Hide/Show Bodies again to open the PropertyManager.
2.
Select the translucent bodies in the graphics area. You can select some or all of the translucent bodies.
3.
Click OK
.
The translucent entities you selected are visible again.
You can also use the shortcut menu to hide a surface without using the PropertyManager to preview the entities you select. To show the hidden surface again, click View, Hide/Show Bodies, select the translucent bodies in the graphics area and click OK
.
NOTES:
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•
You can still select from the FeatureManager design tree to Hide or Show, but it does not open the PropertyManager or display the model in a translucent state.
•
To hide or show an assembly component, click Hide/Show Component
on the Assembly toolbar.
Delete Face With Delete Face
tool, you can do the following:
•
Delete. Deletes a face from a surface body, or deletes one or more faces from a solid body to create surfaces.
•
Delete and Patch. Deletes a face from a surface body or solid body and automatically patches and trims the body.
•
Delete and Fill. Deletes faces and generates a single face to close any gap.
To delete faces from a surface body:
1.
Click Delete Face
on the Surfaces toolbar, or Insert, Face, Delete.
The Delete Face PropertyManager appears. 2.
In the graphics area, click the faces you want to delete. The names of the faces appear under Faces to delete
3.
Under Options, click Delete.
4.
Click OK
.
.
The faces disappear.
Select gray faces to delete
Faces deleted
To delete and patch faces on a surface body:
1.
Follow steps 1 and 2 from the previous procedure.
2.
Under Options, click Delete and Patch.
3.
Click OK
.
The faces disappear, and the adjoining faces extend to form an unbroken surface.
Select gray faces to delete
Blue faces patched
To delete and fill surfaces:
1.
Follow steps 1 and 2 from the previous procedure.
2.
Under Options, click Delete and Fill. The system deletes the faces and replaces them with a single face •
Tangent fill cleared. The fill use contact edges.
•
Tangent fill selected. The fill uses tangent edges.
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3.
Click OK
.
The faces are deleted, and are filled by a single unbroken surface.
Before Delete and Fill To delete faces from a solid body and create surfaces:
1.
Using a solid body, click Delete Face on the Surfaces toolbar, or Insert, Face, Delete. The Delete Face PropertyManager appears.
2.
In the graphics area, click the faces you want to delete. The names of the faces appear under Faces to delete
.
3.
Under Options, click Delete.
4.
Click OK
.
The faces disappear, and a new DeleteFace1 surface body is added to the Surface Bodies folder
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in the FeatureManager design tree.
After Delete and Fill
Delete Hole The Delete Hole dialog box lists any closed profile instances previously deleted from a surface. It allows you to remove one or more instances, without deleting the entire Delete Hole feature from the FeatureManager design tree. NOTE: All entities must be on the same body.
Valid. Both holes are on the same body.
Invalid. Each set of holes is on a separate body. You need to create two instances of Delete Hole to remove all holes.
To edit delete hole instances:
1.
Click the Delete Hole feature in the FeatureManager design tree, right-click and select Edit Definition.
2.
Select the closed profile instance you want to restore from the Hole Edge(s) to remove list.
3.
Press Delete.
4.
Click OK to restore the closed profile to the surface.
To delete a hole from a surface:
1.
Select the closed profile instance on the surface.
2.
Click Delete.
3.
In the Choose Option dialog box, select Delete Holes(s).
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Replace Face You can replace faces in a surface or solid body with new surface bodies. The replacement surface body does not need to have the same boundaries as the old faces. When you replace a face, adjacent faces in the original body automatically extend and trim to the replacement surface body, and the new face trims. Replace Face allows you to do the following:
•
Replace a single face or set of connected faces with a surface body. Example
•
Replace more than one set of connected faces with the same number of surface bodies in a single operation. Example You must list the faces for replacement in the same order as the corresponding replacement surface bodies. Replace Face identifies the pairs of original and replacement faces and performs the replacement.
•
Replace a face in a solid or surface body.
The replacement surface body can be of the following types:
•
Any type of surface feature such as an extrude, loft, fill, and so on.
•
A knit surface body, or a complex imported surface body.
•
Usually wider and longer than the faces you are replacing. However, in some cases when the replacement surface body is smaller than the faces for replacement, the replacement surface body extends to meet the adjacent faces.
The faces for replacement have the following characteristics:
•
Must be connected.
•
Do not need to be tangent.
Replace Face Example - Single Set of Faces To replace a set of connected faces with a surface body:
1.
Make sure that your replacement surface body is wider and longer than the faces you are replacing.
2.
Click Replace Face
, or Insert, Face, Replace.
The Replace Face PropertyManager appears. 3.
Under Replace Parameters do the following: •
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Click the faces you want to replace to place them in the Target faces for replacement box. The faces must be connected, but they do not have to be tangent. If you cannot see the faces, rightclick the replacement surface body and select Hide Surface Body.
•
4.
Click the Replacement surfaces box, then click the replacement surface body to place it in the box. If the replacement surface body is hidden, select it in the FeatureManager design tree.
Click OK
.
The faces are replaced, and the adjacent faces of the original body are trimmed and extended to fit. The new face is trimmed to fit the adacent faces of the original body.
NOTE: If the replacement surface body is still visible, right-click it and select Hide Surface Body. Replace Face Example - Multiple Sets of Faces To replace more than one set of connected faces with surface bodies:
1.
Click Replace Face
2.
Under Replace Parameters do the following: •
, or Insert, Face, Replace.
Click the first set of faces you want to replace to place them in the Target faces for replacement box. You do not have to click them in order, but you need to place the first set together in the list. In this example, select the five faces along the top of the "H", including the vertical faces.
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•
Click the second set of faces to place them in the Target faces for replacement
box.
In this example, select the five faces along the bottom of the "H".
•
3.
Click to highlight the Replacement surfaces box, then click first the replacement surface body for the first group of faces, then the replacement surface body for the second group of faces.
Click OK
.
The faces are replaced, and the adjacent faces of the original body are trimmed and extended to fit. The new faces are trimmed to fit the adjacent faces of the original body.
Sweeps Sweep Overview Sweep creates a base, boss, cut, or surface by moving a profile (section) along a path, according to these rules: •
The profile must be closed for a base or boss sweep feature; the profile may be open or closed for a surface sweep feature.
•
The path may be open or closed.
•
The path may be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
•
The start point of the path must lie on the plane of the profile.
•
Neither the section, the path, nor the resulting solid can be self-intersecting.
You can view the sweep using zebra stripes as you create the sweep. Place the pointer on the sweep, open the shortcut menu, and select View zebra stripes. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear View zebra stripes.
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Sweeps can include: •
Simple sweeps
•
Sweeps using guide curves
•
Sweeps using multiple profiles
•
Sweeps using thin features
Simple Sweep To create a simple sweep:
Sketch on multiple planes, following the tips outlined below: Tips for creating a sweep:
Profile •
The profile must be closed for a base or boss sweep feature.
•
The profile can be open or closed for a surface sweep feature.
Path •
The path can be open or closed.
•
The path can be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
•
The start point of the path must lie on the plane of the profile. Neither the section, the path, nor the resulting solid can be self-intersecting.
You can create a sweep using multiple profiles. You can view the sweep using zebra stripes as you create it. Place the pointer on the sweep, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear View zebra stripes. 1.
Sketch a closed, non-intersecting profile on one plane or on a face.
2.
Create the path that the profile will follow. Use a sketch, existing model edges, or curves.
3.
Click one of the following: • • •
Sweep on the Features toolbar or Insert, Boss/Base, Sweep Insert, Cut, Sweep Swept Surface on the Surfaces toolbar or Insert, Surface, Sweep 1 = Profile 2 = Path
4.
Under Profile and Path, do the following: •
Click Profile
•
Click Path
and select the profile sketch in the graphics area. and select the path sketch in the graphics area.
NOTE: If you preselect either the profile sketch or the path sketch, the sketch is displayed in the appropriate box of the PropertyManager.
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5.
Apply Options if needed.
Sweep preview
Orientation/twist Type: Keep normal constant
Orientation/twist Type: Follow path
Under Options, clear Show preview if you do not want to display a shaded preview of the sweep. Under Orientation and Twist Control, only Keep normal constant and Follow path apply to simple sweeps. The other selections apply only to sweeps using a guide curve. When you select Follow path as the Orientation/twist type, you can select parameters to stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign. 6.
Apply Start/End Tangency if needed.
7.
You can create a Thin Feature sweep.
To create a thin feature sweep: o
Select a Type, either One-Direction, Mid-Plane, or Two-Direction.
o
Examine the preview and click Reverse Direction
o
Enter a Direction 1 Thickness Thickness
Click OK
and if using Two-Direction as the Type, a Direction 2
.
Sweep with solid feature 8.
, if necessary.
Sweep with thin feature
.
Example of Shaded Sweep Preview
Sweep shaded preview
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Sweep feature applied
Sweeps Feature A sweep creates a base, boss, cut, or surface by moving a profile (section) along a path. You can view the sweep using zebra stripes as you create it. Place the pointer on the sweep, open the shortcut menu, and select Zebra stripes preview. Note that if you apply zebra stripes, when you create another sweep, loft, or add a loft section, the zebra stripes display. Use the shortcut menu to clear View zebra stripes. Sweeps with guide curves. An option allows you to clear Merge smooth faces for sweeps with guide curves. Clearing Merge smooth faces results in the following: •
The performance of sweeps with guide curves improves. Sweeps generate faster and merge between adjacent geometry and edges.
•
The swept body is segmented at all points where the guide curve or the path is not curvature continuous (see the example below). Consequently, the lines and arcs in the guide curves are more accurately matched.
Merge smooth faces check box checked
Merge smooth faces check box cleared
When you clear the Merge smooth faces check box, the potential exists that some features created later might fail due to changed geometry. Orientation/twist type option. When you select Follow path as the Orientation/twist type, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign. Profiles always maintain a normal to the path. Profile fluctuations are due to uneven curvature fluctuations along the path. Unless you correct the fluctuations by selecting one of the Orientation/twist type options, the profiles follow the path and shift to adjust to the misaligned path: To create a sweep:
1.
Sketch a profile and a path.
You can create sweeps using multiple profiles.
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Tips for creating a sweep:
Profile •
The profile must be closed for a base or boss sweep feature.
•
The profile may be open or closed for a surface sweep feature.
Path •
The path may be open or closed.
•
The path may be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
•
The start point of the path must lie on the plane of the profile.
Neither the section, the path, nor the resulting solid can be self-intersecting. 2. 3.
Click Swept Boss/Base on the Features toolbar, or Insert, Boss/Base Sweep. Under Profile and Path, do the following: •
Click Profile
•
Click Path
and select the profile sketch in the graphics area. and select the path sketch in the graphics area.
If you preselect either the profile sketch or the path sketch, the sketch is displayed in the appropriate box of the PropertyManager. Clear the Show preview check box if you want to only display the profile and path.
4.
5.
6.
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Under Options, apply any of the following: •
Orientation/twist Type
•
Maintain tangency
•
Advanced smoothing
•
Align with end faces
The following functionality is also available: •
Guide Curves
•
Start/End Tangency
•
Thin Feature
Click OK
.
Sweeps with Mulltiple Profiles
Sweep with multiple separate profiles
Sweep with multiple nested profiles
Sweeps with Guide Curves You can use guide curves to control the intermediate profiles as the sketch is swept along the path. You can view the sweep using zebra stripes as you create it. Place the pointer on the sweep, open the shortcut menu, and select Zebra stripes preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear View zebra stripes. To create a sweep using guide curves:
If you have already created the profiles for a sweep with guide curves, skip to step 4. 1.
Create the guide curves, either as a sketch, a curve, or a model edge.
2.
Create a path for the sweep. This also can be a sketch, curve, or model edge. NOTE: When using guide curves to create a sweep, the path must be a single entity (line, arc, and so on) or the path segments must be tangent (no angled corners). Path - vertical sketch through ellipse Guide curve - spline Profile - ellipse
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3.
Sketch the sweep profile. See some recommendations for creating sweeps with guide curves. You can create a sweep using multiple profiles. The Pierce Point relation is not required for sweeps with guide curves. You can use guide curves without specifying a pierce point between the guide curve and the profile sketch. You can also create the guide curves and the profile sketches in any order.
4.
5.
Click one of the following: •
Swept Boss/Base
•
Swept Cut
•
Swept Surface
on the Features toolbar or Insert, Boss/Base, Sweep
on the Features toolbar, or Insert, Cut, Sweep on the Surfaces toolbar or Insert, Surface, Sweep
Under Profile and Path, do the following: •
Click Profile
•
Click Path
and select the profile sketch in the graphics area. and select the path sketch in the graphics area.
NOTE: If you preselect either the profile sketch or the path sketch, the sketch is displayed in the appropriate box of the PropertyManager. 6.
Click Options to apply the following, if necessary: •
Clear the Show preview check box if you want to only display the profile, path and guide curves.
•
Orientation/twist Type If the sweep includes guide curves, end tangency is controlled by choosing either: Follow path and 1st guide curve or Follow 1st and 2nd guide curves.
•
Maintain tangency If the sweep section has tangent segments, selecting this option causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs can be converted to splines.
•
Advanced smoothing If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces. Sketch arcs can be converted to splines.
7.
8.
Under Guide Curves, do the following: •
Select the Guide Curves
in the graphics area.
•
Click Move Up
•
Click Show Sections Section Number.
•
If necessary, clear the Merge smooth faces check box. Example
or Move Down
to change the order in which to use the guide curves.
, and click the arrows
to view and troubleshoot the profile by
Click Start/End Tangency to apply the following, if necessary: •
None. No tangency is applied.
•
Path tangent. The sweep is normal to the path at the start or end.
•
Direction vector. The sweep is tangent to a selected linear edge or axis, or to the normal of a selected plane. Select Direction vector, then click the edge, axis, or plane.
•
All faces. The sweep is tangent to the adjacent faces of existing geometry at the start or end. This selection is only available when the sweep is attached to existing geometry. NOTE: Tangency options for sweeps are similar to tangency options for lofts. See Loft Tangency Options for examples.
9.
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Click OK
.
Recommendations for Sweeps with Guide Curves The following recommendations will help you when creating a sweep with guide curves. Path and guide curve sketch Create the path and guide curves first; then create the section. A Pierce relation is not required for sweeps with guide curves. The intermediate profiles of the sweep are dependent on both the path and guide curves for their definition. Relations Note that relations such as Horizontal or Vertical may be added automatically as you sketch the section. These relations influence the shape of the intermediate sections, and may produce results that are not what you want. Use Display/Delete Relations desired.
to delete the unwanted relations. This allows the intermediate sections to twist as
Path and guide curve length The path and the guide curves may differ in length. •
If the guide curves are longer than the path, the sweep is as long as the path.
•
If the guide curves are shorter than the path, the sweep is as long as the shortest guide curve.
Guide curves Guide curves may meet at a common point, which is the apex of the swept surface. You can use any of the following items as a guide curve: sketched curves, model edges, or curves.
Preview Intermediate Sweep Sections Intermediate sections in a sweep incrementally preview the section, as the section follows the trajectory set by the path and guide curves. To view the intermediate sections in the sweep:
NOTE: You can activate this option before creating the sweep, if desired. 1.
Right-click the Sweep feature in the FeatureManager design tree and select Edit Definition.
2.
Under Guide Curves, click Show Sections
3.
Click the Up and Down arrows
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.
to scroll through the previews.
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Sweeps Options Sweep Options Under Options, you can do the following: Orientation/twist Type •
With a simple sweep, end tangency is controlled by choosing either Follow path or Keep normal constant.
•
When you select Follow path as the Orientation/twist type, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign.
•
If the sweep includes guide curves, end tangency is controlled by choosing either: Follow path and 1st guide curve or Follow 1st and 2nd guide curves.
Maintain tangency If the sweep section has tangent segments, selecting this option causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs can be converted to splines. Advanced smoothing If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces. Sketch arcs can be converted to splines. Align with end faces Continues the sweep profile to the last face encountered by the path. Sweep Options Align with End Faces Use Align with end faces to continue the sweep profile up to the last face encountered by the path. With Align with end faces selected, the faces of the sweep are extended or truncated to match the faces at the ends of the sweep, without requiring addtional geometry. Align with end faces selected
Align with end faces not selected
Top of helix
Bottom of helix
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Example of Sweep with Thin Features
Sweep with solid feature
Sweep with thin feature
Example of Merge Smooth Faces Option in Sweeps A new option allows you to clear the Merge smooth faces check box for sweeps with guide curves. Previously, there was no check box, and all sweeps merged smooth faces by default. Clearing the Merge smooth faces check box results in the following: •
The performance of sweeps with guide curves improves. Sweeps generate faster and merge between adjacent geometry and edges.
•
The swept body is segmented at all points where the guide curve or the path is not curvature continuous (see the example below). Consequently, the lines and arcs in the guide curves are more accurately matched.
Merge smooth faces check box checked
Merge smooth faces check box cleared
The entities that comprise the Path for sweeps with guide curves need not be tangent. NOTE: When you clear the Merge smooth faces check box, the potential exists that some features created later might fail due to the changed geometry. Sweep Options Advanced Smoothing Advanced smoothing. If the sweep section has circular or elliptical arcs, the sections are approximated, resulting in smoother surfaces. Sketch arcs may be converted to splines. Sweep Options Maintain Tangency Maintain tangency. If the sweep section has tangent segments, selecting this option causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs may be converted to splines.
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Loft Tangency Options Controls the tangency of a loft at the starting and ending profiles. You specify the Start and End Tangency on the Advanced tab of the Loft dialog box. •
None. No tangency is applied.
•
Normal to Profile. The loft is normal to the sketch plane of the profile at the start or end.
•
Direction Vector. The loft is tangent to a selected linear edge or axis, or to the normal of a selected plane. Click the Direction Vector button, then click the edge, axis, or plane.
•
All Faces. The loft is tangent to the adjacent faces of existing geometry at the start or end. This selection is only available when the loft is attached to existing geometry. The examples in this table were created from these profiles. The start profile is the converted face of the existing geometry; the selected model edge is the direction vector.
Start Tangency
Start Tangency
None
None
End Tangency
End Tangency
None
Normal to Profile
Start Tangency
Start Tangency
Normal to Profile
Normal to Profile
End Tangency
Normal to Profile
End Tangency
None
Start Tangency
Start Tangency
All Faces
All Faces
End Tangency
End Tangency
None
Normal to Profile
Start Tangency
Start Tangency
Direction Vector
Direction Vector
End Tangency
Normal to Profile
None
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End Tangency
Start and End Tangency Options for Sweeps With a simple sweep, end tangency is controlled by choosing either Follow path or Keep normal constant in the Orientation/twist Type list. When you use guide curves to create a sweep, you have additional options for controlling the tangency at the ends of the path. You specify the Start tangency type and End tangency type under Start/End Tangency. These tangency options are only effective when you use guide curves in the sweep. Choose from these start and end tangency types: •
None. No tangency is applied.
•
Path tangent. The sweep is normal to the path at the start or end.
•
Direction vector. The sweep is tangent to a selected linear edge or axis, or to the normal of a selected plane. Click the Direction vector button, then click the edge, axis, or plane.
•
All faces. The sweep is tangent to the adjacent faces of existing geometry at the start or end. This selection is only available when the sweep is attached to existing geometry. All faces is available only as a Start tangency type.
Orientation/Twist Control Option
Select Follow path and the section remains at the same angle with respect to the path at all times.
Select Keep normal constant and the section remains parallel to the beginning section at all times.
When you select Follow path, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign.
Select Follow path and 1st guide curve and the twist of the intermediate sections is determined by the vector from the path to the first guide curve. The angle between the horizontal plane and the vector remains constant in the sketch planes of all of the intermediate sections.
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Select Follow 1st and 2nd guide curves and the twist of the intermediate section is determined by the vector from the first to the second guide curve. The angle between the horizontal plane and the vector remains constant in the sketch planes of all of the intermediate sections.
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Orientation/Twist Type - Follow Path Under sweep Options, when you select Follow path as the Orientation/twist type, you can select parameters to stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign. Profiles always maintain a normal to the path. Profile fluctuations are due to uneven curvature fluctuations along the path. Unless you correct the fluctuations by selecting one of the new options, the profiles follow the path and shift to adjust to the misaligned path. The three parameters are: •
None. The default value, indicating that no correction is applied.
With None selected, the profile fluctuates, preventing a smooth sweep. •
Direction vector. Select a plane, planar face, or line to define the vector. When you select a plane or planar face, the normal of the plane or planar face is applied. If you select a line, the line direction provides the direction vector. The section plane (along which the sweep is created), always includes the direction vector as its X-axis. The normal of the plane, the Z-axis, is the plane that contains the direction vector and the path tangent at that point.
The Front plane (shown) is the Direction vector. The profiles do not fluctuate, remaining aligned along the entire path, and creating a smooth sweep. •
All faces. If the path includes neighboring faces, you can select All faces. When the path includes 2 alternative faces, click Next Face to switch faces. The section plane (along which the sweep is created), always includes the face normal as its Y-axis. The normal of the plane, the Z-axis, is the tangent of the path at that point.
All faces selected (as shown). The profiles do not fluctuate, remaining aligned along the entire path, and creating a smooth sweep.
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Thicken Thickens a selected surface. If the surface you want to thicken is comprised of multiple adjacent surfaces, you must first knit the surfaces together before you thicken the surface. To thicken a surface:
1.
Click Thicken
on the Features toolbar, or click Insert, Base (or Boss), Thicken.
2.
Under Thicken Parameters, do the following: •
In the graphics area, select a Surface to Thicken
•
Examine the preview, and select the side of the surface you want to thicken, as shown below.
Thicken Side 1 •
.
Thicken Both Sides
Thicken Side 2
Enter the Thickness . Note that when you select Thicken Both Sides Thickness you specify to both sides.
, it adds the
NOTE: To create a solid, click Create solid from enclosed volume. This option is available only if you created a volume that is fully enclosed by surfaces. 3.
Click OK
.
Original surface
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To cut an existing solid by thickening a surface:
You can thicken a surface to cut a solid and create multibody parts. 1.
Click Thickened Cut
on the Features toolbar, or click Insert, Cut, Thicken.
2.
Under Thicken Parameters, do the following: •
In the graphics area, select a Surface to Thicken
•
Examine the preview, and select the side of the surface you want to thicken. The following example shows the Thicken Both Sides
3.
Click OK
.
option.
.
The Bodies to Keep dialog box appears, which gives you the option to create a multibody part. 4.
You can choose All bodies or Selected bodies. If you chose Selected bodies, the dialog box expands to display the number of bodies available. Click the check boxes of the bodies you want to keep.
5.
Click OK.
Keep Body 1
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Keep Body 2
All bodies
To change the thicken feature:
You can edit the side to thicken, the thickness of the feature, and the bodies you selected to keep. 1.
Right click the feature’s name in the FeatureManager design tree and select Edit Feature.
2.
Examine the preview, and if necessary select one of the following to change the side to thicken: •
Thicken Side 1
•
Thicken Both sides
•
Thicken Side 2
3.
Change the Thickness
4.
Click OK
as necessary.
.
The Bodies to Keep dialog box appears. 5.
Change the bodies to keep, as necessary.
6.
Click OK.
To fill a volume with a loft between two surfaces:
1.
Create adjacent surfaces.
2.
Open a new sketch, sketch a guide curve, and close the sketch.
3.
Click Loft
4.
Click the Profiles box and select the surfaces.
5.
Click the Guide Curve(s) box and select the guide curve sketch.
6.
Click OK
or Insert, Boss/Base, Loft.
. The resulting lofted body is solid.
To cut a part with a surface:
1.
Create a surface in the part model, or import one.
2.
Select the surface in the graphics area.
3.
Click Cut with Surface
on the Features toolbar, or click Insert, Cut, With Surface.
In the PropertyManager, under Surface Cut Parameters, choose the Selected surface for cut. 4.
Note the preview arrow, indicating which side of the part will be cut away and click Flip Cut reverse the direction of the cut, if necessary.
to
5.
Click OK
6.
To hide the surface, if desired, right-click the Surface feature in the FeatureManager design tree and select Hide.
.
You can also cut a part with a surface by using the Up To Surface option when extruding a cut.
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Tools for Features Analysis of Features Draft Analysis Overview Designers of plastic parts and mold tooling manufacturers can use the Draft Analysis tool to check the correct application of draft to the faces of their part. With draft analysis, you can verify draft angles, examine angle changes within a face, as well as locate parting lines, injection, and ejection surfaces in parts. Criteria To perform a draft analysis, specify the following criteria:
•
Direction of Pull. Select the plane used to conduct the draft analysis.
•
Draft analysis types. You can select either of the following: o o
Contour map. The analysis generates a contour map of the face angles. Face classification. The analysis examines each face on the model, based on the draft angle. When you select the Face classification check box and click Calculate, each face is displayed in a different color. NOTE: You must specify both the Direction of Pull and the Draft Angle with either type of analysis.
•
Reverse Direction you selected.
. Change the direction of the draw normal to the Direction of Pull (plane or face)
•
Draft Angle. Enter a reference draft angle, and then compare that reference angle to those currently existing on the model.
Categories The results displayed when you click Calculate depend on the type of draft analysis you select. Each time you change the type of analysis or the parameters, you need to re-calculate. Face Classification In the graphics area, each face displays a color based on the Draft angle you selected. Draft analysis results listed under Color Settings are grouped into four categories, when you specify Face classification: •
•
•
•
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Positive draft. Displays any faces with a positive draft, based on the reference draft angle you specified. A positive draft means the angle of the face, with respect to the direction of pull, is more than the reference angle. Negative draft. Displays any faces with a negative draft, based on the reference draft angle you specified. A negative draft means the angle of the face, with respect to the direction of the pull, is less than the negative reference angle. Draft required. Displays any faces that require correction. These are faces with an angle greater than the negative reference angle, and less than the positive reference angle. Straddle faces. Displays any faces that contain both positive and negative types of draft. Typically, these are faces that requires you to create a split line. NOTE: Display colors may vary. The first time you use draft analysis, the system uses default colors. If you modify the colors, the system will use the new colors you specified.
Find Steep Faces This option is used only to analyze the curved faces on a model where a draft was added. Based on the reference angle, there are points on a curved face that meet the criteria, and other points on the curve that do not meet the criteria specified by the reference angle. On some models that include curved faces, all areas along the curve may meet or exceed the reference angle. In such cases, selecting Find steep faces will not register any results, since any point along the curved face meets or exceeds the reference angle. •
Positive draft. Displays any steep faces with a positive draft, based on the reference draft angle you specified.
•
Negative draft. Displays any steep faces with a negative draft, based on the reference draft angle you specified.
Surfaces When analyzing the draft for surfaces, an additional Face classification criterion is added: Surface faces with draft. Since a surface includes an inside and an outside face, surface faces are not added to the numerical part of the classification (Positive draft and Negative draft). Surface faces with draft lists all positive and negative surfaces that include draft.
Negative draft
Positive draft
No steep faces, as all points along curved face are greater than the reference angle
In the examples below, a draft analysis using Face classification was applied to the model.
No draft analysis applied
Positive draft
Negative draft
Draft required
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Each category includes the following information and capability: •
Number of faces included in the category, shown as the number on the color swatch for that category
•
Toggle display using Show
•
Change the default display colors
•
Save the color classifications with the part when you click OK
or Hide
.
Color Contour Color contour displays the uniform or graduated changes within each face on the model as the angle on the face changes. Based on the reference angle (Draft angle ), the scale in the PropertyManager displays a positive to negative range, with 0 degrees at the center. You can select two display modes: •
Uniform display. The uniform display uses three colors to represent the areas within the faces that have positive draft, negative draft, and that require draft. You can modify the three colors.
•
Transition display. Select the Gradual transition check box to display the variations in the angles on the model where the draft is required. TIP: You can see the individual faces of the model during a color contour calculation by specifying Display HLR edges in shaded mode
on the Views toolbar.
The next time you analyze a model using Color contour, these midrange values appear as the default. NOTE: Using either display mode, move the pointer over an area on the model to display the value of the draft angle dynamically.
Gradual transition check box checked. Note the circled area.
Gradual transition check box cleared. Note the circled area.
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Draft Analysis Using the settings in draft analysis, you can verify draft angles on model faces or you can examine angle changes within a face. To apply a draft analysis to verify draft angles:
1.
Open the model, and click
in the Mold Tools toolbar, or click Tools, Draft Analysis.
2.
Under Analysis Parameters, do the following: •
Select a planar face, a linear edge or an axis to indicate the Direction of Pull.
•
Note the draw direction. To change the draw direction, click Reverse Direction use the handle in the graphics area to reverse direction.
•
Enter a Draft Angle
•
Click Face classification to conduct a face-based draft analysis.
•
If necessary, click the Find steep faces check box. Use steep faces when the model includes curved faces. Selecting Find steep faces separately displays faces that have a portion of the face with less angle than the specified draft angle to the direction of pull.
. You can also
.
When you select Find steep faces, two additional categories, are displayed: o
Positive steep faces
o
Negative steep faces These categories function in the same manner as other face categories (positive draft, negative draft, and so on), but only apply to steep faces.
•
Click Calculate.
The regions of the model display the colors appropriate to their draft angle.
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3.
Examine the results. Note that the colors may not exactly match with the images below, and will depend on your computer settings.
Positive draft
Negative draft Requires draft
Draft Required. Displays faces that require correction. These are faces with an angle less than the specified draft angle. If the model includes curved faces and you checked the Find steep faces check box, examine steep faces as well. When analyzing the draft for surfaces, an additional Face classification criterion is added: Surface faces with draft. Since a surface includes an inside and an outside face, surface faces are not added to the numerical part of the classification (Positive draft and Negative draft). Surface faces with draft lists all positive and negative surfaces that include draft.
Draft Required
Negative steep faces
Positive steep faces Straddle faces. Displays faces that include a combination of positive and negative draft. TIP: To examine draft angles within a face in more detail, use a contour map. Perform the analysis without using Face classification. See "To apply a contour map of draft angles" below. 4.
You can change the default colors, and toggle between Show
or Hide
.
NOTE: You can change colors or toggle the display before or after you complete the steps under Analysis Parameters. •
To change colors: Click Edit Color, select a color from the Color dialog box, and click OK.
•
To Show/Hide a draft category: Click Show
or Hide
to toggle. The default is Show
. TIP: You can combine the Show or Hide function with the number on the color swatch in each draft category to help identify small faces that have a draft problem. 5.
Click OK
to exit the draft analysis. If you want to save the draft analysis colors with the part, click OK.
The next time you open the part, it will use the colors used with the draft analysis.
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To apply a contour map of draft angles:
1.
Open the model, and click
2.
Under Analysis Parameters, do the following:
3.
in the Mold Tools toolbar, or click Tools, Draft Analysis.
•
Select a plane, a planar face, a linear edge or an axis from the graphics area to indicate the Direction of Pull.
•
Note the draw direction. To change the draw direction, click Reverse Direction
•
Enter a Draft Angle
.
.
Click Calculate. The regions of the model display a color according to their draft angle.
Move the pointer over the different areas on the model to display the draft angle at that location.
4.
Under Color Settings, you can toggle between two display modes, and change the colors. •
Clear the Gradual transition check box to display a uniform color gradient. This is the default display.
•
Check the Gradual transition check box to display color variations that reflect the transitions in the draft angles on the model. This displays the range of angles (positive draft through negative draft), based on the Draft Angle you specified. Gradual transition is especially useful with complex models with numerous variations in the draft angle. TIP: You can see the individual faces of the model during a color contour calculation by specifying Display HLR edges in shaded mode
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Gradual transition check box cleared 5.
Gradual transition check box checked.
To change the color display, click Edit Color, select a color from the Color dialog box, and click OK. NOTE: If you selected Gradual transition, you can change only the colors for Positive draft and Negative draft.
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6.
If necessary, under Draft Angle, enter a new value to view angular changes in smaller steps.
7.
If you changed the values under Draft Angle or changed the type of display, click Calculate to re-examine the results.
8.
Click OK
.
Example of Draft Analysis
Part with no draft analysis applied
Positive draft
Negative draft
Draft required
Deviation Analysis The Deviation Analysis tool is a diagnostic tool that calculates the angle between faces. You can select a single edge or a series of edges. The edges can be between faces on a surface, or any edges on a solid. The analysis is based on the number of sample points that you select along the edges. You can examine operations which fail or have the potential for failure in any of the following situations: •
Molds. Investigate problems with mold tooling along the split line of the mold, in conjunction with the Draft Analysis tool. Example
•
Fillets. Identify potential problems along tangent faces where a fillet operation fails. Example
•
Tangency requirements. Check along the edges of lofts, sweeps, or surface fills and verify that tangency requirements are met.
•
Maximum deviation. Identify problem areas along the edges of sweeps, lofts, or surface fills where there is maximum deviation. Example
After you use the Deviation Analysis tool, you can modify the results by controlling the appropriate entities within the model. For example, when you examine an edge along a surface fill, deviation analysis results vary according to the following: •
Curvature Control. Select Contact or Tangent. Normally, Tangent yields a lower deviation between adjoining faces.
•
Optimize surface. Use the standard patch, or, with two, three, and four sided edges, apply the Optimize surface option to use the more efficient simplified patch.
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To apply a deviation analysis:
1.
Open the model with the edges you want to examine. Note: The sample model on the right uses a surface fill.
2.
Click Deviation Analysis Tools, Deviation Analysis.
on the Tools toolbar, or
The Deviation Analysis PropertyManager appears.
3.
Under Analysis Parameters
, select the edges in the graphics area that you want to examine.
4.
Use the slider to select the Number of Sample Points
to include in the analysis.
NOTE: The number of points is based on the size of the window client area. If you select more than one edge, the sample points are distributed across the selected edges, proportional to the edge length. 5.
Click Calculate. The colored arrows display the amount of deviation. The results appear for the following criteria between the adjacent faces: • • •
Maximum Deviation - the maximum deviation error along the selected edge. Minimum Deviation - the minimum deviation error along the selected edge. Average Deviation - the average between the maximum and the minimum values along the selected edge.
NOTE: You can change the display colors for Maximum Deviation and for Minimum Deviation. To change the colors, click Edit Color to display the Color palettes, select a color for each deviation type, and click OK or Calculate to apply the new colors.
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Example of Deviation Analysis with Mold Part
Deviation analysis along edges of mold parts
Example of Deviation Analysis with Fillets
Sweep with edges to fillet
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Example of Deviation Analysis with Lofts
Deviation analysis along edge of loft using 3D sketches Example of Deviation Analysis with Surface Fill
Deviation analysis along edge of surface fill
Manipulation of Features Move/Size Features with Feature Handles Provides handles so you can move, rotate, and resize extruded and revolved features. With multibody parts, you can use Move/Size Features to individually move, resize, or rotate each body in the multibody part document. To display and use the feature handles:
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1.
Click Move/Size Features
on the Features toolbar.
2.
Click the feature you want to work with, either in the FeatureManager design tree or in the graphics area. Double-click the feature to display both the handles and the dimensions of the feature.
3.
Drag the rotate handle
or the resize handle
, to rotate or resize the feature.
4.
To move a feature, you can either: •
Drag the feature to a new location with the move handle. If the feature has locating dimensions or relations that restrict its movement, a message asks you if you want to delete or keep the relations or dimensions. - or -
•
Hold the Alt key as you drag to maintain the dimensions and relations on the feature. The feature is allowed to move, but only in the directions not already controlled by dimensions or relations.
NOTE: When you drag a feature with the move handle, any child feature moves with its parent. When you hold down Shift and drag the child feature, the software tries to maintain the position of the child relative to the parent. This position is based on the child’s dimensions and relations. However, in some cases (for example, when the child feature is under defined, or dimensioned to something other than its parent), the child may not move with the parent as expected. Move/Copy Bodies With multibody parts, you can move, rotate, and copy bodies and surfaces. To move a body or a surface:
1.
Click Move/Copy Bodies
on the Features toolbar, or click Insert, Features, Move/Copy.
The Move/Copy Body PropertyManager appears. 2.
Select the surface or the body in the graphics area. The name of the selected item appears under Bodies to Move/Copy.
3.
Under Translate: Enter values for Delta X
, Delta Y
, and Delta Z
.
- or a.
Click to highlight the Translation Reference box
.
b.
Select an edge in the graphics area to define the translation direction.
c.
Type a Distance
. Type a negative number to switch the translation direction.
- or a.
Click to highlight the Translation Reference box
b.
Select a vertex in the graphics area.
c.
If necessary, click To Vertex
.
to select a second vertex.
The surface moves the direction and distance defined by the vertices. Both the original position of the surface or body and a preview of the moved surface or body appear. NOTE: All changes you make in the PropertyManager are reflected dynamically in the graphics area. 4.
Click OK
.
The surface or body appears in the moved position. Example of move body parts and move multibody parts
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To rotate a body or a surface:
1.
Click Move/Copy Bodies
2.
Select a surface or a body in the graphics area.
3.
Under Rotate: •
Enter values for X Rotation Origin A square marker
•
on the Features toolbar, or click Insert, Features, Move/Copy.
, Y Rotation Origin
, and Z Rotation Origin
.
appears in the graphics area to show the location of the origin.
Enter values for X Rotation Angle Rotation Angle - or -
(angle around the X axis), Y Rotation Angle
, and Z
.
•
Click to highlight the Rotation Reference Entity box
.
•
Select an edge in the graphics area to define the rotation axis.
•
Enter an Angle
.
The original position of the surface or the body and a preview of the rotated surface or the body appear. 4.
Click OK
.
The surface or body appears in the rotated position. Example of rotate solid bodies or surfaces To copy bodies or surfaces:
1.
During moving or rotating a surface or a body, select the Copy check box in the Move/Copy Bodies PropertyManager.
2.
Enter the Number of Copies
.
Previews of the copied surfaces or bodies appear in the graphics area. Each copy increments by the values entered for translation and rotation. Example of copy and rotate bodies Example of Move Bodies
Preview of move multibody solid parts Delta X: 10mm Delta Y: 40mm Delta Z: -30mm
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Preview of move multibody solid parts Translation Reference: vertex indicated To Vertex: vertex indicated
Preview of move multibody surface parts Delta X: 20mm Delta Y: 50mm Delta Z: 0mm
Preview of move multibody surface parts Translation Reference: Point at origin To Vertex: Vertex indicated
Example of Rotate Bodies
Preview of rotate multibody solid parts (the arrow indicates the X-Y rotation origin) X Rotation Origin: 10mm
Preview of rotate multibody solid parts Rotation Reference: Point at sketch origin, as indicated
Y Rotation Origin: 20mm
X Rotation Angle: 12°
X Rotation Angle: 80°
Y Rotation Angle: 16°
Preview of rotate surface (the arrow indicates the X-Y rotation origin) X Rotation Origin: 40mm
Preview of rotate surface Translation Reference: Point at sketch origin, as indicated
Y Rotation Origin: -50mm
X Rotation Angle: 20°
X Rotation Angle: 20°
Z Rotation Angle: -5°
Z Rotation Angle: -5°
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Example of Rotate and Copy Bodies
Preview of rotate and copy multibody solid parts X Rotation Origin: 40mm
Preview of rotate and copy multibody solid parts Rotation Reference: Coordinate system created at the sketch origin
Y Rotation Origin: 40mm X Rotation Angle: 12° X Rotation Angle: 45° Y Rotation Angle: 16°
Preview of rotate and copy surface Rotation Reference: Coordinate system created at the sketch origin
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Preview of rotate and copy multibody surfaces Rotation Reference: Sketch point on plane, parallel to top plane
X Rotation Angle: 30°
X Rotation Angle: -23°
Y Rotation Angle: 5°
Y Rotation Angle: -5°
Z Rotation Angle: 15°
Z Rotation Angle: 0°
Combine Bodies You can combine multiple solid bodies to create a singled-bodied part or another multibody part. There are three ways to combine multiple solid bodies: •
Add. Combines solids of all selected bodies to create a single body.
•
Subtract. Removes overlapping material from a selected main body.
•
Common. Removes all material except that which overlaps.
To use the Add or Common operation type:
1.
Click Combine
on the Features toolbar, or click Insert, Features, Combine.
The Combine1 PropertyManager appears. 2.
Under Operation Type, click Add or Common.
3.
Under Bodies to Combine, select the bodies in the graphics area, or select the bodies from the Solid Bodies folder in the FeatureManager design tree.
4.
Click Show Preview to preview the feature.
5.
Click OK
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To use the Subtraction operation type:
1.
Click Combine
on the Features toolbar, or click Insert, Features, Combine.
The Combine1 PropertyManager appears. 2.
Under Operation Type, click Subtract.
3.
Under Main Body, select the body to keep from the graphics area, or select the body from the Solid Bodies folder in the FeatureManager design tree.
4.
Under Bodies to Subtract, select the bodies whose material you want to remove.
5.
Click Show Preview to preview the feature.
6.
Click OK
.
Delete Body You can delete bodies using the Delete Body feature. To use Delete Body:
1.
Click Delete Solid/Surface
on the Features toolbar, or click Insert, Features, Delete Body.
The Body-Delete PropertyManager appears. 2.
Under Bodies to Delete, select the bodies from the graphics area.
3.
Click OK
.
Choose Option The Choose Option dialog box appears when you select several entities on a model and press Delete. The dialog box is dynamic, with the appropriate selections available depending on what entities you select on the model. Options include the following: •
Delete Feature. Deletes the entire feature and any associated features.
•
Delete Face(s). Displays the Delete Face PropertyManager.
•
Delete Hole(s). Deletes any holes created with a sketch, the Simple Hole, or the Hole Wizard features. From the Delete Face PropertyManager, you can select one or more faces on the solid model to create surfaces.
For example, if you select the two items on the model, as shown below, and press Delete, the Choose Option dialog box appears. Because the Hole Wizard holes were drilled on the non-planar surface prior to creating the offset surface feature, the holes on the offset surface do not appear on the FeatureManager design tree. •
•
•
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Delete Feature. Select to delete the surface offset. You can also delete the cut and the fillet along the edges of the cut. Delete Face(s). Select to display the Delete Face PropertyManager, from which you can delete any other faces on the model. Delete Hole(s). Select to delete the hole on the offset surface.
Select Detailed Preview Detailed Preview •
Ribs
•
Extrudes
•
Draft
is available from the PropertyManager with the following features:
You can use the Detailed Preview PropertyManager with multibody parts to enhance detail and select entities to display: •
Highlight new or modified faces. Inspect what was changed from the previous edit. New or modified faces are highlighted in color, as opposed to appearing shaded.
•
Show only new or modified bodies. Display only new or modified bodies. All other bodies are hidden.
New sketch prior to extrusion
Selected Contours for extrude feature
With the Detailed Preview PropertyManager, the selected options control what displays in the graphics area:
Neither option selected
Show only new or modified bodies selected
Highlight new or modified faces selected
Both options selected
Extrude feature applied to new sketch
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To use detailed preview:
1.
Click Detailed Preview
in the PropertyManager.
2.
In the Detailed View PropertyManager: Click Highlight new or modified faces or Show only new or modified bodies.
3.
Click Detailed Preview
to return to the original PropertyManager.
Wrap This feature wraps a sketch onto a planar or non-planar face. You can create a planar face from cylindrical, conical, or extruded models. You can also select a planar profile to add multiple, closed spline sketches. The wrap feature supports contour selection and sketch reuse. The sketch plane must be tangent to the face, allowing the face normal and the sketch normal to be parallel at the closest point. To create a wrap feature:
1.
Select the sketch you want to wrap from the FeatureManager design tree.
2.
Click Wrap
3.
In the PropertyManager, under Wrap Parameters: a.
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on the Features toolbar, or click Insert, Feature, Wrap.
Select an option: •
Emboss. Create a raised feature on the face.
•
Deboss. Creates an indented feature on the face.
•
Scribe. Creates an imprint of the sketch contours on the face.
b.
Select a non-planar face in the graphics area for Face for Wrap Sketch
c.
Set a value for Thickness
d.
Select Reverse direction, if necessary.
.
.
4.
Under Pull Direction, if Emboss or Deboss is selected, click Pull Direction edge, or a plane. If you select a plane, the direction is normal to the plane.
5.
Click OK
, and select a line, linear
.
Example of Pull Direction Wrap Feature
Pull direction - Plane A
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Pull direction - Plane B
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7 Parts
Overview and Editing Parts Parts Overview The 3D part is the basic building block of the SolidWorks mechanical design software. This section describes parts and some ways to work with them, including: •
Modeling solid multibody parts
•
Applying custom properties
•
Editing properties of features and faces
•
Editing, moving, and copying
•
Using color
•
Controlling material properties
•
Using equations
•
Dependency editing using suppress and unsuppress
•
Derived parts and external references
•
Splitting parts
•
Displaying a section view of the model
•
Annotating parts
•
Specifying lighting characteristics and material properties
Edit Definition In a parts document, you can perform the following types of feature editing operations: •
Edit the definition, the sketch, or the properties of a feature.
•
View the parent and child relationships of a feature.
•
Use the feature handles to move and resize features.
•
Control the access to selected dimensions.
•
Change the order in which features are reconstructed when the part is rebuilt (see Drag and Drop Features).
•
Roll back the part to the state it was in before a selected feature was added.
To perform some of these operations, you use the icons in the FeatureManager design tree, where the features are listed in the order in which they are created. See also color and appearance of parts.
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To edit the definition of a feature:
You can edit the definition of a feature to change its parameters. For example, you can edit the depth of an extruded feature, or the selected edges for a fillet. 1.
Click a feature in the FeatureManager design tree or the graphics area.
2.
Click Edit, Definition or right-click and select Edit Definition, and depending on the selected feature type, the appropriate dialog box appears.
3.
Edit the definition in the dialog box by specifying new values or options.
4.
Click Apply or OK to accept the changes; click Cancel to discard the changes.
Properties of Features and Faces Feature and face properties include: •
Name
•
Color
Feature properties also include the capability to suppress (and then unsuppress) the feature. Suppressing temporarily removes the feature from the model, without deleting it. This can be used to simplify the model, or to create part configurations. See creating a configuration manually. To edit feature properties:
1.
In the FeatureManager design tree or in the graphics area, select one or more features, then click Edit, Properties, or right-click the features and select Feature Properties. (To select multiple features, hold down Ctrl while selecting.)
2.
Enter a new Name if desired in the Feature Properties dialog box.
3.
To suppress the feature, select the Suppressed check box.
4.
To change the appearance of the feature, click Color. The Entity Property dialog box appears.
5.
•
To change the feature color, click Change Color. Select a color from the Color palette or define a custom color.
•
To change material properties such as shininess and transparency, click Advanced.
•
To restore the feature to the original color of the part, click Remove Color.
Click OK.
To edit face properties:
1.
Right-click one or more faces and select Face Properties. The Entity Property dialog box appears.
2.
Enter a face Name if desired. (Face names are used under certain conditions when replacing components in an assembly. See replacing components in an assembly.
3.
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•
To change the face color, click Change Color. Select a color from the color palette or define a custom color.
•
To change material properties such as shininess and transparency, click Advanced.
•
To restore the face to the original color of the feature it belongs to, click Remove Color. (Face colors override colors specified for the feature.)
Click OK.
Dynamic Feature Editing You can see a dynamic feature preview when you drag the entities of a sketch, either with or without opening the sketch itself. The preview updates when you release the mouse button after dragging. To display a dynamic preview without opening a sketch:
1.
Click Move/Size Features
on the Features toolbar.
2.
Click the feature you want to edit. The sketch is highlighted in the graphics area. If more than one sketch is used to create the feature (for example, if the selected feature is a loft or a sweep), all the sketches used in the feature are highlighted. Notice that the model is not rolled back when you edit a feature this way.
3.
Drag the sketch entities as needed. As you modify the sketch, the preview shows you what the resulting feature will look like.
4.
When you are satisfied with the feature, click an empty area of the document window or press Esc to clear the selected sketch entity.
Select feature
Resize feature
Feature resized
NOTE: Even though the fillet feature was created separately from the cut extrude, it moves and changes size with the cut extrude because of parent and child relations. To display a dynamic preview while editing a sketch:
1.
Click Move/Size Features
on the Features toolbar.
2.
Double-click a sketch to open the sketch for editing. The model is rolled back to the selected feature.
3.
Modify the sketch by dragging the sketch entities, changing the dimensions, adding relations, and so on. As you modify the sketch, the preview shows you what the resulting feature will look like.
4.
Exit the sketch to update the feature. See Edit Sketch for more information.
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Chapter 7 Parts
Copying Features You can copy features from one face to another on the same model. You can also copy features from model to model. To copy a feature:
1.
With your cursor highlighting the feature, hold down Ctrl and drag the feature where needed. To copy more than one feature, hold down Ctrl as you select the features.
2.
Drop the feature on the same face or to a different face. If the feature includes locating dimensions or relations that restrict its movement, a dialog box is displayed. You can Delete the relations or dimension, Dangle them, or Cancel copy.
To re-attach dangling dimensions:
1.
Select the sketch and click Edit Sketch. The dangling dimensions are displayed in a different shade.
2.
Click the dangling dimension and drag the red handle to a new attachment point. As you drag, the pointer is displayed until you are on an edge or a vertex that is suitable to re-attach the dimension.
Cut extrude feature with location dimensions 3.
Copy of cut extrude feature with dangling dimensions
Red handle indicates the dangling attachment point
Release the pointer to re-attach the dimension to the new edge or vertex.
To copy features from one part to another part:
Tile the windows, then drag the features from one window to another, or use the Copy tools on the Standard toolbar.
and Paste
Color of Parts You can apply a color to the entire part, selected features (including surfaces or curves), or selected model faces. You can also modify the color by manipulating the shaded appearance of the model. NOTE: Color selections made with the Edit Color tool supercedes colors set on the Document Properties tab. To change the shaded appearance of a part:
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1.
Click Tools, Options, Document Properties, Colors.
2.
Under Model\Feature colors, select Shading.
3.
Click Edit and select a color from the Color palette or click Define Custom Colors and define a color of a new shade or hue.
4.
Click OK to close the Color palette, and click OK to close the Document Properties - Colors dialog box.
To change the color of selected features or the entire part:
1.
Select each feature from the FeatureManager design tree or from the graphics area (use Ctrl to select multiple features).
2.
Click Edit Color color.
3.
If you selected items from the graphics area, in Apply to select Face, Feature, Body, or Part.
4.
Click Apply to see a preview then click OK.
on the Standard toolbar, and select a color from the Color palette or select a Custom
All features selected on the model
Color applied to all features
Color applied to selected features
Material Properties and Appearance of Parts You can change the way light affects any shaded model by changing the material properties. You can apply different properties to the entire model, to a face on the model, or to a feature. Material properties are independent of color. You can also combine the controls in the Material Properties dialog box with lighting, to create different effects. NOTE: The shape of the model, the shading, as well as the lighting, affects material properties. The system comes with a default settings which make the model appear "normal". With some models, changing material properties displays negligible differences between a minimum and a maximum setting. Setting Material properties and lighting both require user experimentation. To change material properties for a part:
1.
Click Tools, Options, on the Document Properties tab, Colors or right-click the icon in the FeatureManager design tree and select Document Properties.
2.
In Model/Feature colors, select Shaded.
3.
Click Advanced to display the Material Properties dialog box.
4.
Use the sliders to control material display properties: •
Ambient. How light is reflected and scattered by other objects
•
Diffuse. How light is scattered equally in all directions on the surface
•
Specularity. How surfaces exhibit highlights
•
Shininess. How solid object alternate between a glossy, reflective surface and a dull, matte surface
•
Transparency. How much light passes through the surface
•
Emission. How light projects from the surface
5.
Click Apply and click OK.
6.
Click OK to close the Document Properties - Colors dialog box.
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Appearance and Material Properties
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All values set to default
Diffuse. Slider set to midpoint (default is maximum)
Ambient. Slider set to minimum (default is maximum)
Shininess. Slider set close to maximum (default is 1/3 of maximum)
Transparency. Slider set to halfway between maximum and minimum (default is minimum)
Emission. Slider set towards maximum (default is minimum)
Edit Color Use Edit Color to change the color of a face, feature, part, or assembly when in shaded mode. NOTE: Colors selelections made with the following procedures supercede colors set on the Document Properties tab. To edit the color of one or more faces in a part document:
1.
Click Edit Color
on the Standard toolbar.
2.
In the graphics area, select one or more faces.
3.
Select a color from the Color palette or define a custom color.
4.
In the Apply To box, make sure Face is selected.
5.
Click OK. Face selected
To edit the color of one or more features in a part document:
1.
Click Edit Color
on the Standard toolbar.
2.
In the FeatureManager design tree, click the name of one or more features. - or In the graphics area, click one or more features.
3.
Select a color from the Color palette or define a custom color.
4.
In the Apply To box, make sure Feature is selected.
5.
Click OK.
Feature (base revolve) selected
To edit the color of a part, component, or assembly:
1.
Click Edit Color
on the Standard toolbar.
2.
In the FeatureManager design tree, click the name of the part, component or assembly.
3.
In the Edit Color dialog box, select a color from the Color palette or define a custom color. - or To restore the default color, click Remove.
4.
Click OK.
Assembly with colors applied to parts
To edit the color of a component in an assembly:
1.
Select the component in the FeatureManager design tree or in the graphics area.
2.
Click Edit Color
3.
In the Edit Color dialog box, select a color from the Color palette or define a custom color and click OK.
on the Standard toolbar.
- or To use the assembly’s default color, click Use assembly, and click OK. NOTE: To remove the color layers that you applied, click Undo
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or click Edit, Undo Edit Color.
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Chapter 7 Parts
Entity Property Displays the properties of faces, surfaces, or edges. To change the color of a face or surface (or multiple faces or surfaces):
1.
Right-click a face or surface, and select Face Properties - or To change the color of multiple faces or surfaces, hold down the Ctrl key and click the faces or surfaces, then right-click and select Face Properties.
2.
Change the color with one of the following methods: •
Change the numeric values for Red, Green, or Blue.
•
Click Remove Color to use the part color.
•
Click Change Color and select a color from the Color palette or click Define Custom Colors and define a new color.
•
Click Advanced and use the sliders to increase or decrease advanced material property values such as ambient, shininess, transparency, and so on.
Example 3.
Under Entity Information, type a name for the face in the Name box, or change the name by typing a new name, if desired.
4.
Click OK.
To change the name of an edge, face, or surface:
1.
Right-click an edge, face, or surface.
2.
Select Edge Properties or Face Properties. The Entity Property dialog box appears.
3.
Under Entity Information, change the name for the edge, face, or surface in the Name box.
4.
Click OK. The name of the edge, face, or surface is changed.
Change Value for Red Change the color of the selected face by changing the numeric value for red. The color displays when you select Shaded view. Change Value for Green Change the color of the selected face by changing the numeric value for green. The color displays when you select Shaded view. Change Value for Blue Change the color of the selected face by changing the numeric value for blue. The color displays when you select Shaded view. Change Color To change the color for the selected face when in Shaded view, click this button. Select a color from the color blocks or create a color with the custom color palette. Use Part Color To use the default part color for the selected face when in Shaded view, click this button. The part color is displayed in the preview box.
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Advanced Properties Use the slider controls to change the material display properties of the selected face. For example, you can make the face more or less transparent (Transparency), or control how much light is projected from the face (Emission). The material display properties are independent of color. You can also combine the controls in the Advanced Properties dialog box with lighting, to create different effects. To set Advanced Properties for a model face:
1.
Right-click a model face and select Face Properties.
2.
In the Entity Property dialog box, click Advanced.
3.
Set the sliders as needed. •
Ambient - light reflected and scattered by other objects
•
Diffuse - light scattered equally in all directions on the surface
•
Specularity - ability to reflect light from a surface
•
Shininess - a glossy, highly reflective surface
•
Transparency - ability to pass light through the surface
•
Emission - ability to project light from the surface
4.
Click Apply to see a preview, or click OK to set the value.
5.
Click OK to close the Entity Property dialog box.
NOTE: The values displayed in the Advanced Properties dialog box are initially system defaults. You have the option to change the values in the Advanced Properties dialog box, and save the new values to a document template. Sample Advanced Properties
System default setting for all sliders
Diffuse slider set to minimum (0%)
Transparency slider set to 50%
Emission slider set to 50%
Only the individually specified slider was moved in each of the examples above. System default were as follows: • • •
Ambient - 100% Diffuse - 100% Specularity - 100%
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• • •
Shininess - 25% Transparency- 0% Emission - 0%
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Chapter 7 Parts
Multibody Parts Multibody Overview Part documents can now contain multiple solid bodies. A folder named Solid Bodies
appears in the
FeatureManager design tree when there are solid bodies in a single part document. The number of solid bodies in the part document is displayed in parentheses next to the Solid Bodies
folder.
For example, when you design a spoked wheel, you know the requirements of the rim and the axle. However, you do not know how to design the spoke. With multibody parts, you can create the rim and axle, then create the spoke to connect the bodies.
You can manipulate multibody solids the same ways you manipulate single solid bodies. For example, you can add and modify features, and change the names and colors of each solid body. You can hide and show solid bodies in the FeatureManager design tree. You can create multiple solid bodies from a single feature with the following commands: •
Extrude boss and cut (including thin features)
•
Revolve boss and cut (including thin features)
•
Sweep boss and cut (including thin features)
•
Surface cut
•
Boss and cut thicken
•
Cavity
Modeling techniques that you can use in a multibody environment include the following: •
Bridging
•
Local Operations
•
Symmetry Modeling
•
Body Intersection
•
Tool Body Modeling
•
Multibody Versus Assemblies
Multibody Parts Versus Assemblies Multibody parts should not replace the use of assemblies. A general rule to follow is that one part (multibody or not) should represent one part number in a Bill of Materials. A multibody part consists of multiple solid bodies that are not dynamic. If you need to represent dynamic motion among bodies, use an assembly. Tools such as Move Component, Dynamic Clearance, Mates, and Collision Detection are available only with assembly documents. You can save an assembly as a multibody part document. This enables you to save complex assemblies as smaller part documents to facilitate sharing files. For example, you have a design of an intricate motor assembly and a potential customer wants to know if it fits in their frame. You can save the motor assembly as a part document and send the part file to potential customers without risking design integrity or transmitting a large assembly document file.
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To save an assembly as a multibody part document:
1.
Open an assembly document.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set the Save as type to Part (*.prt, *.sldprt). A set of options appears at the bottom of the dialog box.
4.
Select one of the following: •
Exterior Faces to save the exterior faces as Surface Bodies
.
•
Exterior Components to save the visible components as Solid Bodies
•
All Components to save all components as Solid Bodies
.
.
NOTE: Components that are hidden or suppressed are not saved when you select All Components. 5.
Click Save.
Modeling Techniques Body Intersection For the body intersection multibody technique, you use the Combine feature and its Common option. Body intersection is a quick way to create complex parts with very few operations, which can result in faster performance. The operation takes multiple solid bodies that overlap one another and leaves only the intersecting volumes of the bodies. For most models that can be represented fully by two or three drawing views, this technique can be used by intersecting either two or three extruded solids. The extrusion sketches are the solid lines represented in the two or three views. The following example shows this technique with the intersection of two extrusions.
Front
Top
Isometric
To create the part described above, you begin with the base part:
And then select the Common option of the Combine feature to use only the overlapping material of the base part.
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Bridging Bridging is a commonly used technique in a multbody environment. Bridging creates a solid that connects multiple solid bodies. This technique is useful when you create portions of the model first and create the connecting geometry afterwards.
For example, when designing a golf club, you might know the specifics of the head and shaft design, but not necessarily how they are connected. You can design the head and the shaft first, then bridge the two bodies. Local Operations You use local operations when you want to perform operations on certain portions of a mulitbody model, but not on others. For example, you design a double-ended measuring cup. You need to shell the two cups and fillet them. However, you do not want to shell the piece that connects the two cups. You can create the part and perform the feature operations on the separate bodies.
When modeling the double ended measuring cups, first create the cups as two separate solid bodies.
Next, shell each body.
Model the connection bar and merge bodies.
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Lastly, fillet the edges. Symmetry Modeling Symmetry modeling simplifies the creation of axis-symmetric parts and also speeds performance for these types of parts. In this approach you make one symmetric body, pattern the bodies to obtain the remaining geometry, then use the Combine feature to glue all of the bodies together. You can use multiple patterns and combine features to create an entire model. For instance, the example below shows the design progression of a symmetrical part. Begin by building the basic piece that you pattern later.
Next, add the end piece, keeping this body separate, but adjacent.
Then pattern the basic piece.
Lastly, mirror the entire part, including the end piece, and combine the bodies.
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Chapter 7 Parts
Tool Body Modeling Use tool body modeling to create complex multibody tools to remove material from a solid body, or add complex shapes to geometry. You create common geometrically shaped bodies in separate part documents, then use the Insert, Part tool to create a multibody part document.
Initial part
Insert part
Use the Combine feature to remove material of inserted part.
Controlling Parts Parent and Child Relations Features are normally built upon other existing features. For example, you create a base extrude feature and then create additional features such as a boss or cut extrude. The original base extrude is the parent feature; the boss or cut extrude is a child feature. The existence of a child feature depends on the parent. A parent feature is an existing feature upon which others depend. Parent/Child include the following characteristics: •
You can only view the relations; you cannot edit them.
•
You cannot reorder a child feature before it’s parent.
To view Parent/Child relations:
1.
In the FeatureManager design tree or in the graphics area, right-click the feature whose relationships you want to see.
2.
Select Parent/Child from the menu.
Equations Creates mathematical relations between model dimensions, using dimension names as variables. When using equations in an assembly, you can set equations between parts, between a part and a sub-assembly, with mating dimensions, and so forth. When you delete a feature or dimension that is used in an equation, you have the option of deleting the equation or not. NOTE: Dimensions driven by equations cannot be changed by editing the dimension value in the model.
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To add an equation:
1.
Click
or Tools, Equations.
2.
Click Add.
3.
In the model or the FeatureManager design tree, double-click on the feature that contains the first dimension you want to use in the equation.
4.
Click on the dimension to paste its name into the equation. (Dimension names are in the form dimension name @ feature or sketch name.)
5.
Complete the equation by typing or clicking on the calculator buttons, or by clicking on other dimensions to paste their names. Equations are solved left to right (i.e., the dimension on the left is driven by the value on the right), in the order in which they appear in the equation list. You can use additional supported functions. You can also insert comments in equations.
6.
Click OK. The equation appears in the Equations window, and the value of the solution is shown in the Evaluates To column.
7.
Click OK, then click or Edit, Rebuild to update the model. (All equations are solved before the geometry is regenerated.) An equation folder appears in the FeatureManager design tree. Right-click the folder to delete or edit existing equations or add a new equation to the document. NOTE: When using any trig function in an equation or dimension dialogue, the value of the angle is interpreted as radians. For example, sin(90) is evaluated as .89 (90radians) not 1.0 (90deg).
To edit equations:
1.
Click
or Tools, Equations, and click Edit All, or right-click
and select Edit equation.
2.
Edit the equations. Each equation must be on a separate line, and dimension names must be enclosed in quotes.
3.
Click OK to close the Edit Equations window.
4.
Click OK to close the Equations window.
5.
Click
or Edit, Rebuild.
Edit and Delete Equations To edit an equation:
1.
Click Equations
or click Tools, Equations and then click Edit All.
- or Right-click the Equations folder 2.
, and select Edit Equation.
In the Edit Equations dialog box, edit the text of the equations as needed, and click OK. The revised equation is displayed in the Equations dialog box. You can also cut and paste equations here to change the order, if necessary. If you make a mistake, click Undo to clear each consecutive value in the New Equation dialog box. You can clear one value each time you click Undo.
3.
Click OK, then click Rebuild
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To delete an equation:
1.
Click Equations - or -
or click Tools, Equations.
Right-click the Equations folder
, and select Delete Equation.
2.
Click the equation number or the status marker for the equation to delete, and click Delete in the Equations dialog box.
3.
Click OK, then click Rebuild
.
Operators and Constants Function
Name
Notes
sin (a)
sine
a is the angle expressed in radians; returns the sine ratio
cos (a)
cosine
a is the angle expressed in radians; returns the cosine ratio
tan (a)
tangent
a is the angle expressed in radians; returns the tangent ratio
atn (a)
inverse tangent
a is the tangent ratio; returns the angle in radians
abs (a)
absolute value
returns the absolute value of a
exp (n)
exponential
returns e raised to the power of n
log (a)
logarithmic
returns the natural log of a to the base e
sqr (a)
square root
returns the square root of a
int (a)
integer
returns a as an integer
sgn (a)
sign
returns the sign of a as -1 or 1 For example: sgn(-21) returns -1
pi
3.14...
Constant pi
Equation Comments and Status Comments in Equations You can add comments to equations, to document your design intent. You can also use comment syntax to prevent an equation from being evaluated. To add a comment to an existing equation:
1.
Click Equations
or click Tools, Equations.
- or Right-click the Equations 2.
folder and select Edit Equation.
If there is only one equation, the Equations and the Edit Equations dialog boxes are displayed. If there is more than one equation, select the equation and click Edit all to display the Edit Equations dialog box.
3.
Type a single quote (‘) at the end of the equation, then enter the comment. Anything after the single quote is ignored when the equation is evaluated. For example: "D2@Sketch1" = "D1@Sketch1" / 2 ‘height is 1/2 width
7-16
To add a comment to a new equation:
1.
Click Equations
or click Tools, Equations.
Click Add and enter the equation. 2.
Type a single quote (‘) at the end of the equation, then enter the comment. Anything after the single quote is ignored when the equation is evaluated. If you want to temporarily prevent an equation from being evaluated, but you do not want to delete it, place a single quote before the equation. The equation is then interpreted as a comment, and it is ignored.
Operators and Functions The following operators and functions are supported: + (plus sign) addition – (minus sign) subtraction * (asterisk) multiplication / (forward slash) division ^ (caret) exponentiation You can also use pi in equations. Its value is calculated to the number of decimal places specified for the document. Equations can also use additional operators and constants. Equation Status When you delete a feature or a dimension that is used in an equation, the software asks you if you want to delete the equation also. Because the order of solving equations is important, you may prefer to keep the equation, and edit it later. If you keep the equation, it has Not Solved status, and is marked with a red exclamation point dialog box. Equations with Solved status are marked with green check marks .
in the Equations
When you rename an assembly that includes an equation between assembly components, the equation is marked with a Read Only status .
Shared Values Using shared values, enables you to link dimension values using named variables. You can set the value of several dimensions to be equal without using multiple equations or relations. When dimensions are linked in this way, any member of the group can be used as a driving dimension. Changing any one of the linked values changes all others to which it is linked. The variable name you specify becomes the name of the linked dimensions, and appears in the Name box of the Dimension Properties dialog box. To link dimension values:
1.
Right-click one of the dimensions that you want to link, and select Link values. The Shared Values dialog box appears. The Value box displays the value of the selected dimension, but you may not change it here.
2.
Enter a Name. This is the variable name that will be used as the dimension name for the linked items. NOTE: You can delete unused dimension names from the Name list. Select the name and press Delete. You cannot delete a name used by another dimension.
3.
Click OK.
4.
Right-click one of the dimensions that you want to link to the first dimension, and select Link Values.
5.
Select the variable name from the list in the Name box, and click OK.
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Chapter 7 Parts
6.
Repeat for as many dimensions as needed. The values of the selected dimensions become linked to the first one. Changing any of the linked values causes the others to change.
The two linked dimensions are the side of the cube (25) and the depth of the cut extrude feature (25). When you change the side of the cube to 10, the linked value changes accordingly. To unlink dimension values:
Right-click the dimension that you want to unlink, and select Unlink value.
Measure Measures distance, angle, radius, and size of and between lines, points, surfaces, and planes in sketches, 3D models, assemblies, or drawings. When you measure the distance between two points, the delta x, y, and z distances are also displayed. When you select a vertex or sketch point, the x, y, and z coordinates are displayed. See Coordinate Systems. To use the measure tool:
1.
Click Measure
on the Tools toolbar or Tools, Measure.
The Measure dialog box appears. NOTE: While the Measure dialog box is in place, you can switch among different documents without closing the dialog box. The name of the currently active document displays in the title bar of the Measure dialog box. If you activate a document that has items already selected, the measurement information updates automatically. 2.
Under Projection on, click Screen to measure the projection on the screen, or click Plane/Face to measure the projection on a selected plane or planar face. When you measure a distance, the program calculates the projected distance (on the plane you selected), and the normal distance (normal to the plane you selected). In Detached drawings, if the model is not loaded, all measurements are reported as 2D projected data.
3.
Select the items to measure. Right-click an edge to use the Select Other, Select Midpoint, Select Tangency, Select Loop, or Clear Selections commands. The selected items appear in the Selected items list, and appropriate values are displayed in the Measurements box. New measurements update dynamically when you change selections. If you select a curve, one of the measured values is chord length. Chord length is the distance between the end points of the curve.
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If you select a single entity, the size of the entity (the length of an edge, the area of a face, and so on) is displayed in the Measurements box.
If you select two entities, the smallest distance between the entities is displayed in the Measurements box.
If a valid measurement cannot be performed with the selected entities, a message in the Measurements box states: Invalid combination of selected entities. 4.
To delete an item from the Selected items list, click the item’s name in the list and press the Delete key, or click the selected item again in the graphics area.
5.
To clear all items from the Selected items list, right-click in the graphics area, and select Clear Selections.
6.
To display the results based on a coordinate system that you defined, select the name from the Output coordinate system list.
7.
To display the results in scientific notation or using different measurement units than the units specified for the active document, click Options to display the Measurement Options dialog box. To change other material properties, click Tools, Options, on the Document Properties tab, select Material Properties.
8.
To temporarily turn off the measure function, right-click in the graphics area, and choose Select from the menu. To turn the measure function back on, click inside the Measure dialog box.
9.
Click Close to close the dialog box.
Measurement Options Use the Measurement Options dialog box to modify measurement units and the material density of parts. Units You can change the measurement units. •
Use Length unit for linear dimensions.
•
Use Angular unit for angular dimensions.
•
Select the Scientific notation check box to display measurements in scientific notation.
When you change the Length unit, the dialog box reacts dynamically depending on which Length unit you select. For example, if you select microinches, mils, inches, or feet & inches, you can also select Fractions, Denominator, and Round to nearest fraction. Display Units To display the results with units other than the units specified for the active document, select one of the following: •
View measurement settings. Displays the units specified in the Measurement Options dialog box.
•
View global settings. Displays the units specified for the active document set in Tools, Options, Document Properties, Units.
•
View system defaults. Displays the system default units for new documents set in the document template.
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Material Properties In Material Properties, select Density to change the density of the material for this document. You can enter the density value using any units. For example, if the units of the part are grams and millimeters, you can enter a density value using pounds and inches. The software converts the value to the document’s units when you click OK. You can also change the density, as well as change options for cross hatch patterns through the Tools menu. Click Tools, Options, on the Document Properties, tab click Material Properties. Accuracy Level You can select between two accuracy level settings: •
Default mass/section property precision. Calculation used in versions previous to 2003 of the SolidWorks software.
•
Maximum property precision (Slower). Provides greater accuracy of the calculation, but the computation is slower.
Dependency Editing You can suppress a feature so you can work on the model with the selected feature temporarily removed from the model. Suppressing a feature not only removes it from the display, but also from any calculations in which it may be involved. Rebuilding complex models occurs faster when features with a large amount of detail are suppressed. The Features toolbar contains the following tools to suppress and unsuppress features of the model. See Suppress and unsuppress. Suppression is governed by the parent and child relations of the features.
Tooth Cut
Unsuppressed
Suppressed
Unsuppressed
Tooth Pattern
Unsuppressed
Suppressed - The child feature is suppressed because it is dependent on the parent feature, and the parent feature is suppressed.
Suppressed - If you unsuppress the parent feature, the child feature is not automatically unsuppressed. If you unsuppress the child feature, however, the parent feature is also unsuppressed.
Dependency editing is one way to control parts. Others methods of controlling parts include:
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•
Rollback
•
Configurations
•
Design tables
Suppress and Unsuppress Features To suppress a feature:
1.
Select the feature in the FeatureManager design tree, or select a face of the feature in the graphics area. To select multiple features, hold down Ctrl as you select.
2.
Click Suppress
on the Features toolbar, or click Edit, Suppress.
- or 1.
In the FeatureManager design tree, right-click a feature, and select Properties.
2.
In the Feature Properties dialog box, select the Suppressed check box, and click OK. The selected feature is removed from the model (but not deleted). The feature disappears from the model view and is shown in gray in the FeatureManager design tree.
To unsuppress a feature:
1.
Select the suppressed feature in the FeatureManager design tree.
2.
Click Unsuppress
on the Features toolbar, or click Edit, Unsuppress.
- or 1.
In the FeatureManager design tree, right-click a feature, and select Properties.
2.
In the Feature Properties dialog box, clear the Suppressed check box, and click OK. If you want to unsuppress a suppressed feature, you must select it using the FeatureManager design tree.
To unsuppress a feature and its dependents:
1.
Select the suppressed parent feature in the FeatureManager design tree.
2.
Click Unsuppress with Dependents Dependents.
on the Features toolbar, or click Edit, Unsuppress with
The selected feature and any features that are dependent on it are returned to the model. - or 1.
Select the child feature in the FeatureManager design tree.
2.
Click Unsuppress with Dependents Dependents.
on the Features toolbar, or click Edit, Unsuppress with
The selected feature and its parent feature are returned to the model.
Derived Parts You can create a new part directly from an existing part. The new part, called a derived part, has the original part as its first feature, and it is linked to that part by means of an external reference. This means that any changes you make to the original part are reflected in the derived part. When a part has an external reference, its name in the FeatureManager design tree is followed by an arrow ->. To see the name, location, and status of the externally referenced document, right-click the derived part, and select List External Refs. There are three types of derived parts: •
Insert part
•
Mirror part
•
Derived component part
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Insert Part Use Insert Part to insert one or more base parts multiple times into a part document. Under Locate Part, select the Launch Move Dialog check box on the Insert Part PropertyManager to define a location for the inserted part. When you insert more than one part, the Locate Part PropertyManager appears automatically. To insert a part:
1.
With a part document open, click Insert Part
2.
Browse to a part document and click Open.
on the Features toolbar, or click Insert, Part.
The Insert Part PropertyManager appears. 3.
4.
Under Transfer, select any combination of the following: •
Axis. Transfers the axis information.
•
Plane. Transfers all planes from the original part.
•
Cosmetic Thread. Transfers cosmetic threads.
•
Surface. Transfers surfaces.
Click OK
.
To change the configuration of the inserted part:
1.
Right-click the part and select List External Refs.
2.
Select Use named configuration, select a configuration from the list, and click OK.
Mirror Part Mirror Part creates a mirrored version of an existing part. This is a good way to create a left-hand version and a right-hand version of a part. Because the mirrored version is derived from the original version, the two parts always match.
This type of mirroring produces a different result than using a mirror pattern. To create a mirrored, derived part:
1.
In an open part document, click a model face or plane about which to mirror the part.
2.
Click Insert, Mirror Part.
3.
In the PropertyManager, select one or more items:
4.
7-22
•
Axis. Select to use an axis as a reference point for the new, mirror part.
•
Plane. Select to use a plane as a reference point for the new, mirror part.
•
Cosmetic Thread. Select to use cosmetic thread, when present, as a reference point for the new, mirror part.
•
Surface. Select to use a surface as a reference point for the new, mirror part.
The mirrored part is opened in a new part window.
Derive Component Part Derive Component Part creates a part from an assembly component. Derived parts created this way include any features created in the context of the assembly. For example, you can create a cavity in a mold assembly, then derive and cut the pieces of the mold. The derived parts maintain the necessary references to the components in the assembly. However, you cannot insert the derived component part back into the assembly. To create a derived part from an assembly component:
1.
In an assembly document, select a component.
2.
Click File, Derive Component Part. The derived part is opened in a new part window. TIP: If you need to include assembly features, use a derived component part. Otherwise, use a base part to optimize system performance.
Split and Save Bodies Use Split to create multiple parts from an existing part. You can create separate part files, and form an assembly from the new parts if needed. With multibody parts, you can use Split to create separate bodies. Create split parts by building separate parts, or by building a single part, and using a trim tool to separate the single part into multiple parts. When you create separate parts, you have the option to Show Bodies, Hide Bodies, or Consume Bodies.
To split a part:
1.
Click Split
on the Features toolbar, or click Insert, Features, Split.
The Split PropertyManager appears. 2.
Select one or more of the following as trimming surfaces: •
Reference planes (Planes extend infinitely in all directions.)
•
Planar model faces (Faces extend infinitely in all directions.)
Original Part •
Revised Original Part
New Part
Sketches (Sketches extrude through all in both directions.)
Original Part
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•
Reference surfaces and non-planar model faces (These do not extend their boundaries. Note that internal holes on reference surfaces or non-planar model faces are closed when splitting the part.)
Original Part
New Parts
The entities appear under Trim Tool. 3.
Click Cut Part. Split lines appear on the part, showing the different bodies formed by the split. Callout boxes appear in the graphics area for up to 10 bodies. As you move your pointer
4.
over a body, the body highlights.
Select a body. The Save As dialog box appears.
5.
Type a name for the new part and click Save. The new part name appears in the Resulting Bodies list and in the callout box. NOTE: You can choose the same name for two different bodies if they are identical. If the bodies are not identical, the software does not let you choose the same name.
6.
Continue selecting bodies in the graphics area and naming new parts as needed. You can save all the bodies as new parts. The bodies that you do not save are not split. They remain with the original part.
7.
Callout boxes are displayed for 10 bodies at a time. Click Next 10 or Previous 10 to scroll through all the callout boxes for a part.
8.
Click OK
.
The new part documents open beneath the original document. Minimize the original document to see them. To split a part into multibody parts: 1.
Click Split on the Features toolbar, or click Insert, Features, Split. The Split PropertyManager appears.
2.
Select a Trim Tool in the graphics area. You can use reference planes, planar model faces, sketches, or reference surfaces as trim tools to create multibody parts. The entities appear under Trim Tool
7-24
.
In the example above, a sketch is the Trim Tool.
3.
Click Cut Part. Split lines appear on the part, showing the different bodies formed by the split. Callout boxes appear in the graphics area for up to 10 bodies. As you move the pointer body, the body highlights.
4.
over a
Select a body. The bodies you choose are listed under Resulting Bodies, and the check box selected. NOTE: Under
In the example above, there are three bodies. The center ring is selected.
is
, you can also select the
check box to choose the bodies. The bodies selected are the bodies you split. 5.
Continue selecting bodies in the graphics area or by selecting the appropriate check box
.
In the File column, double-click each split part to select it and to display the Save As dialog box. 6.
Type a name for the new part and click Save. The new part name appears in the Resulting Bodies list, and, with the complete path, in the callout box.
In the example above, the middle section was split, creating a multibody part.
NOTE: If you clear the check box for a split part after you save it, that part is no longer saved as a separate entity. It remains with the original part.
7.
Under Resultant bodies state, select one of the following: •
Show bodies. All bodies appear in the graphics area. All of the bodies are listed in the
•
FeatureManager design tree under Solid Bodies, and the icons are filled . Hide bodies. Only the bodies that you did not split appear in the graphics area. Bodies that are selected
•
are hidden. All the split bodies are listed in the FeatureManager design tree
under Solid Bodies, but the icons for hidden bodies are blank . Consume bodies. Removes the body from the part. Consumed bodies are not listed in the FeatureManager design tree under
8.
Click OK
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.
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Chapter 7 Parts
New Parts The new parts are derived; they contain a reference to the parent part. Each new part contains a single feature named Stock-<parent part name>-n->. If you change the geometry of the original part, the new parts also change. With multibody parts, the various split parts are listed in the FeatureManager design tree under Bodies.
Solid
Original Part The original part contains all its original features plus a new feature called Split. The solid body displayed in the graphics area is the original solid body minus the new parts. If all bodies in the original part were saved as split bodies, no solid body is displayed. To see the original solid body, move the rollback bar in the FeatureManager design tree above the split feature, or suppress the split feature. If you delete the split feature in the original part, the new parts still exist, but the status of the external reference in the new parts is dangling. You can also save solid bodies after you split the model using the Save Bodies feature. This enables you to save the bodies from a split part to a different folder or with different names to the same folder. To save bodies from multi-body parts:
1.
Click Insert, Features, Save Bodies. The pointer changes to
2.
and the Save Bodies PropertyManager appears.
Select each of the body parts from the graphics area to include in the assembly. •
Callouts. Display the default path and file names.
•
Path. Location of your multibody part.
•
File names. Listed in the Solid Bodies
•
You can also select each part from the File list under Resulting Parts.
folder in the FeatureManager design tree.
3.
Under Resulting Parts, click each file to activate and open the Save As dialog box. You can select a new location and file name for each part.
4.
Under Create Assembly, click Browse, and select a folder to save the assembly as SplitAssembly type (*.sldasm).
5.
Click OK
.
In the FeatureManager design tree, the entities are listed under Solid Bodies
.
Edit Derived Parts Derived part documents have some limitations: •
You can only add features in a derived part document.
•
You cannot delete or modify the features of the original part in the derived part document.
•
You can only edit the original part in its own window.
•
You cannot change the configuration of a derived part using the External References For dialog box.
To edit the original part from which another part is derived:
1.
Right-click the derived part, and select Edit In Context. If the part was derived using an insert part or a mirror part, the original part document is opened. If the part was derived from an assembly component, the assembly document is opened.
2.
Change the original part as needed. The changes are reflected in any derived parts that have an external reference to the original part.
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Create Assembly You can create an assembly from split part in a single step using the Create Assembly feature. The assembly you create is identical to an assembly created manually by opening an assembly document and dragging the part files individually into the assembly document. You can create additional features in the multibody part after using the Create Assembly command. However, these additional features do not appear as individual part files and are not part of the assembly document. To form split parts into an assembly:
1.
Select one or more Split features from the FeatureManager design tree.
2.
Click Insert, Features, Create Assembly.
3.
In the PropertyManager, under Split Features, select a Split part from the FeatureManager design tree.
4.
Click Browse. The Save As dialog box appears.
5.
Browse to the folder where you want to save the assembly, and type a name for the assembly in the File name box.
6.
Click Save.
7.
Click OK
.
The new assembly document opens.
Resolve Ambiguity The Resolve Ambiguity dialog box is displayed when the SolidWorks software identifies two or more valid solutions. Since more than one solution is valid, you are prompted to select the most appropriate solution from the list the solution. The Resolve Ambiguity dialog box can appear in any of the following scenarios. Editing a part within an assembly If you open an assembly and edit a part in that assembly, the Resolve Ambiguity dialog box is displayed when you try to save the changes. Saving the file creates an ambiguity because SolidWorks cannot determine whether you want to save the part or the assembly. To resolve the ambiguity:
1.
Select the part file or the assembly file in the Resolve Ambiguity dialog box.
2.
Click OK to save the selected element.
Converting entities with a closed contour If you select one side of a closed contour sketch (such as a rectangle), and click Convert Entities Ambiguity dialog box is displayed. There are two valid solutions: •
Single segment - only the line segment is converted
•
Closed contour - the entire closed contour sketch is converted
, the Resolve
To resolve the ambiguity:
1.
Select either Single segment or Closed contour from the list.
2.
Click OK to convert the entity you selected.
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Chapter 7 Parts
File Management with External References When you save a part that has external references to another document, the path and the internal ID of the referenced document are saved with the current part. The software needs this information to locate and verify the original document the next time you open the derived part. You can specify whether or not referenced documents are opened when you open a part that has external references. Locating Derived Parts Suppose you create a derived part, then you inadvertently move or rename the original document. When you try to open the derived part, the software notifies you that the externally referenced document (the original) was not found, and you are given a chance to look for it. If you choose not to look, the operation is cancelled. If you decide to look for the referenced document, you have the following choices: •
If you locate and select the original document (in a different directory, or with a new name), the derived part opens using the new name or path. Because the internal ID matches, the external reference updates as expected. When you save the part, the new name or path is saved also.
•
If you select a different document, you are notified that the internal ID does not match. Then you can either accept the selected document anyway, or keep looking.
Rebuild Errors If you accept the selected document, the model may have rebuild errors, especially if you have added features in the derived part document. If the geometry of the document you selected is not the same as the geometry of the original referenced document, the additional features may have rebuild errors.
Feature Statistics Feature Statistics is a tool that displays the amount of time it takes to rebuild each feature in a part. Use this tool to reduce rebuild time by suppressing features that take a long time to rebuild. This tool is available in all part documents. To use feature statistics:
1.
Open a part document.
2.
Click Statistics
on the Tools toolbar, or click Tools, Feature Statistics.
The Feature Statistics dialog box appears with a list of all features and their rebuild times in descending order.
3.
•
Feature Order. Lists each item in the FeatureManager design tree: features, sketches, and derived planes. Use the shortcut menu to edit feature definition, suppress features, and so on.
•
Time %. Displays the percentage of the total part rebuild time to regenerate each item.
•
Time(s). Displays the amount of time in seconds that each item takes to rebuild.
Click Feature Order. This sorts the features to match the FeatureManager design tree.
4.
5.
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Click one of the following: •
Print. Prints the Feature Statistics.
•
Copy. Copies the Feature Statistics so you can paste them into another file.
•
Refresh. Refreshes Feature Statistics.
Click Close.
Model Geometry Overview The Check Entity dialog box enables you to identify undesirable geometry and check model geometry. It is divided into two sections, Check and Check for. •
Check allows you to check Solids, Surfaces, or Features.
•
Click Selected items to display the Items to check box.
This checks a selected face or edge, for the items listed in the Items to check list. Use as a fast check of the selected items to report any errors on faces or edges. You can use this option first, to determine if the model geometry is valid. If you design very complex models, it is a good idea to use this option regularly, after creating several features. Sample of selected items check •
Click All to check some or all of the Solid or Surface features from the model. You can select all Solids, all Surfaces, or both.
It is a fast check of the whole model (or the selected items). It reports any errors on faces or edges. You can also use this option, to determine if the model geometry is valid. •
Click Features to select all the features in the model.
This is slower, especially for complex models, because it examines the model feature by feature, to locate the source of the problem. If any errors are found when you use Selected items, you can use this option to identify which features contain errors •
Check for allows you to select the types of problems that you want to check for:
•
Invalid face(s)
•
Invalid edge(s)
•
Short edge(s)
When you check for Short edge(s), you must specify a minimum edge length. The software reports any edges that are less than the specified length. The number of errors is listed in the Found column. The items are displayed in the Result list box. Additional information is in the message area. You can also check model geometry: •
Maximum radius of curvature
•
Maximum edge gap
•
Maximum vertex gap
The items are displayed in the Result list box. Additional information is in the message area.
Selected Items Check Entity Selected items: Surface body (created with Offset Surface) Check for: • Maximum edge gap • Maximum vertex gap Results: • No errors • 1 open surface found • 4 edges and vertices found with maximum gaps
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Chapter 7 Parts
Checking Model Geometry The SolidWorks software automatically checks the model geometry as you create each feature, to prevent invalid geometry. It also provides additional tools for checking the model, which you can use for the following purposes: •
To examine imported geometry (when you import the body as a whole, from another system, such as an IGES or STEP file)
•
To make sure that the model exports properly to other formats
•
To determine the cause when the model looks wrong
Force Regeneration with Verification on Rebuild By default, each time you add or modify a feature, the feature is checked against any adjacent faces and edges. For most situations, this default level of error checking is adequate, and results in fast rebuilding of the model. However, under certain circumstances, it is recommended that you perform more rigorous checks on the model: •
When the model looks wrong (and you have determined that it is not the result of a display problem)
•
When you have problem exporting the model in different formats
To increase the level of error checking, turn on the Verification on rebuild option. When this option is turned on, the software checks every new or changed feature against all existing faces and edges, not just adjacent faces and edges. Features that cause invalid geometry fail when this option is turned on. NOTE: This option has a negative effect on performance. Rebuilding the model is considerably slower and more CPU-intensive. This option applies to all documents, not just the active document. Use this option only when needed, then be sure to turn it off when you are done. To verify the model with a higher level of error checking:
1.
Click Tools, Options, on the System Options tab, select Performance, and the Verification on rebuild check box.
2.
Press Ctrl + Q to regenerate the entire model. NOTE: When you press Ctrl + Q, it causes a complete rebuild of all the features in the model. The Edit, Rebuild
operation (Ctrl + B) only rebuilds new or changed features and their children.
3.
Examine and correct any features that fail, beginning with the first failed feature in the FeatureManager design tree. Often fixing one failed feature allows subsequent failed features to rebuild successfully.
4.
When you are satisfied that all the errors are corrected, click Tools, Options, on the System Options tab, select Performance, clear the Verification on rebuild check box.
Checking a Planar Surface To check a planar surface:
1.
In the Check Entity dialog box, click Check selected items, select the surface in the FeatureManager design tree, and click Check.
2.
The message reports if the surface is open or closed, and the surface boundary edges are highlighted.
3.
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•
The Result list identifies any invalid edges or faces.
•
The message area lists a description of the results. To highlight an individual result, select the item displayed in the selection box.
Click OK to close the message, then click Close to close the dialog box.
Checking Part Faces or Edges To check a face or edge of a part:
1.
Click Tools, Check to display the Check Entity dialog box.
2.
In Check, click Selected items and select a face or an edge in the graphics area. The name of the item appears in the Item to check box.
3.
In Check for, select the types of problems that you want to review: Invalid face(s), Invalid edge(s), and/or Short edge(s), or any combination of the three.
4.
If you selected Short edge(s), specify a minimum edge length in the spin box. The software reports any edges that are less than the specified length.
5.
Click Check. After checking, the dialog box remains open so you can check additional entities.
6.
•
The Found column displays the number of items found with the specified error.
•
The Result list box displays the items that are either invalid or too short.
•
A message area lists a description of the results. To highlight the individual result, select the item displayed in the selection box.
Click Close to close the dialog box.
Check Entity To check a model for correct geometry:
1.
With a part document active, click Tools, Check.
2.
In the dialog box, select the entity type that you want to verify.
3.
•
All. Checks the entire model. Specify Solids, Surfaces, or both.
•
Selected items. Select items, such as faces, edges, and so on from the graphics area.
•
Features. Select features from the graphics area. As you select each feature, it is highlighted in the FeatureManager design tree.
In the Check for area, check the model for errors or report on the model’s geometry. •
Invalid face(s)
•
Invalid edge(s)
•
Short edge(s)
When you check for Short edge(s), you must specify a minimum edge length. The software reports any edges that are less than the specified length. 4.
Click Check (The dialog box remains open so that you can change the options or select different items to check.)
5.
Click Close to exit the Check Entity dialog box.
Finding the Minimum Radius of Curvature To find the smallest radius of curvature for the model:
1.
Click Tools, Check to display the Check Entity dialog box.
2.
In Check for, select the Minimum radius of curvature check box to determine the face with the smallest radius of curvature.
3.
In Check, you can choose Selected items and then select model faces, splines, or curves in the graphics area. If you select All, the entire part is checked.
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4.
5.
Click Check. (The dialog box remains open so that you can change the options or select different items to check.) •
The Item to check box displays the items you selected from the graphics area.
•
The Result list box displays the minimum radius. In the graphics area, an arrow points to the place on the curve where the minimum radius of curvature is found. (If there are two locations with the same minimum radius, only one is reported.)
•
The message area lists a description of results (the minimum curvature). To highlight the individual result, select the item displayed in the selection box.
Click Close to exit the Check Entity dialog box.
Interrupt Regeneration Press Esc to interrupt the regeneration of parts. This also works with opening parts, rollbacks, and so on. NOTE: When you interrupt the regeneration of a part, the system completes regeneration of the current feature and then places the rollback bar after the feature.
Send To Send the current part document to another system using electronic mail. To mail a part document to another computer:
1.
Click File, Send To.
2.
Enter your mail password, the mailing address, and any other information requested by your mail application. To send an assembly or drawing document, see Send Mail.
Displaying Parts Information Displaying Annotations in Parts You can add annotations to your model to further clarify the information the part document provides. This includes dimensions, notes, symbols, and so on. Then you can import the dimensions and annotations from the model into a drawing (see Detailing Overview). You can control the display of annotations in the part window using shortcut menu selections on the Annotations folder
in the FeatureManager design tree.
To select the types of annotations to display:
1.
In the FeatureManager design tree, right-click Annotations Properties dialog box appears.
2.
Under Display filter, select the annotation types to display (Notes, Datums, and so on), or select the Display all types check box to show all types of annotations available for the part.
3.
Change the values in the Text scale boxes to modify the scale of the text used in the annotation.
4.
Select from the following options:
5.
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and select Details. The Annotation
•
Always display text at the same size. Annotations and dimensions are displayed at the same size regardless of zoom.
•
Display items only in the view orientation in which they are created. An annotation is only displayed when the part is in the same view orientation as when the annotation was inserted. Rotating the part or selecting a different view orientation removes the annotation from the display.
•
Display annotations. All annotation types that are selected in the display filter are displayed.
Click OK.
To toggle the display of annotations:
Right-click Annotations
and select (or clear) the items to display:
•
Display Annotations. All annotation types that are selected in the Annotation Properties dialog box are displayed. This is the same as selecting the Display Annotations check box in the Annotation Properties dialog box.
•
Show Feature Dimensions. This is the same as selecting the Feature dimensions check box in the Display filter of the Annotation Properties dialog box.
•
Show Reference Dimensions. This is the same as selecting the Reference dimensions check box in the Display filter of the Annotation Properties dialog box.
To toggle the display of selected feature dimensions:
To hide an individual dimension, right-click it, and select Hide. To hide all the dimensions of a selected feature, right-click the feature in the FeatureManager design tree, or right-click one of its faces, and select Hide All Dimensions. To re-display the dimensions, right-click the feature or one of its faces, and select Show All Dimensions.
Summary Information You can use the Summary Information dialog box to add more information to a part or assembly document, or to a configuration of the model in the document. Use this type of custom information in the followings ways: •
Apply in a Bill of Materials
•
Add associative dimensions in parts that dynamically update in a Bill of Materials
•
Use as advanced selection criteria for managing assembly configurations
•
Integrate with drawing sheet formats and link notes to document properties
•
Add system-defined, configuration-specific mass properties
To enter or display summary information:
1.
Click File, Properties. The Summary Information dialog box appears.
2.
On the Summary tab, type the appropriate information in the boxes provided for: Author, Keywords, Comments, Title, and Subject. The system provides read-only Statistics about the document’s creation date, the date last saved, and the name of the person who saved the document last. NOTE: If you insert a part identification number in the Title box, you can use that number automatically when you create a bill of materials in an assembly drawing that contains that part.
Summary Info – Custom and Configuration Specific Access to the Summary Information dialog box is through File, Properties. The Custom and the Configuration Specific tabs in the Summary Information dialog box allow you to: •
Specify custom properties for the active part, assembly, or drawing document.
•
Apply configuration-specific properties for the active part or assembly configuration.
•
Add associative dimensions. The dimensions can come from sketches, part features, assembly features, or assembly mates. Since part dimensions are associative, values in the Bill of Materials (BOM) are updated when the dimensions are changed.
•
Edit the list of custom properties.
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• • •
When you type a Name and a Value to add a new Property, you can click OK to add the new property without first clicking Add. If you type a Name and a Value to add a new Property, and then select another name from the list without clicking Add, the first property is automatically added. When you modify an existing custom property, those changes are saved when you click OK. You no longer need to click Modify to apply the changes.
In addition to the BOM, you can use the properties in the following ways: •
As advanced selection criteria for managing assembly configurations
•
In drawing sheet formats and to link notes to document properties If you plan to use the property as a custom column in a Bill of Materials, do not include any spaces in the Name.
To specify custom properties:
1.
Enter a Name for the property, or choose one from the list. You can now specify a Description name, which appears in the Open and Save As dialog boxes.
2.
Select the Type from the list.
3.
Enter a Value for the custom property that is compatible with the selection in the Type box.
4.
Click Add. The Properties box displays the name, values, and type of the custom properties.
To add associative dimensions into custom properties:
1.
Open the part and display the dimensions to add to Custom Properties.
2.
Enter a Name for the property, or choose one from the list.
3.
Select the Type from the list.
4.
Click the dimension in the graphics area. The dimension name @ feature is displayed in Value.
5.
Place your cursor at the end of the dimension name and add additional text, such millimeters. NOTE: Values are cumulative unless you clear the content in the Value box. Cumulative values enable you to include dimensions, units, and other text. For example: Click one dimension in the graphics area, type x in the Value box, and click additional dimensions in the graphics area to display: dimension name1 @ feature x dimension name2 @ feature, and so on.
6.
Click Add. The Properties box displays the name, values, and type of the custom property. Any dimension included in Custom Properties is updated when you modify the dimension in the part.
To edit custom properties:
1.
In the Name box, click the property that you want to change.
2.
Edit the Type or Value as needed.
3.
Click Modify. NOTE: This modifies the custom properties for the current document only. Edit the global custom properties with the Edit List dialog box.
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To delete custom properties:
1.
Click the property in the Properties box that you want to delete.
2.
Click Delete. NOTE: This deletes the custom properties from the current document only. Delete the global custom properties with the Edit List dialog box.
You can add system-defined, configuration-specific mass properties as a custom property, using either the Custom or Configuration Specific tabs. Use the Configuration Specific tab to display with other configuration-specific properties. Mass properties use the following, system-generated format: SW<mass property>@ @configuration@model To add mass properties:
1.
Enter a Name for the mass property.
2.
Select the Type from the list.
3.
Click Mass Properties and select the appropriate mass property from the list.
4.
Click Add. The Properties box displays the name, values, and type of the mass property.
5.
Click OK.
Edit List You can edit the list of custom properties. You can also edit the text file where the properties are stored in any text editor. The default file location is install_dir\lang\english\properties.txt. To edit custom properties:
1.
Click Edit List on the Custom tab of the Summary Information dialog box. The Edit List dialog box with the list of properties appears.
2.
You can do one of the following: •
Add. Type a name in the box and click Add.
•
Delete. Select a property from the list and click Delete.
•
Move Up. Select a property from the list and click Move Up.
•
Move Down. Select a property from the list and click Move Down.
Section Views Overview You can display a view of the model cut through the part or assembly. You can cut through a model or assembly using one of the following: • •
One or more standard planes. You can pre-select a plane, or if no plane is selected, the Front plane is selected by default. One or more planes you create.
•
One or more planar faces, by selecting any planar face on the model.
•
Viewing plane, which is the invisible plane parallel to the screen.
You can view both the section view and the complete view of the model at the same time by splitting your screen into two windows. (Drag the split bars on the bottom or right side of the window frame.) You can now select faces, edges, and vertices formed by a section view. See Section View Selection. Before you can display a section view of an assembly, you must fully resolve any lightweight parts that it contains. Displaying and creating views include: •
Creating section views
•
Using viewing planes
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Section View Selection You can select the faces, edges, and vertices that are created by a section view of a part or assembly. In earlier versions, the section view was for visualization only, and you could not select faces or edges that were cut by the section plane.
NOTE: You cannot open a sketch on a section view face. Measure and Section Properties •
Select a face on the section plane to calculate its section properties. Select edges or vertices to measure.
•
Select truncated faces to measure lengths or calculate section properties. Truncated faces are faces cut by the section plane.
Truncated Faces Convert Entities For functions other than Measure and Section Properties, the truncated faces act as if they are not truncated. For example, if you open a sketch on a truncated face and convert the edges, the edges of the full face are converted.
Full Face is Converted
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Section Views in Models Section views use a plane to display a cutaway of a part or assembly. To create a section view of the model:
1.
Click Section View
on the View toolbar or click View, Display, Section View.
The Section View dialog box appears. 2.
Click one or more planes in the FeatureManager design tree, or click one or more planar faces on the model. Alternatively, you can pre-select planes or planar faces before you click View, Display, Section View. If nothing is selected, the Front plane is used by default. To pre-select multiple planes or faces, hold down the Ctrl key as you select.
3.
Click a plane in the Section Plane(s)/Face(s) box, then use the arrows to set a value in the Section Position box to move the plane and change the section cut. You can also use the viewing plane.
4.
Click the Flip the Side to View check box to reverse the viewing direction of the section cut. (Not available if you are using the viewing plane.)
5.
Select a Preview/Display mode:
6.
•
When Preview is selected, the section view is updated whenever any item in the dialog box is changed. If you need to adjust more than one setting, especially with a large part or assembly, this option may not be efficient.
•
When Preview is cleared, click Display to update the section view. You can make multiple changes to the settings, then click Display again to update the view with all the changes at once.
Click OK.Example NOTE: You can view both the section view and the complete view of the model at the same time by splitting your screen into two windows. (Drag the split controls on the bottom or right side of the window frame.) You can revolve, size, and shade the views independently.
Using Viewing Planes for Section Views Instead of model faces and planes, you can use a viewing plane to cut the section view. The viewing plane is an invisible plane that is parallel to the screen, and normal to your line of sight. The initial position for this plane is the center of the part body bounding box. As you rotate the part, the angle of the viewing plane relative to the part body changes, cutting the part at a different angle. To use the viewing plane to cut a section view:
To use the viewing plane to make a section cut, click Use Viewing Plane in the Section View dialog box. You can offset the Section Position of the viewing plane. The Flip the Side to View option is not available when you use the viewing plane. To change the section view:
1.
Click Section View
or click View, Modify, Section View.
2.
Change the settings in the Edit Section View dialog box, and select a different plane if needed.
3.
Click OK.
To return to a normal view of the model:
Click Section View
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or click View, Modify, Section View again to deselect the command.
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Sample Section Views
Model with no section view
Model using plane 45° to Plane1 and Section Position -5.00mm
Model using plane 45° to Plane1, Section Position -5.00mm, and Flip side to view
Model using Viewing Plane and Section Position 26.50mm
Mass Properties and Section Properties Displays the density, mass, volume, surface area, center of mass, inertia tensor, and principal axes of inertia of a part or assembly model. A tri-colored reference 3D triad displays at the origin. A red 3D triad displays at the centroid of the part or assembly along with the mass properties and section properties.
Before you can calculate mass properties or section properties of an assembly, you must fully resolve any lightweight parts that it contains. See also Loading Additional Model Data. Mass Properties To evaluate components or solid bodies in assembly and multibody part documents, click the component or body, and click Recalculate. If no component or solid body is selected, the mass properties for the entire assembly or multibody part are reported.
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To display mass properties:
1.
Click Mass Properties
on the Tools toolbar or click Tools, Mass Properties.
NOTES: •
You evaluate different entities without closing the Mass Properties dialog box. Clear the selections, then select the entity, and click Recalculate.
•
The results are displayed in the Mass Properties dialog box, and the principal axes and center of mass are displayed graphically on the model.
2.
Click Options if you want to display the Measurement Options dialog box and to display the results using different units than the units specified for the active document.
3.
Click Print if you want to print the results directly from this dialog box.
4.
Click Copy if you want to copy the information to the clipboard, then paste it into another document.
5.
Click Close to close the dialog box.
NOTE: When you save the document, you can update the mass properties information. This enhances system performance, since the next time you access mass properties, the system does not need to recalculate the values (if the document is unchanged). To set this option, click Tools, Options, on the System Options tab, click Performance, and click the Update mass properties while saving document check box. Section Properties You can evaluate section properties for multiple faces and sketches that lie in parallel planes. Clear the selections, then select the entity, and click Recalculate. NOTE: When you evaluate more than one entity, the first selected face defines the plane for section property calculation. To display section properties for multiple entities:
1.
2.
Select any of the following that lie in parallel planes: •
one or more planar model faces
•
a face on a section plane
•
the crosshatch section face in a section view of a drawing
•
a sketch (click the sketch in the FeatureManager design tree or right-click the feature and select Edit Sketch)
Click Tools, Section Properties. The results are displayed in the Section Properties dialog box.
Curvature You can display a part or assembly with the surfaces rendered in different colors according to the local radius of curvature. Curvature is defined as the reciprocal of the radius (1/radius), in current model units. By default, the greatest curvature value displayed is 1.0000, and the smallest value is 0.0010. As the radius of curvature decreases, the curvature value increases, and the corresponding color changes from black (0.0010), through blue, green, and red (1.0000). As the radius of curvature increases, the curvature value decreases. A planar surface has a curvature value of zero (1/8). To render curved surfaces in colors and display curvature radius:
1.
Click Tools, Options. The Options dialog box appears with the System Options tab active.
2.
On the System Options tab, click Display/Selection, and make sure that the Dynamic highlight from graphics view check box is selected.
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3.
Click View, Display, Curvature. The curvature of the model is displayed in color. When you point to a model surface, a spline, or a curve, the curvature value and the radius of curvature are displayed beside the pointer.
4.
To remove the color, click View, Display, Curvature to clear the check mark.
To render an individual model face in colors:
1.
Right-click the model face and select Face Curvature. The curvature of the selected face is displayed. When you point to the model face, the curvature value and the radius of curvature are shown beside the pointer.
Model with no color applied to curved surface 2.
Model with color applied to selected curved surfaces (zero curvature is black)
To remove the color, right-click the model face and click Face Curvature to clear the check mark.
To set values for the color scale for displaying curvature:
1.
Click Tools, Options. The Options dialog box appears with the System Options tab active.
2.
On the Document Properties tab, click Colors.
3.
Click Curvature.
4.
Select the curvature value edit boxes that you want to change and enter new values. You can modify the values at five intervals on the color scale; values are interpolated for the intermediate colors in the range. See sample of curvature values for some common radius values.
5.
Click Apply to preview the color scale changes with the new values.
6.
Click OK to save the new settings.
Curvature Values for Common Radius Values
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Radius
Curvature
Radius
Curvature
0.125
8
10
0.1
0.25
4
20
0.05
0.5
2
25
0.04
0.75
1.333
30
0.033
1
1
40
0.025
1.5
0.667
50
0.02
2
0.5
75
0.013
2.5
0.4
100
0.01
3
0.333
125
0.008
4
0.25
200
0.005
5
0.2
250
0.004
7.5
0.133
500
0.002
Curvature Options Defines the colors associated with the curvature of models. Curvature is equal to the inverse of the radius of the curve (curvature = 1/radius). By default, the greatest curvature is represented by red, and the least curvature is represented by black. For example, if you display curvature on a cube, all sides display as black. This is because the radii of flat faces are infinite and the curvature is zero. As the curvature increases (and the radius decreases), the corresponding color values change from black, through blue, green, and red. You can change the curvature values at both ends of the scale and at three points in the middle so that the curvature values increment within a narrower or wider range, or increment more or less rapidly. To set the curvature values:
1.
Click Tools, Options, click the Document Properties tab, and click Colors.
2.
Click Curvature.
3.
Select the curvature value edit boxes that you want to change and enter new values.
4.
Click Apply to see how the color scale changes in response to the new curvature values. The intermediate curvature values also change appropriately.
5.
Click OK to save the new settings, and click OK again to close the Color dialog box.
Curvature Display You can display a surface, part, or assembly with the curved surfaces rendered in different colors according to their local radius of curvature. To define the colors, click Tools, Options, and click the Document Properties tab. Select Colors and click Curvature. You can also display the curvature value of sketch segments and curves in a closed sketch. To render curved surfaces in colors, and to display the radius of curvature values:
Click View, Display, Curvature. While the Curvature menu item remains selected, •
The value of the curvature radii is displayed next to the pointer when you point at curved surfaces.
•
The curvature of the model is displayed in colors related to the radii of the curvature. To remove the curvature display, click View, Display, Curvature again (to clear the check mark).
To toggle curvature display for individual faces:
Right-click a curved face and select Face Curvature from the menu. NOTE: The curvature display for faces can be toggled on or off using the shortcut menu, except when Curvature is turned on with View, Display, Curvature.
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To display curvature values for sketch entities in a closed sketch:
1.
Click Tools, System Options, Display/Selection, and select Dynamic highlight from graphics view.
2.
Click OK.
3.
Now you can click View, Display, Curvature in the main menu. The curvature value is displayed next to the pointer when you point at sketches or curves.
Zebra Stripes Zebra stripes allow you to see small changes in a surface that may be hard to see with a standard display. Zebra stripes simulate the reflection of long strips of light on a very shiny surface. With zebra stripes, you can easily see wrinkles or defects in a surface, and you can verify that two adjacent faces are in contact, are tangent, or have continuous curvature. See Zebra Stripes on Boundaries for more information.
Part Zebra Stripes To view a part with zebra stripes:
1.
Click View, Display, Zebra Stripes. The Zebra Stripes PropertyManager appears, and the part is displayed with zebra stripes.
2.
Under Settings, do the following: •
Adjust the Number Of Stripes
•
Adjust the Width Of Stripes
•
Adjust the Stripe Accuracy . Move the slider from low accuracy (left) to high accuracy (right) to improve the quality of the display. Note that increasing the display accuracy also increases the display calculation time.
•
Change the Color Of Stripes and Color Of Background. Click Edit Color, choose a new color from the Color palette, and click OK. The new color appears in the color box and in the graphics area.
•
Select one of the following: •
.
Spherical Map. Available on all systems. The part appears to be inside a large sphere that is covered on the inside with strips of light. The zebra stripes are always curved (even on flat faces) and display singularities.
Singularities
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.
•
Cube Map. Available on systems with a graphics card that supports cube texture maps. If your computer does not have this type of graphics card, SolidWorks does not allow you to select this option. The part appears to be inside a large square room that is covered with strips of light on the walls, ceiling, and floors. The zebra stripes are straight on flat faces, and do not display singularities. The cube map display shows unstriped bands. Unstriped bands are the reflections of the corners of the "room."
No stripes 3.
Click OK
Spherical Map
Cube Map
.
To turn off zebra stripes:
Click View, Display, Zebra Stripes, or right-click the part in the graphics area and click Zebra Stripes. Zebra Stripes are deselected. Face Zebra Stripes You can improve the accuracy of your display by selecting only those faces that you want displayed with zebra stripes. To view a face with zebra stripes:
1.
Right-click a face in the graphics area and select Face Zebra Stripes. The Zebra Stripes PropertyManager appears, and the face is displayed with zebra stripes.
2.
Adjust the display as described previously.
3.
Click OK
.
To turn off face zebra stripes:
Click View, Display, Zebra Stripes, or right-click in the graphics area and click Face Zebra Stripes. Zebra Stripes are deselected. NOTE: It may be helpful to use zebra stripes in conjuction with the Curvature display.
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Zebra Stripes on Boundaries You can visually determine what type of boundary exists between surfaces by using zebra stripes. Contact Zebra stripes do not match at the boundary.
Tangency Zebra stripes match at the boundary, but there is an abrupt change in direction.
Curvature Continuous Zebra stripes continue smoothly across the boundary. Curvature continuity is an option when creating face blend fillets.
Fillet
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Tangent
Curvature Continuous
Lighting Lighting Overview You can adjust the direction, intensity, and color of light in the shaded view of a model. You can add light sources of various types, and modify their characteristics to illuminate the model as needed. The properties of the light sources work with the material properties of the model. If you change material properties of the model, you can enhance or reduce the effect of the light properties. Light Types There are several types of light source: •
Ambient light. Illuminates the model evenly from all directions. In a room with white walls, the level of ambient light is high, because the light reflects off the walls and other objects.
•
Directional light. Comes from a source that is infinitely far away from the model. It is a columned light source consisting of parallel rays from a single direction, like the sun. The rays of a Directional light point toward the center of the model.
•
Point light. Comes from a very small light source located at a specific coordinate in the model space. This type of light source emits light in all directions. The effect is like a tiny light bulb floating in space.
•
Spot light. Come from a restricted, focused light with a cone-shaped beam that is brightest at its center. A spot light can be aimed at a specific area of the model. You can adjust the position and distance of the light source relative to the model, and you can adjust the angle through which the beam spreads.
System Lighting Defaults By default, the Lighting folder light.
in the FeatureManager design tree contains one Ambient light and one Directional
•
You can turn the Ambient light on or off, but you cannot delete it or add additional Ambient lights.
•
You can turn the Directional light source on or off, or delete it. You can also add additional Directional light sources.
•
The maximum number of light sources in any document is nine (the Ambient light and eight others in any combination).
Basic Lighting Controls To add a light source:
1. 2.
Right-click the Lighting folder
or any existing light.
Select Add Spot Light (or Add Directional Light, or Add Point Light) - or Click View, Lighting, Add Spot (or Add Directional, or Add Point).
To delete a light source:
1.
Click the
to expand the Lighting folder
and display the light sources.
2.
Select Spot Light (or Directional Light, or Point Light) and press Delete. - or Click View, Lighting, Delete, Spot (or Directional, or Point).
To turn off a light, without deleting it:
1. 2.
Click the
to expand the Lighting folder
and right-click the light source.
Select Properties. - or Click View, Lighting, Properties (Ambient, Directional, Spot, or Point).
3.
In the Ambient, Directional, Spot, or Point Light Properties dialog box, click to clear the On check box.
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To modify the lighting properties:
1.
Right-click the light source in the Lighting folder
2.
Edit the properties as needed. The light properties that are available depend on the type of light source. See: •
Ambient Light Properties
•
Directional Light Properties
•
Point Light Properties
•
Spot Light Properties
and select Properties.
3.
As you edit each light, a graphical representation of the light source is displayed, indicating the color and direction of the light.
4.
Click OK.
Ambient Light You can control the intensity and the color of ambient light. To control ambient light:
1.
In the FeatureManager design tree, click
2.
Right-click Ambient and select Properties.
3.
In the Ambient Light Properties dialog box, you can do the following: •
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Slider right: high ambience
Click Edit to display the Color palette, and select colored ambient light rather than the default white light.
White ambient light •
Ambient Off
Move the slider from left (for low intensity) to right (for high intensity).
Slider left: low ambience •
folder.
Clear the On check box to eliminate the ambient light from the model. You can turn ambient light off, but you cannot delete the ambient light.
Ambient On •
to expand the Lighting
Red ambient light
Click Use as default to save the current ambient setting as your default setting.
NOTE: The results vary widely. They depend on multiple combinations, including the color of the model, the degree of ambience (intensity), as well as the color of the light. For example, changing the color of the ambient light produces more noticeable results with high ambience than with low ambience.
Directional Light Properties Basic Tab On the Basic tab, a Directional light source has the following Intensity properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
See also Ambient light for information on Basic properties. Direction Tab On the Direction tab, specify the following properties: •
Direction. Specify the direction from which the light arrives, relative to the origin. You can use the sliders to specify the values for Longitude and Latitude, or you can enter a value in degrees.
Directional light with default placement •
Directional light with change in Latitude
Directional light with change in Latitude and Longitude
Lock to model. When this check box is selected, the light moves along with the model when you rotate the model. The light always shines on the same area of the model because the position of the light relative to the model is maintained.
To keep the light in the same position in the model space, clear the Lock to model check box. When you rotate the model, the light shines on different areas of the model because the position of the light remains fixed in space. As you edit the Directional light, a graphical representation of the light source is displayed, indicating the color and direction of the light. After you finish, click OK.
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Chapter 7 Parts
Point Light Properties Basic Tab On the Basic tab, a Point light includes the following Intensity properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
See also Ambient light for information on Basic properties. Position Tab On the Position tab, specify the Position of the light source relative to the origin. Select the type of coordinate system, and specify the values: •
Spherical (Longitude, Latitude, Distance)
•
Cartesian (X, Y, Z)
Point light with default placement and default values
•
Point light with default placement, change to green color and Specularity at maximum
Point light with increase in Brightness (Basic) and changes to Position, using Cartesian coordinates
Lock to model. When this check box is selected, the light moves along with the model when you rotate the model. The light always shines on the same area of the model because the position of the light relative to the model is maintained.
To keep the light in the same position in the model space, clear the Lock to model check box. When you rotate the model, the light shines on different areas of the model because the position of the light remains fixed in space. As you edit the Point light, a graphical representation of the light source is displayed, indicating the color and direction of the light. After you finish, click OK.
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Spot Light Properties Basic Tab On the Basic tab, a Spot light includes the following Intensity properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
See also Ambient light for information on Basic properties. Position Tab On the Position tab: •
Position. The Position is the location of the light source relative to the center of the scene. Like a Point light, you can use either Spherical or Cartesian coordinates.
•
Target. The Target is where the light strikes the model or the surrounding scene. Only Cartesian coordinates (X, Y, Z) are available.
The Spot light also includes an Advanced tab where you can set Cone Angle, Exponent, and Attenuation. As you edit each light, a graphical representation of the light source is displayed, indicating the color and direction of the light. After you finish, click OK.
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Chapter 7 Parts
Lighting - Basic All light sources have the following properties: •
Color. To change the color, click Edit, select a new color from the palette, and click OK.
•
On. To turn the light on or off, select or clear the On check box.
•
Configurations. Select This Configuration, All Configurations, or Specify Configurations.
•
Use as default. If you want to save the settings for the current light, and use them in new documents, click Use as default.
•
Intensity. Move the Ambient slider to adjust the level of light. The level changes equally on all sides of the model.
Directional, Point, and Spot lights have these additional properties: •
Brightness. This slider controls the brightness of the light source. A higher value results in more light on the side of the model closest to the source.
•
Specularity. This slider controls the extent to which shiny surfaces exhibit bright highlights where the light strikes them. A higher value results in more dramatic highlights and a shinier appearance.
Low Specularity
High Specularity
Lighting - Advanced Exponent. The exponent controls how tightly the beam of light is concentrated. A low exponent value produces a focused, cone-shaped beam of light with sharp edges. The intensity of the light is similar at the center of the beam and at the edges. With a high exponent value, the beam is brightest at the center. The intensity decreases toward the edges of the beam, and the edges of the beam appear softer. Cone Angle. The cone angle specifies the angle through which the beam spreads. A small angle produces a narrow beam of light. Attenuation. The attenuation is the property that decreases the intensity of the light as the distance increases. The values A, B, and C are multipliers in the following equation (D is the distance): attenuation = 1 / A + (B * D) + (C * D2) As the values for A, B, and C increase, the amount of light that reaches the target decreases.
Low values
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High values
Lighting - Position and Direction Direction. For a Directional light, specify the direction from which the light arrives, relative to the origin. You can use the sliders to specify the values for Longitude and Latitude, or you can enter a value in degrees. For a Point or Spot light, select the type of coordinate system, then specify the values: •
Spherical (Longitude, Latitude, Distance)
•
Cartesian (X, Y, Z)
For a Directional light, type a position or use the sliders to set values for the following: •
Latitude
•
Longitude Lock to model. • In these examples, notice the position of the Spot light relative to the model when the model is rotated. Original position •
When selected, the light moves along with the model when you rotate the model. The light always shines on the same area of the model because the position of the light relative to the model is maintained.
Lock to model selected •
To keep the light in the same position in the model space, clear this check box. When you rotate the model, the light shines on different areas of the model because the position of the light remains fixed in space. Lock to Model cleared
Target. (Spot light only). • The Target is where the light strikes the model or the surrounding scene. Only Cartesian coordinates (X, Y, Z) are available.
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8 Mold Design
Mold Tools Toolbar The Mold Tools toolbar provides tools for creating molded parts and assemblies. Scale Parting Lines Ruled Surface Parting Surfaces Tooling Split Cavity Draft Split Line Offset Surface Ruled Surface Radiate Surface Planar Surface Knit Surface Draft Analysis Undercut Detection
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Chapter 8 Mold Design
Understanding Mold Design Creating a mold design in the SolidWorks software requires the following items: •
Design parts - The parts that you want to mold.
•
A mold base - The part that holds the cavity feature of the design part.
•
An interim assembly - The assembly in which the cavity is created.
•
Derived component parts - The parts that become the halves of the mold after you cut them (recommended).
You can create a mold using a sequence of integrated tools that control the mold creation process. With the model finished, you can use these mold tools to analyze and correct deficiencies with either SolidWorks or imported models. Mold tools span from initial analysis to creating the tooling split. The process is as follows: •
Undercut Detection model from ejecting.
•
Parting Lines . This tool has two functions: o Verifies the you have draft on your model, based on the angle you specify. o
. Use the Undercut Detection tool to identify trapped areas that prevent the
Creates a parting line from which you create a parting surface. The Parting Lines tool includes the option to select an edge and have the system Propagate
to all edges.
. Models often include openings which you need to shut-off to prevent leakage from
•
Shut-off Surfaces core-to-cavity.
•
Parting Surfaces . Parting surfaces extrude from the parting line to separate mold cavity from core. You can also use a parting surface to create an interlock surface. In such instances, you can create a separate surface to separate mold cavity from core.
•
Ruled Surface . Ruled surfaces are used with imported parts when the draft analysis shows that sections of the model require draft. You can also use the Ruled Surface tool to create an interlock surface.
•
Tooling Split . The Tooling Split tool creates the core and cavity by automatically populating the core, cavity and parting surface, based on the steps followed earlier.
The Mold Tools toolbar also includes additional tools common to the mold process, such as Scale as well surface modeling tools such as Planar Surface
and Knit Surface
, Cavity
,
.
You combine the design parts and mold base in the interim assembly. Then, you create a cavity feature in the context of the interim assembly. This relates the mold base to the design part in the event that the design part changes shape. You cannot edit mold features within an assembly.
8-2
Mold Tools - Undercut Detection The Undercut Detection tool finds trapped areas in a model that cannot be ejected from the mold. These areas require a slide, which usually slides in a perpendicular direction to the core and cavity segments as these are separated. Undercut detection does not detect with imported surface parts, or surface parts generated in SolidWorks. Undercut analysis is not based on the parting line. To run an undercut detection:
1.
Click Undercut Detection
2.
In the PropertyManager, under Analysis Parameters: •
in the Molds toolbar, or click Insert, Molds, Undercut Detection.
Click Coordinate input to set coordinates along the X, Y and Z axes. This controls the Direction of Pull. - or -
•
3.
Select a plane, face, or edge as the Direction of Pull
.
Click Calculate.
Under Undercut Faces, the number of faces appears. 4.
5.
Under Undercut Faces: •
Click Show
•
Click Edit Color to display the Color palette and change the color for either the undercut faces or the normal faces.
•
Clear Save color if you do not want to save the new color definition upon exit.
Click OK
SolidWorks 2004 Reference Guide
, or Hide
for either the undercut faces or the normal faces.
.
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Chapter 8 Mold Design
Scaling Factor and Draft in Mold Design Scaling Factor When you create a mold you must account for the scaling factor. The scaling factor is the amount the material in the mold shrinks or expands as it solidifies. The scaling factor depends on the type of material used and the shape of the mold, and is expressed as a percentage of the linear size (not volume) of the design part. The software scales the cavity by the specified scaling factor, using this formula: Cavity size = part size * (1 + scaling factor/100) For example: Desired adjustment
Scaling factor in % (enter this number)
Resulting cavity size
2% material shrinkage (cavity larger than part)
2.0
part size * 1.02
2% material expansion (cavity smaller than part)
-2.0
part size * 0.98
Creating Drafts for Molds You may need to add draft angles to molded design parts to make it possible to remove the finished part from the mold. If you have a SolidWorks model, you can use the Split Line
tool to split faces and the Draft
tool to add
tool with either SolidWorks or imported models to add draft, correct
draft. You can also used the Ruled Surface flawed surfaces, or create interlock surfaces.
Mold Tools - Parting Lines Parting lines lie along the edge of the molded part, between the core and the cavity surfaces. They are used to create the parting surfaces, and to separate the surfaces. You create the parting lines after the model is scaled and proper draft is applied. To create parting lines:
8-4
1.
Click Parting Lines
on the Mold toolbar, or click Insert, Molds, Parting Line.
2.
In the PropertyManager, under Mold Parameters: •
Select a flat face or a plane as the Direction of Pull.
•
Note the direction of the arrow, and click Reverse
•
Set a value for Draft Angle
•
Click Draft Analysis.
.
if necessary.
3.
Inspect the model for draft, and compare the colors to those displayed under Mold Parameters. You should have a combination of Positive and Negative draft. If draft is required:
Positive and Negative draft
4.
•
With a SolidWorks model, click Draft
on the Molds toolbar, or click Insert, Molds, Draft.
•
With an imported model, click Ruled Surface Ruled Surface.
on the Molds toolbar, or click Insert, Molds,
Under Parting Lines, do one of the following: •
If the model includes a chain of edges that runs between positive and negative faces (that includes no straddle faces), the parting lines are selected automatically.
•
If the model includes multiple chains, the longest chain is selected automatically.
•
If you want to automatically select a different chain of edges: a. b.
Right-click and select Clear Selections. Select an edge.
c.
Click Propagate
to display all the edges under Edges.
Propagate to all edges automatically •
5.
If you want to manually select each edge: a.
Click Add selected edge
b.
Click Select next edge
c.
Click Zoom to the selected edge
Click OK
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. , and repeat until all the edges appear under Edges. for detail of the edge selection area.
.
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Chapter 8 Mold Design
Mold Tools - Ruled Surfaces With imported geometry, you cannot use draft tools from the SolidWorks application to correct surfaces that require draft. The Ruled Surface command can create ruled surfaces that are either perpendicular or tapered from the selected edges. You can also use the ruled surfaces to create interlock surfaces. To create a ruled surface:
1.
Click Ruled Surface
2.
In the PropertyManager, under Type, select an option:
3.
4.
5.
6.
on the Molds toolbar, or click Insert, Molds, Ruled Surface.
•
Tangent to Surface. Ruled surface is tangent to the surfaces that share an edge.
•
Normal to surface. Ruled surface is normal to the surfaces that share an edge.
•
Tapered to Vector. Ruled surface is tapered to the specified vector.
•
Perpendicular to Vector. Ruled surface is perpendicular to the specified vector.
•
Sweep. Ruled surface is built by creating a swept surface using selected edges as guide curves.
Under Distance/Direction: •
Set a value for Distance
.
•
With Tapered to Vector, or Perpendicular to Vector: o
Select an edge, a face, or a plane as the Reference Vector.
o
Click Reverse Direction
o
With Tapered to Vector only, set an Angle
, if necessary. .
Under Edge Selection: •
Select the edges used as the base for the ruled surfaces
•
Click Alternate Side, if necessary.
Under Options: •
Clear Trim and knit to manually trim and knit the surfaces.
•
Clear Connecting Surface to remove any connecting surfaces. Connecting surfaces are usually created between sharp corners.
Click OK
.
Mold Tools - Shut Off Surfaces After you create the parting lines, you need to shut off any open areas to prevent leakage. The liquid filling the mold must not connect the cavity side of the part with the core side of the part. To create shut off surfaces:
1.
Click Shut-off Surfaces
on the Mold toolbar, or click Insert, Molds, Shut-off Surfaces.
In the PropertyManager, under Edges, all the edges that belong to open surfaces appear. 2.
8-6
Inspect the arrows that show the direction of the shut-off surface.
Incorrect direction
Correct direction
Incorrect direction: note the uneven surface
Correct direction: note the smooth surface
3.
If necessary, click the arrow to shift the direction.
4.
Click OK
.
Mold Tools - Parting Surfaces After you determine the parting lines and create the shut off surfaces, you create the parting surfaces. Parting surfaces extrude from the parting lines, and are used to separate the mold cavity from the core. To create a tooling split (the next step in the process), you need at least three surface bodies in the Surface Bodies
folder.
To create parting surfaces:
1.
Click Parting Surfaces
on the Molds toolbar, or click Insert, Molds, Parting Surface.
2.
In the PropertyManager, under Mold Parameters, select an option: •
Tangent to surface. Parting surface is tangent to the surface of the parting line.
•
Normal to surface. Parting surface is normal to the surface of the parting line.
•
Perpendicular to pull. Parting surface is perpendicular to the direction of pull. This is the most common.
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Chapter 8 Mold Design
Tangent to surface 3.
Normal to surface
Perpendicular to pull
Under Parting Surfaces: •
Set a value for Distance.
•
Click Reverse offset direction
•
If you selected Tangent to surface or Normal to surface, you can set a value for Angle changes the angle from perpendicular to the direction of pull.
•
Smoothing. You can apply a smoother transition between adjacent surfaces. o
Sharp
, if necessary. . This
is the default value.
Smooth gives you the option to set a value for Distance between adjacent edges. A higher value creates a smoother transition between adjacent edges. Under Options: o
4.
•
Clear knit all surfaces to prevent surfaces from knitting by default. With most models, the surfaces are created correctly. However, if you need to repair a gap between adjacent surfaces, you can use surface tools such as Lofted Surface
• 5.
on the Surfaces toolbar, or Ruled Surface
on the Molds
toolbar. When you clear knit all surfaces, use Knit Surface in the Molds toolbar to manually knit the surfaces after the repairs. Clear Show Preview if you want to optimize system performance.
Click OK
.
With most mold parts, you need to also create interlocking surfaces. Interlock surfaces help prevent the core and cavity blocks from shifting, and are located along the perimeter of the parting surfaces. Usually, they have a 5 degree taper. With simpler models, you can create interlock surfaces using the same tools you used to create the parting surface.
8-8
Mold Tools - Tooling Split After you define a parting surface, use the Tooling Split tool to create the core and cavity blocks for the model. To create a tooling split, you need at least three surface bodies in the Surface Bodies folder. This model includes an interlock surface. It was created using the Ruled Surface tool using other surface modeling tools.
and it was finished
To create the tooling split:
1.
Select a face or plane on which to sketch an outline that separates the core and cavity segments.
2.
Click Tooling Split
3.
Orient the model so that the surface or plane you selected is normal to.
4.
Sketch a rectangle that extends beyond the model edge, but is within the parting surface boundaries.
5.
Close the sketch to open the Tooling Split PropertyManager. Under Core
, the Core Surface Bodies appear.
Under Cavity 6.
on the Molds Tools toolbar, or click Insert, Molds, Tooling Split.
, the Cavity Surface Bodies appear.
In the PropertyManager, under Block Size: •
Set a value for Depth in Direction 1
.
•
Set a value for Depth in Direction 2
.
•
Select Interlock surface if you want the system to create an interlock surface.
With most models, creating an interlock surface manually provides better control than relying on automatic creation. 7.
Under Parting Surface
8.
Click OK
SolidWorks 2004 Reference Guide
, select the parting surface created earlier.
.
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Chapter 8 Mold Design
Tooling split preview
Tooling split applied
Interlock Surface With most mold parts, you need to create interlock surfaces. Interlock surfaces help prevent the core and cavity blocks from shifting, and are located along the perimeter of the parting surfaces. Usually, they have a 5 degree taper.
Finishing the Interlock Surface
Lofted Surface
Ruled Surface Use Ruled Surface, rather than Extend Surface to maintain the correct taper.
Extend Surface To facilitate Trim Surface.
Trim Surface , using Mutual to remove material adjacent to the horizontal ruled surface. Knit Surface
8-10
after trim.
Create a plane, parallel to Top Plane. Sketch rectangle to create a planar surface.
Planar Surface
Trim Surface , using Standard to trim below the planar surface.
After trim, the planar surface is ready as the basis for tooling split operation.
Mold Tools - Insert Cavity To create a mold cavity:
1.
Prepare the interim assembly.
2.
In the assembly window, right-click the mold base in the graphics area or in the FeatureManager design tree and select Edit Part. - or Click the mold base, and click Edit Component
on the Assembly toolbar.
You are editing the part, not the assembly. The changes you make are reflected in the original part file of the mold base. If you do not want to affect the original mold base, use Save As in the mold base part document to save it with a different name for use in each new mold assembly. Otherwise, the original mold base includes the cavity you are about to insert. See also Editing Referenced File Locations. 3.
Click Cavity
4.
In the PropertyManager, under Design Components, select the design parts from the FeatureManager design tree.
SolidWorks 2004 Reference Guide
on the Mold Tools toolbar, or click Insert, Mold, Cavity.
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Chapter 8 Mold Design
5.
Under Scale Parameters: a.
b.
6.
Select the point about which scaling occurs for Scale About. •
Component Centroids. Scales the cavity for each part about its own centroid.
•
Component Origins. Scales the cavity for each part about its own origin.
•
Mold Base Origin. Scales the cavity for each part about the origin of the mold base part.
•
Coordinate System. Scales the cavity for each part about the selected coordinate system.
Enter the Scaling Factor in %. A positive value expands the cavity, a negative value shrinks the cavity. See Scaling Factor. •
Uniform scaling. Select Uniform scaling, and enter a value to scale in all directions.
•
Non-uniform scaling. Clear Uniform scaling, and enter a scaling value for the X, Y, and Z directions.
Click OK
.
A cavity in the shape of the design part is created. The cavity size reflects the scaling factor you specified.
Any changes you make to the design part automatically update the cavity in the mold base, as long as the update path is available. See also External References.
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9 Assemblies
Assemblies You can build complex assemblies consisting of many components. The components of an assembly can include both individual parts and other assemblies, called sub-assemblies. For most operations, the behavior of components is the same for both types. Components are linked to the assembly file. Assembly documents have the .sldasm extension. To create an assembly from a part:
1.
Click Make Assembly from Part/Assembly from Part.
on the Standard toolbar, or click File, Make Assembly
An assembly opens with the Insert Component PropertyManager active. 2.
Click in the graphics area to add the part to the assembly.
The following topics describe the basics of creating an assembly from components you have already built, and general information about working with assemblies of any kind. •
Design methods
•
Adding assembly components
•
Assembly mating
•
Working with sub-assemblies
•
Simplifying large assemblies
•
Using advanced component selection methods
•
Exploding an assembly view
•
Customizing the appearance of an assembly
•
Smart Fasteners
Design Methods You can create an assembly using bottom-up design, top-down design, or a combination of both methods. Bottom-up Design Bottom-up design is the traditional method. In bottom-up design, you create parts, insert them into an assembly, and mate them as required by your design. Bottom-up design is the preferred technique when you are using previously constructed, off-the-shelf parts. An advantage of bottom-up design is that because components are designed independently, their relationships and regeneration behavior are simpler than in top-down design. Working bottom-up allows you to focus on the individual parts. It is a good method to use if you do not need to create references that control the size or shape of parts with respect to each other.
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Chapter 9 Assemblies
Top-down Design Top-down design is different because you start your work in the assembly. You can use the geometry of one part to help define other parts, or to create machined features that are added only after the parts are assembled. You can start with a layout sketch, define fixed part locations, planes, and so on, then design the parts referencing these definitions. For example, you can insert a part in an assembly, then build a fixture based on this part. Working top-down, creating the fixture in context, allows you to reference model geometry, so you can control the dimensions of the fixture by creating geometric relations to the original part. That way, if you change a dimension of the part, the fixture automatically is updated.
The FeatureManager Design Tree in an Assembly FeatureManager Design Tree Conventions The FeatureManager design tree displays the names of these items in an assembly window: •
Top-level assembly (the first item in the tree)
•
Lighting
•
Assembly planes and origin
•
Components (sub-assemblies and individual parts)
•
Mategroup and mating relations
•
Assembly features (cuts or holes) and component patterns
, Annotations
, MateReferences
, and Simulation
folders
You can expand or collapse each component to view its detail by clicking beside the component name. To collapse all the items in the tree, right-click the assembly icon at the top of the tree, and select Collapse Items. You can use the same component multiple times within an assembly. Each component has the suffix
•
To display the hierarchy, right-click the assembly name in the FeatureManager design tree, and select Show Hierarchy Only. The FeatureManager design tree displays only the components (both parts and sub-assemblies), but no lower level detail.
•
9-2
To display the detail again, repeat the procedure, selecting Show Feature Detail.
To view an assembly by dependencies or by features:
•
To display the dependencies, right-click the assembly name in the FeatureManager design tree and select Tree Display, View Mates and Dependencies or click View, FeatureManager Tree, By Dependencies. Dependent items (instead of features) are listed under each component. Dependent items include mates and component patterns. You can view a component's features and planes by expanding the Features under the component.
•
folder
To display the features again, right-click the assembly name in the FeatureManager design tree, and select Tree Display, View Features or click View, FeatureManager Tree, By Features.
Component Icons in the FeatureManager Design Tree Resolved. The component is fully loaded into memory and all of its features and mates are editable. Lightweight. A feather overlay appears on the icon of a lightweight part. Out-of-Date Lightweight. A red feather overlay appears on the icon of an out-of-date lightweight part. Suppressed. A gray icon indicates that the component is not in use in the active configuration. Hidden. A transparent icon indicates that the component is active, but invisible. Hidden Lightweight. A transparent feather over a transparent component indicates that the component is lightweight and hidden. Hidden, Out-of-Date, and Lightweight. A transparent icon with a red feather overlay indicates that the component is hidden, out-of-date, and lightweight.
Viewing Mates View Mates displays a list of the mates for one or more components or sub-assemblies in an assembly. It is a useful tool to use when the number of mates gets large. To view the mates for a component:
1.
Right-click a component and select View Mates. The left panel splits to show the FeatureManager design tree and a list of the component's mates. TIP: To view the mates for more than one component, hold down Ctrl and select the components, then right-click and select View Mates. Mates between selected components are listed in bold.
2.
Click a mate to highlight the mated entities in the graphics area.
To view the mates for a sub-assembly:
Right-click a sub-assembly and select View Mates. Mates between sub-assembly reference geometry (such as planes), and reference geometry or components outside the sub-assembly are listed. Mates between the components of a sub-assembly are not listed. Mates between sub-assembly components and components outside the sub-assembly are not listed.
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Chapter 9 Assemblies
To view mates between the components of a sub-assembly:
1.
Expand
the sub-assembly in the FeatureManager design tree.
2.
Expand
the mategroup.
The mates are listed in the split panel display. To view the mates for a sub-assembly component:
1.
Expand
the sub-assembly.
2.
Right-click the component and select View Mates. The component's mates are listed.
Adding Components to an Assembly When you place a component (either an individual part or a sub-assembly) in an assembly, the component file is linked to the assembly file. The component appears in the assembly; the component data remains in the source component file. Any changes you make to the component file update the assembly. There are many ways to add components to a new or existing assembly: •
Use the Insert Component PropertyManager.
•
Drag from an open document window.
•
Drag from Windows Explorer.
•
Drag a hyperlink from Internet Explorer.
•
Drag within the assembly for additional instances of existing components.
•
Drag from the Feature Palette window.
•
Use Insert, Smart Fasteners to add bolts, screws, nuts, pins, and washers.
Insert Components To insert components into an assembly:
1.
Click Insert Components Assembly.
on the Assembly toolbar, or click Insert, Component, Existing Part/
Open documents that you previously saved appear under Part/Assembly to Insert. 2.
Select a part or assembly from the list, or click Browse to open an existing document.
3.
Click Keep Visible
4.
Click in the graphics area to place the component.
to add more than one instance of a component or more than one component.
If Keep Visible is not selected, the PropertyManager closes. If Keep Visible is selected, click again in the graphics area to add another instance of the selected component. Alternatively, you can repeat steps 2 through 4 to add a different component. Options
9-4
•
Start command when creating new assembly. Select to open this PropertyManager when you create a new assembly. Clear if your first assembly task is commonly something other than inserting components.
•
Graphics preview. Select to see a preview of the selected document in the graphics area under your pointer.
Adding Components from an Open Document Window To add components by dragging and dropping from an open document window:
1.
Open the destination assembly document, and open the source document (either the component document itself, or another assembly document that contains the component.)
2.
Click Window, Tile Horizontally (or Tile Vertically).
3.
Drag the component icon from the FeatureManager design tree of the source window, and drop it in the destination assembly window. If you are adding an individual part (not a sub-assembly), you can also drag the part from the graphics area of the source window. You can inference the assembly origin. If the component has multiple configurations, you can select which configuration to insert. Click the ConfigurationManager tab configuration.
in the source window, then drag and drop the name of the desired
Adding Components from Windows Explorer To add components by dragging and dropping from Windows Explorer:
1.
Open an assembly.
2.
Open Windows Explorer. Browse to the folder that contains the desired component.
3.
Drag the document icon from the Explorer window. A preview of the component appears.
4.
Drop it in the graphics area of the assembly window. You can inference the assembly origin. If the component has multiple configurations, the Select a configuration dialog box appears. Select the configuration you want to insert, and click OK.
Adding Components from Internet Explorer You can add a part from a hyperlink to an assembly. You can also drag and drop assemblies and .zip files from hyperlinks, but they open in their own window rather than as components of the assembly. To add a part from a hyperlink in Internet Explorer:
1.
In Internet Explorer, navigate to a location that contains hyperlinks to SolidWorks part files.
2.
Drag a hyperlink from the Internet Explorer window. A preview of the component appears.
3.
Drop it in the graphics area of the assembly window. The Save As dialog box appears.
4.
Browse to the folder where you want to save the part, enter a new name if desired, and click Save. The part document is saved to the specified folder.
5.
If the part has multiple configurations, the Select a configuration dialog box appears. Select the configuration you want to insert, and click OK. The part is added to the assembly.
Adding Components by Dragging and Dropping To add another component instance by dragging and dropping:
1.
With an assembly open, hold the Ctrl or Shift key, then drag a component either from the FeatureManager design tree, or from within the graphics area. A preview of the component appears.
2.
Drop it in the graphics area. You can inference the assembly origin. When you add a new instance of a component, the instance number suffix (component
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Inferencing to the Assembly Origin When you insert a component by various means, you can inference the assembly origin. Look for the pointer shown here when you point to the origin.
When you inference the assembly origin: •
the component is fixed (f)
•
the component origin is coincident with the assembly origin
•
the planes of the component and the assembly are aligned
You can also drop a component in the tree of the assembly window to inference the origin. The component is fixed only if it is the first component in the assembly.
Deleting Components from an Assembly To delete a component from an assembly:
1.
Click the component in the graphics area or in the FeatureManager design tree.
2.
Press the Delete key, click Edit, Delete, or right-click and select Delete.
3.
Click Yes to confirm the deletion. The component and all its dependent items (mates, component patterns, explode steps, and so on) are removed.
Saving an Assembly and Its Components When you save an assembly, the path and name of each referenced component is saved in the assembly document. For this reason, you must exercise caution when you save or rename a component document, or move it to a different folder. Under the File menu, there are several ways to save an assembly document. Whichever method you use, the current locations of all referenced components (parts and sub-assemblies) are saved with the assembly document.
9-6
•
Save. When you use Save, you save the assembly document, and any referenced component documents that have changed.
•
Save As. When you use Save As, you save a copy of the assembly document with a new name or path. You can create a new folder in the Save As dialog box if needed. After you use Save As, you are working in the new assembly document. The original assembly document is closed without saving.
•
Save as copy. Click the Save as copy check box in the Save As dialog box to save a copy of the assembly document, with a new name or path, without replacing the active document. You continue to work in the original assembly document.
•
With both Save As and Save as copy, if any of the components have changed since the last Save operation, you are notified that they need to be saved also. If you agree to save them, they are saved in their original referenced locations.
Saving an Assembly in Various Ways The following table lists the effects of saving an assembly in various ways. For this example, assume that these are the active documents: Assembly document
c:\test\Assem1
Referenced part documents
c:\test\PartA c:\test\PartB (changed since the last save)
Saved files
Active assembly after saving
Referenced File Locations
Save
c:\test\Assem1 c:\test\PartB
c:\test\Assem1
c:\test\PartA c:\test\PartB
Save As c:\final\Assem2
c:\final\Assem2 c:\test\PartB
c:\final\Assem2
c:\test\PartA c:\test\PartB
Save as copy c:\final\Assem2
c:\final\Assem2 c:\test\PartB
c:\test\Assem1
c:\test\PartA c:\test\PartB
Find References, then Copy files to c:\final
c:\final\PartA c:\final\PartB
c:\test\Assem1
c:\test\PartA c:\test\PartB
Replace Components An assembly and its components may go through many revisions during the course of a design cycle. This is especially true in a multi-user environment where several users can work on the individual parts and sub-assemblies. A safe, efficient way to update the assembly is to replace the components as needed. NOTES: •
You can replace a part with a sub-assembly or vice versa.
•
You can replace one, more than one, or all instances of a component at the same time.
To replace one or more components:
1.
Click Replace Components on the Assembly toolbar, click File, Replace, or right-click a component and select Replace Components. The Replace PropertyManager appears.
2.
Select the components to replace in the Replace these component(s) check box to replace all the instances of the selected component.
box. Select the All instances
3.
Click Browse to locate the replacement component for the With this one
4.
Under Configuration, select Match name to allow the software to try to match the configuration name of the old component with a configuration in the replacement component. Select Manually select to choose the matching configuration in the replacement component.
5.
Select Re-attach mates to allow the software to try to re-attach existing mates to the replacement component.
6.
Click OK
box.
.
The selected component instances are replaced. If you chose Manually select, choose the configuration to open in the Configurations dialog box. If you selected the Re-attach mates check box, the Mated Entities PropertyManager appears.
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Reload Documents Allows you to Reload documents. This is useful if you have read-only access to a document and you want to reload the latest version with any changes made by a colleague. To reload a document:
1.
Click File, Reload in a part or assembly document, or right-click a component in an assembly and select Reload.
2.
Select Open as read-only if you do not want to save any changes to the file. NOTE: If you have write-access to a sub-assembly then you reload it as read-only, you still have writeaccess to the individual components of the sub-assembly. You must reload each of the sub-assembly components as read-only to relinquish write-access privileges.
3.
Click OK. See also Replace Components.
Edit Referenced File Locations You can edit the locations of referenced parts: •
To open different parts for an assembly or drawing, - or -
•
To save selected assembly or drawing parts to a new location or filename.
NOTES: •
When saving, if the part filename already exists in the new location, you are prompted to confirm that you want to replace the part.
•
Only open documents appear in the list. For example, you must resolve lightweight components to see them in the list.
To edit part location:
1.
Click File, Open, References, or click File, Save As, References.
2.
In the New pathname list, select a path or filename that you want to edit , or click Select All.
3.
You can edit the path or filename using one of the following methods:
4.
•
Select a list entry by double-clicking. Browse to a new folder or type a new name in the Open dialog box, then click Open.
•
Select the check box for a list entry and click Browse to change to a new drive or directory path. The new drive or path appears in the New folder box.
•
Click Replace and enter a word to find and a word to replace with. (For example, change "\samples" to "\archive" to move one or all part files to the archive directory.) Click the Match case check box if the case is significant in the search.
Click OK to make the changes and exit the dialog. Click Cancel to exit without saving your changes.
Replace Mated Entities The Mated Entities PropertyManager helps you reattach dangling mate entities. You can list all of the mated entities in the assembly or in a particular component. Then you can replace any of the mated entities to satisfy the mates. For example, if you have a mate between two faces and you remove one of the faces from a model (by a cut or a fillet), the mate becomes dangling. You can use the Mated Entities PropertyManager to select a replacement face to satisfy the mate again.
9-8
To replace dangling mate entities:
1.
Right-click a mate, a component, or a mategroup and select Replace Mate Entities to replace the entities for a single mate, all the mates on a component, or all the mates in the assembly, respectively. - or Select a mate, a component, or a mategroup, then click Replace Mate Entities toolbar to replace the mate entities for the selected entity.
on the Assembly
The Mated Entities PropertyManager appears. Dangling mates appear with an X and satisfied mates appear with a checkmark in the Mate Entities list. 2.
Select an entity to replace in the Mate Entities list, then select a replacement entity. The replacement entity appears in Replacement Mate Entity
.
3.
Select Show all mates to show all satisfied and dangling mates. When cleared, only the dangling mates are shown.
4.
Click Flip Mate Alignment to toggle the alignment of the mate.
5.
Click Disable Preview to turn off the preview of the replacement mate.
6.
Click OK
to accept the new entities.
Assembly Statistics You can generate a report of the components and mates in an assembly. To generate a report of assembly statistics:
Click Statistics following items:
on the Tools menu, or click Tools, Assembly Statistics. The report includes the
•
total number of components
•
number of unique parts and sub-assemblies
•
number of suppressed, resolved and lightweight components
•
number of top-level mates
•
maximum depth of the assembly hierarchy (for nested sub-assemblies). When you are finished reading the report, click OK to close the dialog box.
Component Properties Lets you view or change the properties of a component. To view or change component properties:
1.
Right-click the component in the FeatureManager design tree and select Component Properties.
2.
Under General properties: o
o
o
Component Name. The part name is displayed, but usually is read-only. (If you want to change a component name, you must clear the Update component names when documents are replaced check box in the External References Options dialog box. Instance ID. The instance is 1 for the first time the component is used in the assembly; if it is used more than once, each occurrence is assigned a consecutive instance identification number. Full Name. The combination of the Component Name and Instance ID. You can copy the full name from this box, and paste it into table cells when creating a design table.
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o
o
Component Description. The description is read-only in this dialog box. You set it in the Summary Information dialog box of the component. Model Document Path. The path to the component document is displayed. You can click Browse to search for a replacement component. The last saved or in-use configuration of the replacement component is used.
3.
Select Configuration specific properties. The properties available depend on the type of assembly component you selected.
4.
Click OK when you finish making your changes.
Assembly Instance Color Lets you specify the color for selected component instances. •
Click Use Assembly to use the default color specified for the current assembly document, and override the color specified in the referenced part document. If different colors are specified for individual faces in the part document, these are overridden also.
•
Click Change Color to select a different color from the color palette, or to define a custom color for the selected instance.
•
Click Remove Color to return the selected component to the color specified in the referenced part document. This includes any colors specified for individual faces in the part document.
•
Click Advanced to set lighting display characteristics, such as transparency, shininess, and so on.
Arranging Components Assembly PropertyManager From this PropertyManager, you can do the following: •
Move a component.
•
Rotate a component.
•
Detect collisions with other components.
•
Activate Physical Dynamics
•
Dynamically detect the clearance between components. NOTE: The selections under Options appear in each of the topics listed above, as necessary for that topic.
Positioning Components in an Assembly Once a component is in an assembly, you can move it, rotate it, or fix its location. This is useful for rough placement of the components in the assembly. You can then position the components precisely using mating relationships. As you add mating relationships, you can move the components within the unconstrained degrees of freedom, visualizing the mechanism’s behavior. You can position a component in any of the following ways:
9-10
•
Fix the position of a component.
•
Move or rotate a component.
•
Add mates to a component.
•
Add SmartMates.
•
Use Physical Simulation.
Fixing the Position of a Component You can fix the position of a component so that it cannot move with respect to the assembly origin. By default, the first part in an assembly is fixed; however, you can float it at any time. It is recommended that at least one assembly component is either fixed, or mated to the assembly planes or origin. This gives a frame of reference for all other mates, and helps prevent unexpected movement of components when mates are added. •
A fixed component has a (f) before its name in the FeatureManager design tree.
•
A floating, under defined component has a (-) before its name in the FeatureManager design tree.
•
A fully defined component does not have a prefix.
To fix or float an assembly component:
1.
Right-click the component in the graphics area or the component’s name in the FeatureManager design tree.
2.
Select Fix or Float from the menu, depending on how you want the component to behave. NOTE: You cannot fix or float an instance in a component pattern.
Moving a Component To move components by dragging:
Drag a component in the graphics area. The component moves within its degrees of freedom. To prevent this behavior, click Tools, Options, System Options, Assemblies. Clear Move components by dragging, then click OK. To move components with a triad:
1.
Right-click a component and select Move with Triad.
2.
Drag the arm
3.
Drag the wing
4.
Drag the center sphere
5.
Right-click the center sphere and select from the following:
of the triad to move along the axis coincident with the arm. of the triad to move along the plane coincident with the wing. to a linear or planar entity to align the triad with the entity.
•
Show Translate XYZ Box. Moves the component to a specific XYZ coordinate.
•
Show Translate Delta XYZ Box. Moves the component by a specific amount.
•
Align to Component or Align to Assembly. Aligns the triad's axes to the component's or assembly's axes.
To move components with the PropertyManager:
1.
Click Move Component
on the Assembly toolbar, or click Tools, Component, Move.
The Move Component PropertyManager appears, and the pointer changes to 2.
Select one or more components in the graphics area.
3.
Select an item from the Move o o
.
list to move the components in one of following manners:
Free Drag - Select a component and drag in any direction. Along Assembly XYZ - Select a component and drag in the X, Y, or Z direction of the assembly. The coordinate system appears in the graphics area to help orient you. To select the axis you want to drag along, click near that axis before dragging.
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o
o
o
Along Entity - Select an entity, then select a component to drag along that entity. If the entity is a line, an edge, or an axis, the component you move has one degree of freedom. If the entity is a plane or a planar face, the component you move has two degrees of freedom. By Delta XYZ - Type an X, Y, or Z value in the PropertyManager, and click Apply. The component moves by the amount you specify. To XYZ Position - Select a point of a component, type an X, Y, or Z coordinate in the PropertyManager, and click Apply. The component’s point moves to the coordinate you specify. If you select something other than a vertex or point, the component’s origin is placed at the coordinate you specify.
You can select and move one component or group of components after another while the Move Component tool is active. 4.
Under Advanced Options, select This configuration to apply the movement of the components to only the active configuration.
5.
Click OK
or click Move Component
again when finished.
NOTES: •
You cannot move a component whose position is fixed or fully defined.
•
You can only move a component within the degrees of freedom allowed by its mating relationships.
Rotating a Component To rotate a component by dragging:
Right-click a component, hold down the right mouse button, and drag the component. The component rotates within its degrees of freedom. To prevent this behavior, click Tools, Options, System Options, Assemblies. Clear Move components by dragging, then click OK. To rotate a component with a triad:
1.
Right-click a component and select Move with Triad.
2.
Use the right-mouse button to drag the arm arm.
of the triad to rotate about the axis coincident with the
3.
Drag the center sphere
4.
Right-click the center sphere and select from the following:
to a linear or planar entity to align the triad with the entity.
•
Show Rotate Delta XYZ Box. Rotates the component by a specific amount about the specified arm of the triad.
•
Align to Component or Align to Assembly. Aligns the triad's axes to the component's or assembly's axes.
To rotate a component with the PropertyManager:
1.
Click Rotate Component
on the Assembly toolbar, or click Tools, Component, Rotate.
The Rotate Component PropertyManager appears, and the pointer changes to 2.
9-12
Select one or more components in the graphics area.
.
3.
Select an item from the Rotate
list to rotate the components in one of the following manners:
o
Free Drag - Select a component and drag in any direction.
o
About Entity - Select a line, an edge, or an axis, then drag a component around the selected entity.
o
By Delta XYZ - Type an X, Y, or Z value in the PropertyManager, and click Apply. The component moves around the assembly’s axes by the angular value you specify.
You can rotate one component or group of components after another; the tool remains active until you click it again, or select another tool. 4.
Under Advanced Options, select This configuration to apply the rotation of the components to only the active configuration.
5.
Click OK
or click Rotate Component
again when finished.
NOTES: •
You cannot rotate a component whose position is fixed or fully defined.
•
You can only rotate a component within the degrees of freedom allowed by its mating relationships.
Assembly Mates Mates create geometric relationships between assembly components. As you add mates, you define the allowable directions of linear or rotational motion of the components. You can move a component within its degrees of freedom, visualizing the assembly's behavior. Some examples include: •
A coincident mate forces two planar faces to become coplanar. The faces can move along one another, but cannot be pulled apart.
•
A concentric mate forces two cylindrical faces to become concentric. The faces can move along the common axis, but cannot be moved away from this axis.
Other topics about mates include: •
Mate PropertyManager
•
Standard Mates
•
Advanced mates including Cam Follower Mates, Gear Mates, Limit Mates, and Symmetry Mates.
•
SmartMates
Mate PropertyManager Mate Selections Select the faces, edges, planes, and so on that you want to mate together. See Standard Mates by Entity or see one of the mate types listed below. Standard Mates Angle, Coincident, Concentric, Distance, Parallel, Perpendicular, and Tangent mates are under Standard Mates. All the mate types are always shown in the PropertyManager, but only the mates that are applicable to the current selections are available. Toggle the Mate Alignment as necessary. Advanced Mates Cam, Gear, Limit, and Symmetric mates are under Advanced Mates. Toggle the Mate Alignment as necessary.
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Mates The Mates box contains all the mates added while the PropertyManager is open or all of the mates that you are editing. When there are multiple mates in the Mates box, you can select one to edit that mate. To edit more than one mate at a time, select multiple mates in the FeatureManager design tree, then right-click and select Edit Feature. All the mates appear in the Mates box. Options •
Add to new folder. When selected, new mates appear in a folder in the mategroup in the FeatureManager design tree. When cleared, new mates appear in the mategroup.
•
Show pop-up toolbar. When selected, the Mate pop-up toolbar appears when you add standard mates. When cleared, you add standard mates in hte PropertyManager.
•
Show preview. When selected, a preview of a mate occurs when you make enough selections for a valid mate.
•
Use for positioning only. When selected, components move to the position defined by the mate, but a mate is not added to the FeatureManager design tree. A mate appears in the Mates box so you can edit and position the components, but nothing appears in the FeatureManager design tree when you close the Mate PropertyManager. This check box is an alternative to adding many mates, then later deleting those mates in the FeatureManager design tree.
Standard Mates The valid mating relationships are: •
Coincident: positions selected faces, edges, and planes (in combination with each other or combined with a single vertex) so they share the same infinite line. Positions two vertices so they touch
•
Parallel: places the selected items so they lie in the same direction and remain a constant distance apart from each other
•
Perpendicular: places the selected items at a 90 degree angle to each other
•
Tangent: places the selected items in a tangent mate (at least one selection must be a cylindrical, conical, or spherical face)
•
Concentric: places the selections so that they share the same center point
•
Distance: places the selected items with the specified distance between them
•
Angle: places the selected items at the specified angle to each other
To add a standard mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
In the PropertyManager, under Mate Selections, select the entities that you want to mate together for Entities to Mate . The Mate pop-up toolbar appears with a default mate selected and the components move into place to preview the mate. The preceding occurs if you select Show pop-up toolbar and Show preview under Options in the PropertyManager.
9-14
3.
Click Add/Finish Mate
4.
Click OK
or select a different mate type.
to close the PropertyManager.
Standard Mates by Entity Mates create geometric relationships, such as coincident, perpendicular, tangent, and so on. Each mate is valid for specific combinations of geometry. Select one of the geometry types below to view its valid mates. Cam
•
Cam/Cylinder - Tangent
•
Cam/Plane - Tangent
•
Cam/Point - Coincident
Circular or Arc Edge
•
Circular or Arc Edge/Cone - Coincident, Concentric
•
Circular or Arc Edge/Line - Concentric
•
Circular or Arc Edge/Cylinder - Concentric, Coincident
•
Circular or Arc Edge/Plane - Coincident
•
Circular or Arc Edge/Circular or Arc Edge - Coincident
•
Cone/Circular or Arc Edge - Coincident, Concentric
•
Cone/Cone - Angle, Coincident, Concentric, Distance, Parallel, Perpendicular
•
Cone/Cylinder - Angle, Concentric, Parallel, Perpendicular
•
Cone/Extrusion - Angle, Parallel, Perpendicular
•
Cone/Line - Angle, Concentric, Parallel, Perpendicular
•
Cone/Plane - Tangent
•
Cone/Point - Coincident, Concentric
•
Cone/Sphere - Tangent
Cone
Cylinder
•
Cylinder/Cam - Tangent
•
Cylinder/Cone - Angle, Concentric, Parallel, Perpendicular
•
Cylinder/Cylinder - Angle, Concentric, Distance, Parallel, Perpendicular, Tangent
•
Cylinder/Extrusion - Angle, Parallel, Perpendicular, Tangent
•
Cylinder/Line - Angle, Coincident, Concentric, Distance, Parallel, Perpendicular, Tangent
•
Cylinder/Plane - Distance, Tangent
•
Cylinder/Point - Coincident, Concentric, Distance
•
Cylinder/Sphere - Concentric, Tangent
•
Cylinder/Circular Edge - Concentric, Coincident
•
Cylinder/Surface - Tangent
Extrusion
•
Extrusion/Cone - Angle, Parallel, Perpendicular
•
Extrusion/Cylinder - Angle, Parallel, Perpendicular, Tangent
•
Extrusion/Extrusion - Angle, Parallel, Perpendicular
•
Extrusion/Line - Angle, Parallel, Perpendicular
•
Extrusion/Plane - Tangent
•
Extrusion/Point - Coincident
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Line
•
Line/Cone - Angle, Concentric, Parallel, Perpendicular
•
Line/Cylinder - Angle, Coincident, Concentric, Distance, Parallel, Perpendicular, Tangent
•
Line/Extrusion - Angle, Parallel, Perpendicular
•
Line/Line - Angle, Coincident, Distance, Parallel, Perpendicular
•
Line/Plane - Coincident, Distance, Parallel, Perpendicular
•
Line/Point - Coincident, Distance
•
Line/Sphere - Concentric, Distance, Tangent
•
Line/Circular Edge - Concentric
•
Plane/Cam- Tangent
•
Plane/Cone - Tangent
•
Plane/Cylinder - Distance, Tangent
•
Plane/Extrusion - Tangent
•
Plane/Line - Coincident, Distance, Parallel, Perpendicular
•
Plane/Plane - Angle, Coincident, Distance, Parallel, Perpendicular
•
Plane/Point - Coincident, Distance
•
Plane/Sphere - Distance, Tangent
•
Plane/Circular Edge - Coincident
•
Plane/Surface - Tangent
•
Point/Cam - Coincident
•
Point/Cone - Coincident, Concentric
•
Point/Cylinder - Coincident, Concentric, Distance
•
Point/Extrusion - Coincident
•
Point/Line - Coincident, Distance
•
Point/Plane - Coincident, Distance
•
Point/Point - Coincident, Distance
•
Point/Sphere - Coincident, Concentric, Distance
•
Point/Surface - Coincident
•
Sphere/Cone - Tangent
•
Sphere/Cylinder - Concentric, Tangent
•
Sphere/Line - Concentric, Distance, Tangent
•
Sphere/Plane - Distance, Tangent
•
Sphere/Point - Coincident, Concentric, Distance
•
Sphere/Sphere - Concentric, Distance, Tangent
•
Surface/Cylinder - Tangent
•
Surface/Plane - Tangent
•
Surface/Point - Coincident
Plane
Point
Sphere
Surface
9-16
Mate Alignment You can set the alignment condition of standard and advanced mates in the Mate PropertyManager. The alignment conditions for a mate are: •
Aligned direction.
: places the components so the normal or axis vectors for the selected faces point in the same
•
Anti-Aligned : places the components so the normal or axis vectors for the selected faces point in opposite directions. These examples show the effect of changing the alignment condition for Coincident and Distance mates.
Aligned
Anti-aligned
Coincident
Distance
Mate Reference Mate references specify one or more entities of a component to use for automatic mating. When you drag a component with a mate reference into an assembly, the SolidWorks software tries to find other combinations of the same mate reference name and mate type. If the name is the same, but the type does not match, the software does not add the mate. Here are some items to note about mate references: •
Components. You can add mate references to part and assembly components. In assemblies, you can select assembly geometry (such as a plane in the assembly) or component geometry (such as the face of a component.)
•
Multiple mate references. A component can contain more than one mate reference. The MateReferences folder in the FeatureManager design tree holds all mate references. For example, you can have a component in an assembly with two mate references, bolt and washer. When you drag a fastener with a mate reference named bolt into the assembly, mates are added between the entities with the same mate reference name.
•
Multiple mated entities. Each mate reference can contain up to three mated entities: a primary, secondary, and tertiary reference entity. Each of these entities can have an assigned mate type and alignment. The primary reference entity on one component must mate to the primary reference entity on another component. For example, a shaft can have its cylindrical face assigned to a concentric mate and its planar end face assigned to a coincident mate. When you drag that component into an appropriate location in an assembly, the SolidWorks software adds both mates.
•
SmartMates. When the SmartMates PropertyManager is open, the software adds mates via mate references before it adds geometric SmartMates.
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To define a mate reference:
1.
In a part or an assembly, click Mate Reference Reference Geometry, Mate Reference.
on the Reference Geometry toolbar, or click Insert,
The Mate Reference PropertyManager appears. 2.
Under Reference Name, type a name for the mate reference.
3.
Under Primary Reference Entity: o
o
Select a face, edge, vertex, or plane for the Primary reference entity potential mates when dragging a component into an assembly. Select a Mate Reference Type mate for the reference entity.
. The entity is used for
and a Mate Reference Alignment
4.
If desired, repeat Step 3 to add secondary and tertiary entities.
5.
Click OK
to define the default
.
The mate reference is added to the FeatureManager design tree in the MateReferences
folder.
To capture a mate reference from an existing mate:
1.
Edit a component in the context of an assembly.
2.
Click Mate Reference
3.
In the PropertyManager, under References to Capture, select an entity or a mate.
.
The entity, mate, and alignment of the mate appear under Primary Reference Entity. 4.
Type a name under Reference Name and click OK
to add the mate reference to the component.
Mategroups When you create a new assembly, an empty mategroup is automatically included in the FeatureManager design tree. Each mating relationship that you create is added to this mategroup. The entry for each mating relationship includes the names of the components involved. All the mates within a mategroup are solved together; the order in which they appear within the mategroup does not matter. You can perform operations such as Replace Mate Entities on all the mates in a mategroup by selecting the mategroup in the FeatureManager design tree. You can add mates to a folder within a mategroup to sort the mates. Right-click the mates and select Add to New Folder or drag the mates into an existing folder. Additionally, you can select the Add to new folder check box under Options in the Mate PropertyManager.
9-18
Modifying a Mating Relationship To modify a mating relationship:
1.
Expand the mategroup in the FeatureManager design tree. Right-click one or more mates, and select Edit Feature. The mates appear under Mates in the PropertyManager and the related geometry is highlighted in the graphics area.
2.
In the PropertyManager, select the mate to edit under Mates and change the desired options. •
Mate Alignment (Aligned or Anti-aligned) on mates which imply a direction
•
Flip Dimension to reverse the direction in which a Distance or Angle mate is measured
•
Value of an Angle or Distance mate
•
Select a different mate type.
3.
To replace one entity with another, click the entity to replace in the Mate Selections then select the new entity.
4.
Click OK
box, press Delete,
to make the change.
NOTE: To change only the dimension value of a Distance or Angle mate, double-click the mate in the FeatureManager design tree, then double-click the dimension to edit. Enter the new value in the Modify box, then click Rebuild
.
Angle Mate You can add an angle mate between the combinations shown below: Cone - Cone - Cylinder - Extrusion - Line Cylinder - Cone - Cylinder - Extrusion - Line Extrusion - Cone - Cylinder - Extrusion - Line
Line - Cone - Cylinder - Extrusion - Line Plane - Plane
NOTE: •
A Cylinder refers to the cylinder's axis.
•
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
•
You must type an angle value in the Angle box in the Mate PropertyManager. The default value is the current angle between the selected entities.
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Coincident Mate You can add a coincident mate between the combinations shown below: Cone - Circular/Arc Edge - Cone - Point Cylinder - Line - Point - Circular/Arc Edge Extrusion - Point Line - Cylinder - Line - Plane - Point
Plane - Line - Plane - Point - Circular/Arc Edge Point - Cam - Cone - Cylinder - Extrusion - Line - Plane - Point - Sphere - Surface Sphere - Point
Circular/Arc Edge - Cone - Plane - Cylinder - Circular/Arc Edge Surface - Point
NOTE: •
Mates between two cones must use cones of the same half-angle.
•
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
Concentric Mate You can add a concentric mate between the combinations shown below: Cone - Circular/Arc Edge - Cone - Cylinder - Line - Point Cylinder - Cone - Cylinder - Line - Point - Sphere - Circular/Arc Edge
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Line - Cone - Cylinder - Sphere - Circular/Arc Edge Point - Cone - Cylinder - Sphere Sphere - Cylinder - Line - Point - Sphere
Circular/Arc Edge - Cone - Line - Cylinder - Circular/Arc Edge
Distance Mate You can add a distance mate between the combinations shown below: Cone - Cone Cylinder - Cylinder - Line - Plane - Point Line - Cylinder - Line - Plane - Point - Sphere
Plane - Cylinder - Line - Plane - Point - Sphere Point - Cylinder - Line - Plane - Point - Sphere Sphere - Line - Plane - Point - Sphere
NOTES: •
A Line can also refer to an axis in this instance.
•
You must type a distance value in the Distance box in the Mate PropertyManager. The default value is the current distance between the selected entities.
•
Mates between two cones must use cones of the same half-angle.
Parallel and Perpendicular Mates You can add a parallel or perpendicular mate between the combinations shown below: Cone - Cone - Cylinder - Extrusion - Line Cylinder - Cone - Cylinder - Extrusion - Line Extrusion - Cone - Cylinder - Extrusion - Line
Line - Cone - Cylinder - Extrusion - Line - Plane Plane - Line - Plane
NOTE: •
A Cylinder refers to the cylinder's axis.
•
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
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Tangent Mate You can add a tangent mate between the combinations shown below: Surface - Plane - Cylinder
Line - Cylinder - Sphere Plane - Cam - Cone - Cylinder - Extrusion - Sphere - Surface Sphere - Cone - Cylinder - Line - Plane - Sphere
Cone - Plane - Sphere Cylinder - Cam - Cylinder - Extrusion - Line - Plane - Sphere - Surface Extrusion - Cylinder - Plane
NOTE: •
An Extrusion refers to a single face of an extruded solid or surface feature. Extrusions with draft are not allowed.
Cam-Follower Mates A cam-follower mate is a type of tangent or coincident mate. It allows you to mate a cylinder, plane, or point to a series of tangent extruded faces, such as you would find on a cam. You can make the profile of the cam from lines, arcs, and splines, as long as they are tangent and form a closed loop. The following picture shows three followers which stay in contact with the cam as it rotates.
To add a cam-follower mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
Under Advanced Mates, click Cam
3.
Under Mate Selections, select the tangent faces on the cam for Entities to Mate
. .
Right-click one of the faces and click Select Tangency. This selects all the tangent faces in one step.
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4.
Click in Cam Follower and select a face or vertex on the cam follower.
5.
Click OK
.
6.
The follower is mated to all of the cam surfaces, allowing the follower to stay in contact with the cam as it rotates. A cam-follower mate for a cam made from a set of tangent surfaces appears in the FeatureManager design tree as CamMateCoincident or CamMateTangent. A cam-follower mate for a cam made from a single surface appears as Coincident or Tangent.
Gear Mates Gear mates force two components to rotate relative to one another about selected axes. Valid selections for the axis of rotation for gear mates include cylindrical and conical faces, axes, and linear edges. Other notes include: •
You can mate any two components that you want to rotate relative to one another. You do not have to mate two gears.
•
Similar to other mate types, gear mates do not prevent interference or collisions between components. To prevent interference, use Collision Detection or Interference Detection.
To add a gear mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
In the PropertyManager, under Advanced Mates: •
Click Gear
.
•
Type a value for Ratio to set the gear ratio.
•
Select Reverse to change the direction of rotation of the gears relative to one another.
3.
Under Mate Selections, select the rotation axes on the two gears for Entities to Mate
4.
Click OK
.
.
Limit Mates Limit mates allow components to move within a range of values for distance and angle mates. You specify a starting distance or angle as well as a maximum and minimum value.
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To add a limit mate:
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
In the PropertyManager, under Advanced Mates: •
Click Distance
or Angle
.
•
Set Distance or Angle to define the starting distance or angle.
•
Select Flip Dimension to move the entities to opposite sides of the dimension.
•
Set Maximum Value extents of the limit mate.
and Minimum Value
to define the maximum and minimum
3.
Under Mate Selections, select the entities to mate together for Entities to Mate
4.
Click OK
.
.
A LimitDistance or LimitAngle mate is added to the assembly. Symmetry Mate A symmetry mate forces two similar entities to be symmetric about a plane or planar face of a component or a plane of the assembly. The following entities are allowed in symmetry mates: •
Points such as vertices or sketch points
•
Lines such as edges, axes, or sketch lines
•
Planes or planar faces
•
Spheres of equal radii
•
Cylinders of equal radii
Please note the following items about symmetry mates: • Symmetry mates do not mirror the entire component about the plane of symmetry. • Symmetry mates only relate the selected entities to one another. In the illustration, the two highlighted faces are symmetric about the highlighted plane. Notice the two components are upside down with respect to one another. That is because the highlighted faces only are symmetric, not all of the faces of both components. To add a symmetry mate:
9-24
1.
Click Mate
on the Assembly toolbar, or click Insert, Mate.
2.
Under Advanced Mates, click Symmetric
3.
Under Mate Selections, select the two entities to be symmetric for Entities to Mate
4.
Click in Symmetry Plane and select the plane of symmetry.
5.
Click OK
.
. .
SmartMates You can create some types of mating relationships automatically. Mates created with these methods are referred to as SmartMates. •
You can create mates when you insert a part in the assembly, by dragging the part in specific ways from an open part window. The entity that you use to drag determines the types of mates that are added. See Geometry-Based Mates, Feature-Based Mates, and Pattern-Based Mates.
•
You can specify a mate reference in the part document. A mate reference identifies the entity to use for mating when you insert the part from a file. See Defining a Mate Reference.
•
You can create mates by inferring potential mate partners when you move a part within the assembly. See Adding SmartMates While Moving Components.
Geometry-Based Mates You can create some types of SmartMates by dragging parts into assemblies using certain model geometry. You inference the geometry of existing components to create mates as you drop the new parts. To create mates automatically, based on model geometry:
1.
Drag a part from an open part window into the graphics area of the assembly window, but do not drop it immediately. Use one of the following entities to drag the part: a linear or circular edge, a temporary axis, a vertex, a planar face, or a cylindrical/conical face. When the pointer is over an entity of another component that is a potential mate partner, the pointer changes to indicate the mate or mates that will result if the part is dropped at this location. A preview of the part snaps into place.
2.
If the preview indicates that you need to change the alignment condition, press the Tab key to flip the alignment (aligned/anti-aligned).
3.
Drop the part. The mates are added automatically. The following types of automatic mates are supported: Mating entities
Type of mate
2 linear edges
Coincident
2 planar faces
Coincident
2 vertices
Coincident
2 conical faces, or 2 axes, or 1 conical face and 1 axis
Concentric
2 circular edges (the edges do not have to be complete circles)
Concentric (conical faces) coincident (adjacent planar faces)
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Pointer
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Feature-Based Mates You can add mates automatically between features that have a "peg-in-hole" relationship. The requirements are as follows: •
One of the features must be a base or boss, and the other must be a hole or a cut.
•
The features may be extruded or revolved.
•
The conical faces that are used in the mate must both be of the same type (either a cone or a cylinder, not one of each type).
•
There must be a planar face adjacent to the conical face of both features.
Click for an example of feature-based mates. To create SmartMates using features:
1.
In the FeatureManager design tree of a part document, select a feature with a cylindrical or conical face. Drag the feature name into an assembly graphics window. When the pointer is over another cylindrical or conical face, it changes to indicate the mates that will result if the part is dropped at this location.
A preview of the part snaps into place. If the preview indicates that you need to change the alignment condition, press the Tab key to flip the alignment (aligned/anti-aligned). 2.
Drop the part. Two mates are applied: a Concentric mate between the cylindrical or conical faces, and a Coincident mate between the planar faces that are adjacent to the conical faces.
Example of Feature-Based Mates If you mate the cylindrical base of a screw to the cylindrical face of a countersunk hole, the planar face at the end of the screw mates to the planar face at the bottom of the hole. If you mate the conical boss of the screw to the conical face of the hole, the planar face on the head of the screw mates to the planar face at the top of the hole. If you create the whole screw as a single revolved base, then mate it to either face of the hole, the top planar faces are mated. When the set of faces matches this way, the coincident mate is applied where the faces meet at the largest circular edge.
Pattern-Based Mates In some special cases, you can create as many as three SmartMates at once. Each part must have a circular pattern of cylindrical holes (or bosses) on a planar face with a circular edge.
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To add SmartMates based on a feature pattern:
1.
Drag the component into the assembly using the circular edge. When the pointer is over another circular edge, it changes to to indicate the mates that will result if the component is dropped at this location. A preview of the part snaps into place.
2.
Press the Tab key to rotate the part that you are dragging, to align it with the desired pattern instance.
3.
Drop the component.
The following mates are added: o
A Concentric mate is added between the cylindrical faces.
o
A Coincident mate is added between the adjacent planar faces.
o
If possible, an additional Concentric mate is added between the pattern instance on the part that you are dragging and one on the part that is already in the assembly.
Adding SmartMates While Moving Components You can add SmartMates when you move a component in an assembly, even if the component is used in other mates. As you drag the component into place, you can infer potential mate partners for creating geometry-based SmartMates. NOTE: If a component is already used in other mates, you can only move it within the degrees of freedom allowed by those mates. Also, you cannot add SmartMates to an instance in a component pattern. To create SmartMates while moving a part:
1.
Hold down Alt and drag a component over potential mate pointers. The component becomes transparent and the pointer changes when it is over a valid mate partner.
2.
Drop the component to apply the mate.
To create SmartMates with the Move Component PropertyManager:
1.
Click Move Component
on the Assembly toolbar.
2.
In the PropertyManager, under Move, click SmartMates
3.
Double-click a component then click a valid mate partner.
.
The Mate pop-up toolbar appears and you can add a SmartMate.
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Deleting a Mating Relationship You can delete mates. When you delete a mate, it is deleted in all configurations of the assembly. To delete a mating relationship:
1.
Click the mate in the FeatureManager design tree.
2.
Press the Delete key, click Edit, Delete, or right-click and select Delete.
3.
Click Yes to confirm the deletion.
Suppressing a Mating Relationship You can suppress mates to prevent them from being solved. This allows you to experiment with different types of mates without over defining the assembly. To suppress a mate in the active configuration:
1.
Right-click the mate in the FeatureManager design tree, and select Properties.
2.
Select Suppressed, and click OK. To unsuppress the mate, repeat the process, and clear the Suppressed check box. You can also select one or more mates and click Suppress (or Unsuppress toolbar, or click Edit, Suppress (or Unsuppress), This Configuration.
) on the Features
To suppress a mate for one or more configurations:
1.
Select one or more mates and click Edit, Suppress (or Unsuppress), Specified Configurations (or All Configurations). If you select Specified Configurations, a dialog box appears.
2.
Select the configurations you want to change from the list, and click OK.
Mate Diagnostics Mate Diagnostics is a tool that allows you to identify mating problems in an assembly. You can examine the details of mates that are not satisfied, and identify groups of mates which over define the assembly. Versions of the software after SolidWorks 2001 may find a mating error that went undetected in earlier versions of SolidWorks. These are primarily conflicts between mates and in-context features. Remember that when this error occurs, it is important to understand that the mate problem is not a new one. It existed in earlier versions of SolidWorks but was not detected by the software. Mate Diagnostics can help you identify these errors. An assembly with one or more mates that are not satisfied has a red flag
next to the mategroup. An assembly with
one or more over defined mates and mates that are all satisfied has a yellow flag
next to the mategroup.
To diagnose mating problems:
1.
Expand
the mategroup
.
Mates which are not satisfied are highlighted with a red flag
.
Mates which are satisfied, but over define the assembly, are highlighted with a yellow exclamation point . 2.
Click Tools, Mate Diagnostics, or right-click the assembly, mategroup, or any mate in the mategroup, and select Mate Diagnostics.
3.
In the PropertyManager, under Analyze problem, click Diagnose. One or more subsets of mates with problems appear. In the graphics area, components that are not related to the current subset become transparent. A message appears with information on the mating problem.
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4.
Under Not satisfied mates, click a mate. The entities in the unsolved mate are highlighted in the graphics area. A message tells you the distance or angle by which the mated entities are currently misaligned. Mates that appear under Analyze Problem and Not Satisfied Mates appear in bold.
5.
6.
Right-click a mate in the PropertyManager and select: •
Suppress.
•
Edit Mates. Opens the Mate PropertyManager so you can edit the mate.
•
Toggle alignment. Toggles the mate alignment between aligned and anti-aligned. (Available only for mates with alignment problems.)
Click OK
.
NOTE: Mate Diagnostics analyzes only one mategroup at a time. Sub-assembly mategroups are not included in the analysis of a top-level assembly mategroup. You can analyze the mategroup in any sub-assembly separately. Conflicting Mates At times a mate can not be satisfied because the components are already constrained in such a way that they can not move into the mate. The components can be fixed or mated to other components. Example The bottom faces of these two blocks are mated to the same plane:
If you add a coincident mate between the side of one block and the side of the other, the blocks can move into the mate:
If you add a coincident mate between the bottom of one block and the top of the other, you get an error. The first block cannot be simultaneously mated to the plane and to the top of the second block, because the bottom of the second block is also mated to the plane. How Mate Diagnostics helps In this example, when you click Diagnose in Mate Diagnostics, the program lists three conflicting mates. These mates are the two Coincident mates to the plane and the bottom face to top face Coincident mate. When you click on the problem mate, Mate Diagnostics tells you that the mated faces are not coincident, that instead they are 40mm (the height of the block) apart. How you can fix the problem Delete or edit one of the conflicting mates.
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Design Errors and Mating Sometimes the geometry in or between your components appears to be accurate, but is slightly wrong. For example, you can have the following situations: •
Two components that look parallel, but are positioned to be slightly diverging.
•
An imported block that appears to have orthogonal sides, but the angle between two faces is actually 90.1 degrees.
•
Two components that appear to be the same height, but are slightly different.
•
Bolt holes in two components that should be the same distance apart, however one component was made using rounded metric units, and one using rounded English units.
These design errors (and others) can sometimes lead to mating errors. Example Suppose your intention is to align these two blocks so that they are coincident on one side and one end as shown. Your visual inspection makes you believe the blocks are each orthogonal.
You first add a coincident mate between the sides:
Then add a coincident mate between the ends:
The blocks do not move into the mate and a mating error appears in the FeatureManager design tree. How Mate Diagnostics helps When you click on the problem mate in Mate Diagnostics, a message appears which tells you that the faces in the mate are not parallel, and lists the angle between the faces. How you can fix the problem Change the geometry of one of the blocks so that the faces are parallel. Because your intention was for both blocks to be orthogonal, examine the blocks for the cause of the non-orthogonal geometry. In this case, the sketch for the base extrusion of one of the blocks was not a rectangle. You do not have to delete the problem mate. After you correct the geometry in your parts, the mate will be satisfied.
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Errors in Solving Mates If changes in a component remove an entity (face, edge, and so on,) that is involved in a mate, the mate cannot be solved. The mate is not deleted, however. The mate is suppressed, and is displayed in the FeatureManager design tree with an error symbol. Suppressed mates are not considered when the remaining mates are solved. Sometimes adding many mates can cause the position of a component to be over defined. To correct the situation, suppress the mates on the component individually, then test the degrees of freedom by dragging the component. That way you can identify and delete the mate that is causing the conflict. In-Context Mating Conflicts An in-context mating conflict can occur when you delete an Inplace mate then add a mate between a part that was created in the context of an assembly and another component. Example
Red block is in-context, blue block is fixed
Delete Inplace mate, add Distance mate
Mate solves by moving red block
Red block updates, but sketch origin moves
The red block was created in the context of the assembly by converting and extruding a face of the blue block. If you delete the Inplace mate and add a distance mate between the parts, the following occurs: 1.
SolidWorks tries to solve the distance mate by moving the red block. As the red block moves, the origin of the sketch for the base extrude of the red block moves.
2.
SolidWorks then updates the sketch for the base extrude of the red block by converting the sketch entities from the face of the blue block. The blocks appear exactly as they did previously, except that the origin of the sketch for the red block has moved relative to the blocks. If you have a drawing of the red block, the geometry may appear to have "walked" off the edge of the drawing.
In versions earlier than SolidWorks 2001Plus, the distance mate was not marked as an error, although it is clearly not satisfied. Mate Diagnostics detects this type of error, lists the Distance mate as not satisfied, and displays a message about the geometry of the mated faces. Mates to Dangling Geometry One type of mate error occurs when you change the geometry of a component so that the mate can no longer be satisfied. Example
Concentric Mate
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Dangling Concentric Mate
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In this example, there is a concentric mate between the two cylinders. Then, the sketch for the base feature of the bottom component changes from a circle to a rectangle. The cylindrical face of the bottom component no longer exists. The concentric mate to that face can no longer be solved. How Mate Diagnostics helps When you click Diagnose in Mate Diagnostics, a message appears telling you that a mate has dangling geometry. The mate and the missing geometry (in the example above, the cylindrical face of the bottom component) are listed. How you can fix the problem Delete the mate, or edit its definition to include different entities. Mating Conflicts with Sketch Relations If you have a sketch relation between a part sketch entity and assembly-level geometry, that sketch relation may come into conflict with a mate. Example
Add Colinear relation between line and assembly-level plane.
Relation is satisfied.
Add Distance mate between side of component and assembly-level plane.
Mating error. Part origin (at red arrow) moves.
In this example, the assembly-level plane cannot be both colinear with one side of the rectangular sketch, and at a distance from the side of the part created from that sketch. When you apply the distance mate, the part moves into the mate, and then the sketch updates to place the edge of the rectangle back at the assembly-level plane. If you have a drawing of the block, the geometry may appear to have "walked" off the edge of the drawing, since the part origin has moved. Mate Diagnostics detects this type of error, lists the Distance mate as not satisfied, and displays a message about the geometry of the mated faces.
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Physical Simulation Physical Simulation allows you to simulate the effects of motors, springs, and gravity on your assemblies. Physical Simulation combines simulation elements with SolidWorks tools such as mates and Physical Dynamics to move components around your assembly. To create a simulation:
1.
Add simulation elements. See Linear or Rotary Motors, Springs, and Gravity.
2.
Record the simulation. See Recording and Replaying a Simulation.
3.
Playback the simulation. See Recording and Replaying a Simulation.
NOTES: •
A simulation that you record is valid for as long as you do not make changes to the assembly. If you delete, suppress, move, replace, fix, float, or change a component that is included in a recorded simulation, the simulation is no longer valid.
•
Physical Simulation uses the Sensitivity setting of Physical Dynamics to check for collisions. To change this setting, click Move Component slider.
•
, select Physical Dynamics under Options, then move the Sensitivity
You can suppress and configure the suppression state of the Simulation folder in the FeatureManager design tree and its simulation elements. Suppressing the folder also suppresses its elements.
Linear or Rotary Motors Linear and rotary motors are simulation elements that move components around an assembly using Physical Simulation. Physical Simulation combines simulation elements with other tools such as mates and Physical Dynamics to move components in a realistic manner within the components degrees of freedom. See Recording and Replaying a Simulation for more information on creating a simulation. NOTES: •
Motors move components in a selected direction, but they are not forces. Motor strength does not vary based on component size or mass. For example, a small cube moves at the same speed as a large cube if the Velocity slider is set to an equal value.
•
If another force (for example, a collision with another component) causes a motor's Direction Reference to change orientation, the motor will move the component in the new direction.
•
It is recommended that you do not add more than one motor of the same type to the same component.
•
Motion due to motors supersedes motion due to gravity or springs. If you have a motor moving a component to the left and a spring pulling a component to the right, the component moves to the left.
To add a linear motor:
1.
Click Linear Motor
on the Simulation toolbar, or click Insert, Simulation, Linear Motor.
The Linear Motor PropertyManager appears. 2.
Select a linear or circular edge, a planar, cylindrical, or conical face, or an axis or a plane of a component as the Direction Reference. Click Reverse Direction , if necessary. If you select a circular edge or conical face, the Direction Reference is parallel to the axis of the cylinder. If you select a plane or a planar face, the Direction Reference is normal to the entity.
3.
Move the Velocity slider to to the right to increase the speed of the motor or to the left to decrease the speed. The Velocity is the speed at which a component moves if no other force acts on it.
4.
Click OK
.
A LinearMotor
SolidWorks 2004 Reference Guide
icon is added to the FeatureManager design tree under the Simulation
icon.
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Chapter 9 Assemblies
To add a rotary motor:
1.
Click Rotary Motor
on the Simulation toolbar, or click Insert, Simulation, Rotary Motor.
The Rotary Motor PropertyManager appears. 2.
Select a linear or circular edge, a planar, cylindrical, or conical face, or an axis or a plane of a component as the Direction Reference. Click Reverse Direction
, if necessary.
The Direction Reference is the direction of rotation, not the axis of rotation. The Direction Reference is parallel to the axis of rotation. The software moves the component about its center of mass taking into account mates and other relations to the component. If you select a linear edge, the Direction Reference revolves around the edge. If you select a planar face, the Direction Reference revolves around the normal of the face. 3.
Move the Velocity slider to to the right to increase the speed of the motor or to the left to decrease the speed. The Velocity is the speed at which a component moves if no other force acts on it.
4.
Click OK
.
A RotaryMotor
icon is added to the FeatureManager design tree under the Simulation
icon.
Linear Springs Linear springs are simulation elements that move components around an assembly using Physical Simulation. Physical Simulation combines simulation elements with other tools such as mates and Physical Dynamics to move components in a realistic manner within the components degrees of freedom. NOTES: •
Springs apply a force to a component. A spring with a higher spring constant will move a component faster than a spring with a lower spring constant. Also, a component with a smaller mass will move faster than a component with a larger mass if acted upon by an equal strength spring.
•
Motion due to a spring stops when the spring reaches its free length.
•
Motion due to motors supersedes motion due to springs. If you have a motor moving a component to the left and a spring pulling a component to the right, the component moves to the left.
See Recording and Replaying a Simulation for more information on creating a simulation. To add a spring:
1.
Click Linear Spring
on the Simulation toolbar, or click Insert, Simulation, Linear Spring.
The Linear Spring PropertyManager appears. 2.
Select two Spring Endpoints points.
to connect the spring. You can select linear edges, vertices, or sketch
If you select an edge, the Spring Endpoint attaches to the midpoint of the edge. 3.
Type a value for Free Length to determine if the spring is stretched or compressed.
4.
Type a value for Spring Constant to determine the strength of the spring.
5.
Click OK
.
A LinearSpring
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icon is added to the FeatureManager design tree under the Simulation
icon.
Gravity Gravity is a simulation element that moves components around an assembly using Physical Simulation. Physical Simulation combines simulation elements with other tools such as mates and Physical Dynamics to move components in a realistic manner within the components degrees of freedom. See Recording and Replaying a Simulation for more information on creating a simulation. NOTES: •
You can define one gravity simulation element per assembly.
•
All components move at the same speed under the effect of gravity regardless of their mass.
•
Motion due to motors supersedes motion due to gravity. If you have a motor moving a component to the left and gravity pulling a component to the right, the component moves to the left without any pull to the right.
To add gravity:
1.
Click Gravity
on the Simulation toolbar, or click Insert, Simulation, Gravity.
The Gravity PropertyManager appears. 2.
Select a linear edge, a planar face, a plane, or an axis as the Direction Reference. Click Reverse Direction , if necessary. If you select a plane or a planar face, the Direction Reference is normal to the selected entity.
3.
Move the Strength slider to to the right to increase the gravitational strength or to the left to decrease the strength.
4.
Click OK
.
A Gravity
icon is added to the FeatureManager design tree under the Simulation
icon.
Recording and Replaying a Simulation Physical Simulation allows you to simulate the effects of motors, springs, and gravity on your assemblies. When you record a simulation, the affected components move to a new location in the assembly. You can then replay the simulation to view it again. NOTES: •
You cannot interact with the assembly components when you are recording a simulation. You cannot use the Move Component
or Rotate Component
tools to move components during the simulation.
•
If there is an initial collision between two or more components, Physical Simulation ignores collisions between these components while recording a simulation. If the components no longer collide due to the motion of a simulation, Physical Simulation takes subsequent collisions between the components into account.
•
When you record a simulation, components with in-context references may move if you do not fully define the position of the components. Be cautious when using Physical Simulation in an assembly with in-context references.
•
When replaying a simulation, the components do not actually move to their original positions. Temporarily, the components appear in their original positions in the graphics area to show the start of the simulation. The replay of the simulation is for graphical purposes only.
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To record a simulation:
1.
Add simulation elements. See Linear or Rotary Motors, Springs, and Gravity.
2.
Click Calculate Simulation
on the Simulation toolbar.
The components move within their degrees of freedom according to the simulation elements. The degrees of freedom are determined by the mates on the component and collisions with other components. 3.
Click Stop Record or Playback on the Simulation toolbar to end the simulation. Sometimes the simulation stops automatically if the components can no longer move within their degrees of freedom. The components are in their new position.
4.
If desired, click Reset Components original position.
on the Simulation toolbar to return the components to their
To replay a simulation:
1.
Click Replay Simulation
to replay the simulation from the beginning to the end.
2.
Click a tool on the Animation Controller pop-up toolbar. For example, you can continuously replay the simulation or replay it at one-half speed.
Sub-assemblies Working with Sub-assemblies When an assembly is a component of another assembly, it is referred to as a sub-assembly. You can nest subassemblies in multiple levels, to reflect the hierarchy of your design. Creating a Sub-assembly There are several ways to create a sub-assembly: •
You can create an assembly document as a separate operation, then make it a sub-assembly by inserting it as a component in a higher-level assembly.
•
You can insert a new, empty sub-assembly at any level of the assembly hierarchy while you are editing a top-level assembly, then add components to it in a variety of ways.
•
You can form a sub-assembly by selecting a group of components that are already in the assembly. This creates a sub-assembly and adds components to it in a single step.
Modifying a Sub-assembly •
As you develop an assembly, you can modify its sub-assemblies in these ways:
•
You can dissolve a sub-assembly into individual components, thereby moving the components up one level in the assembly hierarchy.
•
You can edit the assembly structure by moving components up or down in the hierarchy, or to a different branch of the hierarchy. There are two ways to do this:
•
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•
Drag and drop the components to move them from one assembly to another.
•
Click Tools, Reorganize Components. This method can be easier to use when the FeatureManager design tree is very long, and therefore requires a lot of scrolling.
You can change the order of the components within a level of the hierarchy.
Forming a New Assembly from Existing Components You can form a sub-assembly from components that are already in the assembly, thereby moving the components down one level in the assembly hierarchy. It is a good idea to position and mate at least one of the components before you begin, then select that component first. To form a new assembly from existing components:
1.
In the FeatureManager design tree, select the components (individual parts or sub-assemblies) that you want to group into a sub-assembly. Hold the Ctrl key while you select. All the components must be at the same level within a single parent assembly.
2.
Right-click one of the selected components, and select Form New Sub-assembly Here. - or Select the components, then click Insert, Component, Assembly from [Selected] Components. The Save As dialog box appears.
3.
Browse to a different folder if needed, enter a File name, and click Save. A new assembly document is saved in the folder you specify. A new sub-assembly is inserted at the level where the selected components were located, and the components are moved into the new sub-assembly.
Sub-assembly from Selected Components In this example, P1 and P2 are selected to form a new sub-assembly, S1.
Instead of referencing the individual component documents P1 and P2, assembly A now references the sub-assembly document S1. Any mates that exist between components P1 and P2 move from the mategroup of assembly A to the mategroup of sub-assembly S1.
Dragging Components to Edit the Assembly Structure To reorganize components in sub-assemblies by dragging components:
Drag the component icon in the FeatureManager design tree, and drop it on the icon for the destination assembly (either the top-level assembly, or a sub-assembly at any level of the hierarchy). If the destination assembly is expanded, you can also drop the icon in the component section of the destination assembly. As you drag, watch for the
pointer.
To move multiple components at once, hold Ctrl as you select the icons. All the components selected for a move operation must be from the same level of a single assembly. If any components or features will be deleted as a result of the move, the Assembly Structure Editing dialog box appears, with a list of the affected items. TIP: If you are removing the last component of a sub-assembly, the empty sub-assembly is left in the FeatureManager design tree. If you want to move the last component up a level and remove the empty sub-assembly at the same time, dissolve the sub-assembly instead.
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Assembly Structure Editing To modify the assembly structure:
1.
Click Tools, Reorganize Components.
2.
Select the components that you want to move, either in the FeatureManager design tree or in the graphics area. The selected components are listed in the Components to move box. All the components selected for a single operation must be at the same level in one parent assembly.
3.
Click the Destination assembly box, then click the appropriate assembly icon in the FeatureManager design tree. If any components or features will be deleted as a result of the move, the dialog box expands to display a list of the affected items. See Effects of Assembly Structure Editing.
4.
Click Move. The component icons appear at the end of the component section of the destination assembly.
Effects of Assembly Structure Editing When you dissolve a sub-assembly, or reorganize the components at any level, the mates and any features that reference the selected components are affected. Therefore, decisions about hierarchical groupings should be made early in development of a complex assembly, in order to minimize the effects on these items. •
Mates move to the mategroup of the lowest common parent. For example, assume that there is a mate between P1 and P2, in the mategroup of the nested sub-assembly S3. • If you move P1 up one level (into S1), the mate moves to the mategroup of S1, the lowest common parent on the same branch. • If you move P1 into S2 (a different branch), the mate moves to the mategroup of the top-level assembly A, because A is the only common parent. • If you dissolve S3, the mate moves to the mategroup of sub-assembly S1.
•
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Component patterns have these specific limitations: •
If you move the seed component of a pattern into a different assembly, the pattern feature and all the instances generated by the pattern are deleted.
•
If you dissolve a sub-assembly that has a component pattern, the pattern feature and pattern instances are deleted. The seed component becomes a component of the assembly at the next higher level.
•
You cannot move individual instances generated by the pattern.
•
Assembly feature cuts and holes are deleted.
•
Equations may not solve. This is because, in many cases, the instance number suffix
•
Explode steps that explode the reorganized component are deleted.
•
Piping sub-assemblies are subject to some special rules. See SolidWorks Piping Help for more information.
Changing the Order of Components You can change the order of the components within a level of the assembly hierarchy. By default, assembly components appear in the FeatureManager design tree in the order in which they are added. The same order is used in a bill of materials in a drawing of the assembly. By changing the order in the assembly, you can control the order in the bill of materials. To change the order of components:
Drag and drop the icons in the FeatureManager design tree to rearrange the order. The component is placed below the icon where you drop it (the highlighted icon). Watch for the
pointer.
To place a component directly below a sub-assembly, press Alt to change from a reorganize operation (with the pointer) to a reorder operation.
Inserting a New Sub-assembly You can insert a new, empty sub-assembly at any level of the assembly hierarchy. Then you can add components to it in a number of ways. To insert a new sub-assembly:
1.
In the FeatureManager design tree, right-click either the top-level assembly icon or the icon for an existing sub-assembly, and select Insert New Sub-assembly. - or Click New Assembly
on the Assembly toolbar, or click Insert, Component, New Assembly.
The Save As dialog box appears. 2.
Browse to a different folder if needed, enter a File name for the new assembly document, and click Save. An empty sub-assembly is inserted as the last component of the selected assembly, and a new assembly document (.sldasm) is created and saved in the folder you specify.
3.
Add components to the sub-assembly: •
To move a component that is already in the assembly into the sub-assembly, see Dragging Components to Edit the Assembly Structure or Assembly Structure Editing.
•
To add an existing, saved component to the sub-assembly, right-click the sub-assembly icon in the FeatureManager design tree, and select Edit Sub-assembly. Then insert components using any of the methods in Adding Components to an Assembly.
•
To insert a new component into a sub-assembly, you must edit the sub-assembly in its own window. You cannot insert a new component into a sub-assembly while you are editing the top-level assembly. Also, you cannot insert a new component while you are editing the sub-assembly in the context of a higher level assembly. Right-click the sub-assembly icon in the FeatureManager design tree, and select Open <subassembly.sldasm> to open the sub-assembly in its own window. Then add a new component.
Dissolving a Sub-assembly You can dissolve a sub-assembly into individual components, thereby moving the components up one level in the assembly hierarchy. To dissolve a sub-assembly:
In the FeatureManager design tree, right-click the sub-assembly you want to dissolve, and select Dissolve Subassembly. You can also select the sub-assembly icon and click Edit, Dissolve Assembly. The components become components of the immediate parent assembly, and the sub-assembly is removed. The assembly document itself is not deleted from the folder where it is stored.
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Example of Dissolving a Sub-assembly In this example, when you dissolve sub-assembly S1, components P1 and P2 become components of the top-level assembly A.
Instead of referencing the sub-assembly document S1, assembly A now references the individual component documents P1 and P2. Any mates that exist between components P1 and P2 move to the mategroup of assembly A.
Changing the Editing Focus Manually For some types of editing operations, you need to specify that the changes you are making belong to the subassembly, and not to the top-level assembly. This includes any case where the edits could be successfully applied to either one. For example, you can add an assembly feature hole either to a sub-assembly, or to the top-level assembly, with different results. You must activate the sub-assembly to perform these editing operations: •
Add a component into the sub-assembly. You cannot add a new component in the context of a sub-assembly.
•
Delete a component from a sub-assembly.
•
Add a component pattern, an assembly feature cut or hole, a sketch, or reference geometry to the subassembly.
•
Use dynamic assembly motion on sub-assembly components. You can fix, float, and move sub-assembly components when the sub-assembly is active, to visualize the movement within the sub-assembly.
•
Add a mate between components of the active sub-assembly (both at the same level in the hierarchy, or one at a lower level, in a nested sub-assembly of the active sub-assembly).
NOTE: While a sub-assembly is active, the mates in the top-level assembly that position the sub-assembly with respect to the top-level are temporarily ignored. Top-level mates are solved again when you return to editing the toplevel assembly and click Rebuild
.
You cannot add a mate between a component within an active sub-assembly and a component outside the active subassembly. To activate a sub-assembly for editing in context:
Right-click the sub-assembly icon in the FeatureManager design tree, and select Edit Sub-assembly. When you activate a sub-assembly, it turns pink, and the rest of the assembly turns gray, just as it does when you edit a part. When you edit a component of a sub-assembly, only the individual part being edited turns pink.
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Automatic Change of Editing Focus For some types of editing operations, the software recognizes that the changes you are making belong to the subassembly, and not to the top-level assembly. In those cases, the editing focus automatically changes from the top-level assembly to the sub-assembly. If you edit any of the following items that belong to a sub-assembly, the editing focus changes automatically: •
sketch
•
component pattern
•
mate
•
assembly feature (cut or hole)
•
reference geometry.
Similarly, if you edit a feature (the definition or the sketch) of a sub-assembly component, the software automatically changes to Editing Part mode. References that you make while editing a sub-assembly component are always made in the context of the top-level assembly, not the sub-assembly that contains it. If you add a mate between a sub-assembly component and some geometry outside that sub-assembly, the focus changes to the sub-assembly automatically. The mate is added to the lowest level assembly that contains both components (the lowest common parent).
Limitations in Sub-assembly Editing Most of the operations available for editing a sub-assembly on its own are available when editing a sub-assembly in context. However, there are a few operations that cannot be performed while editing a sub-assembly in context: •
creating a new component in context
•
inserting or modifying a weld bead
For these operations, you must open and edit the sub-assembly in its own window.
Flexible Sub-Assemblies You can make sub-assemblies flexible. This allows movement of the individual components of a sub-assembly within the parent assembly. An example of the benefit of this function is when you want to move the components of a piston sub-assembly in a motor assembly. You can move the individual components of the piston while still grouping the components as a subassembly. Please note the following regarding flexible sub-assemblies: •
Mates. The mates in a flexible sub-assembly are solved simultaneously with the mates of the parent assembly. Therefore, moving or rotating a sub-assembly component does not violate the mates in the subassembly or its parent. A component moves only within its degrees of freedom according to its mates.
•
Configurations. Each flexible sub-assembly must have its own unique configuration. This is because the position of a component in one flexible sub-assembly could be in a different position in another configuration of the flexible sub-assembly.
To make a sub-assembly flexible:
1.
Right-click a sub-assembly in the FeatureManager design tree and select Component Properties. The Component Properties dialog box appears.
2.
Under Solve as, click Flexible, then click OK.
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Working with Parts Within an Assembly Working with Parts within an Assembly In top-down assembly design, you build and modify parts within the context of an assembly. Parts created or modified in the context of an assembly contain external references and time-dependent features. Some of the techniques for working with parts in an assembly include: •
Create and edit components within the context of the assembly. That way, you can use the geometry of one component to help define another. When you create references between components, the models are fully associative. Changes you make to a referenced component cause the others to update accordingly.
•
Start with a layout sketch that defines fixed component locations, planes, and so on, then design the parts referencing these definitions.
•
Create assembly features that are added only after the components are assembled. These assembly features exist only in the context of the assembly.
•
Place patterns of components, either by referencing a pattern feature on one of the components, or by creating a pattern in the assembly.
•
Merge the bodies of assembly components by using a join operation.
External References An external reference is created when one document is dependent on another document for its solution. If the referenced document changes, the dependent document changes also. In an assembly, you can create an in-context feature on one component that references the geometry of another component. This in-context feature has an external reference to the other component. If you change the geometry on the referenced component, the associated in-context feature changes accordingly. An in-context feature updates automatically if the update path is available. The update path is contained in the assembly where you create the reference. Update paths for in-context features are displayed in the FeatureManager design tree. If the update path is not available (for example, if the assembly document is closed), updating occurs the next time you open the assembly that contains the update path. See Understanding the Update Path for more information. FeatureManager design tree conventions In the FeatureManager design tree, any item with an external reference has a suffix that indicates the status of the reference: •
The suffix -> means that the reference is in-context. It is solved and up-to-date.
•
The suffix ->? means that the reference is out-of-context. The feature is not solved or not up-to-date. To solve and update the feature, open the assembly that contains the update path.
•
The suffix ->* means that the reference is locked.
•
The suffix ->x means that the reference is broken.
See Locking and Breaking External References for more information. To list the external references on a part or feature:
Right-click the part or the feature with the external reference, and select List External Refs. The referenced components, features, and entities are listed, as well as the status of each reference. See Rules for External References for more information. TIP: To reduce the size of the FeatureManager design tree, you can hide all of these in-context icons. Rightclick the top-level assembly icon
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and select Hide Update Holders.
Understanding the Update Path Consider the example of an assembly that contains two components: a mold base and a design component. In the context of the assembly, you create a cavity feature in the mold base, with an external reference to the design component. The update path for the cavity feature is therefore contained in the assembly. Now, suppose that you need to change the design component and you need to update the mold base accordingly. •
If the assembly is open, the cavity feature in the mold base updates automatically when you make the changes to the design component.
•
If the assembly is closed, the cavity feature cannot be updated to reflect the changes until you open the assembly, thereby making the update path available.
Locking and Breaking External References You can lock, unlock, or break the external references of a component. When you lock the external references on a component, the existing references no longer update and you cannot add any new references to that component. Once you unlock the external references, you can add new references or edit the existing references. When you break the external references, the existing external references no longer update and you can add new references to the component. To lock, unlock, or break the external references:
1.
Right-click the feature or the component with the external references in the FeatureManager design tree and select List External Refs. The External References For dialog box appears.
2.
Click Lock All to lock all of the external references for this component. The suffix for the component changes from -> to ->*.
3.
Click Unlock All to unlock the references for this component. The suffix for the component changes back to ->.
4.
Click Break All to permanently break the external references for this component. The suffix for the component changes to ->x. To list the broken references in the External References For dialog box, select the List Broken References check box.
5.
Click OK to close the dialog box.
Rules for External References •
A component cannot have an external reference to itself (a circular reference).
•
You cannot reference one instance of a part to create a feature on another instance of the same part, even if the instances are in different configurations.
•
You cannot replace a part with another part created by deriving the second part from the first. See Derive Component Part for more information.
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List External References You can list the external references of any component or feature created in the context of an assembly. You can also list the references for various types of derived parts. To list the external references for a feature, an assembly component, or a derived part:
Right-click the feature, component, or part in the FeatureManager design tree and select List External Refs. This operation is only available for items that have external references. The External References For dialog box appears. o
The Part or Assembly box displays the path and name of the assembly in which the component or feature was created.
o
Configuration. Select the configuration of the referenced component to use for a derived part.
o
The Feature column lists each in-context item (sketches, features, and so on) in the selected part.
o
o o
o
The Data column describes the type of data used to create the item (converted edge or face, converted or offset sketch entity, body, and so on). The Status of each reference. This can be In context or Out of context, Locked, or Broken. The Referenced Entity describes the actual item being used, and the name of the document that contains the item. The Feature’s Component column displays the name of the component in which the affected feature exists. This information is displayed only when the Referenced entity is in a different component in an assembly; this column does not apply to derived parts.
To lock, unlock, or break external references, see Locking and Breaking External References.
Searching for Referenced Documents When opening a referenced document, SolidWorks performs a search to locate the document. For example, this search may occur when you open a drawing and the referenced assembly cannot be found or when you resolve a lightweight component in an assembly. When a referenced document is found, the software updates the path to the referenced document in the parent document. When you save the parent document, the updated path is saved as well. The Rules column below describes the search routine that the software uses to locate a missing referenced document. The Examples column shows the paths that the software checks using the following scenario:
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•
The assembly was last saved as C:\zz\a1.sldasm. You move the assembly to D:\ss\tt\a1.sldasm.
•
The first part in the assembly was last saved as C:\qq\p1.sldprt. You do not move this part.
•
The second part in the assembly was last saved as C:\zz\yy\xx\p2.sldprt. This part is missing either through deletion, renaming, or some other file management mistake.
•
There are two paths in the Folders list of the File Locations Options dialog box: D:\aa\bb\ and E:\cc\dd\
•
You click File, Open to open a1.sldasm in its new location.
Rules
Examples
1.
Uses any open document with the same name.
If p2.sldprt is in another open document, SolidWorks uses this version of p2.sldprt.
2.
Searches the first path that you specify in the Folders list in the File Locations Options dialog box.
D:\aa\bb\p2.sldprt
NOTE: You must select the Search file locations for external references check box in the External References Options dialog box or else SolidWorks ignores the paths that you specify. 3.
Searches the path in Step 2 plus the last folder in the path where the referenced document was last saved.
D:\aa\bb\xx\p2.sldprt
4.
Searches the path in Step 2 plus the last two folders in the path where the referenced document was last saved.
D:\aa\bb\yy\xx\p2.sldprt
5.
Repeats Step 4 until the full original path has been appended to the the path in Step 2.
D:\aa\bb\zz\yy\xx\p2.sldprt
NOTE: This concept of adding one folder at a time from the full path will be called "recursive searching" in the following steps. 6.
Recursively searches the first path in the Folders list, then recursively searches the path where the referenced document was last saved.
D:\aa\xx\p2.sldprt D:\aa\yy\xx\p2.sldprt D:\aa\zz\yy\xx\p2.sldprt D:\xx\p2.sldprt D:\yy\xx\p2.sldprt D:\zz\yy\xx\p2.sldprt
7.
Repeats Steps 2 through 6 for the other folders in the Folders list.
E:\cc\dd\p2.sldprt E:\cc\dd\xx\p2.sldprt E:\cc\dd\yy\xx\p2.sldprt E:\cc\dd\zz\yy\xx\p2.sldprt E:\cc\xx\p2.sldprt E:\cc\yy\xx\p2.sldprt E:\cc\zz\yy\xx\p2.sldprt E:\xx\p2.sldprt E:\yy\xx\p2.sldprt E:\zz\yy\xx\p2.sldprt
8.
Searches the path of the active document, then recursively searches the path where the referenced document was last saved.
D:\ss\tt\p2.sldprt D:\ss\tt\xx\p2.sldprt D:\ss\tt\yy\xx\p2.sldprt D:\ss\tt\zz\yy\xx\p2.sldprt D:\ss\xx\p2.sldprt D:\ss\yy\xx\p2.sldprt D:\ss\zz\yy\xx\p2.sldprt D:\xx\p2.sldprt D:\yy\xx\p2.sldprt D:\zz\yy\xx\p2.sldprt
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9.
Searches the path where you last opened a document, then recursively searches the path where the referenced document was last saved.
same as Step 8
NOTE: In most cases, the path of the active document and the path where you last opened a document are the same. The two paths are different if you click File, Open to open one document, then drag and drop an assembly from Windows Explorer into that document. The path of the active document is the path from Windows Explorer and the path where you last opened a document is the path from File, Open. 10. Searches the path where the software last found a referenced document.
C:\qq\p2.sldprt This is the location of p1.sldprt.
11. Searches the full path where the document was last saved without a drive designation.
This is useful if you save a part with a UNC path such as \\machine\folder\p2.sldprt.
12. Searches the full path where the document was last saved with its original drive designation.
C:\zz\yy\xx\p2.sldprt
13. Allows you to browse for the document yourself.
n/a
Search Results In an assembly document, lists the part and sub-assembly documents that are components of the active assembly. This is useful if you have several versions of the component files. In a part document, lists externally referenced documents, if they exist. To list the referenced files then copy the listed files to a new directory:
1.
Click File, Find References.
2.
In the dialog box, click Print to print the contents of the dialog box.
3.
Click Copy list to copy the contents of the dialog box to the Windows clipboard so you can paste the list into a text editor.
4.
To copy the files: a.
Click Copy files. NOTE: This option is not available for parts with in-context references. To copy files in this case, open the assembly that is listed, and click File, Find References.
5.
b.
To retain the directory structure of the file copies, click Yes when prompted to preserve directory structure. To copy all files to a single folder, click No.
c.
Browse to the desired folder in the Browse For Folder dialog box and click OK.
Click Close to close the dialog box.
Saving Assemblies with In-context Features There are some special considerations when you save an assembly with in-context features:
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•
Parts that have features defined in the context of an assembly must maintain the association with the parent assembly in order to update correctly, both inside and outside of the assembly context.
•
If you need two versions of the same part (one that includes the in-context features, and one that does not include them), you must edit the referenced file locations when you save the assembly. This prevents the incontext features from affecting the original part document.
Editing Parts in the Assembly Context While editing an assembly, you can: •
Create a new part in the assembly window
•
Edit an existing component in the assembly window
•
Open an existing component document in its own window
Creating a Part in an Assembly You can create a new part in the context of an assembly. That way you can use the geometry of other assembly components while designing the part. The new part has its own part file so you can modify it independently from the assembly. You can also create a new sub-assembly in the context of the top-level assembly. See Creating a Sub-assembly for more information. To create a part within an assembly:
1.
Click New Part on the Assembly toolbar, or click Insert, Component, New Part. The default part template on the Default Templates Options page is used.
2.
In the Save As dialog box, enter a name for the new part and click Save. The new part is saved in its own document so you can edit it separately. The component pointer
3.
appears.
If the assembly is empty, select a plane from the FeatureManager design tree. Otherwise, select a plane or planar face on which to position the new part. The name of the new part appears in the FeatureManager design tree, and a sketch is automatically opened in the new part. An Inplace (coincident) mate is added between the Front plane of the new part and the selected plane or face. The new part is fully positioned by the Inplace mate. No additional mates are required to position it. If you wish to reposition the component, you need to delete the Inplace mate first.
4.
Construct the part features, using the same techniques you use to build a part on its own. Reference the geometry of other components in the assembly as needed. NOTE: If you extrude a feature using the Up To Next option, the next geometry must be on the same part. You cannot use the Up To Next option to extrude to a surface on another component in the assembly or a surface of an assembly feature.
5.
Click File, Save, then select the part name in the Resolve Ambiguity dialog box, or select the assembly name to save the entire assembly and its components.
6.
To return to editing the assembly, right-click the assembly name in the FeatureManager design tree, or rightclick anywhere in the graphics area, and select Edit Assembly:assembly_name, or click Edit Part
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Editing a Part in an Assembly Editing a part while in an assembly allows you to modify a component without leaving the assembly. You can also reference surrounding geometry while creating new features. The sketches that you create while editing a part in the assembly can use any edge or can be dimensioned to any edge of any part. Features may use end conditions such as Up to Surface to another component. You can change the transparency of assembly components while editing a part. To edit a part while in an assembly:
1.
Right-click the part and select Edit Part, or click Edit Part
on the Assembly toolbar.
The title bar shows the name of the part in the assembly that is open for editing as part_name in assembly_name.sldasm. Note that the message in the status bar indicates that you are now editing the part document even though the entire assembly is visible. NOTE: When you edit a part in the context of an assembly, the referenced configuration in the assembly becomes the active configuration in all open windows (for example, if the part is open in its own window). If the part is used in another open assembly document, with the Use component’s in-use or last saved configuration option selected, those instances are also affected. For more information, see Component Configurations in an Assembly. 2.
Make the necessary changes to the part.
3.
To return to editing the assembly, right-click the assembly name in the FeatureManager design tree, or rightclick anywhere in the graphics area, and select Edit Assembly:assembly_name, or click Edit Part
.
Transparency During Part Editing There are several options for displaying component transparency while editing parts. These settings affect only the components that are not being edited. The illustrations below show the results of applying different settings during editing of the sphere in this assembly. The sphere is completely enclosed by blocks, some of which have transparency applied as a component property.
To set the scope of transparency to use during part editing:
1.
Click Tools, Options, System Options, Display/Selection.
2.
Under Assembly transparency for in-context edit, select Force assembly transparency, and move the slider to the desired transparency level.
3.
Click OK.
To set the transparency of the components you are not editing:
1.
Select a component and click Edit Part
on the Assembly toolbar.
The component you are editing turns opaque pink. The appearance of the other components depends on the assembly transparency settings you choose. 2.
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Click Change Assembly Transparency •
Opaque
•
Maintain Transparency
•
Force Transparency
on the Assembly toolbar, and select from the following:
. Components are opaque. . Components retain their individual transparency settings. . Components use the transparency level you set.
Opaque
Maintain Transparency
Force Transparency
TIP: Additionally, you can right-click any blank area and set Assembly Transparency on the shortcut menu to Opaque, Maintain Transparency, or Force Transparency. 3.
Edit the part as needed.
4.
Click Edit Part
to return to editing the assembly, and to turn off transparency.
Time-Dependent Features Time-dependent features are the basis of top-down design. They include: •
Assembly features (assembly feature cuts or holes, and weld beads)
•
Components that are created in the context of the assembly
•
In-context features, reference geometry, and sketches that reference other components
•
Component patterns
When a time-dependent feature references components that have already been positioned by mates, the features become dependent on both the components and the mates that position the components. To view these dependencies, right-click the feature and select Parent/Child. Mates are solved together as a system within a mategroup. Each assembly has a single default mategroup. The order in which mates are added to the mategroup does not matter; all the mates are solved at the same time.
Tips for Mating with Time-Dependent Features It is good design practice to only reference time-dependent features for mating when that is the only way you can achieve the design intent of the assembly. You can edit the positions of the components with more flexibility when time-dependent features are not involved because the order of evaluation does not matter. When positioning a component to geometry that depends on a time-dependent feature, it is good design practice to mate components to the time-dependent feature first, then add additional mates as needed.
Adding a Component Pattern You can create a pattern of components in the assembly in one of the following ways: •
You can create a local linear or circular pattern of components.
•
You can place a pattern of components in an assembly based on a feature pattern of an existing component. This is called a derived component pattern.
•
You can place a pattern of components in an assembly based on a feature pattern of assembly features.
To toggle the visibility or suppression state of all of the components in the pattern, right-click the pattern feature in the FeatureManager design tree, and select Hide components, Show components, Suppress, or Unsuppress. You can dissolve a component pattern to make its components independent. One benefit is that you can individually move and rotate components that were in the pattern. One drawback is that you cannot hide and suppress all the components in the pattern because the pattern feature is gone.
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Linear Component Pattern You can create a linear pattern of components in an assembly in one or two directions. To create a linear pattern of components:
1.
Click Insert, Component Pattern, Linear Pattern.
2.
In the PropertyManager, under Direction 1:
3.
•
Select a linear edge or a linear dimension for Pattern Direction.
•
Click Reverse Direction
if necessary.
•
Type a value for Spacing
. This is the value between the centers of the instances.
•
Type a value for Number of Instances seed components.
. This is the total number of instances including the
Repeat for Direction 2 for a bidirectional pattern. Select Pattern seed only to pattern the seed component only in the second direction. When cleared, SolidWorks patterns all of the instances generated by Direction 1 and the seed component in the second direction.
4.
Click in Components to Pattern
5.
To skip instances, click in Instances to Skip area. The pointer changes to
, then select the seed components. and select the preview of the instance in the graphics
when it is over a preview in the graphics area.
6.
To restore instances, select the instance in Instances to Skip and press Delete.
7.
Click OK
.
The new components appear under LocalLPattern in the FeatureManager design tree. By default, all instances use the same configuration as the seed components. To change the configuration, edit the component properties of an instance. Circular Component Pattern You can create a circular pattern of components in an assembly. To create a circular pattern of components:
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1.
Click Insert, Component Pattern, Circular Pattern.
2.
In the PropertyManager, under Parameters: •
Select an axis or a linear edge for Pattern Axis. The pattern revolves around this axis.
•
Click Reverse Direction
•
Type a value for Angle
•
Type a value for Number of Instances seed components.
•
Select Equal Spacing to set the Angle to 360°. You can change the value to a different angle. The instances equally space themselves along the total angle.
if necessary. . This is the angular value between the centers of the instances. . This is the total number of instances including the
3.
Click in Components to Pattern
4.
To skip instances, click in Instances to Skip area. The pointer changes to
, then select the seed components. and select the preview of the instance in the graphics
when it is over a preview in the graphics area.
5.
To restore instances, select the instance in Instances to Skip and press Delete.
6.
Click OK
.
The new components appear under LocalCirPattern in the FeatureManager design tree. By default, all instances use the same configuration as the seed components. To change the configuration, edit the component properties of an instance. Feature Driven Pattern You can create a pattern of components based on an existing pattern. To use an existing pattern to create a pattern of components:
1.
Click Insert, Component Pattern, Feature Driven.
2.
Select the seed components for Components to Pattern
3.
Click in Driving Feature and select the pattern feature in the FeatureManager design tree or a face of a pattern instance in the graphics area.
4.
Click OK
.
.
The new components appear under DerivedLPattern or DerivedCirPattern in the FeatureManager design tree. By default, all instances use the same configuration as the seed components. To change the configuration, edit the component properties of an instance. To skip instances:
1.
Right-click the pattern feature in the FeatureManager design tree and select Edit Feature.
2.
Click in Instances to Skip The pointer changes to
and select the preview of the instance in the graphics area. when it is over a preview in the graphics area.
You cannot skip instances when creating a derived component pattern; you must edit the feature.
Mirror Components - Overview You can create new components by mirroring existing part or sub-assembly components. The new components can either be a copy or a mirror of the original components. A mirrored component is sometimes called a "right-hand" version of the original "left-hand" version. Some important items to note include: •
If the original components change, so do the copied or mirrored components.
•
Mates between the original components can be preserved in the copied or mirrored components.
•
Configurations in the original components appear in the copied or mirrored components.
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The difference between a component that you copy and one that you mirror is described as follows: Copy
Mirror
No new documents are created.
A new document is created.
The geometry of the copied component is identical to the original component; only the orientation of the component is different.
The geometry of the new component is mirrored; thus it is different from the original component.
Here is an example of a sub-assembly that includes a mirrored and copied component. The support has been mirrored so the opening for the jaw is on the correct side. The jaw has been copied since the geometry did not need to change. The mates that hold the jaw to the support have been preserved.
Mirror Components Step 1: Selections You must select a plane of symmetry and the components to mirror or copy. To mirror or copy one or more components:
1.
Click Insert, Mirrored Components.
2.
In the PropertyManager, under Selections, select a plane or planar face for Mirror plane as the entity to mirror about.
3.
Select one or more components that you want to mirror or copy for Components to Mirror. You can select from the graphics area or from the FeatureManager design tree. If you select a sub-assembly in the FeatureManager design tree, all of its components are selected as well.
4.
Set the state (mirror or copy) for each component: •
Toggle between
and
where:
indicates that the component is copied. The geometry of a copied component is unchanged from the original, only the orientation of the component is different. indicates that the component is mirrored. The geometry of the mirrored component changes to create a truly mirrored component. •
•
Right-click the component name to select: o
Mirror All Children - Mirrors the sub-assembly and all of its children.
o
Mirror All Instances - Mirrors all instances of the selected component.
o
Copy All Instances - Copies all instances of the selected components.
Click
next to a sub-assembly to show its children. You can select
or
for each child.
5.
To preserve any mates between the selected components when you mirror more than one component, select Recreate mates to new components.
6.
Click Next
.
If you chose to mirror components, you go to Step 2: Filenames to choose names for your new parts. If you did not mirror components, you go to Step 3: Orientation.
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Mirror Components Step 2: Filenames Select a name and a location for each of the components you are mirroring. You can create a new part or subassembly from the component or use an existing part or sub-assembly. For example, if you previously made a mirror of your component in an earlier operation, you can use that part. To specify the name and location for a new part or subassembly:
1.
Select a component under Filenames. A proposed name for the mirrored part appears below.
2.
To change the part name, type a new name for the part over the proposed name or click existing part.
3.
Repeat steps 1 and 2 for the other components in the list.
4.
To place the new parts in a common folder:
5.
a.
Select Place files in one folder.
b.
Click Choose to browse to a new folder.
to browse to an
To change the name defaults: a.
Select prefix or suffix for Add.
b.
Type the prefix or suffix in the box below. The new part names automatically appear with the chosen prefix or suffix attached.
6.
Click Next
to go to Step 3: Orientation.
Mirror Components Step 3: Orientation Select an orientation for the components you are copying. To change the orientation of the components:
1.
Select a component from the list and click Reorient Component to toggle through the possible alignments until the desired preview appears. Repeat for all of your components.
2.
Click Apply to All to set all of the components to the same orientation.
3.
Click Reset Orientations to set all of the components back to the default orientation.
4.
To see a preview of the components, select the Preview mirrored components or Preview instanced components check boxes.
5.
Click OK
.
Reorder and Roll Back in Assemblies Reorder Changing the order of assembly items in the FeatureManager design tree is dictated by parent/child relationships, just as it is with features in parts. •
You can reorder sketches, features, and reference geometry that belong to the assembly.
•
You can reorder components within their own level of the assembly hierarchy. See Changing the order of components.
•
You can reorder mates within the mategroup.
•
You cannot reorder mategroups, component patterns, in-context features, or any default assembly items (default planes, Annotations or Lighting folders, and so on).
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Roll Back You can roll back reference geometry, sketches, component patterns, assembly features and in-context features. In general, rolling back assembly items behaves the same as rolling back features in parts. The following behaviors are specific to assemblies: •
If you roll back an assembly pattern, the components generated by that pattern are rolled back.
•
You cannot roll back into the section of the FeatureManager design tree that lists the components (that is, after some of the components are added, or before others). This is because components are not timedependent. Hide or suppress the components instead.
Assembly Layout Sketch You can design an assembly from the top-down using layout sketches. You can construct one or more sketches showing where each assembly component belongs. Then, you can create and modify the design before you create any parts. In addition, you can use the layout sketch to make changes in the assembly at any time. The major advantage of designing an assembly using a layout sketch is that if you change the layout sketch, the assembly and its parts are automatically updated. You can make changes quickly, and in just one place. To use an assembly layout sketch, do the following:
•
Create a sketch in the assembly in which various sketch entities represent parts in the assembly. Indicate a tentative location for each component, capturing the overall design intent.
•
Reference the geometry in the layout sketch when you create each component. Use the layout sketch to define the component size, shape, and location within the assembly; make sure that each part references the layout sketch.
Example of Using an Assembly Layout Sketch The following example is typical of an automobile engine accessory drive belt system. The system has several pulleys and idlers, connected by a serpentine belt. 1.
Create an assembly sketch. Use circles to represent the outer rims of the pulleys. Use tangent lines between the circles to represent the serpentine belt. Dimension the size and location of each pulley.
2.
For each pulley, insert a new part, sketch a circle, add a Coradial relation with the corresponding circle in the layout sketch, then extrude the sketch. Add other features to the pulley parts as needed.
3.
Using the layout sketch as a guide, create the belt around the pulleys as another new part.
You can change the location or the size of the pulleys by editing the layout sketch. The assembly now consists of a belt and a set of pulleys whose locations and sizes are driven by the layout sketch. The advantage of this type of design is clear when you have to make changes to the design.
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For example, working in the layout sketch, you can: •
Rearrange the pulleys so that a slipping pulley has more of its surface covered by the belt.
•
Make a driven pulley larger so less torque is required to turn it.
•
Drag the pulleys and belt to dynamically experiment with different locations.
•
Set an angle dimension to specify how much of each pulley must be covered by the belt.
•
When you exit the layout sketch, the assembly and the parts are updated.
If you designed this assembly without a layout sketch, you would need to change many dimensions, or move components in the assembly, then rebuild each time. The layout sketch does not have to be the master plan for a design. If you had a model of an engine with some fixed pulley locations, you could make the circles in the layout sketch coincident with the known locations of the pulleys in the model. You would still have the freedom to drag the other pulleys to different locations, and the assembly would update automatically when you made changes.
Assembly Features While in an assembly, you can create cut or hole features that exist in the assembly only. You determine which parts you want the feature to affect by setting the scope. You can create a pattern of assembly features in the same manner as you create a pattern of features in a part. This is useful for creating cuts or holes that are added after the components are actually assembled, and that affect more than one component. When you want to add a cut or hole to a single component in an assembly, it is better to edit the part in context than to use an assembly feature. While it is not a requirement, it is good practice to fully define the positions of the components of the assembly, or fix their locations before you add assembly features. This helps prevent unexpected results if the components are moved later.
Creating an Assembly Feature Assembly feature cuts and holes affect the assembly only; the individual part files are not affected. You can set the scope before you create an assembly feature, or you can edit the scope afterwards. To create an assembly feature cut :
1.
Open a sketch on a face or plane, and sketch a profile of the cut. The profile can contain more than one closed contour.
2.
Click Insert, Assembly Feature, Cut, Extrude or Revolve.
3.
Set the options as needed in the Cut-Extrude or Cut-Revolve PropertyManager.
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To create an assembly feature hole:
1.
Click the planar face approximately where you want to create the hole.
2.
Click Insert, Assembly Feature, Hole, Simple or Wizard.
3.
Set the options as needed in the Hole PropertyManager or Hole Definition dialog box.
To create an assembly feature pattern:
1.
Create an assembly cut or hole.
2.
Click Insert, Assembly Feature, and select one of the following: Linear Pattern, Circular Pattern, Table Driven Pattern, Sketch Driven Pattern.
To edit an assembly feature:
Right-click the assembly feature in the FeatureManager design tree, and select either Edit Sketch, Edit Definition, or Feature Scope.
Feature Scope When creating an feature in an assembly or a multibody part, you must determine which components or bodies you want to be affected by the feature. By setting the scope, you can selectively choose the components or bodies you want the feature to impact. To set the scope for an assembly feature:
1.
Select an assembly feature to set the scope for that feature. If you do not select a feature, you specify the feature scope for the next assembly feature that you create.
2.
In an assembly, select Edit, Feature Scope.
3.
Select the components that this assembly feature will affect by clicking the components or the component names in the FeatureManager design tree. The selected component names appear in the Edit Assembly Feature Scope dialog box.
4.
Click OK.
To set the scope for a feature in a multibody part:
1.
Create the feature as usual. Features that allow you to set the scope include Cut-Extrude and Cut-Revolve features.
2.
In the PropertyManager, under Feature Scope, select All bodies or Selected bodies.
3.
If you chose Selected bodies, click Auto-select to allow the software to determine which bodies to affect. Clear Auto-select to select bodies for Solid Bodies to Affect.
Joining Parts You can join two or more parts to create a new part. The join operation removes surfaces that intrude into each other's space, and merges the part bodies into a single solid volume. Creating a Joined Part To join parts:
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1.
Create the parts that you want to join, then create an assembly containing the parts.
2.
Position the parts as desired in the assembly. The parts may either touch each other or intrude into one another.
3.
Save the assembly but do not close the window.
4.
Insert a new part into the assembly: o o
o
5.
Click Insert, Component, New Part. Enter a name for the new part and click Save. Click a plane or planar face on a component on which to position the new part.
Click Insert, Features, Join. The Join PropertyManager appears.
6.
In either the FeatureManager design tree or the graphics area, click the components you want to join. The names appear under Parts to Join.
7.
Select the Hide Parts check box to hide the original components after the join is complete.
8.
Select the Force Surface Contact check box if you want to join any coincident faces (as well as intruding volumes). The software finds the affected faces, then extends the face with the smallest area into the other component, and fills in any resultant gaps.
9.
Click OK
to create the joined part.
Before join - coincident faces 10.
After Join - faces are removed
To exit from Editing Part mode, right-click in the graphics area, and select Edit Assembly:assembly_name.
Editing a Joined Part To edit the definition of the joined part to add or remove components:
1.
In the FeatureManager design tree of an assembly, right-click the Join feature of the joined part and select Edit Feature. - or In the graphics area of an assembly, right-click the joined component and select Edit Feature.
2.
Click the parts that you want to remove from the joined component, or click additional parts to be joined to the existing component. To remove all the parts, right-click in the graphics area, and select Clear Selections. The components that make up the joined component are listed under Parts to Join.
3.
Click OK
. The joined component updates to reflect the changes.
NOTE: The joined part is fully associative to the original parts and to the assembly. Any changes made to the original parts are reflected in the joined part. If the parts move relative to each other in the assembly, the joined part changes also.
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Identifying the Parts in a Joined Part To identify which parts are used to create a joined part, either:
•
Right-click the joined component and select List External Refs. The referenced components appear in the Referenced Entity column.
•
Expand the joined component in the FeatureManager design tree, then expand the Join feature to see the absorbed references.
Weld Beads You can add a variety of weld types to an assembly. The weld bead becomes a new assembly component created in the context of the assembly. See Working with Parts within an Assembly. You can do the following: •
View the available weld types
•
Create and edit weld beads
•
Select faces for weld beads more easily
•
Automatically create weld symbols
Weld Types The following weld types are supported for the ISO and ANSI dimensioning standards: ISO
ANSI
Butt
Square
Square Butt
Scarf
Single V Butt
V Groove
Single Bevel Butt
Bevel
Single V Butt with Root
U Groove
Single Bevel Butt with Root
J Groove
Single U Butt
Flare-V
Single J Butt
Flare-Bevel
Backing Run
Fillet
Fillet
Seam
Seam
Flange-Edge Flange-Corner
Creating and Editing Weld Beads To add a weld bead between components:
1.
Insert the components in an assembly, and add mates to position them as needed for the specific weld type you plan to use.
2.
Click Insert, Assembly Feature, Weld Bead.
3.
In the Weld Bead Type dialog box, select a weld Type from the list, then click Next.
4.
In the Weld Bead Surface dialog box:
5.
•
Select a Surface Shape from the list (Flat, Convex, or Concave).
•
Specify the Top Surface Delta, the Bottom Surface Delta and Radius as required for the Type and Surface Shape selected. See Surface Delta and Radius.
Click Next. The Weld Bead Mate Surfaces dialog box appears. Be sure to read the information in the dialog box about selecting faces for the weld type you have chosen.
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6.
Select the necessary faces. For all welds, you must select Contact Faces. Depending on the type of weld you are adding, you may also need to select Stop Faces and Top Faces. Click each box, then select the faces in the graphics area. See Weld Face Selection Tips for more information. Contact Faces are the faces that are joined by the weld bead. Select a face (or a set of adjacent faces) on each component. Stop Faces are the faces that define the beginning and the end of the weld bead. On each component, select two faces (or two sets of adjacent faces) that share an edge with the contact faces. Top Faces are the faces from which to measure the Top Surface Delta. On each component, select one face that shares an edge with a contact face.
7.
Click Next.
8.
In the Weld Bead Part dialog box, either accept the default name for the Weld Bead Part, or enter a new part name, and click Finish.
To edit a weld:
1.
In the FeatureManager design tree, expand the Bead component.
2.
Right-click the Weld Bead feature and select Edit Feature.
3.
In each of the dialog boxes, change the parameters as needed. Click Next to continue, then click Finish when you reach the last dialog box.
Surface Delta and Radius When you add a weld bead with a Surface Shape of Convex or Concave, you must specify the Top Surface Delta. For a backing run weld, you also specify the Bottom Surface Delta. If the Surface Shape is Flat, there is no surface delta. For a convex weld, the top surface delta is the distance between the highest point on the bead and the contact faces.
For a concave weld, the distance is measured below the top surface rather than above.
For a fillet weld, you also specify the Radius. The radius is measured as the radius of an imaginary ball rolling along the seam. The edges of the weld bead are at the points of tangency, where the ball meets the contact faces. In the illustrated fillet weld, the specified Radius is 10mm, and the Top Surface Delta is 2mm.
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Weld Face Selection Tips When components have complex shapes, or when the mates place the components very close to each other, selecting the faces for a weld can be difficult. There are several ways you can make it easier: •
Change the view to Wireframe
or Hidden Lines Visible
.
•
Rotate the model using Rotate View
•
Set the Selection Filter to Filter Faces
•
Temporarily add some space between the components. You can do this by editing the values of Angle and Distance mates or suppressing one or more mates, then moving the components apart slightly.
. You can change the orientation then select the faces. .
After you complete the weld bead, edit or unsuppress the mates as needed to restore the components to the correct positions. Then click Rebuild
to update the weld bead.
Automatic Weld Symbols When you create a weld, a weld symbol is automatically attached to the weld bead component in the assembly.
To add more detailed specifications to the default weld symbol:
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1.
In the assembly document or in a drawing document, right-click the symbol and select Properties, or double-click the symbol.
2.
Specify the dimensions, symbols, and other options that you want to include, and click OK.
Simplifying Assemblies Simplifying Large Assemblies Large assemblies can consist of hundreds of components. You can simplify a complex assembly by toggling the visibility of the components, and by changing the suppression state of components. Large Assembly Mode is a collection of system options that improves the performance of assemblies. You can turn on Large Assembly Mode at any time, or you can set a limit for the number of components, and have Large Assembly Mode turn on automatically when that limit is reached. You can customize Large Assembly Mode, and you can combine it with other simplification methods (such as toggling the visibility and changing the suppression state). There are several reasons to simplify an assembly: •
To improve system performance, and to reduce rebuild times, especially with very large assemblies.
•
To create simplified views of the assembly that include certain components, and exclude others.
•
To create design variations of the assembly, with different combinations of components, and different configurations of the components themselves.
Large Assembly Mode Large Assembly Mode is a collection of system options that improves the performance of assemblies. You can turn on Large Assembly Mode at any time, or you can set a limit for the number of components, and have Large Assembly Mode turn on automatically when that limit is reached. Two notes about saving an assembly with Large Assembly Mode active: •
If you save an assembly with Large Assembly Mode active, SolidWorks ignores the Automatically activate Large Assembly Mode option (Tools, Options, System Options, Large Assembly Mode) the next time you open the assembly. The assembly opens with Large Assembly Mode active.
•
If you save an assembly that contains sub-assemblies with Large Assembly Mode active, SolidWorks does not save the sub-assemblies in Large Assembly Mode. To save a sub-assembly in Large Assembly Mode, you must open the sub-assembly in its own window, activate Large Assembly Mode, and save.
SolidWorks is pre-set with recommended Large Assembly Mode options, but you can customize the options as needed. To turn on Large Assembly Mode:
Click Large Assembly Mode
on the Assembly toolbar, or click Tools, Large Assembly Mode.
The options are enabled.
Lightweight Components You can load an assembly with its active components fully resolved or lightweight. Both parts and sub-assemblies can be lightweight. •
When a component is fully resolved, all its model data is loaded in memory.
•
When a component is lightweight, only a subset of its model data is loaded in memory. The remaining model data is loaded on an as-needed basis.
You can improve performance of large assemblies significantly by using lightweight components. Loading an assembly with lightweight components is faster than loading the same assembly with fully resolved components. Lightweight components are efficient because the full model data for the components is loaded only as it is needed. Only components that you select, and components that are affected by changes that you make in the current editing session, become fully resolved. Assemblies with lightweight components rebuild faster because less data is evaluated. Mates on a lightweight component are solved, and you can edit existing mates.
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To enable lightweight loading of components:
1.
Click Tools, Options, System Options, Performance.
2.
Under Assemblies, select Automatically load components lightweight.
To open an assembly with lightweight components:
1.
Click File, Open. The Open dialog box appears.
2.
Select Lightweight, browse to the assembly file, and click Open. When this check box is selected, all components are loaded lightweight when you open an assembly. Components in the feature scope of an assembly feature can be loaded lightweight. When you point at a lightweight part in the graphics area, a feather pointer surrounded by a bounding box.
is displayed, and the body is
NOTE: Lightweight parts are only used when the model is in Shaded mode. If the model was last saved in Hidden Lines Removed, Hidden In Gray, or Wireframe mode, lightweight parts are not used. To set one or more resolved components to lightweight:
1.
For a single component, right-click the component and select Set to Lightweight.
2.
For an entire assembly, right-click the top level assembly icon and select Set Resolved to Lightweight. This option is available for a sub-assembly and its components when you right-click the sub-assembly.
Toggling the Visibility You can toggle the display of assembly components. You can remove the component completely from view or make it 75% transparent. Turning off the display of a component temporarily removes it from view, allowing you to work with underlying components. Hiding or showing a component affects only the visibility of the component. Hidden components have the same accessibility and behaviors as shown components in the same suppression state (see suppression states of components). Toggling the visibility does not affect the rebuild or evaluation speed. Display performance improves, however. To toggle the visibility of a component (part or sub-assembly):
1.
In the FeatureManager design tree or in the graphics area, right-click the component, and select Properties. To change several components at once, hold the Ctrl key as you select the components, then right-click and select Properties.
2.
In the dialog box, under Visibility, select Hide Model.
3.
Click OK. To show the components again, select the components in the FeatureManager design tree, then edit the Component Properties.
To toggle the transparency of a component:
Select the component, then click Change Transparency
on the Assembly toolbar.
Other ways to toggle the visibility:
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•
Right-click the component, and select Hide Component or Show Component. This method changes only the visibility of the active configuration.
•
Select the component, then click Hide/Show Components changes only the visibility of the active configuration.
•
Select the component, then click Edit, Hide (or Show, or Show with Dependents), This Configuration (or All Configurations, or Specified Configurations).
on the Assembly toolbar. This method
Component Suppression States Depending on the scope of the work you plan to do at any given time, you can specify an appropriate suppression state for the components. This can reduce the amount of data that is loaded and evaluated as you work. The assembly displays and rebuilds faster, and you make more efficient use of your system resources. There are three suppression states for assembly components: •
Resolved
•
Suppressed
•
Lightweight
To change the suppression state of components:
1.
In the FeatureManager design tree or the graphics area, right-click the desired component, and select Properties. To change several components at once, hold the Ctrl key as you select the components, then right-click and select Properties.
2.
In the dialog box, under Suppression State, select the desired state.
3.
Click OK.
Other ways to change the suppression state:
•
Click a component, then click Change Suppression State on the Assembly toolbar. This method changes only the suppression state of the active configuration. -orClick Edit, Suppress (or Unsuppress), This Configuration (All Configurations, Specified Configurations). If you select Specified Configurations, a dialog box appears. Select the configurations you want to change from the list, and click OK.
•
To fully resolve (unsuppress) a suppressed component, right-click the suppressed component, and select Set to Resolved. This resolves all configurations of the component.
•
To fully resolve all lightweight parts, right-click the assembly icon at the top of the FeatureManager design tree, and select Set Lightweight to Resolved.
NOTE: You cannot set specific configurations of components to lightweight. Resolved Resolved (or unsuppressed) is the normal state for assembly components. A resolved component is fully loaded in memory, fully functional, and fully accessible. All its model data is available, so its entities can be selected, referenced, edited, used in mates, and so on. Suppressed You can use the suppressed state to remove a component temporarily from the assembly, without deleting it. It is not loaded in memory, and it is no longer a functional member of the assembly. You cannot see a suppressed component, or select any of its entities. A suppressed component is removed from memory, so loading speed, rebuild speed, and display performance are improved. Because of the reduced complexity, evaluation of remaining components occurs faster. However, mates that involve the suppressed components are suppressed also. As a result, the positions of components in the assembly can become under defined. In-context features that reference suppressed components may also be affected. When you restore a suppressed component to the fully resolved state, conflicts can occur. Therefore, use the suppressed state carefully when modeling.
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Loading Additional Model Data When an operation requires model data that is not loaded for a lightweight component, the software fully resolves the part for you, to gain access to the additional data. This happens automatically when you do any of the following things: •
Click a part in the graphics area. When you click, the part becomes fully resolved, and the entity (face, edge, etc.) where you clicked is selected and highlighted.
•
Right-click a part or feature, and select Edit Part, Edit Sketch or Edit Feature. The part becomes fully resolved, and you are in Editing Part mode.
•
You can choose to automatically resolve any lightweight components that are out-of-date. Click Tools, Options, then Performance on the System Options tab. Select Always resolve from the Check out-ofdate lightweight parts list. If you select Indicate from the list then components that are out-of-date have a feather with red stripes next to them in the FeatureManager design tree.
Certain global operations require that many parts be fully resolved at once: •
Mass Properties
•
Interference Detection
•
Exploded View
•
Advanced Show/Hide, Advanced Selection
•
Section view of the assembly model
•
editing equations that involve lightweight parts
•
Physical Dynamics and Physical Simulation
•
exporting to other file types (IGES, SAT, and so on) You do not have to resolve parts before exporting to TIFF or JPEG.
To specify what you want to happen when you request one of these operations, click Tools, Options, then Performance on the System Options tab. Choose one of these options under Resolve lightweight components: •
Always. All lightweight parts are fully resolved for you, and they are included in the operation.
•
Prompt (default). A dialog box appears, asking if you want the software to resolve the lightweight parts for you. Click Yes to fully resolve the parts and continue, or click Cancel. If you also click Always resolve (before you click Yes or Cancel), the option is set to Always.
NOTE: When a lightweight part becomes fully resolved, all instances of the part, in any configuration, in any open assembly documents, become fully resolved.
Comparison of Components Suppression States
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Resolved
Lightweight
Suppressed
Hidden
Loaded in memory
Yes
Partially
No
Yes
Visible
Yes
Yes
No
No
Features available in FeatureManager design tree
Yes
Yes 3
No
No
Faces and edges accessible for adding mates
Yes
Yes 3
No
No
Mates solved
Yes
Yes
No
Yes
In-context features solved
Yes 1
Yes
No
Yes
Assembly features solved
Yes
Yes
No
Yes
Considered in global operations
Yes
On demand 2
No
Yes
May be edited in-context
Yes
Yes 3
No
No
Load and rebuild speed
Normal
Faster
Faster
Normal
Display speed
Normal
Normal
Faster
Faster
1 In-context features on resolved parts that reference lightweight parts update automatically. 2 Global operations include Mass Properties, Interference Detection, Exploded View, Advanced Selection and Advanced Show/Hide, solving equations, displaying section views, and exporting to other file formats. When lightweight components are present, the software prompts you to either resolve them, or cancel the operation. 3 Lightweight components are resolved automatically when selected for this operation.
Assembly Envelopes An assembly envelope is a special type of assembly component. It is a reference component, and it is ignored in global assembly operations (Bill of Materials, Mass Properties, and so on). This functionality allows you to select components based on their positions with respect to the envelope volume (inside, outside, or crossing). You can use an envelope by itself to quickly change the visibility of assembly components. You can also use an envelope (either alone or in combination with file properties), to select components for other editing operations, such as suppress, copy, or delete. The envelope component must be a solid volume (not shelled). This is because selection with envelopes is based on interference between the volumes of the functional assembly components and the envelope component. It is not based on the containment of components within the bounding box of the envelope component. Envelope components are displayed in a light blue transparent color when you use Shaded view mode. An Envelope feature is added to the ConfigurationManager for each envelope component that you create. Also, envelope components are identified in the FeatureManager design tree.
Apply Envelope Lets you specify selection criteria to hide or show assembly components, based on their positions relative to an envelope component. To apply criteria to an envelope:
1.
In the ConfigurationManager, right-click the Envelope component, and select Show/hide using envelope. The Apply Envelope dialog box appears.
2.
Choose one or more Criteria for selecting the components: •
Inside envelope. Components that are completely inside the envelope are selected. This includes components that are inside the envelope, but have a face that is coincident with the outside of the envelope.
•
Outside envelope. Components that are completely outside the envelope are selected. This includes components that are outside the envelope, but have a face that is coincident with the outside of the envelope.
•
Crossing envelope. Components that cross the boundary of the envelope are selected.
3.
Choose Show part components or Hide part components.
4.
Specify what to do with any component that does not meet the selection criteria:
5.
•
With Show part components, you can either Hide it (regardless of current display state), or Leave its show/hide state as is.
•
With Hide part components, you can either Show it (regardless of current display state), or Leave its show/hide state as is.
Click OK. The display is updated to hide or show components according to your selections.
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Creating Assembly Envelopes You can create an assembly envelope using an existing part file or in the context of the assembly. To create an assembly envelope from a file:
1.
Click Insert, Envelope, From File.
2.
In the Open dialog box, select the part file to use as an envelope, then click Open.
3.
Click in the assembly window where you want to place the envelope component. You can mate the envelope component to the other components in the assembly to position it precisely.
To create an assembly envelope in the assembly context:
1.
Click Insert, Envelope, New.
2.
In the Save As dialog box, enter a name for the new envelope component, then click Save. A part document with this name is created.
3.
Click a face or plane in the assembly window where you want to begin sketching the envelope component. The Front plane of the new envelope component is mated to the selected face or plane with an Inplace mating relation.
4.
Create the base feature and any additional features of the envelope component. You can reference the geometry of the assembly components as you create the envelope component. If any of the referenced entities changes, the envelope updates accordingly.
5.
When you are done defining the new envelope component, right-click anywhere in the graphics area, and select Edit Assembly:assembly_name.
Removing Assembly Envelopes To remove an assembly envelope:
1.
Select the envelope component in either the FeatureManager design tree or the graphics area. You can also select the Envelope feature in the ConfigurationManager.
2.
Press the Delete key or click Edit, Delete. Both the envelope component and the Envelope feature are deleted.
Select Using Envelope Lets you select components for editing operations, based on their positions relative to an envelope component.
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1.
In the ConfigurationManager, right-click the Envelope component and click Select using envelope. The Apply Envelope dialog box appears.
2.
Choose one or more check boxes for selecting the components: •
Inside envelope. Components that are completely inside the envelope are selected. This includes components that are inside the envelope, but have a face which is coincident with the outside of the envelope.
•
Outside envelope. Components that are completely outside the envelope are selected. This includes components that are outside the envelope, but have a face which is coincident with the outside of the envelope.
•
Crossing envelope. Components that cross the boundary of the envelope are selected.
3.
Click the Select Components in Top Assembly Only check box to treat sub-assemblies as a single entity for selection with envelopes. When this check box is selected, you can apply an envelope to an entire subassembly if one or more of its components meets the selection criteria.
4.
Click OK. Components that meet the selection criteria are selected and highlighted.
Component Selection by Properties You can select components for editing operations based on properties. Properties include those specified under File, Properties, Custom and Configuration Specific, as well as some properties that are specific to SolidWorks documents, including Part volume, Configuration name, Document name, and Part mass. For example, you assign the custom property System to each component in an assembly. You specify the name of the system the component belongs to as the value. Then you select all components that have the custom property System whose value is Cooling Or Heating. This selects all the components that belong to either the cooling system or the heating system of the assembly. Before you can use these component selection methods in an assembly, you must fully resolve any lightweight parts that it contains. See Lightweight Components and Loading Additional Model Data for more information.
Advanced Hide/Show Components For show and hide operations in an assembly, you can also control the visibility of components that do not meet the specified criteria. You use the same methods to select the components as described in the previous section, Component Selection by Properties. To define advanced visibility criteria:
1.
In the ConfigurationManager, right-click the active configuration, and select Advanced Show/Hide.
2.
Under Define additional criteria, select a Property from the list or type in a property name. Properties include those listed in the default list under File, Properties, on the Custom tab, plus several special SolidWorks properties. NOTE: Custom property names added by you do not show on the list, but you can enter them in the Property box.
3.
Select a Condition, and enter a Value. For most properties, conditions include is (exactly), is not, and contains (a text string which is part of the text of the value. For example, the value "simplified" contains the string "sim".) For the SolidWorks special property Part volume, conditions include is inside, is crossing, and is outside, and the values that are available include the names of any envelopes that you have defined.
4.
Click Add to include the selection criteria in the Criteria list.
5.
To add another criteria to the list, click And or Or as a logical operator for combining the criteria, then specify another Property, Condition, and Value. Click Add after specifying each new criteria.
6.
When you have specified all the necessary criteria, click Apply. The selected components are highlighted. If needed, you can modify the selection, and click Apply again.
7.
Under Operations, click Show part components or Hide part components to specify the visibility of the components that meet the criteria.
8.
Specify what to do with any component that does not meet the criteria:
9.
•
If you clicked Show part components in Step 7, you can either Hide it (regardless of current display state), or Leave its show/hide state as is.
•
If you clicked Hide part components in Step 7, you can either Show it (regardless of current display state), or Leave its show/hide state as is.
Click Apply. If needed, you can modify the selection, and click Apply again.
10. If you want, you can Save Criteria for future use, or Load Criteria that you saved earlier. See Saving and Reloading Selection Criteria. 11. Click Close when you are satisfied with the selections.
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Advanced Component Selection You define the selection criteria by specifying the properties, conditions, and property values of components you want to select. To define advanced selection criteria:
1.
Click Tools, Advanced Select.
2.
Under Define additional criteria, select a Property from the list. Properties include those listed under File, Properties, on the Custom or Configuration Specific tabs, plus several special SolidWorks properties.
3.
Select a Condition, and enter a Value. •
For most properties, conditions include standard mathematical operators.
•
For some properties, conditions include is (exactly), is not, and contains. You use contains to specify a text string which is part of the text of the value; for example, the value "simplified" contains the string "sim".
•
For the SolidWorks special property Part volume, conditions include is inside, is crossing, and is outside. The values that are available are the names of any envelopes that you have defined. See Assembly Envelopes.
4.
Click Add to include the selection criteria in the Criteria list.
5.
To add another criteria to the list, click And or Or as a logical operator for combining the criteria, then specify another Property, Condition, and Value. Click Add after specifying each new criteria.
6.
To delete a criteria from the list, click in the first column of the Criteria list box, beside the criteria to delete. A blue box appears beside the selection. Click Delete.
7.
When you have specified all the necessary criteria, click Apply. The selected components are highlighted. If needed, you can modify the selection, and click Apply again.
8.
If you want, you can Save Criteria for future use, or Load Criteria that you saved earlier. See Saving and Reloading Selection Criteria.
9.
Click the pushpin
if you want to keep the dialog box open for further selections and operations.
10. Perform the desired editing operation, such as Suppress, Hide, or Copy.
Saving and Reloading Selection Criteria When you use Advanced Component Selection or Advanced Show/Hide Components, you can save the selection criteria to a file. Then you can load the criteria later, to quickly apply the same set of selection criteria whenever you want. To save selection criteria:
1.
In the Advanced Component Selection or Advanced Show/Hide Components dialog box, specify a set of selection criteria.
2.
Click Save Criteria.
3.
In the Save Criteria dialog box, browse to the folder where you want the file to be stored, enter a file name, and click Save. The query is saved with the extension .sqy.
To reload selection criteria:
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1.
In the Advanced Component Selection or Advanced Show/Hide Components dialog box, click Load Criteria.
2.
In the Load Criteria dialog box, browse to and select the query file (.sqy), and click Open. The query is loaded, and the criteria are listed in the dialog box.
Displaying Assemblies Exploding an Assembly View For manufacturing purposes, it is often useful to separate the components of an assembly to visually analyze their relationships. Exploding the view of an assembly allows you to look at it with the components separated. While an assembly is exploded, you cannot add mates to the assembly. An exploded view consists of one or more explode steps. An exploded view is stored with the assembly configuration with which it is created. Each configuration can have one exploded view. You can add Explode Lines to an exploded view to indicate component relationships. Before you can explode an assembly, you must fully resolve any lightweight parts that it contains. See Lightweight Components and Loading Additional Model Data for more information.
Assembly Exploder To automatically explode an assembly with few components:
1.
Click Exploded View on the Assembly toolbar, or right-click the configuration name in the ConfigurationManager, and select New Exploded View.
2.
Click Auto Explode.
3.
Examine the Step Parameters, and modify if necessary.
4.
Click OK.
To create separate explode steps for an exploded view:
1.
Click New
. The Assembly Exploder dialog box expands.
2.
Click an edge or face that is parallel to the direction you want to explode for Direction to explode along.
3.
If the preview arrow points in the wrong direction, select Reverse direction.
4.
Click the components you want to explode for Components to explode.
5.
Select Explode related components together to reposition all components that are mated to the components in Components to explode.
6.
If you selected a component that is part of a sub-assembly: •
Click Entire sub-assembly to explode the selected component and all other components belonging to the sub-assembly.
•
Click Component part only to explode only the selected part, leaving the rest of the sub-assembly in place.
7.
Click Apply
8.
Drag the green drag handle to position the components as desired, or to explode the components by a precise distance, type a value for Distance.
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. The components explode from the assembly.
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9.
Click Apply
to update the step.
10. To add more explode steps to the exploded view, repeat the process for each component or group of components. Remember to click Apply after defining each step. 11. When you are satisfied with the completely exploded view, click OK. To edit the explode steps:
1.
Select the Explode Step you want to edit, or use the
buttons to examine and edit each step in turn.
As you select each step, the drag handle appears and the components involved are highlighted or enclosed in bounding boxes. 2.
Edit the explode step by dragging the green handle, changing the distance or direction, and so on, until the component is positioned as desired.
3.
To change the Components to explode or the Direction to explode along, click the corresponding box, then click the desired entities to select or deselect them.
4.
To clear the contents of a box and start again, click the box, then right-click in the graphics area, and select Clear Selections.
5.
To undo the changes to a step, click Undo
6.
Click Apply
7.
To delete an explode step, click Delete
8.
Click OK to finish the view.
.
after editing each step. .
Exploding and Collapsing an Exploded View An exploded view is stored with the assembly configuration in which it is created. Each assembly configuration can only have one exploded view. TIPS: •
You can copy an exploded view from one configuration to another.
•
You can only drag an exploded view from the active configuration to another configuration.
•
You cannot delete an exploded view from an inactive configuration.
To explode and collapse an exploded view:
1.
Click the ConfigurationManager tab
2.
Click the
3.
To explode:
4.
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.
beside the desired configuration, and beside the ExplView feature to see the Explode Steps.
•
Double-click the ExplView feature.
•
Right-click the ExplView feature and select Explode.
•
Right-click the ExplView feature and select Animate explode to display the Animation Controller pop-up toolbar while the assembly explodes.
To collapse, repeat step 3 substituting Collapse in the second bullet and Animate collapse in the third bullet.
Alternative Method for Editing an Exploded View To edit an exploded view without the Assembly Exploder dialog box:
1.
Double-click the ExplView feature in the ConfigurationManager to explode the view.
2.
Right-click the component you want to reposition, and select Show Explode Steps. The drag handles for the explode steps on the selected component are displayed.
3.
Drag the component by the green drag handle to the new position.
4.
Repeat as needed for each component, then collapse the assembly.
Explode Line Sketch An Explode Line Sketch is a type of 3D sketch that you add to an exploded view in an assembly. In an explode line sketch, you can add explode lines to indicate the relationship between assembly components. To insert an explode line sketch:
1.
Create an exploded view in an assembly.
2.
Click Explode Line Sketch
on the Assembly toolbar, or click Insert, Explode Line Sketch.
The Route Line PropertyManager appears. and Jog Sketch Line
tools on the Explode
3.
Add explode lines as needed using the Route Line Sketch toolbar. The lines appear in phantom font.
4.
Add additional lines using the 3D sketch tools, if needed. All lines appear in phantom font.
5.
Close the sketch. The sketch appears in the ConfigurationManager under ExplView
To edit an explode line sketch:
1.
In the ConfigurationManager, click
to expand ExplView
2.
Right-click 3DExplode
3.
Edit the sketch as you would for any 3D sketch, or add more explode lines.
4.
Close the sketch.
Jog Line You can jog sketch lines in 2D or 3D sketches in part, assembly, and drawing documents. Jog lines are automatically constrained to be parallel or perpedicular to the original sketch line. You can drag and dimension jog lines.
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To jog a sketch line:
1.
In an open sketch with a line, or in a drawing with a sketched line, click Jog Line Sketch toolbar, or click Tools, Sketch Tools, Jog Line.
2.
Click a line to begin the jog.
3.
Move the pointer to preview the width and depth of the jog.
on the Explode
In 3D sketches, press Tab to change the plane of the jog. 4.
Click again to complete the jog. The Jog Line tool stays active so you can insert multiple jogs.
Example of Jog Lines A jog with dimensions in a 2D sketch line.
Jogs in 3D sketch lines in different planes.
Image Quality in Assemblies You can control the Shaded and Wireframe quality of assembly components by changing the image quality of the assembly. When you change the image quality of the assembly, you can choose to apply the assembly’s settings to each of the referenced components. To change the image quality for all components in an assembly:
1.
Click Tools, Options, Document Properties, Image Quality.
2.
Select Apply to all referenced part documents.
3.
Move the Shaded and draft quality HLR/HLV resolution or Wireframe and high quality HLR/HLV resolution sliders.
4.
Click OK.
Color and Appearance in Assemblies By default, components that you add to an assembly are displayed using the color specified in the original part document. This is true for Shaded and all wireframe display modes. You can override the part color for selected instances, or use the default color for the assembly. You can also modify material properties such as Transparency and Shininess. These changes do not affect the original part document.
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To change the color of selected component instances:
1.
Click a component in the FeatureManager design tree or in the graphics area. To select multiple components, hold Ctrl as you select.
2.
Click Edit Color
3.
Click OK.
on the Standard toolbar. See Color and Optics.
To edit the color and advanced properties of selected component instances:
1.
Right-click a component and select Properties.
2.
Click Color. •
To apply a new color, click Change Color, choose a color from the palette, and click OK.
•
To use the default color for the assembly document, click Use Assembly.
•
To restore the component to the original color specified in the part document, click Remove Color.
3.
Click Advanced to set other properties for the selected component, such as Transparency and Shininess.
4.
Click OK. The color of the selected instances changes, but not the referenced part document.
To change the color of a component and its original part document:
1.
Right-click a component and select Edit Part.
2.
Click Tools, Options, Document Properties, Colors.
3.
Select Shading in Model\Feature colors, and click Edit.
4.
Select a new color, click OK to close the Color dialog box, and OK again to close the Options dialog box.
5.
To return to editing the assembly, right-click the assembly icon at the top of the FeatureManager design tree, and select Edit Assembly.
To toggle the wireframe display color of components:
Click View, Display, Use Component Color in HLR/HLV. •
When this menu item is selected, assembly components appear in the wireframe/HLR color of the component.
•
When this menu item is cleared, assembly components appear in the wireframe/HLR color of the assembly.
Annotations in Assemblies To specify the display of annotations in an assembly, right-click the Annotations folder in the FeatureManager design tree, and select Details. In the Annotation Properties dialog box, you have these options: •
Display filter. Select which annotation types, if any, to display by default. To select specific types, clear the Display all types check box, and select the types you want.
•
Text scale. Adjust the size of the text as needed.
•
Always display text at the same size. When checked, all annotations and dimensions are displayed at the same size, regardless of zoom.
•
Display items only in the view orientation in which they are created. When checked, any annotation is displayed only when the model is viewed in the same orientation as when the annotation was added.
•
Display assembly annotations. Toggles the display of annotations, including annotations that belong to the assembly, and annotations that are displayed in the individual part documents.
•
Use assembly’s setting for all components. Sets the display of all annotations to match the setting for the assembly document, regardless of the setting in the individual part documents. Use this option along with Display assembly annotations to display different combinations of annotations.
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Preventing Interference Between Components Interference Detection In a complex assembly, it may be difficult to visually determine whether components interfere with each other. You can determine the interference between components and examine the resulting interference volumes. To detect interference:
1.
Click Interference Detection
on the Assembly toolbar, or click Tools, Interference Detection.
By default, the top-level assembly appears under Selected Components unless you pre-selected other components. If you check an assembly for interference, all of its components are checked. 2.
Under Options, select Treat coincident as interference to report coincident entities as interference volumes. When cleared, coincident entities are ignored.
3.
Click OK
to check for interference.
The following occurs: •
The interference volumes appear under Results.
•
The components for the selected interference appear under Component 1 and Component 2.
•
The volume of the selected interference highlights in the graphics area. The volume of the interference is in the form of length, width, and height of the bounding box around the area of interference.
4.
Select other interference volumes under Results to examine other results.
5.
Clear the Selected Components box, select new components, and click OK for interference.
6.
Click Cancel
to check other components
when done.
Collision Detection You can detect collisions with other components when moving or rotating a component. The software can detect collisions with the entire assembly or a selected group of components. You can find collisions for either the selected components or for all of the components that move as a result of mates to the selected components. Physical Dynamics is an option in Collision Detection that allows you to see the motion of assembly components in a realistic way. With Physical Dynamics enabled, when you drag a component, the component applies a force to components that it touches, and moves the components if they are free to move. To detect collisions as you move or rotate components:
1.
Click Move Component
2.
In the PropertyManager, under Options, select Collision Detection.
3.
Under Check between, select: o
o
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or Rotate Component
on the Assembly toolbar.
All components - If the component you are moving touches any other component in the assembly, the collision is detected. These components - Select components for the Components for Collision Check box, then click Resume Drag. If the component you are moving touches a selected component, the collision is detected. Collisions with items that are not in the box are ignored.
4.
Select Dragged part only to check for collisions with only the components that you selected to move. When cleared, the components that you selected to move, plus any other components that move because of mates with the selected components, are checked.
5.
Select Stop at collision to stop the motion of the component when it touches any other entity.
6.
Under Options, select: o
Highlight faces - The faces that touch the component you are moving are highlighted.
o
Sound - The computer beeps when a collision is detected.
o
Ignore complex surfaces - Collisions are only detected on the following surface types: planar, cylindrical, conical, spherical, and torodial. NOTE: The This configuration check box does not apply to Collision Detection, Physical Dynamics, or Dynamic Clearance. It applies only to Move Component or Rotate Component.
7.
Move or rotate the component to detect collisions.
8.
Click OK
to finish and exit.
Physical Dynamics Physical Dynamics is an option in Collision Detection that allows you to see the motion of assembly components in a realistic way. With Physical Dynamics enabled, when you drag a component, the component applies a force to components that it touches. The effect is to move or rotate contacted components within their allowable degrees of freedom. The dragged component reacts to a collision by rotating within its allowable degrees of freedom or by sliding against a constrained or partially constrained component to allow the drag to continue. Physical Dynamics propagates throughout the assembly. The dragged component can push aside a component, which then moves into and pushes aside another component, and so on. Physical Dynamics works best and is most meaningful on assemblies that have only a few degrees of freedom. Add all appropriate mates prior to running Physical Dynamics. You cannot use Physical Dynamics and Dynamic Clearance at the same time. To move a component using physical dynamics:
1.
Click Move Component
or Rotate Component
on the Assembly toolbar.
2.
In the PropertyManager, under Options, select Physical Dynamics.
3.
Move the Sensitivity slider to change the frequency with which Physical Dynamics checks for collisions. Move the slider to the right to increase the sensitivity. At the most sensitive setting, the software checks for collisions every .02mm (in model units). At the least sensitive setting, the check interval is 20mm. Use the most sensitive settings only for very small components, or for components with complex geometry in the collision area. When you use the maximum sensitivity when checking for collisions between larger components, the drag is very slow. Use only the sensitivity setting you need to see the motion in your assembly.
4.
If needed, specify the components to participate in the collision: a.
Click These components.
b.
Select components for Components for Collision Check.
c.
Click Resume Drag. Choosing specific components in Collision Detection improves the performance of Physical Dynamics. Choose only those components that are directly involved in the motion you are testing.
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5.
Drag a component in the graphics area. When Physical Dynamics detects a collision it adds a contact force between the colliding parts and allows the drag to continue. The force remains as long as the two parts touch. When the two parts no longer touch, the force is removed. You can select one component after another within a single command.
6.
Click OK
.
Initial Collisions If the component you drag has an initial collision with another component, SolidWorks displays a message in the graphics area and all components involved in the collision turn transparent. Physical Dynamics is turned off for collisions between the transparent components. You can continue the drag, and collide with and apply a force to other components. To activate a collision between initially colliding components
1.
Drag your component until it no longer interferes.
2.
Release the drag.
3.
Drag again. The components are no longer transparent, and Physical Dynamics works.
Dragging by Center of Mass When you click a component to drag it, a center of mass symbol appears at the component's center of mass. If you click the symbol and drag the component, you are dragging by the center of mass. If you click outside the symbol and drag, you are dragging by the point on the body you clicked. You apply a moment arm to a component if you drag outside the center of mass, which causes the component to rotate within the allowable degrees of freedom. NOTE: The center of mass symbol appears during Move, but not during Rotate. The Free Drag option in Rotate Component is by definition rotation about the center of mass.
Dynamic Clearance You can dynamically detect the clearance between components when moving or rotating a component. As you move or rotate a component, a dimension appears indicating the minimum distance between the selected components. Additionally, you can prevent two components from moving or rotating within a specified distance of one another. To dynamically detect the clearance between components:
1.
Click Move Component
or Rotate Component
on the Assembly toolbar.
2.
In the PropertyManager, select Dynamic Clearance.
3.
Click in Components for Collision Check
4.
Click Stop at Specified Clearance and type a value in the box to prevent the selected components from moving within the specified distance.
5.
Drag one of the selected components in the graphics area.
, select the components to check, then click Resume Drag.
Notice a dimension appears in the graphics area and in the PropertyManager. This dimension is the minimum distance between the selected components; the dimension dynamically updates as you drag the component. Also, in the PropertyManager, a value appears in brackets. This is the minimum distance found during the drag operation.
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6.
Under Options, select: o
o
Sound - The computer beeps when the minimum distance in the Stop at Specified Clearance box is reached. Ignore complex surfaces - Clearances are only detected on the following surface types: planar, cylindrical, conical, spherical, and torodial. NOTE: The This configuration check box does not apply to Collision Detection, Physical Dynamics, or Dynamic Clearance. It applies only to Move Component or Rotate Component.
7.
Click OK
to finish and exit.
Smart Fasteners Smart Fasteners Overview Smart Fasteners automatically adds fasteners (bolts and screws) to your assembly if there is a hole, hole series, or pattern of holes, that is sized to accept standard hardware. It uses the SolidWorks Toolbox library of fasteners, which has a large variety of ANSI Inch, Metric and other standard hardware. Smart Fasteners follows the copy parts options in the SolidWorks Toolbox Configure Browser dialog box to determine if fasteners are added to an assembly as a configuration of an existing part or as a copy of an existing part.
Assembly with various types of holes
Assembly with Smart Fasteners
Holes for Smart Fasteners Smart Fasteners adds fasteners to available hole features in assemblies. The holes can be assembly or part features. You can add fasteners to specific holes or patterns, faces or components, or to all available holes. Smart Fasteners is feature-based. Fasteners are placed in Hole Wizard holes, simple holes, and cylindrical cut features. Smart Fasteners does not recognize holes in derived, mirrored, or imported bodies. If you extrude a sketch of a rectangle with a circle in it as a base feature, Smart Fasteners does not recognize the inside of the boss as a hole, because the cylinder is not a separate feature. See Unsupported Hole Types for more information on hole recognition.
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Fasteners Hole Wizard holes are fitted with matching bolts or screws. For other types of holes, you can configure Smart Fasteners to add any type of bolt or screw as a default. The fasteners are automatically mated to the holes with concentric and coincident mates. Hardware Stacks Smart Fasteners can add nuts and washers to your fasteners. Nuts and washers are automatically mated to the fastener with a concentric mate, and to the fastening surface with a coincident mate. Configurations The added fasteners are fully parameterized parts. Each Smart Fastener is shown in the FeatureManager, and can be expanded to show individual features. Smart Fasteners added to hole patterns use a fastener pattern derived from the hole pattern. The fasteners are all the same type and size, but you can use different configurations of the fastener in the pattern. For example you can make some bolts longer than others. Editing You can change your fasteners with the Edit Smart Fasteners command. It is not recommended to edit the individual parameters of a Toolbox part using Edit Sketch or Edit Definition. These functions do not update the Toolbox database.
Smart Fasteners PropertyManager Smart Fasteners inserts bolts and screws into selected holes in your assembly. The fasteners are fully parameterized SolidWorks parts from the Toolbox library. NOTE: You must enable Toolbox to use Smart Fasteners. To enable Toolbox:
1.
Click Tools, Add-ins.
2.
Select SolidWorks Toolbox and SolidWorks Toolbox Browser.
3.
Click OK.
To add Smart Fasteners to an assembly:
1.
Select one or more holes, face, or component. If you select a component, Smart Fasteners finds all available holes in that component. If you select a face, Smart Fasteners finds all available holes that pass through the surface.
2.
Click Smart Fasteners
on the Assembly toolbar, or click Insert, Smart Fasteners.
If you pre-selected a hole, face, or component, new fasteners appear in the assembly and under Fasteners in the PropertyManager. 3.
To add fasteners: a.
Select holes, faces, or components.
b.
Under Selection, click Add. New fasteners appear in the assembly and under Fasteners.
c.
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Click Populate All to add fasteners to all the holes in the assembly.
4.
Change the fastener parameters if needed.
5.
Add nuts and washers if needed.
6.
Click OK
.
Fastener Defaults The length of a new fastener is the next smallest national standard length for a blind hole, and the next longest national standard length for a through hole. When holes are deeper than the longest fastener length, the longest one is used. For a Hole Wizard hole, the fastener type matches the type of hole, and the diameter is the appropriate size. For a Simple Hole or cylindrical cut, you can specify a default fastener type. The fastener diameter is the next smallest national standard size. The PropertyManager Fasteners List The Fasteners list in the Smart Fasteners PropertyManager shows each fastener in your assembly. You can expand each item to show: •
Top Stack. Washers under the head of the fastener.
•
Bottom Stack. Washers and nuts at the end of the fastener.
•
Series 1, Series 2, and so on. Separate hole series that use this fastener. Expand a Series to show: o
Top Stack.
o
Hole features.
o
Bottom Stack. Available for through holes only.
Right-click a fastener to change fastener type, delete it, or change the fastener parameters. Drag and drop a hole feature to create a new series or assign it to a different fastener. Smart Fasteners does not automatically add nuts or washers. You must add these by editing the fastener or the series. See Smart Fasteners Hardware Stacks for more information on adding hardware to fasteners.
Smart Fasteners Bolts and Screws
Askew Head Bolt
Binding Head Screw
Binding Head Miniature Screw
Countersunk Bolt
Countersunk Elevator Bolt
Countersunk Square Neck Bolt
Fillister Head Screw
Fillister Head Chamfered Miniature Screw
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Fillister Head Oval Crown Miniature Screw
Flat Head Screw
Flat Head Miniature Screw
Heavy Hex Bolt
Heavy Hex Structural Bolt
Hex Lag Screw
Hex Screw
Hex Washer Screw
Oval Head Screw
Pan Cross Head Screw
Pan Head Miniature Screw
Pan Slot Head Screw
Round Head Bolt
Round Head Fin Neck Bolt
Round Head Ribbed Neck Bolt
Round Head Screw
Round Head Square Neck Bolt
Round Head Step Bolt
Socket Button Head Cap Screw
Socket Countersunk Head Cap Screw
Socket Head Cap Screw
Socket Head Shoulder Screw
Square Bolt
T-Head Bolt
Truss Head Screw
Hex Flange Screw
Square Lag Screw
Smart Fasteners Nuts Size comparison of Regular and Heavy Hex Nuts:
Styles: Both Hex Nuts and Heavy Hex Nuts are available in Hex, Hex Flat, Hex Flat Jam, Hex Jam, and Hex Slotted styles.
Hex
Hex Flat
Hex Jam
Hex Slotted
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Miscellaneous Nut Styles:
Acorn High Crown
Hex Thick
Acorn High Crown 61
Acorn Low Crown
Heavy Hex Square
Hex Thick Slotted
Smart Fasteners Washers Type A Washers Selected washers have a smaller hole than preferred washers. Narrow washers are slightly thinner than wide washers.
Preferred Narrow Flat
Preferred Wide Flat
Selected Narrow Flat
Type B Washers Narrow washer is slightly thinner than wide and regular washers.
Wide Flat
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Regular Flat
Narrow Flat
Selected Wide Flat
Spring Lock Washers
Regular
Heavy
Hi-Collar
Extra Duty
Unsupported Hole Types Smart Fasteners inserts fasteners into series of holes in assemblies. •
Holes must be a supported type.
•
Not all hole types are supported by Smart Fasteners. Unsupported hole types include: o
Single holes
o
Base extrude formed from a sketch with inside circles
o
Mirrored Hole Wizard holes
o
Holes from imported, derived, or mirrored parts
o
Mismatched patterned holes
o
Holes with a large difference in radius
o
Misaligned holes
o
Aligned holes with large gaps between holes
Single holes The hole must pass through at least two components.
Unsupported
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Base extrude with inside circles
A base extrude with inside circles appears to form holes. Although geometrically identical to holes, they are not separate features, and are not recognized by Smart Fasteners. Holes from imported, derived, or mirrored parts If holes in an imported part, derived base part, or mirrored part come from the parent part, they are not recognized by Smart Fasteners. However, holes you put into imported, derived, or mirrored parts are recognized because they are separate features. Mismatched patterned holes If a hole is part of a pattern in one component, it must be part of an identical pattern in the other components through which the fastener hole passes. The patterns must be identical in the number of holes. If a hole in one component is part of a pattern, it cannot form a series with a hole in another component that was created as a separate feature that is not part of a pattern.
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Unsupported
Unsupported
Supported
Supported
Large differences in radius If any hole in a series is more than twice the radius of the smallest hole in the series, Smart Fasteners does not recognize the holes.
Unsupported hole series - 45 > 2(20)
Supported hole series - 35 < 2(20)
Misaligned holes Holes are unsupported if they are misaligned. If Smart Fasteners does not insert a fastener into a hole series that appears aligned and is otherwise appropriate, check for a small geometric misalignment (see Measure). Large gaps between holes If the length of the series from start to finish is greater than 5 times the total depth of all the individual holes, the series is not recognized during Populate All. You can add Smart Fasteners into specific holes in the long series by selecting them during insert.
Editing Smart Fasteners You can change the type, size, length, and other editable dimensions of a Smart Fastener. You can flip Smart Fasteners in through holes. You can also change the type of fastener assigned to a hole, or split a bolt series by dragging a hole to a different fastener. To edit Smart Fasteners:
Right-click Smart Fastener in the FeatureManager design tree and select Edit Smart Fastener. The Smart Fasteners PropertyManager appears. To flip Smart Fasteners:
1.
Expand the fastener in the Smart Fasteners PropertyManager.
2.
Right-click the Series you want to flip and select Flip. The heads of the fasteners in the selected series flip to the other side of the joint.
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To change the type of Smart Fastener:
1.
Right-click a fastener in the Smart Fasteners PropertyManager and select Change fastener type. The Smart Fastener dialog box appears.
2.
3.
Select from the following: •
Standard. Select a national or user-defined standard.
•
Type. Choose a type of bolt or screw from the list.
•
Fastener. Choose from specific fasteners based on the Standard, Category, and Type you selected. The Toolbox Browser displays the full range of available fasteners. You can also view an online glossary of bolts and screws.
Click OK.
To change the parameters of Smart Fasteners:
1.
Right-click a fastener or Series and select Properties. A dialog box opens with a list of dimensions and features which can be changed. Dimensions that cannot be changed are not listed.
2.
Select a parameter to change and choose a new value or option from the list. Repeat for other parameters as needed.
3.
Click OK.
NOTE: It is not recommended to edit the individual parameters of a Toolbox part using Edit Sketch or Edit Definition. These functions do not update the Toolbox database.
Smart Fasteners Hardware Stacks Smart Fasteners does not automatically add nuts or washers to fasteners. You can add standard nuts and washers to Smart Fasteners in the Smart Fasteners PropertyManager. Each Series of fasteners has an associated Top Stack (washers added under the head of the fastener) and Bottom Stack (washers and nuts added to the end of the fastener). You can expand each fastener series to see its Top Stack and Bottom Stack. If you add hardware to the Top Stack or Bottom Stack at the fastener level, that hardware appears in each Series. If you add hardware to the Top Stack or Bottom Stack at the Series level, it appears in that Series only. NOTE: You cannot add hardware to a Bottom Stack for blind or tapped holes. See Smart Fastener Defaults for options to associate the size and length of a fastener to the hardware stack. To add washers under a bolt head:
1.
If you are not in the Smart Fasteners PropertyManager, right-click the Smart Fastener in the FeatureManager design tree, and select Edit Smart Fasteners. The Smart Fasteners PropertyManager appears.
2.
Click
to expand the fastener tree.
3.
If you want to add washers to one Series only, click
4.
Double-click Top Stack for either the fastener or the Series.
to expand that Series
The Top Stack Components dialog box appears. 5.
In row 1, select a Component and Quantity.
6.
Click the box under Properties. The properties dialog box appears, where you can change the component's properties and assign a part number.
7.
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If you want to add other sizes or types of washers to the Top Stack, select a second component in row 2 of the properties dialog box, a third component in row 3, and so on. If you add more than one type of washer, the first is next to the bolted surface, and the subsequent washers are added toward the bolt head.
NOTE: To remove a component from the stack, select None from the component list.
Top Stack Order
Bottom Stack Order
To add nuts and washers at the end of a bolt:
1.
Repeat steps 1 to 3 from the procedure above.
2.
Double-click Bottom Stack. The Bottom Stack dialog box appears.
3.
Add hardware as described in the procedure above. Add washers first, and the nut last. The hardware appears in order from the bolted surface toward the end of the bolt.
NOTE: If you add hardware at the Series level, and then add hardware at the fastener level, you overwrite the Serieslevel hardware.
Drag-and-Drop Editing of Smart Fasteners Splitting Hole Series In an assembly with a series of aligned holes, the design may call for a number of short fasteners or one long fastener. Smart Fasteners automatically assigns a single long fastener to the hole series. You can then split the hole series into multiple series, each with its own fastener. NOTE: To split the series, you must have separate hole features within the series. For example, you cannot split a series of holes formed from an assembly-level hole feature, since that is a single feature.
Single fastener assigned to hole series.
Hole series split. New fastener lengths.
To split a hole series:
1.
If you are not in the Smart Fasteners PropertyManager, right-click the Smart Fastener in the FeatureManager design tree, and select Edit Smart Fasteners. The Smart Fasteners PropertyManager appears.
2.
Under Fasteners, click
3.
Click
to expand the fastener tree.
to expand the Series.
Separate hole features are listed in order between Top Stack and Bottom Stack. In this example there are four hole features.
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4.
Select the first hole feature that you want to split off from the series, (in this example, the third hole feature), and drag it to the fastener name at the top level of the tree. The first and second hole features stay with the original series, and the third and fourth hole features form a new series. When you select a hole feature for a new series, that hole feature and all the ones following it in the fastener list move into the new series.
5.
A message box appears. Select one of the following options: •
Click Yes to calculate new fastener lengths for both series.
•
Click No to keep the original fastener length for both series.
A new Series is added to the list, and another set of fasteners appears in the graphics area in the selected holes. The fasteners have the same properties (except for length) as the parent fastener. You can edit the properties at the fastener level or at the Series level. Reassigning Holes One way to change the properties of Smart Fasteners is to reassign the fastener hole to a different fastener. See Editing Smart Fasteners for other ways to change fastener properties. To reassign a hole:
1.
If you are not in the Smart Fasteners PropertyManager, right-click the Smart Fastener in the FeatureManager design tree, and select Edit Smart Fasteners.
2.
Expand the fastener and Series for the hole you want to reassign.
3.
Select the hole series in the PropertyManager design tree and drag it to another Smart Fastener in the tree. The hole series moves under the new Smart Fastener in the tree, and the new fastener appears in the graphics area.
Smart Fasteners Part Numbers You can assign part numbers and descriptions to Smart Fasteners. The part numbers become part of the Toolbox database, and are available to you in other assemblies. To assign part numbers and descriptions to Smart Fasteners:
1.
In the Smart Fasteners PropertyManager, right-click a fastener group in the Fasteners list and select Properties.
2.
Select List by Part Number or List by Description.
3.
Click Add. The Toolbox - New Part Number dialog box appears.
4.
Accept the default part number or type your own in the Part Number box. Type a description in the Description box.
5.
Click OK
.
Mark Up-to-date If you change a hole containing Smart Fasteners, you might get the following warning: Hole series has changed. Please verify that current fastener is correct. The affected fastener is marked with a flag
in the FeatureManager design tree.
To clear the warning:
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1.
Check to see that the fastener is correct.
2.
Right-click the fastener in the FeatureManager design tree and select Mark upto date.
Configuring Bolt Patterns in Smart Fasteners Smart Fasteners added to hole patterns use a bolt pattern derived from the hole pattern. The fasteners are all the same and there is only one fastener listed in the Smart Fasteners PropertyManager. If you want to change the properties of some bolts in the pattern, (for example, make them longer), you can specify different configurations of the bolt. Each time you specify a Smart Fastener, you add it to your Toolbox database. Smart Fasteners follows the copy parts options in the SolidWorks Toolbox Configure Browser dialog box to determine if fasteners are added to an assembly as a configuration of an existing part or as a copy of an existing part. To change the parameters of an individual fastener in a pattern:
1.
Click
to expand the Smart Fastener in the FeatureManager design tree.
2.
Click
to expand the DerivedLPattern (or DerivedCPattern).
All fasteners in the pattern are listed. 3.
Right-click a fastener in the list and select Properties. The Component Properties dialog box appears.
4.
Under Referenced configuration, select Use named configuration.
5.
Select a bolt from the list. NOTE: If you do not see the configuration you want, you can add a new configuration to the Toolbox database using the procedure below.
6.
Click OK. The revised bolt appears.
To add a new fastener configuration to the Toolbox database:
1.
Click
to expand the Smart Fastener in the FeatureManager design tree.
2.
Right-click the fastener component and select Edit Toolbox Definition. The properties dialog box for the fastener appears.
3.
Select new parameters for the fastener. For example, choose a different length or drive type.
4.
Click OK. All fasteners in the series change to the new configuration. You can now change individual bolts in the bolt pattern to use either the old or the new configuration.
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Smart Fasteners Defaults You can configure default fasteners for different standards and hole types. You can also make the fastener's length change when the hardware stack changes, and make the stack hardware size change when the fastener size changes. To set Smart Fasteners defaults:
1.
Click Toolbox, Browser Configuration. The Configure Browser dialog box appears.
2.
Click the Smart Fasteners tab.
3.
Choose from the following options: •
•
•
4.
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Default Fasteners. •
Holes without standards. Choose a default Standard and a default fastener.
•
Holes with standards. Choose a default fastener for each Standard.
Fastener Update. Select the following check boxes to associate Smart Fasteners and hardware stack dimensions. •
Change fastener length when stack components are added or removed. Fastener length increases when you add additional stack hardware, and decreases when you remove stack hardware. Fastener length changes by standard increments and cannot be longer than the longest national standard.
•
Change stack components when fastener size is changed. Nut and washer sizes automatically change when the fastener size changes.
Stack Components. Select from options to limit the available washer types, depending on the size of your Smart Fastener.
Click OK.
•
Exact match. Limits the available types to washers that exactly match your fastener size.
•
Greater than tolerance. Limits the available types to hole diameters that match your fastener size within the tolerance you type.
•
Unrestricted. All washer types available.
10 Configurations
Configurations Overview Configurations allow you to create multiple variations of a part or assembly model within a single document. Configurations provide a convenient way to develop and manage families of models with different dimensions, components, or other parameters. To create a configuration, you specify a name and properties, then you modify the model to create the design variations you want. •
In part documents, configurations allow you to create families of parts with different dimensions, features, and properties, including custom properties.
•
In assembly documents, configurations allow you to create: o o
simplified versions of the design by suppressing or hiding components. families of assemblies with different configurations of the components, different parameters for assembly features, different dimensions, or configuration-specific custom properties.
You can create configurations manually, or you can use a design table to create multiple configurations simultaneously. Design tables provide a convenient way to create and manage configurations in an easy-to-use worksheet. You can use design tables in both part and assembly documents, and you can display design tables in drawings. Custom properties created in design tables are automatically added to the Configuration Specific tab in the Summary Information dialog box.
ConfigurationManager The ConfigurationManager on the left side of the SolidWorks window is a means to create, select, and view multiple configurations of parts and assemblies in a document. You can split the ConfigurationManager and either display two ConfigurationManager instances, or combine the ConfigurationManager with the FeatureManager design tree, PropertyManager, or third party applications that use the panel. The icons in the ConfigurationManager denote whether the configuration was created manually table .
or with a design
To activate the ConfigurationManager:
Click the ConfigurationManager tab
at the top of the left panel.
Each configuration is listed separately. To return to the FeatureManager design tree:
Click the FeatureManager design tree tab
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Show Preview You can display configuration previews of a part or assembly in the PropertyManager. You do not have to open a configuration to see it, which saves time in complex parts and assemblies. To display a configuration preview in the PropertyManager:
1.
In the ConfigurationManager, right-click the configuration you want to preview and select Show Preview. The FeatureManager design tree automatically splits, and the configuration preview appears in the PropertyManager. NOTE: If the preview does not appear, open each configuration, and save the document in each configuration. The next time you select Show Preview, the preview appears.
2.
While the preview is displayed, click any other configuration in the ConfigurationManager to update the preview.
3.
Click anywhere in the graphics area to hide the preview.
Configurations and In-context Components You can have more than one instance of an in-context component that is geometrically different in an assembly. To accomplish this, you must have the following: •
A driving part with two configurations.
•
An sub-assembly with two configurations.
•
In the sub-assembly, create a driven part with two configurations. The driven part is built in the context of the sub-assembly referencing the different geometry in the two configurations of the driving part. The configurations in the driving part, driven part, and sub-assembly do not need to have the same name. But, you must correctly organize the configuration names that represent each combination of geometrically different components.
Here is an example to show how to place components that are geometrically different into the same assembly: 1.
Create a cylindrical part called tube.
2.
Create two configurations of tube called large and small. Each configuration has a different diameter for the cylinder.
3.
Add tube to a sub-assembly called pipes and create two configurations of the sub-assembly called large and small. Each configuration of the sub-assembly, pipes, use tube in its large and small configurations.
4.
Create a part called plug in the context of the sub-assembly, referencing the different diameters of tube. Plug must have two configurations large and small that match the driving component, tube.
5.
Insert two instances of the sub-assembly, pipes, into a main assembly called plumbing. Set one instance of pipes to the large configuration and the other to the small configuration. You now have two instances of the driven part, plug, that are geometrically different in the same assembly. The important detail is matching the configurations of the driving part, driven part, and sub-assembly.
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Configure Document When you open an assembly document, you can specify the configuration name to use for the parts contained in the assembly. You can also create a new configuration when you open an assembly, and either suppress or resolve all of the components at once. To use specific part configurations contained in an assembly:
1.
Click File, Open.
2.
In the Open dialog box: a.
Select an assembly document.
b.
Select the Advanced check box.
c.
Click Open.
The Configure Document dialog box appears. 3.
Select the Use specified configuration for part references when available check box, and type a part Configuration name. Any part that has a configuration with the specified name uses that configuration.
4.
Click OK. The document opens with the selected configuration.
To open a new configuration of an assembly:
1.
Click File, Open.
2.
In the Open dialog box:
3.
a.
Select an assembly document.
b.
Select the Advanced check box.
c. Click Open. In the Configure Document dialog box: •
To open the assembly with all the components resolved, click New configuration showing all referenced models.
•
To open the assembly with all the components suppressed, click New configuration showing assembly structure only.
4.
Type a name for the new configuration in the Configuration name box.
5.
Click OK. The assembly opens in the new configuration.
Configure Document for View / Configurations The Configure Document for View dialog box appears if you opened a drawing whose configuration no longer exists. The Configurations dialog box appears if you replaced a component in an assembly, and clicked the Manually select option. If either of these dialog boxes appears, select a configuration to use, then click OK.
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Manual Configurations Creating a Configuration Manually To create a configuration manually, you specify its properties, then modify the model to create variations in the new configuration. To create a configuration manually:
1.
In either a part or assembly document, click the ConfigurationManager tab FeatureManager design tree to change to the ConfigurationManager.
at the top of the
2.
In the ConfigurationManager, right-click the part or assembly name and select Add Configuration.
3.
In the Add Configuration dialog box, type a Configuration Name and specify properties for the new configuration. You can specify a configuration specific color.
4.
Click OK.
5.
Click the FeatureManager design tree tab
6.
Modify the model as needed to create the design variation.
7.
Save the model.
to return to the FeatureManager design tree.
Add Configuration/Configuration Properties This dialog box controls the following properties when you add a configuration or edit configuration properties: Configuration Name. Type a name for the configuration. The name must not include the forward slash (/) or at sign (@). A warning message appears when you close the dialog box if the name field contains either of these characters, if the field is blank, or if the name already exists. Description. Type a description that identifies the configuration. (Optional) Comment. Type additional descriptive information about the configuration. (Optional) Use configuration specific color. To specify a color for the configuration, select this check box, then click Color to choose a color from the color palette. •
If the color for wireframe and HLR modes is the same as the color for shaded mode, the configurationspecific color applies to all three modes. If the color is not the same for all three modes, then the configuration specific color applies to shaded mode only. To be sure the colors are the same for the three modes, select the Apply same color to wireframe, HLR and shaded check box in Tools, Options, Document Properties, Colors.
•
To apply a configuration-specific color to components in an assembly, right-click the selected components in the FeatureManager design tree, select Component Properties, and click Color. In the Assembly Instance Color dialog box, click Use Assembly and click OK.
Properties for newly inserted items. These check boxes control what happens when new items are added to another configuration, and then this configuration is activated again. For assemblies, the following check boxes are available:
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•
Suppress features and mates. When selected, new mates and features added to other configurations are suppressed in this configuration. Otherwise, new mates and features are unsuppressed in this configuration also.
•
Hide component models. When selected, new components added to other configurations are hidden in this configuration. Otherwise, new components are shown in this configuration also.
•
Suppress component models. When selected, new components added to other configurations are suppressed in this configuration. Otherwise, new components are resolved in this configuration also.
For parts, the following check box is available: •
Suppress features. By default, newly added features are unsuppressed in the active configuration. This option controls what happens when new features are added to another configuration, then this configuration is activated again. When selected, new features added to other configurations are suppressed in this configuration. Otherwise, new features are unsuppressed in this configuration also.
Part number displayed when used in a bill of materials. Click to specify how the assembly or part is listed in a Bill of Materials. •
Select one of the following: o
Document Name. The part number is the same as the document name.
o
Configuration Name. The part number is the same as the configuration name.
o
User Specified Name. The part number is a name that you type.
Don’t show child components in BOM when used as sub-assembly (assemblies only). When selected, the subassembly is always shown as a single item in the bill of materials. Otherwise, the child components may be listed individually in the BOM, when Show parts only or Show assemblies and parts in an indented list is selected. NOTE: After you create a configuration, if you right-click the configuration name in the ConfigurationManager and select Properties, the Configuration Properties dialog box appears. Click Custom to access Configuration Specific properties in the Summary Information dialog box.
Properties for Newly Inserted Items These options control what happens to this configuration when you add new items to another configuration. The options that are available depend on the type of document. Check box cleared
Check box selected
New features are included (not suppressed)
New features are suppressed
Suppress features and mates
New features* and mates are included (not suppressed)
New features* and mates are suppressed
Hide component models
New components are shown
New components are hidden
Suppress component models
New components are resolved (not suppressed)
New components are suppressed
Part documents Suppress features Assembly documents
* New features in assemblies include assembly feature cuts and holes, component patterns, reference geometry, and sketches that belong to the assembly (not to one of the assembly components).
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Derived Configurations Derived configurations allow you to create a parent-child relationship within a configuration. By default, all parameters in the child configuration are linked to the parent configuration. If you change a parameter in the parent configuration, the change automatically propagates to the child. You can override any configurable parameter in the derived configuration so that the parameter is no longer linked to the parent. Consider the following example. Part1 has three configurations: •
Configurations A and C are top-level configurations. Configuration B is a derived configuration of configuration A.
•
The following table shows the effect on configurations B and C when you change configuration A. Change configuration A and apply the change to:
Effect on configuration B
Effect on configuration C
This Configuration
Changes
Does not change
Specify Configurations (specify configuration A)
Changes
Does not change
All Configurations
Changes
Changes
Example of derived configurations. To create a derived configuration manually:
1.
In the ConfigurationManager, right-click a configuration and select Add Derived Configuration.
2.
In the dialog box, enter the appropriate configuration properties.
3.
Under Part number displayed when used in a bill of materials, select from:
4.
•
Document Name. The part number is the same as the document name.
•
Configuration Name. The part number is the same as the configuration name.
•
Link to Parent Configuration. The part number is the same as the parent configuration name.
•
User Specified Name. The part number is a name that you type.
•
Don't show child components in BOM when used as sub-assembly (assemblies only). When selected, the sub-assembly is always shown as a single item in the bill of materials. Otherwise, the child components can be listed individually in the BOM, when Show parts only or Show assemblies and parts in an indented list is selected.
Click OK. The derived configuration is added to the ConfigurationManager underneath its parent.
To create a derived configuration with a design table:
The column header in a design table for controlling derived configurations uses this syntax: $PARENT The column header is not case sensitive. In the table body cells, type the parent configuration names.
10-6
You cannot specify a parent configuration in a design table if its child configuration was created first, unless the parent configuration already existed in the model.
Valid: Parent created before derived configuration
Invalid: Parent created after derived configuration
This Configuration When you select This Configuration, the changes you make to the model are reflected in the current configuration only. Specify Configurations When you select Specify Configurations, the changes you make to the model are reflected in the configurations that you specify. All Configurations When you select All Configurations, the changes you make to the model are reflected in each of the model's configurations. Example of Derived Configurations This part contains three configurations: A, B, and C. Configuration A is the parent of configuration B, and configuration C is a top-level configuration, similar to configuration A.
Original configuration A (parent)
Modified configuration A
Configuration B (derived)
Configuration C
The extrude in configuration A is modified from 120mm to 60mm. In the Modify dialog box, when This Configuration is selected, the dimension changes in configurations A and B, but not C.
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Activating a Configuration To activate a different configuration:
1.
Click the Configuration Manager tab
to change to the ConfigurationManager.
2.
Right-click the name of the configuration you want to view and select Show Configuration. - or Double-click the configuration name. The named configuration becomes the active configuration, and the view of the model updates to reflect the newly selected configuration.
Configurable Items for Parts You can vary the design of part configurations as follows: •
Modify feature dimensions.
•
Suppress features, equations, and end conditions.
•
Use different sketch planes, sketch relations, and external sketch relations.
•
Set individual face colors.
•
Control the configuration of a base part.
•
Control the configuration of a split part.
•
Control the driving state of sketch dimensions.
•
Create derived configurations.
•
Define configuration-specific properties.
Sketch Dimensions in Configurations You can control the driving state of sketch dimensions in specified configurations to control the behavior of your model. To control the driving state of sketch dimensions:
1.
Right-click a dimension, and select Properties. The Dimension Properties dialog box appears.
2.
Select the Driven check box.
3.
Click Specify Configs. A dialog box appears.
4.
Select the configurations you want to apply the new settings to: This configuration, All configurations, or Specify configurations.
5.
Click OK.
6.
Click OK again to close the Dimension Properties dialog box. The sketch dimension is driven.
10-8
Sketch Planes in Configurations The plane on which a sketch lies is configurable through the Sketch Plane PropertyManager. You can place a single sketch on different planes in different configurations. To change a sketch plane in a configuration:
1.
In the FeatureManager design tree, right-click a sketch and select Edit Sketch Plane. The Sketch Plane PropertyManager appears.
2.
In the graphics area, click the face or plane on which you want the sketch to lie. - or Select a plane from the flyout FeatureManager design tree on which you want the sketch to lie.
3.
Under Configurations, select the configurations to which you want the new sketch plane to apply: This configuration, All configurations, or Specify configurations.
4.
Click OK
.
The sketch changes planes in the selected configurations. Sketch Relations in Configurations You can control the suppression state of sketch relations per configuration. To suppress or unsuppress sketch relations:
1.
Right-click a sketch in the FeatureManager design tree, and select Edit Sketch.
2.
Click Display/Delete Relations
3.
In the PropertyManager, under Configurations (at the bottom of the PropertyManager), select the configurations to which you want the sketch relations to apply: This configuration, All configurations, or Specify configurations (these options are only available if there is more than one configuration in the model).
on the Dimensions/Relations toolbar.
NOTES: •
You must select a configuration prior to changing sketch relations. When you change sketch relations, the change is immediately applied to the selected configuration.
•
If you selected Specify configurations, you cannot clear the active configuration.
4.
Under Relations, select the sketch relations to suppress or unsuppress.
5.
Select or clear Suppressed. When Suppressed is selected, the sketch relation's Information Status Driven.
6.
Click OK
changes from Satisfied to
, and exit the sketch.
The sketch relation is applied to the selected configurations. To suppress or unsuppress sketch relations in a design table:
The column header in a design table for controlling sketch relations uses this syntax: $STATE@<sketch_relation>@<sketch_name> For example, to control the suppression state of the first fixed relation in Sketch2, the column heading syntax is $STATE@Fixed1@Sketch2. The column header is not case sensitive.
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In the table body cells, type S for suppressed or U for unsuppressed. Sketch relations and sketch entities include an assigned number (such as Fixed1) in the Sketch Relations PropertyManager. Example of a design table that controls the suppression state of a sketch relation:
End Conditions in Configurations You can change the end condition of extruded features in specified configurations. To change the end condition of extruded features in specified configurations:
1.
In the FeatureManager design tree, right-click an extruded feature and select Edit Feature.
2.
In the PropertyManager, change the End Condition to the desired settings.
3.
Under Configurations, select the configurations to which you want the new end condition to apply: This configuration, All configurations, or Specify configurations.
4.
Click OK
.
The end condition is applied to the selected configurations.
Configurable Items for Assemblies You can vary the design of assembly configurations as follows:
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•
Change the suppression state (Suppressed, Resolved) or visibility (Hide, Show) of components.
•
Change the referenced configuration of components.
•
Change the dimensions of distance or angle mates, or suppression state of mates.
•
Modify the dimensions or other parameters of features that belong to the assembly. This includes assembly feature cuts and holes, component patterns, reference geometry, and sketches that belong to the assembly (not to one of the assembly components).
•
Suppress features that belong to the assembly.
•
Define configuration-specific properties, such as end conditions and sketch relations.
•
Create derived configurations.
•
Change the suppression state of the Simulation folder in the FeatureManager design tree and its simulation elements. (Suppressing the folder also suppresses its elements.)
Modifying a Configuration Dimension To modify a dimension value for a selected configuration, do one of the following: •
Control the value in a design table.
•
Double-click the feature to display the dimension. Then double-click the dimension, change the value in the Modify box, and select one of the following (these options are only available if there is more than one configuration in the model): o
This Configuration
o
All Configurations
o
Specify Configuration(s)
This applies in part and assembly documents, to all types of feature dimensions, the values used in mates (distance or angle), the number of instances in patterns, and so on.
Editing a Configuration To edit a configuration:
1.
Activate the desired configuration.
2.
Change to the FeatureManager view, then: •
In a part document, change the suppression state of features, modify dimensions, and so on, as needed.
•
In an assembly document, change the suppression state or visibility of components, and so on, as needed.
To edit the configuration properties:
1.
Right-click the configuration name, and select Properties. The Configuration Properties dialog box appears.
2.
Edit the name, comments, or properties as desired.
3.
Click Custom to add or modify custom properties for the configuration.
4.
Click OK.
To suppress or hide features or components:
1.
Select the features or components to suppress or hide (or to unsuppress or show).
2.
Click Edit and choose from the following menu items: In parts: •
Suppress
•
Unsuppress
•
Unsuppress with Dependents
In assemblies:
3.
•
Hide
•
Show
•
Show with Dependents
•
Suppress
•
Unsuppress
•
Unsuppress with Dependents
Each menu item has the following choices: •
This Configuration
•
All Configurations
•
Specified Configurations
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4.
If you selected Specified Configurations, a dialog box appears with a list of configurations and buttons to Select All and Reset Selection. Select configurations in the list and click OK.
Special Assembly Configurations You can create new assembly configurations, by either suppressing or resolving all of the components at once. Open the assembly in a new configuration with one of these options: •
structure only shown (all components suppressed)
•
all referenced models shown (all components resolved)
To suppress or resolve all components in a new assembly configuration:
1.
Click File, Open.
2.
Browse to the desired assembly document, select the Advanced check box, and click Open.
3.
In the Configure Document dialog box, select either:
4.
•
New configuration showing all referenced models. Opens the complete assembly. The components are all resolved and shown, regardless of their suppression and visibility state when last saved. All components appear in the assembly model.
•
New configuration showing assembly structure only. Opens the assembly structure only. The components are suppressed, regardless of their state when last saved. No components appear in the assembly model until you change their suppression state to resolved.
Type a new Configuration name, and click OK. The assembly opens in the new configuration.
Component Configurations in an Assembly If a component (either an individual part or a sub-assembly) has more than one configuration, you can specify which configuration to use for each instance in the assembly. You can also specify certain configuration-specific properties for the component. To specify component configurations and configuration-specific properties:
1.
Right-click the component name in the FeatureManager design tree, or right-click a component face, and select Properties.
2.
In the dialog box, select from the following options: •
Visibility. Allows you to Hide Model and change component color.
•
Referenced configuration. Controls options for referenced configurations: o
Use component’s “in-use” or last saved configuration Any instances with this option use the active configuration (if the document is open), or the configuration that was active when it was saved. When you open an assembly, any active components that are not already open in their own windows are loaded into memory. If you change the configuration in the component’s own window, the newly selected configuration is placed in memory; any instances that use this option update when you return to the assembly. When you edit a part in the context of an assembly, the referenced configuration in the assembly becomes the active configuration in all open windows (for example, if the part is open in its own window, or in use in another open assembly, with this property selected). To change the active configuration for a component that is not already open, right-click the component name in the FeatureManager design tree, and select Open Part or Open Assembly. Then, in the model document, make the desired configuration active.
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You cannot change the referenced configuration of a suppressed component, because suppressed components are removed from memory. However, if you open the document of a suppressed component and change the configuration, the newly selected configuration is used if you restore the component to the resolved state. The words, "in-use" are displayed next to the component name in the FeatureManager design tree if a component is "in-use." o
Use named configuration To always use a specific configuration regardless of the configuration currently in memory, select this option and choose a configuration from the list. It is good design practice to use named configurations when components have multiple configurations, to prevent the in-use configuration from affecting the assembly in unexpected ways.
o
Use same configuration as pattern seed component If the selected component is an instance of a component pattern, this is the default setting. To specify a configuration that is different from the seed component, select Use named configuration, and choose a configuration from the list.
•
Change properties in. Allows you to set properties in This Configuration, All Configurations, or Specify Configuration(s). The Change properties in list is only available in assemblies with more than one configuration.
3.
•
Suppression state. Controls the suppression state of the component.
•
Solve as. Sets the component as Rigid or Flexible.
•
Exclude from bill of materials. Omits this component from the bill of materials.
Click OK. If you selected Specify Configuration(s) for Change properties in, a dialog box appears for you to select the desired configurations.
If the selected component is a component of a sub-assembly, you can do the following:
1.
2.
Under Visibility, choose which visibility properties to use: •
Use visibility properties specified in configuration
•
Override visibility properties specified in configuration
Under Solve as, select Rigid or Flexible.
Deleting a Configuration You can delete a configuration with either of the following methods: •
Manually
•
Within a design table
NOTE: Deleting a configuration does not delete any features or components. To delete a configuration manually:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
Right-click the name of the configuration you want to delete, and select Delete. You are asked to confirm the deletion of the configuration.
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3.
Click Yes. The selected configuration is deleted.
To delete a configuration within a design table:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
In the FeatureManager design tree, right-click Design Table and select Edit Table or Edit Table in New Window. The worksheet appears in the window. (If you select Edit Table in New Window, the worksheet opens in a separate Excel window.)
3.
Click the numbered cell beside the configuration name that you want to delete (this selects the whole row), then click Edit, Delete. You can also right-click the numbered cell, and select Delete. NOTE: Do not press the Delete key to delete the row. Pressing Delete clears the contents of the cells and leaves an empty row. Any rows below an empty row are ignored.
4.
When you click outside the table, the table is evaluated, and you are asked to confirm the deletion of the configuration.
5.
Click Yes. The selected configuration is deleted.
Design Table Configurations Creating a Design Table To create a design table, you define the names of the configurations you want to create, you specify the parameters you want to control, and you assign values for each parameter. There are several ways to create a design table: •
Insert a new, empty design table in the model, and enter the design table information directly in the worksheet. When you finish entering the design table information, the new configurations are automatically created in the model.
•
Have the SolidWorks software automatically create the design table. SolidWorks loads all configured parameters and their associated values from a part or assembly.
•
Create a design table worksheet as a separate operation in Microsoft Excel. Save the worksheet, then insert it in the model document to create the configurations.
You can insert a partially completed worksheet, then edit it later to add more configurations, to control additional parameters, or to update values. When you use design tables in the SolidWorks software, it is important to format the tables properly.
Creating a Design Table as a Separate Excel File You can create a design table as a separate Excel file, then use the Design Table PropertyManager to insert the file in your model. NOTES:
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•
When you use design tables in the SolidWorks software, it is important to format the tables properly.
•
If you copy and paste the contents of a design table to a new worksheet in Microsoft Excel, follow the instructions below.
To create a design table as a separate Excel file:
1.
Open Microsoft Excel and create a worksheet.
2.
In the first column (row header cells A2, A3, and so on), type the names of the configurations that you want to create. Leave cell A1 blank. The names can include numerics, but must not include the forward slash (/) or at (@) characters.
3.
In the first row, (column header cells B1, C1, and so on), type the parameters that you want to control. Column headers are not case sensitive.
4.
Type the parameter values in the spreadsheet cells.
5.
Save the worksheet.
6.
Open the model document where you want to insert the design table.
7.
Click Insert, Design Table.
8.
In the Design Table PropertyManager, under Source: a.
Click From file.
b.
Click Browse and open the Excel file. You can also select Link to file, which links the table to the model. A linked design table reads all of its information from an external Excel file. When a design table is linked, any changes you make to the table outside of SolidWorks are reflected in the table within the SolidWorks model, and vice versa. The path to the Excel file appears above the Browse button. If you update a linked design table in Microsoft Excel, then open the SolidWorks model, you can choose to update either: the model with the design table values
o
- or the design table with the model values
o
You can set the update options in Tools, Options, System Options, External References. Set Update out-of-date linked design tables to to Model or Excel File. 9.
Click OK
.
The worksheet appears in the model document, and the Excel menus and toolbars replace the SolidWorks menus and toolbars. 10. Edit the design table if necessary. When you finish editing, click anywhere outside the table to close it. A message indicates the names of any new configurations that were generated by the design table, and the SolidWorks menus and toolbars reappear. The Design Table icon
appears in the FeatureManager design tree.
To display the configurations added by the design table, click the Configuration tab at the bottom of the window. Double-click the configuration name, or right-click the configuration name and select Show Configuration.
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Inserting a Design Table A design table allows you to build multiple configurations of parts or assemblies by specifying parameters in an embedded Microsoft Excel worksheet. NOTES: •
When you use design tables in the SolidWorks software, it is important to format the tables properly.
•
To use design tables, it is strongly recommended that you have Microsoft Excel 97 or later installed on your computer.
There are several different ways to insert a design table. Click one of the following for instructions on how to insert a design table: To have the SolidWorks software insert a design table automatically:
1.
In a part or assembly document, click Design Table Table.
on the Tools toolbar, or click Insert, Design
2.
In the PropertyManager, under Source, select Auto-create.
3.
Set the Edit Control settings and Options, as desired.
4.
Click OK
.
Depending on the settings you selected, a dialog box may appear that asks which dimensions or parameters you want to add. An embedded worksheet appears in the window, and the SolidWorks toolbars are replaced with Excel toolbars. Cell A1 identifies the worksheet as Design Table for: <model_name>. 5.
Click anywhere outside of the worksheet (but in the graphics area) to close the design table.
To insert a blank design table:
1.
In a part or assembly document, click Design Table Table.
2.
In the PropertyManager, under Source, click Blank.
3.
Set the Edit Control settings and Options, as desired.
4.
Click OK
on the Tools toolbar, or click Insert, Design
.
Depending on the settings you selected, a dialog box may appear that asks which dimensions or parameters you want to add. An embedded worksheet appears in the window, and the SolidWorks toolbars are replaced with Excel toolbars. 5.
Cell A1 identifies the worksheet as Design Table for: <model_name>. Cell A3 contains the default name for the first new configuration, First Instance.
6.
In row 2, type the parameters that you want to control. Leave cell A2 blank. Notice that cell B2 is active. You can also enter parameters by double-clicking the feature or dimension in the graphics area or in the FeatureManager design tree. When you double-click a feature or dimension, its associated value appears in the First Instance row.
7.
In column A (cells A3, A4, and so on), type the names of the configurations that you want to create. The names can include numerics, but must not include the forward slash (/) or at (@) characters. You can change the configuration name in cell A3 (First Instance) if you want.
10-16
8.
Type the parameter values in the worksheet cells.
9.
When you finish adding information to the worksheet, click outside the table to close it. A message lists the configurations that were created.
10. Click OK. The design table is inserted in the model, and Design Table
appears in the FeatureManager design tree.
To insert an external Microsoft Excel file as a design table:
1.
In a part or assembly document, click Design Table Table.
on the Tools toolbar, or click Insert, Design
The Design Table PropertyManager appears. 2.
Under Source: •
Click From file, then click Browse to locate the Excel file.
•
To link the design table to the model, select the Link to file check box. A linked design table reads all of its information from an external Excel file.
NOTE: If you update a linked design table in Microsoft Excel, then open the SolidWorks model, you can choose to update either: o
the model with the design table values - or -
o
the design table with the model values
You can set the update options in Tools, Options, System Options, External References. Set Update out-of-date linked design tables to to Model, Excel file, or Prompt. 3.
Set the Edit Control settings and Options, as desired.
4.
Click OK
.
An embedded worksheet appears in the window, and the SolidWorks toolbars are replaced with Excel toolbars. 5.
Click anywhere outside of the worksheet (but in the graphics area) to close the design table.
Design Table PropertyManager Use the Design Table PropertyManager to select design table settings when you insert a design table. Source •
Blank. Inserts a blank design table where you fill in the parameters.
•
Auto-create. Automatically creates a new design table, and loads all configured parameters and their associated values from a part or assembly.
•
From file. References a Microsoft Excel table. Click Browse to locate the table. You can also select the Link to file check box, which links the table to the model. When a design table is linked, any changes you make to the table outside of SolidWorks are reflected in the table within the SolidWorks model, and vice versa.
Edit Control •
Allow model edits to update the design table. If you change the model, the changes are updated in the design table.
•
Block model edits that would update the design table. You are not allowed to change the model, if these changes would update the design table.
NOTE: When you click a setting under Edit Control, you set the level of bi-directional control on the design table.
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Options Add new rows/columns in the design table for: •
New parameters. Adds new rows and columns to the design table if you add a new parameter to the model.
•
New configurations. Adds new rows and columns to the design table if you add a new configuration to the model. Warn when updating design table. Warns you that the design table will change based on the parameters you updated in the model.
•
Add Rows and Columns You made a change to the model, and the SolidWorks software wants to know if you want to add the new configurations or parameters to the design table. NOTE: The Add Rows and Columns dialog box appears because when you created the design table for this model, you selected New parameters or New configurations in the Design Table PropertyManager. To add rows and columns to the design table:
1.
In the Add Rows and Columns dialog box, select the configurations and parameters you want to add from the Configurations and Parameters boxes. NOTE: To select multiple features, hold down Ctrl as you select.
2.
If you do not select certain items in the Configurations and Parameters boxes, select the Show unselected items again check box to see these items next time this dialog box opens.
3.
Click OK. The selected items are added to the design table.
Creating Configurations with a Design Table A design table allows you to build multiple configurations of parts or assemblies by specifying parameters in an embedded Microsoft Excel worksheet. The design table is saved in the model document and is not linked to the original Excel file. Changes you make in the model are not reflected in the original Excel file. However, you can link the model document to the Excel file if you wish. To use design tables, it is strongly recommended that you have Microsoft Excel 97 or later installed on your computer. Parts. You can control the following items in a part design table: •
dimensions and suppression state of features
•
configuration properties, including part number in a bill of materials, derived configurations, equations, sketch relations, comments, and custom properties
Assemblies. You can control the following parameters in an assembly design table:
10-18
•
components - suppression state, visibility, referenced configuration
•
assembly features - dimensions, suppression state
•
mates - dimensions of distance and angle mates, suppression state
•
configuration properties - part number and display in a bill of materials (when used as a sub-assembly), derived configurations, equations, sketch relations, comments, custom properties
Formatting a Design Table When you use design tables in the SolidWorks software, it is important to format the tables properly. This topic shows how to format a design table with: •
Automatically created design tables
•
Manually created design tables
•
Blank rows and columns
•
Invalid criteria
Automatically Created Design Tables When you select Auto-create or Blank in the Design Table PropertyManager, the SolidWorks software automatically creates the Excel file. Automatically created design tables include the Family cell. By default, cell A2 is reserved as the Family cell. This cell determines where the parameter and configuration data begins. The Family cell contains no text, however, in Excel, the Name Box displays Family.
When you edit a design table, you can create rows above and columns to the left of the Family cell. The example below is a valid design table as long as configuration names and SolidWorks parameters are kept below and to the left of the Family cell.
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Manually Created Design Tables When you select From file in the Design Table PropertyManager, you insert a design table by browsing to the location of the Excel file. When you manually create a design table, you type configuration names in the first column (row header cells A2, A3, and so on), and you type parameters in the first row (column header cells B1, B2, and so on). Cell A1 must be blank. The example below is a valid design table as long as cell A1 is blank.
Design Tables With Blank Rows and Columns When the SolidWorks software processes a design table, it processes each configuration in the column with configuration names (top to bottom), then processes each parameter in the parameter row (left to right). If the sofware encounters a: •
blank cell in the parameter row, it goes to the next configuration name and applies the associated parameters
•
blank cell in the configuration name column, it stops processing because it assumes the design table has ended
In the example below, only the Default configuration is processed by the software. Because row 4 is blank, configurations C1 and C2 are not processed.
Invalid Criteria The SolidWorks software stops processing a design table if it reaches invalid parameters in a cell. A summary of design table parameters is available. If you enter information to the left of the parameters row or below the configuration name column, the SolidWorks software warns of an invalid value, and stops processing the design table without completing the remaining rows and columns. If this happens, some configurations will not update properly.
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Manually Add Parameters in a Design Table When you use design tables in the SolidWorks software, it is important to format the tables properly. To manually add certain types of parameters in a design table, with the appropriate worksheet cell active: •
Dimensions. Double-click a dimension in the graphics area. (Make sure that the necessary dimensions are displayed before you insert the new design table.) The Dimension@Feature or Dimension@Sketch parameter is inserted in the cell.
•
Feature suppression. Double-click a face of the feature. The $STATE@Feature parameter is inserted in the cell.
•
Component suppression. Double-click a face of the component. The $STATE@component
As you continue to add parameters this way, the adjacent cell (C2, D2, and so on) is activated automatically. Each parameter is added to the header row, and the current value is displayed in row 3. Column headers are not case sensitive.
Numerical Configuration Name If a configuration name in a design table contains only numbers, Excel interprets the name as a numeric value, instead of text. This is not a problem, except in the following cases: •
If the value begins with zeroes, the leading zeroes are removed.
•
If the value is more than 12 characters long, it is displayed in scientific notation.
To correct the problem, right-click the header cell for column A (to select the whole column), and select Format Cells. On the Number tab, under Category, select Text.
Editing a Design Table When you use design tables in the SolidWorks software, it is important to format the tables properly. 1.
In the FeatureManager design tree, right-click Design Table and select Edit Table or Edit Table in New Window. The worksheet appears in the window. (If you select Edit Table in New Window, the worksheet opens in a separate Excel window.)
2.
Edit the table as needed. You can change the parameter values in the cells, add rows for additional configurations, or add columns to control additional parameters. Since design tables appear in drawings, you may wish to change their appearance while editing them in the model documents. You can edit the format of the cells, using the Excel functions to modify fonts, alignment, borders, and so on.
3.
Click outside of the table to close it. (If you are working with the design table in a separate window, click File, Close.)
4.
If you receive a confirmation message that the design table generated new configurations, click OK. The configurations update to reflect your changes.
Deleting a Design Table 1.
Right-click Design Table in the FeatureManager design tree and select Delete.
2.
Click Yes to confirm the deletion.
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Saving Design Tables You can save design tables directly in the SolidWorks software. To save a design table:
1.
In a document with a design table, select Design Table File, Save As.
in the FeatureManager design tree, then click
- or Right-click Design Table in the FeatureManager design tree and select Save Table. The Save Design Table dialog box appears. 2.
Type a File name, then click Save. The design table is saved as an Excel file (*.xls).
NOTE: Due to a Microsoft limitation, changes to linked design tables may not be saved if they contain values that are linked to other spreadsheets. To save the design table, you can: •
Remove the linked values from the design table
•
Clear Link to file in the Design Table PropertyManager to unlink the design table from the model
Deleting a Configuration You can delete a configuration with either of the following methods: •
Manually
•
Within a design table
NOTE: Deleting a configuration does not delete any features or components. To delete a configuration manually:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
Right-click the name of the configuration you want to delete, and select Delete. You are asked to confirm the deletion of the configuration.
3.
Click Yes. The selected configuration is deleted.
To delete a configuration within a design table:
1.
In the ConfigurationManager, activate a configuration that you want to keep. The configuration that you want to delete must not be active.
2.
In the FeatureManager design tree, right-click Design Table and select Edit Table or Edit Table in New Window. The worksheet appears in the window. (If you select Edit Table in New Window, the worksheet opens in a separate Excel window.)
3.
Click the numbered cell beside the configuration name that you want to delete (this selects the whole row), then click Edit, Delete. You can also right-click the numbered cell, and select Delete. NOTE: Do not press the Delete key to delete the row. Pressing Delete clears the contents of the cells and leaves an empty row. Any rows below an empty row are ignored.
4.
When you click outside the table, the table is evaluated, and you are asked to confirm the deletion of the configuration.
5.
Click Yes. The selected configuration is deleted.
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Specifying Design Table Parameters Specifying Design Table Parameters When used in a design table, the names of dimensions, features, components, and configurations must match the name in the model. To ensure an exact match, you can copy and paste the name from the Properties dialog box for the selected item. You can use multiple languages in a design table. However, the language for the value in a table body cell must be in the same language as the parameter in the corresponding column header. For example, if the parameter in the column header is in English, then the corresponding value in the table body cell must also be in English. The next column header can be in another language, such as Japanese, but its corresponding value in the table body cell must also be in Japanese. NOTES: • When you use design tables in the SolidWorks software, it is important to format the tables properly. •
If the design table has been saved in English and then opened in Japanese, only English and Japanese will work. You cannot add another language, such as Polish, unless you use a Polish version of SolidWorks, or you have previously opened, closed, or saved the design table in a Polish version of SolidWorks.
•
Design tables used in versions prior to SolidWorks 2003 do not support multiple languages.
To copy and paste a dimension, feature, component, or configuration name:
1.
Right-click the item (dimension, feature, or configuration), and select Properties. For a component, select Component Properties from the shortcut menu.
2.
In the dialog box, copy (Ctrl+C) the item name (for dimensions and components, be sure to copy the Full name).
3.
Paste (Ctrl+V) the name into the appropriate column header cell.
Parameter specifications: •
Some parameter specifications that appear in the column header cells include a keyword, such as $CONFIGURATION, or $COMMENT. The parameter keywords are not case-sensitive.
•
Some parameters (suppression state, visibility, or referenced configuration of a component) also include a component name and instance number. These parameters use this syntax: $KEYWORD@component
Multiple instances: You can specify multiple instances of a component in a single column header cell. Use the following syntax for the instance numbers: •
<*> all instances
•
<1-4> range of instances
•
<1,3,6> non-consecutive instances, separated by commas
•
<1,3-6,8> combination, separated by commas
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Example: This is an example of a design table that creates three configurations, adds a comment for each one, suppresses a feature, and controls a dimension.
Do not include any rows or columns with blank headers in the middle of the design table. The SolidWorks software stops evaluating the data when it reaches a row or column that has an empty header cell. Data that appears in or after a row or column with an empty header is ignored. Summary of Design Table Parameters
NOTES: •
When you use design tables in the SolidWorks software, it is important to format the tables properly.
•
The parameter syntax (header cells) are not case sensitive. Parameter Syntax (header cell)
Legal Values (body cell)
Default if Value is Left Blank
$configuration@part_name
configuration name
not evaluated
$configuration@
configuration name
not evaluated
$comment
any text string
empty
$partnumber
any text string
configuration name
$state@feature_name
Suppressed, S Unsuppressed, U
Unsuppressed
dimension@feature
any legal decimal value for the dimension
not evaluated
$parent
parent configuration name
property is undefined
$prp@property
any text string
property is undefined
$state@equation_number@equations
Suppressed, S Unsuppressed, U
Unsuppressed
$state@lighting_name
Suppressed, S Unsuppressed, U
Unsuppressed
$state@sketch relation@sketch name
Suppressed, S Unsuppressed, U
Unsuppressed
$user_notes
any text string
not evaluated
$color
32-bit integer specifying RGB (red, green, blue) color
zero (black)
Yes, Y No, N
No
Parts only
Parts and Assemblies
Assemblies only $show@component
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$state@component
Resolved, R, Suppressed, S
Resolved
$configuration@component
configuration name
Component's "in-use" or last saved configuration NOTE: If the component uses a derived configuration, and the value is left blank, the configuration used is linked to its parent.
$never_expand_in_BOM
Yes (never expand) No (allow to expand)
No
Dimensions in Design Tables Design tables can control dimensions as follows: •
In a part document, you can use a design table to control the dimensions in sketches and in feature definitions.
•
In an assembly document, you can control dimensions that belong to assembly features. This includes mates (angle or distance), assembly feature cuts and holes, and component patterns (spacing or instance count). You cannot control the dimensions of a component contained in the assembly.
The column header in a design table for controlling dimensions uses this syntax: Dimension@Feature or Dimension@Sketch
When you specify values, be sure to use the system of units specified for the model document (click Tools, Options, Document Properties, Units).
•
You can display dimensions that are driven by design tables in a different color. Click Tools, Options, System Options, Colors. Select Dimension, Controlled by Design Table in System colors and change the color.
Example of a design table that controls feature dimensions:
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Chapter 10 Configurations
Dimensions The Dimensions dialog box appears after you select the Auto-create option in the Design Table PropertyManager and click OK
. The SolidWorks software asks you which dimensions you want to add to the design table.
NOTE: The Dimensions dialog box appears if the model has only one configuration. To add dimensions to the design table:
In the Dimensions dialog box, select the dimensions you want to add to the design table (hold down Ctrl to select more than one dimension), then click OK. Component Configuration The column header in a design table to control component configuration uses this syntax: $CONFIGURATION@component
Component Visibility The column header in a design table for controlling component visibility uses this syntax: $SHOW@component
10-26
Example of a design table that controls component visibility:
Component Suppression State The column header in a design table to control the suppression state of a component uses this syntax: $STATE@component
Suppression of Features In a part document, you can suppress any feature. In an assembly document, you can suppress features that belong to the assembly. These include mates, assembly feature holes and cuts, and component patterns. Sketches and reference geometry may also belong to an assembly. You cannot control the suppression of a feature that belongs to an individual assembly component. In a design table, there are two ways to specify the suppression of features. •
Method 1 (recommended). The column header for controlling feature suppression uses this syntax: $STATE@feature where feature is the name of the feature. For example, the column labeled $STATE@Hole1 controls the suppression of the first hole. In the table body cells, type the value for the desired suppression: Suppressed (or S), Unsuppressed (or U). If a cell is left blank, the default is Unsuppressed.
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•
Method 2. Type only the feature name in the column header cell. To suppress the feature, leave the table body cell blank. To include the feature, type any string in the body cell. This is the syntax that was used in SolidWorks 98 and earlier versions, and is included for backward compatibility.
You can also suppress individual features with the shortcut menu. To suppress individual features with the shortcut menu:
1.
Right-click the feature you want to suppress in the FeatureManager design tree and select Properties.
2.
In the dialog box:
3.
•
Select Suppressed.
•
Select This Configuration, All Configurations, or Specify Configuration(s).
Click OK.
Base Parts You can control the configuration of a base part with a design table. This is available in part documents only. The column header in a design table for controlling base part configurations uses this syntax: $CONFIGURATION@<part name> where <part name> is the name of the base part. The column header is not case sensitive. In the table body cells, type the base part's configuration names. For example, to use the default configuration of a base part named washer.sldprt, the column heading syntax is $CONFIGURATION@washer. The table body cell value is Default. Example of a design table that controls a base part configuration:
Component Part Number When you create configurations with a design table, the software automatically sets options in the Configuration Properties dialog box. Under Part number displayed when used in a bill of materials, the Configuration Name is selected. A bill of materials for an assembly that contains the document lists the part configuration name in the PART NO. column. In a design table, the $PARTNUMBER parameter lets you specify a different value for the PART NO. column of the BOM. For an assembly document, this is the part number used when this configuration of the assembly appears in the BOM as a sub-assembly. The column header uses this syntax:
10-28
$PARTNUMBER The column header is not case sensitive. In the table body cells, type the part number for each configuration. The $PARTNUMBER parameter now includes the document name or the parent name (derived configurations only) in a bill of materials. The following table shows values that can be used with this parameter: Value
Property Used
$DOCUMENT
Document name
$PARENT
Parent configuration name
$CONFIGURATION
Configuration name
any text
Custom name
blank
Configuration name
If multiple configurations of the same document are used in an assembly, the BOM lists each configuration by name as a separate item number. If you do not want each configuration listed separately in the BOM, do one of the following: •
Assign the same value for the $PARTNUMBER parameter in all the configurations.
•
After the design table creates all of the configurations, edit the properties of each configuration, and select Document Name. To override the document name, you can use the Title specified under File, Properties for the component document.
Example of a design table that controls the value of a part number in a BOM with custom names:
Comment The Configuration Properties dialog box has a Comment box, where you can enter a description, or other additional information about the configuration. In a design table, the column header for entering information in this box for each configuration uses this syntax: $COMMENT The column header is not case sensitive. In the table body cells, enter the comments for the configuration. Comments are optional; if a cell is left blank, the Comment box is empty.
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Example of a design table with a comment parameter:
Equations in Configurations You can suppress or unsuppress equations in specified configurations. To suppress or unsuppress equations in specified configurations:
1.
Click Tools, Equations.
2.
In the dialog box, under the Active column, select or clear the check boxes next to the equations you want to unsuppress or suppress. When you clear a check box, you suppress the configuration.
3.
Click Configs.
4.
In the dialog box, select the configurations to which you want the equation to apply: This configuration, All configurations, or Specify configurations.
5.
Click OK.
6.
Click OK again to close the Equations dialog box.
7.
Click Rebuild
.
The equation is applied to the selected configurations. To suppress or unsuppress equations in a design table:
The column header in a design table for controlling equations uses this syntax: $STATE@equation_number@EQUATIONS The column header is not case sensitive. In the table body cells, type S for suppressed or U for unsuppressed. Example of a design table that controls the suppression state an equation:
10-30
Expand in BOM You can control how the assembly is listed in a BOM, when this configuration is used as a sub-assembly. The column header in the design table uses this syntax: $NEVER_EXPAND_IN_BOM This corresponds to the Don’t show child components in BOM when used as sub-assembly option in the Configuration Properties dialog box. The column header is not case sensitive. •
When turned off, the sub-assembly is expanded if you select either Parts only or Indented assemblies when you insert the BOM.
•
When turned on, the sub-assembly is never expanded, regardless of the option you select when you insert the BOM. The effect is the same as selecting Top level only.
In the table body cells, to turn on the option (never expand) type Yes (or Y). To turn off the option (allow to expand), type No (or N). If a cell is left blank, the default is No. Example of a design table that controls how the assembly is listed in a BOM:
Lighting in Design Tables Lights in the Lighting
folder can be suppressed in a design table.
The column header in a design table for controlling lights uses this syntax: $STATE@
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Chapter 10 Configurations
Split Parts You can control the configuration of a split part with a design table. This is available in part documents only. The column header in a design table for controlling split part configurations uses this syntax: $CONFIGURATION@
Custom Properties The column header in a design table to specify a custom property uses this syntax: $PRP@property where property is the name of a custom property. You can use one of the custom properties listed in the Summary Information dialog box (click File, Properties, Configuration Specific), or you can add a new custom property. NOTES: •
The column header is not case sensitive.
•
If you plan to use the custom properties as columns in the bill of materials, do not use property names that contain spaces.
For example, use the header $prp@Cost to control the custom property Cost for each configuration. In the table body cells, type the property value for each configuration. If a cell is blank, the property is undefined for the configuration. Properties that are associated with model parameters (dimensions and mass properties) update automatically when the model parameters change. To add a custom property to a design table:
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1.
Insert a design table into your model.
2.
In the design table spreadsheet: a.
For each column with a custom property, label the column in the form $prp@property; for example, $prp@length.
b.
In each column, type in the variable name of the property in the form "name@@configuration@model"; for example, "D2@Sketch1@@[email protected]".
Include the quotation marks and be sure the file name extension (.SLDPRT) is uppercase. c. 3.
In new columns, add the standard design table information, for example, D2@Sketch1 as the header, and dimension values in the column.
Click outside the design table to close it. Custom properties added in a design table appear automatically on the Configuration Specific tab of the Summary Information dialog box. You can use these properties in Notes and Bills of Materials. Example of a design table that specifies custom properties:
User Notes The design table can include additional columns or rows for information only (notes, intermediate calculations, and so on). Use the keyword $USER_NOTES in the header of any column or row that you do not want evaluated. You may use as many of these rows or columns as you need. However, you may not include rows or columns with empty headers in the middle of the table. The column header is not case sensitive. Example of a design table that uses notes:
Color Parameter The design table can include a column for configuration-specific colors. The value is a 32-bit integer that specifies RGB (red, green, blue). If no value is specified, zero (black) is used. If you know the 32-bit integer value of a color, you can type the number directly into the design table in a column with the $COLOR parameter as the header. If you do not know the 32-bit integer value, you can calculate it in the design table with the RGB component values. To determine the red, green, and blue components of a color:
1.
Click Edit Color on the Standard toolbar.
2.
In the PropertyManager, under Color Properties: a.
Click a color in Pick a Color palette.
b.
Select RGB.
c.
Select Numeric.
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d.
Note the component numbers next to Red Component of Color , and Blue Component of Color
3.
Click OK
, Green Component of Color
.
.
To calculate a color value in a design table:
1.
Click Insert, Design Table.
2.
In the Design Table PropertyManager, choose the design table settings, then click, choose the design table settings, then click OK
3.
.
In the design table: a.
Type $USER_NOTES in cells B2, C2, and D2, and type $COLOR in cell E2. The column header is not case sensitive. You may have to insert columns so that these parameters appear in cells B2 through E2.
b.
Type integers in cells B3, C3, and D3 for the red, green, and blue components of a color.
c.
Type the following formula in cell E3: = MAX(MIN(B3,255),0) + MAX(MIN(C3,255),0)*16*16 + MAX(MIN(D3,255),0) *16*16*16*16 The formula ensures that each component value is between zero and 255. Make sure there are no extra spaces before the = sign in the cell.
d.
Type other color components in the appropriate rows and copy the formula, adjusted for the row number, into the corresponding cells in column E.
The following table lists some typical colors, their components, and the equivalent integer values. Color
Red
Green
Blue
Integer
Black
0
0
0
0
Red
255
0
0
255
Orange
255
128
0
33023
Green
0
255
0
65280
Blue
0
0
255
16711680
Purple
255
128
255
16744703
Turquoise
0
255
255
16776960
White
255
255
255
16777215
If the color for wireframe and HLR modes is the same as the color for shaded mode, the configuration-specific color applies to all three modes. If the color is not the same for all three modes, then the configuration-specific color applies to shaded mode only. To set the color the same for wireframe, HLR, and shaded modes:
10-34
1.
Click Tools, Options, Document Properties, Colors.
2.
Select Apply same color to wireframe, HLR and shaded.
3.
Click OK.
Design Tables in Drawings Design Tables in Drawings If a model document uses a design table to generate multiple configurations, you can display the table in a drawing of that model. This way, a single drawing can represent all the configurations. You can label the dimensions with letters or short, descriptive names, instead of using the full dimension names and the values. For example, instead of D1@BaseExtrude, you can use a label such as A or thickness as the column header in the table, and display the label instead of the value of the dimension in the drawing view. Displaying a Design Table in a Drawing 1.
2.
In the part or assembly document, edit the design table as needed. The design table is displayed in the drawing exactly as it appears in the model document. •
Drag the resize handles on the corners and sides of the table to adjust the boundaries of the table. Make sure that all the rows and columns that you want are displayed, and remove any empty rows or columns.
•
Hide any rows (or columns) in the middle of the table that you do not want to display in the drawing. Right-click the numbered cell at the left of the row (or the lettered cell at the top of the column) to select the whole row (or column), and select Hide.
•
Adjust the column width, row height, text alignment, borders, fonts, and so on, as needed to meet your company standards.
If you want to use labels (letters or names) for the dimensions: a.
Insert a new row between the header row (the row containing the full dimension names) and the row for the first configuration.
b.
In the new row, type a label for each dimension.
c.
Hide the header row as described in step 1.
3.
In a drawing of the part or assembly, select a drawing view.
4.
Click Insert, Tables, Design Table. The design table appears, and you can drag it into place on the sheet.
5.
If you need to change the size of the design table, right-click the table, and select Properties.
6.
In the dialog box, specify a value for Width or Height, or type a Scale value, then click OK. To restore the table to its original size, right-click the table, and select Reset Size.
7.
If you are using labels, modify the dimensions in the drawing view: a.
Right-click a dimension, and select Properties.
b.
In the dialog box, click Modify Text.
c.
Delete
d.
Click OK.
e.
Click OK again to close the Dimension Properties dialog box.
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Chapter 10 Configurations
Design Table in a Drawing The following illustrates how a design table and the dimensions it controls might appear in a drawing.
Editing a Design Table in a Drawing
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1.
Double-click the design table in the drawing. The model opens in its own window, and the design table opens for editing.
2.
Modify the table as needed. When you are done, click outside of the table to close it.
3.
Return to the drawing window, and click Rebuild
to see the updated table.
11 Drawings
Drawings Overview You can create 2D drawings of the 3D solid parts and assemblies you design. Parts, assemblies, and drawings are linked documents; any changes that you make to the part or assembly change the drawing document. One-way associativity can be set between drawings and models during the software installation. This prevents changes to model dimensions, thereby preventing changes to the model itself from within a drawing. This option can be reset only with a new installation of the software. Generally, a drawing consists of several views generated from the model. Views can also be created from existing views. For example, a section view is created from an existing drawing view. When you select a view on a drawing sheet, the view name appears in the PropertyManager title. You can open existing drawings from inside part and assembly documents. Right-click the top item in the FeatureManager design tree or anywhere on the model in the graphics area and select Open Drawing. SolidWorks looks for a drawing with the same name as the model, in the same folder as the model. If the drawing exists, it opens automatically. If such a drawing is not found, a browse window appears so you can locate a drawing manually. To replace components in assembly drawings, use File, Open and click References. Edit the references in the Edit Referenced File Locations dialog box. When you open a drawing of a large assembly, you are prompted with the option to open the drawing in Large Assembly Mode. When you save or close a drawing without all the sheets loaded into memory, you are prompted to update the drawing. If you choose to update, all drawing views on all sheets are updated. The prompt appears only once per drawing document per SolidWorks session. If you choose not to update, the views on sheets that were not loaded do not appear in the SolidWorks view-only mode or in the SolidWorks Viewer. Topics about drawings include: •
Setting options
•
Creating a Drawing
•
Customizing Sheet Formats
•
2D sketching in drawings
•
Drawing Documents
•
Creating standard views (model views and standard 3 views)
•
Creating derived views, such as detail, section, projected, broken, and so on
•
Aligning and displaying views
•
Printing and sending drawings
Dimensions, notes, datums, geometric tolerances, and other annotations are discussed in Detailing.
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Chapter 11 Drawings
Getting Started in Drawings Setting Options for Drawing Documents A variety of options customize drawings to your company’s standards and to the requirements of your printer or plotter. System drawing options Click Tools, Options, System Options, Drawings. Specify various display and update options for views. The settings on the System Options tab apply to all documents. Other system options for drawings are found under the following topics: •
Display Style. Drawing view display mode and tangent edge display.
•
Area Hatch/Fill. Hatch or solid fill, pattern, scale, and angle of area hatches.
•
Large Assembly Mode. Default settings for performance of drawings of large assemblies.
Document-specific detailing options Click Tools, Options. On the Document Properties tab, select Detailing. The settings on the Document Properties tab apply to the active document only. Other document properties for drawings are found under the following topics: •
Dimensions
•
Notes
•
Balloons
•
Arrows
•
Virtual Sharps
•
Annotations Display
•
Annotations Font
•
Tables
•
View Labels
Page Setup Set to meet your printer or plotter requirements. Click File, Page Setup to specify such properties as page margins and orientation, scale of printed drawing, and custom headers and footers. Drawing sheets You can customize the following properties of drawing sheets: •
Sheet Format. Customize information blocks and text.
•
Sheet Properties. Change the sheet size and orientation, sheet scale, and 1st or 3rd angle projection.
Templates Customize drawing templates to conform to the standards of your workplace. You can set drawing, detailing, and standards options in templates. You can also save drawing documents to be used as drawing templates. Tables (Bills of Materials, Hole Tables, Revision Tables, and Weldment Cut Lists) also use templates that you can customize and save.
11-2
Creating a Drawing Drawings consist of one or more views generated from a part or assembly. The part or assembly associated with the drawing must be saved before you can create the drawing. You can create a drawing from within a part or assembly document. Drawing files have the .slddrw extension. A new drawing takes the name of the first model inserted. The name appears in the title bar. When you save the drawing, the name of the model appears in the Save As dialog box as the default file name, with the default extension .slddrw. You can edit the name before saving the drawing. To create a drawing from within a part or assembly document:
1.
Click Make Drawing from Part/Assembly
on the Standard toolbar.
2.
Select a Sheet Format/Size, then click OK.
3.
Specify properties in the Model View PropertyManager, then place the view in the graphics area.
To create a new drawing:
1.
Click New
on the Standard toolbar, or click File, New.
2.
In the New SolidWorks Document dialog box, select Drawing
3.
Select a Sheet Format/Size, then click OK.
4.
In the Model View PropertyManager, select a model from Open documents or browse to a part or assembly file.
5.
Specify options in the PropertyManager, then place the view in the graphics area.
, then click OK.
Sheet Format/Size You select a sheet format when you open a new drawing. The standard sheet formats include links to system properties and custom properties. Sheet formats help create drawings with a uniform format. Drawing sheet formats are OLE documents in which you can embed objects such as bitmaps. To select a sheet format:
1.
Click New
2.
Select Drawing
3.
Select from the following, then click OK. •
•
on the Standard toolbar. , then click OK.
Standard sheet size. Select a standard sheet size, or click Browse and locate a custom sheet format file. o
Reload. If you make changes to the Sheet Format, click to return to the default format.
o
Display sheet format. Display border, title block, and so on.
Custom sheet size. Specify a Width and Height.
To select a different sheet format in an existing drawing document, right-click in the graphics area and select Properties. To save a sheet format, click File, Save Sheet Format.
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Chapter 11 Drawings
Sheet Properties You can set the sheet properties when you add a sheet to a drawing or modify existing sheet properties. To specify sheet properties:
1.
In the active drawing sheet, right-click the sheet icon in the FeatureManager design tree, or in any blank area of the drawing sheet, or on the sheet tab at the bottom of the drawing window, and select Properties. - or For a drawing sheet that is not active, right-click the sheet icon in the FeatureManager design tree, or on the sheet tab at the bottom of the drawing window, and select Properties. - or Right-click in any blank area of the drawing sheet, or on the sheet tab at the bottom of the drawing window, and select Add Sheet.
2.
Specify properties as described below and click OK.
Name. Enter a title in the box. Scale. Set a scale for the sheet. Type of projection. Select First angle or Third angle for Standard 3 View projection. Next view label. Specify the letter of the alphabet to be used for the next section and detail views. Next datum label. Specify the letter of the alphabet to be used for the next datum feature symbol. Sheet Format/Size •
•
Standard sheet size. Select a standard sheet size, or click Browse and locate a custom sheet format file. o
Reload. If you make changes to the Sheet Format, click to return to the default format.
o
Display sheet format. Display border, title block, and so on.
Custom sheet size. Specify a Width and Height.
Use custom property values from model shown in. If more than one model is shown on the sheet and the drawing contains notes that are linked to custom properties of a model, select the view thatcontains the model whose properties you want to use. If you do not specify otherwise, the properties of the model in the first view inserted into the sheet are used. See Linking Notes to Document Properties.
Multiple Drawing Sheets You can add sheets to the drawing at any time. To add a sheet:
1.
Click Insert, Sheet. You can also right-click any sheet tab or any sheet icon in the FeatureManager design tree, and select Add Sheet.
2.
The Sheet Properties dialog box appears, with the default name of the next new sheet in sequence, for example, Sheet2.
3.
Specify the sheet details as described in Sheet Properties, and click OK.
To view a different sheet:
•
Click the sheet tab of the desired sheet.
•
Right-click the sheet tab or the sheet icon in the FeatureManager design tree, and select Activate.
To delete a sheet:
1.
Right-click any sheet tab or any sheet icon in the FeatureManager design tree, and select Delete. You can also click anywhere in the graphics area and press Delete to delete the active sheet.
2.
11-4
Click Yes in the Confirm Delete dialog box.
Sheet Formats, Sheets, and Views Ownership of items in drawings is dependent on what is active when the item is created. Sketch entities, notes, and other items can belong to the drawing sheet, to an individual view, or to the drawing sheet format. In general, you must activate the owner of an item in order to edit the item. NOTE: Dimensions and annotations that are attached to model geometry are exceptions to this rule. They belong to the view where they are attached, regardless of whether the view is active when you create the item. For example, you can activate a view, and create a construction line that belongs to the view. If you move or delete the view, the construction line is moved or deleted also. To edit the construction line, you must activate the view again. You can create the same construction line on the sheet, when no view is active. However, if you move or delete the views on the sheet, the construction line is not affected. To edit the construction line, the sheet itself must be active. Similarly, you must activate the sheet format to edit any items that are owned by the sheet format. While the sheet format is active, the sheet is hidden, including all the items that belong to the sheet, and all the views.
Customizing Sheet Formats You can customize drawing sheet formats to match your company’s standard format. The sheet formats provided with the SolidWorks software do not conform to any standard. However, the following linked custom properties are automatically included in all the provided sheet formats and are populated if the information is in either the system properties or the custom properties of the drawing document. System properties are automatically available when you insert a note. You enter custom properties on the Summary Information - Custom tab for drawing, part, or assembly documents as appropriate. System properties linked to fields in the system sheet formats
SW-File Name (in DWG. NO. field) SW-Sheet Scale SW-Current Sheet SW-Total Sheets Custom properties of drawing documents linked to fields in the system sheet formats
CompanyName CheckedBy CheckedDate DrawnBy DrawnDate EngineeringApproval EngAppDate ManufacturingApproval MfgAppDate QAApproval QAAppDate Custom properties of parts or assemblies linked to fields in the system sheet formats
Description (in TITLE field) Weight Material Finish Revision To edit the drawing sheet format:
1.
Click Edit, Sheet Format, or right-click any blank area on the drawing sheet, or the sheet icon in the FeatureManager design tree, and select Edit Sheet Format. If the sheet does not already have a sheet format, you create one if you select Edit Sheet Format, then click Rebuild.
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Chapter 11 Drawings
2.
Edit the sheet format as described below.
3.
Click Edit, Sheet, or right-click any blank area on the drawing sheet, or the sheet icon in the FeatureManager design tree, and select Edit Sheet.
To edit existing text in the title blocks:
Double-click the text. You can edit the text in place, then click outside the text box to exit the edit mode. - or Right-click and select Properties. The Note PropertyManager appears. Change any items you wish, and click OK
.
To move, delete, or add lines or text:
•
To delete, click the line or text and press the Delete key.
•
To move, click the line or text and drag to a new location.
•
To add lines, click Line
•
To add text, click Note on the Annotations toolbar, or click Insert, Annotations, Note. Specify the text properties, then click to place the text in the desired location.
, or Tools, Sketch Entity, Line.
Table Anchor Points The standard sheet formats supplied with the software include anchor points for placing the tables in specific locations on the sheet. To set the anchor points, expand SheetFormats for the sheet in the FeatureManager design tree. Right-click one of the four anchors, select Set Anchor, then click where you want the anchor point on the sheet. When you set the anchor point from the FeatureManager design tree, you are automatically in Edit Sheet Format mode. When you are finished, right-click in the graphics area and select Edit Sheet. You can also right-click a sketch point in the sheet format, and select Set as Anchor, one of the four anchors. The anchor point is highlighted, and its visibility toggles when you click the icon. NOTE: You can add an anchor point to drawings that you created in versions earlier than SolidWorks 98Plus. Right-click the sheet, and select Edit Sheet Format. Then right-click a sketch point (add one if needed), and select Set as Anchor. If the sheet does not already have a sheet format, you create one when you perform this procedure. OLE Objects To add objects from other applications, such as bitmaps of your company logo, standard note text from a file, and so on, click Insert, Object. You can either create a new object or insert one from a file. Objects can be linked or embedded in drawing sheet files.
Saving Sheet Formats To save the sheet format:
1.
Click File, Save Sheet Format.
2.
Edit File name. You can overwrite standard formats or create custom formats. Sheet format files have extension .slddrt and are located in
3.
Click Save. Custom properties in the document are saved with the sheet format and added to any new documents that use the format.
11-6
Linking Notes to Document Properties To automatically insert information in a drawing, you can link note text in the drawing sheet or drawing sheet format to document properties. For the procedure to add a link in a note, see Link to Property. All SolidWorks documents have the following system-defined properties: Property Name
Value
SW-Author
Author field in Summary Information dialog box
SW-Comments
Comments field in Summary Information dialog box
SW-Configuration Name
Configuration name in ConfigurationManager of part or assembly
SW-Created Date *
Created field in Summary Information dialog box *
SW-File Name
document name, no extension
SW-Folder Name
document folder with backslash at the end
SW-Keywords
Keywords field in Summary Information dialog box
SW-Last Saved By
Last Saved By field in Summary Information dialog box
SW-Last Saved Date *
Last Saved field in Summary Information dialog box *
SW-Long Date *
current date in long format *
SW-Short Date *
current date in short format *
SW-Subject
Subject field in Summary Information dialog box
SW-Title
Title field in Summary Information dialog box
*The formats of the dates are language and region dependent. For details, see Start/Settings/Control Panel/ Regional Settings/Date on your computer. Additionally, drawings have the following system-defined properties: Property Name
Value
SW-Current Sheet
sheet number of the active sheet
SW-Sheet Format Size
sheet size of the active sheet format
SW-Sheet Name
name of the active sheet
SW-Sheet Scale
scale of the active sheet
SW-Template Size
template size of the drawing template
SW-Total Sheets
total number of sheets in the active drawing document
You can link a note to the properties of the model shown in the drawing (the SW-File Name property, for example, or a user-defined custom property in the model document). While you are editing the sheet format, a variable for the property name is displayed (in the form $PRP: "<property name>"). When you return to editing the sheet, the value of the property, if found, is displayed. If the property value cannot be found, the note displays ERROR!
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Chapter 11 Drawings
The Drawing Window The drawing window includes a FeatureManager design tree that is similar to the design tree in the part and assembly windows. The FeatureManager design tree for drawings consists of a hierarchical list of items pertaining to the drawing. There is an icon for each sheet; under each sheet, there are icons for the sheet format and each view. You can reorder sheets of drawing documents in the FeatureManager design tree. Drag one sheet at a time to the desired location. The sheet tabs are updated automatically. A symbol beside an item’s icon indicates that it contains associated items. Click the display its contents.
to expand the item and
Standard views contain the feature list for the part or assembly shown in the view. Generated views, such as detail or section views, contain different, view-specific items (detail circles, section lines, and so on). You can zoom to a view by right-clicking the view and selecting View, Zoom to Selection or right-clicking the view name in the FeatureManager design tree and clicking Zoom to Selection. You can zoom to the sheet by right-clicking the sheet name in the FeatureManager design tree and clicking Zoom to Selection. The drawing window has rulers at the top and left side. The rulers (and the status line) show the position of the pointer on the sheet. To turn the ruler display on or off, click View, Rulers. To specify the major and minor ruler line graduations, click Tools, Options, Document Properties, Grid/Snap. Specify the Major grid spacing and Minor-lines per major settings. Some types of views are linked to their parent views: Detail, Section, Auxiliary, and Projected Views, for example. Right-click on the detail circle or section line and select Jump to Detail View (or Section View). Right-click the child view and select Jump to Parent View. Projected Views (including the side and top views of Standard 3 Views) and Auxiliary Views have jumps only from the child to the parent.
Views of Parts and Assemblies You can generate drawings of a part or assembly in a variety of view types: Standard 3 View, Model, and Relative views. The part or assembly document must be saved before you can create drawing views of it. •
From existing views on the active sheet, you can create Projected, Auxiliary, Detail, Crop, Section, Aligned Section, Broken-out Section, or Broken views.
•
Explode lines in exploded views of assemblies are displayed in drawings of the exploded configurations.
•
You can also create an Empty view for sketching or annotations. For more information, see 2D Sketching.
For some operations, you need to select a view; for others, you activate a view. •
Selecting a view allows you to create a projected view, to insert break lines for a broken view, to move the view on the sheet, and to resize the view boundary. A selected view has a green border (blue in Detached drawings) with drag handles. To select a view, click an empty area within the view boundary.
•
Activating a view allows you to sketch entities in that view. This is necessary for sketching section lines, and for defining profiles for detail views. To edit the sketch entity, the view to which it belongs must be active. The border of an active view is a shadowed box.
You can set an option that causes drawing views to activate automatically when the pointer passes over them. Click Tools, Options, System Options, Drawings. Select or clear the Dynamic drawing view activation check box. •
When Dynamic drawing view activation is selected, the view closest to the pointer position is activated automatically. To stop the dynamic activation temporarily, you can lock the focus on a view or on the sheet. Right-click the view or the sheet, and select Lock View Focus or Lock Sheet Focus.
•
Lock View Focus allows you to add sketch entities to a view, even when the pointer is close to another view. You can be sure that the items you are adding belong to the view you want.
•
Lock Sheet Focus allows you to add sketch entities to the sheet. Otherwise, the sketch entities belong to the view that is closest to where you begin sketching. To return to dynamic activation mode, right-click again, and select Unlock View Focus (or double-click a different view) or Unlock Sheet Focus (or double-click any view).
11-8
•
When Dynamic drawing view activation is cleared, double-click anywhere within a view’s boundary to activate the view, or right-click within the boundary and select Activate View. To de-activate a view, either double-click again, activate a different view, or right-click and select Activate Sheet.
View Boundaries When the pointer passes over the edge of a drawing view, the view boundary is highlighted. The size of the view boundary is calculated automatically, based on the size, shape, and orientation of the model shown in the view. You can adjust the size of the view boundary (enlarging the view boundary may make it easier to select or activate a view). You cannot make the view boundary smaller than the model displayed in the view. View boundaries, and the views they contain, can overlap. To change the size of the view boundary:
1.
Select the view.
2.
Point to a green drag handle at the corner or side of the boundary.
3.
When the pointer changes to resize
, drag the handle as needed to resize the boundary.
To turn the boundary display on/off:
Click Tools, Options, System Options, Drawings. Select the Display drawing view borders check box. When selected, the boundary of each view is displayed as a thin gray box. When cleared, the boundaries are hidden. This option applies to all the views in the drawing. Even if the boundaries are hidden, they still are highlighted when the pointer passes over them, and an active view still displays a shadowed box. If the model contained in the view is not in the active or last-saved configuration, the border is dashed.
Scales in Drawings Scales in drawings apply to sheets or views. The scale for the active drawing sheet appears in the status line at the bottom of the window, and the scale for the active view appears in the view PropertyManager. You can also scale a drawing when you print it. Setting Scales To set the scale of a drawing sheet:
•
For an existing drawing sheet, right-click the sheet and select Properties. In the Sheet Properties dialog box, edit the values of Scale.
•
For a new drawing sheet, right-click an existing sheet or the sheet tab and select Add Sheet, or click Insert, Sheet. In the Sheet Properties dialog box, edit the values of Scale for the new sheet. The scale of the drawing sheet applies to: o
New and existing drawing views that are not set to custom scales
o
New views that are not autoscaled
The default drawing sheet scale is 1:1. To set the scale of a drawing view:
•
For existing drawing views, select a view or views. In the view PropertyManager, select Use parent scale or Use sheet scale, or select Use custom scale and edit the values.
•
For new drawing views where the PropertyManager appears during view insertion (such as Model, Projected, Predefined, and so on), select Use custom scale under Scale in the PropertyManager and edit the values.
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Chapter 11 Drawings
Autoscaling •
Automatically scale new drawing views in the Drawings Options controls the scaling of new views as follows: o
o
When selected, the SolidWorks software automatically scales the views to best fit on the drawing sheet, and the scale of the drawing sheet becomes the same as the scale of the views. When cleared, the views are inserted at the scale of the drawing sheet. When you insert Projected Views, Auxiliary Views and Section Views, the scale is set to Use parent scale. If you change the scale of a parent view, the scale of all child views that use the parent scale is updated.
•
If a drawing sheet contains multiple Predefined Views, the views are scaled automatically when a model is inserted. If a drawing sheet contains only one Predefined View, the view uses the Custom Scale, if specified, or (if no scale is specified) the drawing sheet scale.
Dimension Type Dimensions in drawings are either: •
True. Accurate model values.
•
Projected. 2D dimensions.
The dimension type is set when you insert a drawing view. You can view and change the dimension type in drawing view PropertyManagers. The rules for dimension type are: •
SolidWorks specifies Projected type dimensions for standard and custom orthogonal views and True type dimensions for isometric, dimetric, and trimetric views.
•
If you create a projected or auxiliary view from another view, the new view uses Projected type dimensions, even if the original view used True type dimensions.
•
When inserting views in other orientations, such as custom views that are not orthogonal, you are prompted for the dimension type.
•
The dimension type does not change if you change the orientation of a named view.
Crosshatch in Drawings Crosshatch is added to drawings of section views, including section views of multibody parts and weldments. You can add a crosshatch pattern to a model face or a closed sketch profile in drawings with area hatch/fill. To set options for crosshatch patterns, in a part document click Tools, Options, Document Properties, Material Properties. Crosshatch patterns alternate between components in assemblies, or between bodies in multibody parts and weldments. Crosshatch identifiers are language-independent, so you can save a drawing in one language and open it in a different language, the crosshatch patterns are recognized.
2D Sketching in Drawings You can create drawing geometry using 2D sketched geometry only, without reference to existing models or assemblies. This sketched geometry can be controlled by relations (collinear, parallel, tangent, and so on), as well as parametric dimensions. To display a grid, right-click the active drawing sheet and select Display Grid.
11-10
Sketch tools and sketch relations work the same way in a drawing document as they do in a part or assembly document. The only difference is that instead of sketching on model planes or faces, you sketch on the drawing sheet or in an active view. For information about using sketch tools and sketch relations, see Sketching in SolidWorks and Geometric Relations. Empty View You can create an empty drawing view to contain your sketch geometry. When this view is activated, all sketch geometry added belongs to this view. The sketch geometry can then be scaled, moved, and deleted as a group while still retaining the editability of the individual sketch entities. To create an empty drawing view:
1.
Click Insert, Drawing View, Empty.
2.
Click to place the view in the graphics area.
3.
Resize as necessary.
Importing Sketch Geometry You can import DXF/DWG files into a SolidWorks drawing. Then you can insert that geometry into a sketch to create model features in a part. For more information, see DXF/DWG Files(*.dxf,*.dwg). 2D Emulator The SolidWorks software includes an add-in application that allows you to create sketch entities by entering commands in text form. For more information, see 2D Emulator.
Quality in Drawings Drawings take advantage of lightweight assemblies and optimized drawing files to improve performance in opening drawings and creating drawing views, especially for large assembly drawings. Drawings can be: •
High Quality. All model information is loaded into memory.
•
Draft Quality. Only minimum model information is loaded into memory. Used in Lightweight and Detached drawings. Some edges may appear to be missing, and print quality may be slightly degraded. You can annotate views in draft quality without resolving the model.
A drawing can contain views in both modes. The SolidWorks software sets the options so that most drawing views are created in High Quality, but views for assemblies in Large Assembly Mode are created in Draft Quality. To set the option for drawing view quality:
1.
Click Tools, Options, System Options, Display Style.
2.
Under Display quality for new views, select High Quality or Draft Quality, then click OK.
To set the option for views of assemblies in large assembly mode:
1.
Click Tools, Options, System Options, Large Assembly Mode.
2.
Under Drawings, Default display quality for new views, select High Quality or Draft Quality, then click OK.
If a drawing contains views in High Quality, and you set a component to lightweight, a message prompts you to convert the views to Draft Quality. You can set an option for SolidWorks to convert affected views automatically.
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Chapter 11 Drawings
To specify how to convert drawing views to draft quality:
1.
Click Tools, Options, System Options, Performance.
2.
Under Assemblies, Automatically convert drawing to draft quality when unloading components, select:
3.
•
Always - convert views to draft quality when components are set to lightweight.
•
Prompt - display a message with a choice to convert.
•
Never - do not convert any views.
Click OK.
To set assembly components to lightweight or resolved:
Right-click a component and select Set to Lightweight or Set to Resolved. When a component is lightweight, a feather appears on the part icon and when the pointer
in the FeatureManager design tree
hovers over the part in the graphics area.
Convert to Draft Quality When you insert a drawing view into a lightweight drawing, the view must be in Draft Quality for the drawing to remain lightweight. Click: •
Yes to convert the view to Draft Quality
•
No to continue in High Quality (the model is resolved)
To avoid this message: •
Select Always create Draft Quality views in the dialog box
•
Set the Display quality for new views to Draft Quality in Tools, Options, System Options, Display Style
Sending Drawing Documents Electronically You can send drawing documents by electronic mail. You can choose to send only the drawing itself, or you can send the drawing and all referenced documents. This function uses the electronic mail application installed on your system. To mail a drawing document to another computer:
1.
With a drawing document active, click File, Send To.
2.
In the Send Mail dialog box, select one of the following: •
Drawing_name.slddrw only
•
Drawing_name.slddrw and other documents it references A list of the referenced documents, the number of documents, and the combined size of the documents is displayed. NOTE: The size of the combined documents may be important to you because mailing large size documents may cause transmission problems. If you choose to send the drawing and referenced documents, you do not have to send all the documents. You can:
11-12
•
Select a filename you do not want to send, and click Remove.
•
Select a removed filename and click Attach to replace the file.
•
Click Attach All to return all the removed files.
3.
Click OK to send the documents.
4.
Enter your mail password, the mailing address, and any other information requested by your mail application.
Types of Drawing Documents Drawing Documents Drawings are normally created with the model resolved; that is, all information about the model is available in the drawing document. You can improve performance in creating, opening, and working in drawing documents with the following: •
Detached Drawings. The model is not loaded into memory. Create when saving drawings. You can add detailing without the model. You are prompted when the model is required. When you load the model, it loads completely. You can save drawings as either resolved or detached, so you can save a detached drawing as a regular drawing and vice versa.
•
Lightweight Drawings. A subset of model data is loaded into memory; the remaining model data is loaded as needed. In a new drawing, create a lightweight drawing by specifying draft quality views. For existing drawings, select Lightweight when opening the drawing. Opening a lightweight drawing is faster than opening the same drawing with fully resolved models. You can toggle between resolved and lightweight mode while in a drawing. Lightweight is the default mode for Large Assembly Mode.
•
Reduced display data drawing files. Tessellated data for shaded and draft views is not saved with drawing documents when you clear the drawing option, reducing file size. The data is available in the model file. Resolved
Lightweight
Detached
yes
yes
no
normal
faster
somewhat slower (load required)
always resolved
resolve/lightweight
load completely, no unload
high
low
not as low as lightweight
not in all cases
yes
not in all cases
View creation
normal
faster
normal
Display quality
draft or high quality
draft only
draft or high quality
normal
feather on drawing view icon (for lightweight view) and on pointer (for lightweight part)
blue view border, axis and highlighting colors different, broken link on drawing icon and view icon
yes
no
yes
Model required Load, rebuild performance Resolve/load models Memory footprint Produce largest SolidWorks assembly drawings
Appearance
Line font per edge
Detached Drawings Detached drawings are designed so you can open and work in drawing files without the model files being loaded into memory or even being present. To create a detached drawing:
1.
Click Save on the Standard toolbar (for a new drawing) or File, Save As (for drawing that has been saved previously).
2.
In the Save As dialog box, select Detached Drawing (*.slddrw) for Save as type.
3.
Specify the file name, then click Save. You can save regular drawings as Detached drawings, and vice versa.
Detached drawings can be in Draft Quality, but they cannot be Lightweight drawings.
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Chapter 11 Drawings
View borders in Detached drawings are blue. When the referenced model is loaded into memory, the view borders change to the regular view border color. To see the view borders, select Display drawing view borders in Tools, Options, System Options, Drawings. In the FeatureManager design tree, the icons for Detached drawings display a broken link: Drawing icon for Detached drawing Drawing view icon for Detached drawing with model not loaded If the referenced model is needed for an operation within a Detached drawing, you are prompted to load the model file. You can load the model manually by right-clicking a view and selecting Load Model. When you create a drawing of a large assembly, a dialog box appears asking if you would like to use Detached format for the drawing because of improved performance. You can choose to use Detached format or continue with no change in format. When a Detached drawing is out of sync with its model, it prints with a watermark that states: SolidWorks Detached - Out-of-Sync Print Advantages of Detached Drawings You can send Detached drawings to other SolidWorks users without sending the model files. You also have more control over updating the drawing to the model. Members of the design team can work independently on the drawing, adding details and annotations, while other members edit the model. When the drawing and the model are synchronized, all the details and dimensions added to the drawing update to any geometric or topological changes in the model. Performance The time required to open a drawing in Detached format is significantly reduced because the model files are not loaded. Because the model data is not loaded into memory, more memory is available to process drawing data, which has significant performance implications for large assembly drawings. You have control over when to load the model, which takes time to load and update the drawing. File Size The Detached format requires storing more edge data and less surface data. Therefore, some files are larger when converted to Detached, while others are smaller. In general, if your drawings have section views, the file size should decrease. If the drawings do not have section views, the file size may increase. File size is directly related to the number of visible edges in the drawing. For example, if your parts have patterns of features with many instances, it is more likely that the file size will increase when converted to Detached format. Updating Views Some changes, such as changes to a section line, detail circle, scale, or projection angle, require a view update. When a drawing view requires an update, the view is displayed with a crosshatch pattern.
Working in Detached Drawings When opening a Detached drawing, the software checks all sheets in the drawing to be sure that they are synchronized with the model. If not, you are warned. If a Detached drawing is open, and you open a model document, either from File, Open or by right-clicking a view and selecting Open model name, the drawing does not synchronize with the model until you load the model.
11-14
To load the model:
1.
Right-click a view containing the model you want to load, and select Load Model. The Confirm Load Model dialog box appears.
2.
Select the Don't prompt me again in this or any future session check box if you want to prevent this message from appearing again.
3.
Click Yes to continue loading the model.
Operations Available in Detached Drawings Without the Model Following are some of the capabilities available when the model is not loaded: •
Save and Open drawings
•
Add o o
•
Annotations (Note, Surface Finish Symbol, Datum Feature Symbol, Datum Target, Geometric Tolerance, Weld Symbol, Center Mark)
o
New views (Empty, Detail, Crop)
o
New views of parts only (Auxiliary, Projected, Section, Broken-out Section)
o
Balloons (with asterisks, which are resolved to item numbers when the model is loaded)
o
Virtual sharps
Change o o
•
Dimensions
Scales of sheets or views Line Color, Line Style, and Line Thickness of model edges, silhouette edges, and sketch entities for both parts and assemblies
o
View alignments
o
Crop Views, and Auxiliary and Projected Views of parts
o
Bill of Materials, Balloons
Select o
Hidden Lines Removed (HLR), Hidden Lines Visible (HLV), Wireframe, and Tangent edge display. You can show views in Shaded mode if the views have previously been saved in Shaded mode. If any view is saved in Shaded mode, then all views of the same model can be shown in Shaded mode, and new views of the same model can be shown in Shaded mode.
o
Imported planes, sketches, origins, and axes
o
Section view edges
o
Cosmetic threads, including referencing and dimensioning
o
Model edges and vertices
o
Silhouette edges
o
Faces
o
Copy, Cut, and Paste views
•
Inference, reference, and dimension to model edges, vertices, and center points
•
Hide and show edges
•
Update the drawing with the Rebuild tool
•
Measure
•
True reference dimensions
•
View temporary axes
•
3D highlighting
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Chapter 11 Drawings
Operations Requiring the Model When the model is not loaded, the model entities do not appear in the FeatureManager design tree and the following operations are not available: •
•
Import o
Design Tables
o
Model items (dimensions, annotations, origins, planes, axes, or sketches)
o
Reference planes and axes into existing layers
Add o
•
o
Bills of Materials
o
Hole Callouts or Cosmetic Threads
Change o
o
•
New views (Standard 3 View, Named, Relative, Broken) and new views of assemblies (Auxiliary, Projected, Section, Broken-out Section)
Values or properties of feature dimensions (also origins and other reference geometry) imported from the model Hatch scales
Select o
Model faces
o
Surfaces
o
Component Line Font item from shortcut menu
•
Hide/Show Components or Hide Behind Plane
•
Export to non-SolidWorks file formats such as DXF/DWG
Lightweight Drawings Lightweight drawings are analogous to lightweight assemblies. When a drawing is lightweight, only a subset of its model data is loaded in memory. The remaining model data is loaded as needed. Performance of drawings of large assemblies is improved significantly with lightweight drawings. Loading a lightweight drawing is faster than loading the same drawing with fully resolved parts. Lightweight drawings are efficient because the full model data is loaded only as it is needed. Only parts that you select, and parts that are affected by changes that you make in the current editing session, become fully resolved. To load a drawing as lightweight:
When you open a drawing, select Lightweight in the Open dialog box. To set assembly components to lightweight or resolved:
Right-click a component and select Set to Lightweight or Set to Resolved. When a component is lightweight, a feather appears on the part icon and when the pointer
in the FeatureManager design tree
hovers over the part in the graphics area.
A feather in the FeatureManager design tree also indicates lightweight views
.
Lightweight drawings use Draft Quality views. You can specify new views to be Draft Quality in Tools, Options, System Options, Display Style. If you insert a view into a lightweight drawing as High Quality, you are prompted to convert the view to Draft Quality so that the drawing can remain lightweight. Detached drawings cannot be lightweight drawings.
11-16
With lightweight drawings, you can: •
Create all types of drawing views
•
Attach annotations to models in views
•
Specify edge properties
•
Highlight and dynamically select edges and vertices
•
Set drawings of sub-assemblies to lightweight or resolved
If you print a lightweight drawing when it is out of synchronization with its model, the drawing prints with a watermark: SolidWorks Lightweight - Out-of-Date Print
Standard Drawing Views Standard Drawing Views The standard views that generally begin a drawing are: Standard 3 View Model View Relative View Predefined View Empty View
Standard 3 View The Standard 3 View option under Insert, Drawing View creates three related default orthographic views of a part or assembly displayed at the same time. For information on the orientation of the Standard 3 View, see First Angle and Third Angle Projection. The alignment of the top and side views is fixed in relation to the front view. The top view can be moved vertically, and the side view can be moved horizontally. The top and side views are linked to the front view. Right-click a top or side view and select Jump to Parent View. The parent view can be on the same sheet or another sheet. For more information about arranging views on a sheet, see Moving Views and Rotating Views. There are several ways to create a Standard 3 View drawing. To create a Standard 3 View when starting a new drawing document:
1.
Open a new drawing.
2.
In the Model View PropertyManager, select a model from Open documents or browse to a model file, then click Next
.
3.
Under Orientation, select *Front, then place the view in the graphics area.
4.
With the Projected View PropertyManager open, place the two other views, then click OK
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Chapter 11 Drawings
Creating the Standard 3 View by the standard method:
1.
Open the part or assembly document, or a drawing document that contains a view of the model you want.
2.
Open a new drawing.
3.
Click Standard 3 View The pointer changes to
4.
on the Drawing toolbar, or click Insert, Drawing View, Standard 3 View. .
Select the model in one of these ways: •
To add the views of a part, in a part window, click a face, or anywhere in the graphics area, or click the part name in the FeatureManager design tree.
•
To add the views of an assembly, in an assembly window, click an empty region of the graphics area, or click the assembly name in the FeatureManager design tree.
•
To add the views of an assembly component, in an assembly window, click a face on the part, or click the name of either an individual part or a sub-assembly in the FeatureManager design tree.
•
In a drawing window, click a view that contains the desired part or assembly, either in the FeatureManager design tree or in the graphics area.
The drawing window returns to the front (if necessary) and the three views are placed in the drawing. Creating the Standard 3 View from a file:
If you prefer not to open the model document, you can still create a drawing of it. 1.
In a drawing, click Standard 3 View
.
2.
Right-click in the graphics area and select Insert From File.
3.
Browse to the desired model document, and click Open.
Creating the Standard 3 View by the drag-and-drop method:
The default view created when you drag and drop a part or assembly into a drawing is the Standard 3 View. 1.
Open a new drawing window.
2.
Drag a part or assembly document from Windows Explorer or from the Feature Palette window, and drop it into the drawing window, - or Drag the name from the top of the FeatureManager tree of an open part or assembly document, and drop it into the drawing window. The views are added to the drawing.
Creating the Standard 3 View from a hyperlink in Internet Explorer:
1.
In Internet Explorer (version 4.0 or later), navigate to a location that contains hyperlinks to SolidWorks part files. For example, on the SolidWorks web site, in the Support section, navigate to the Solid Modeling Library page. You may also be able to obtain SolidWorks parts from certain third-party vendors.
2.
Drag the hyperlink from the Internet Explorer window, and drop it in an open drawing window. The Save As dialog box appears.
3.
Navigate to the directory where you want to save the part, enter a new name if desired, and click Save. The part document is saved locally, and the views of the part are added to the drawing.
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Standard 3 View PropertyManager Insert a part or assembly model into a drawing as a Standard 3 View. To insert a standard 3 view:
1.
In a drawing document, click Standard 3 View Standard 3 View.
on the Drawing toolbar or click Insert, Drawing View,
2.
Select a part or assembly document under Open documents - or Click Browse and browse to a file.
3.
Click OK
.
First Angle and Third Angle Projection Standard 3 Views are in either third angle or first angle projection. In third angle projection, the default front view from the part or assembly is displayed at the lower left. and the other two views are the top and right views. In first angle projection, the front view is displayed at the upper left and the other two views are the top and left views. For information about setting the default projection, see Sheet Properties.
3rd angle projection
1st angle projection
Model View The Model View PropertyManager appears when you create a new drawing, or when you insert a model view into a drawing document. You select an orientation for the view from the view names in the model document: •
Standard views (Front, Top, Isometric, and so on)
•
Current Model View (available only for open models and only until you place the view)
•
Custom views that you created by zooming and rotating the model, enabling Perspective if desired, then saving the view by name. The entire model is displayed, even if the selected view orientation displays a partial, zoomed-in view. You cannot activate a perspective view or add dimensions or annotations it.
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Example of Model View The drawing shows a Top View, an Isometric View, and a User-defined Model View.
To insert a model view into a drawing:
1.
Click Model View
on the Drawing toolbar, or click Insert, Drawing View, Model.
2.
In the Model View PropertyManager, select an Open document under Part/Assembly to insert, or browse to a part or assembly file. If you click Standard 3 View
, the PropertyManager changes to Standard 3 View, and the list of
open documents is available. Select a model and click OK 3.
Click Next
.
You can also click Standard 3 View of the selected model. 4.
to insert a Standard 3 View.
at this point, then click OK
to insert a Standard 3 View
Specify the view orientation, scale, and so on, then place the view. When you place the model view, if you selected an orthogonal view orientation, the Projected View PropertyManager appears. You can place any number of projected views for any orthogonal view in the drawing. To prevent the Projected View PropertyManager from appearing, clear Auto-start projected view under Options in the Model View PropertyManager.
5.
Click OK
.
To change the orientation of a model view:
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1.
Select a model view.
2.
In the Model View PropertyManager, double-click a standard orientation or a custom orientation under Orientation.
Model/Predefined/Empty View PropertyManager This PropertyManager opens when you insert a Model View, a Predefined View, or an Empty View into a drawing, or when you select an existing Model, Predefined, or Empty View. The properties available depend on the type of view selected. Part/Assembly to insert Select a document from Open documents or click Browse and browse to a part or assembly file. The list of Open documents includes saved models (parts and assemblies) open in SolidWorks windows, plus models that already appear in drawing views, whether open in a window or not. Thumbnail Preview View a preview of the model selected in Open documents. Options Start command when creating new drawing. Available when inserting a model into a new drawing. The Model View PropertyManager appears whenever you create a new drawing. When you create a drawing with Make Drawing from Part/Assembly in a part or assembly document, the Model View PropertyManager appears even if you clear this check box. Auto-start projected views. Available when inserting an orthogonal view. The Projected View PropertyManager appears when you place an orthogonal model view. View Orientation View Orientation. Double-click a view orientation in the list to change the orientation of the selected view. Preview. Select to see a preview of the model while inserting a view. When cleared, only the outline of the view boundaries is shown. Insert Model For Predefined Views only. Select a model from the list under Part/Assembly of models open in the SolidWorks session, or click Browse and browse to a model file. Reference Configuration
For sheet metal flat patterns only. Select a model configuration name from the list. Flat Pattern Options
For sheet metal flat patterns only. Configuration name. You can edit the flat pattern configuration name (which appears underneath the model configuration name in the model ConfigurationManager) that appears in the box. Update Name. Click to update the configuration name in the Named View PropertyManager and in the model ConfigurationManager. View direction. Click Flip view to flip the view horizontally.
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Display Style Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Choose the scale for the view to be the same as the sheet scale or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). More Properties After you create a view or select an existing view, you can click More Properties to open the Drawing View Properties dialog box.
Relative to Model View A Relative to Model View is an orthographic view defined by two orthogonal faces or planes in the model and the specification of their respective orientations. Example of Relative to Model View A true view of an angled face perpendicular to the front face of a model is created as follows.
Specify the angled face as Front
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Specify the front face as Left
Place the resulting view
To insert a relative view:
1.
Click Relative View
on the Drawing toolbar, or click Insert, Drawing View, Relative To Model. The
2.
pointer changes to . Select the model, using one of the methods described in Standard 3 View.
3.
Under Orientation, First orientation in the PropertyManager, select an orientation (Front, Top, Left, and so on), and select the face in the graphics area for that orientation in the drawing view.
4.
Under Second orientation, select another orientation, orthogonal to the first, and select another face in the graphics area for that orientation in the drawing view. A relative view can show one body or all the bodies in a model. To show one body, select both faces from the same body.
5.
Click OK
and return to the drawing document. The pointer changes to
.
6.
In the PropertyManager, select properties (Scale, Bodies, and so on), then click in the graphics area to place the view.
7.
Click OK
.
If the angle of the face in the model changes, the views update to maintain the orientation as originally specified. Relative View PropertyManager in Drawings The Relative View PropertyManager opens when you insert a Relative View into a drawing, or when you select an existing Relative View. When you go to a model document to select model faces, the PropertyManager displays different choices. Display Style Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality
•
Draft quality
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Use sheet scale. Use custom scale. Set a scale for the views.
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Bodies When placing a view of a model with multiple bodies, choose: •
Selected body. The body from which you have selected faces.
•
All bodies. All bodies in the model document.
Dimension Type Select either Projected or True. More Properties After you create the new view or select an existing view, you can click More Properties to open the Drawing View Properties dialog box. Relative View PropertyManager in Models When you create a Relative View in a drawing, you select planar faces in a model document as described below, then return to the drawing document to place the view. Orientation Select two faces in different orientations to define the orientation of the body in the relative view. To create a relative view of one body, select faces from the same body. •
First orientation. Select the orientation, then select a face in the graphics area.
•
Second orientation. Select the orientation, then select another face in the graphics area.
Drawing View Orientation Select the relative faces of a Relative to Model View in this dialog box. To create the relative view:
1.
Click on a face on the part.
2.
Select the direction you want the selected face to be orientated towards, then click OK.
3.
Click on a second face, then select its orientation and click OK.
4.
Activate the drawing window, and click where you want to place the Relative View.
Predefined Views You can define any orthogonal, projected, or named view in a drawing sheet and the populate the view. You can save a drawing document with predefined views as a document template. To insert a predefined view into a drawing:
1.
In a drawing document, click Predefined View
, or click Insert, Drawing View, Predefined.
2.
Click in the graphics area to place the view.
3.
In the Predefined View PropertyManager, select a View Orientation as Display Style, Scale, or Dimension Type.
4.
Click OK
.
You can populate the view as you insert it, or you can populate it later.
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and specify other options such
You can add Projected Views to a predefined view. For example, if you insert a front view, you can project top and right views to create a predefined Standard 3 View. Projected views are automatically oriented and aligned to the original view. You can copy and paste predefined views. To populate predefined views:
•
Drag. Drag a model from the FeatureManager design tree of an open part or assembly document into the drawing document. All available predefined views are populated.
•
Insert Model. Right-click in a predefined view and select Insert Model. In the Insert Model PropertyManager, select a model from the Open documents list, or click Browse and browse to a model file. The view and all its related views (such as projected views) are populated when you click OK
•
Select. Select a predefined view. In the Predefined View PropertyManager, under Insert Model, select a name from the Part/Assembly list of models open in the current session. The view and all its related views (such as projected views) are populated when you click OK
•
.
.
Browse. Select a predefined view. In the Predefined View PropertyManager, under Insert Model, click Browse and browse to a model file. The view and all its related views (such as projected views) are populated when you click OK
.
When you populate predefined views, the scale of the views is determined as follows: o o
If a drawing sheet contains more than one predefined view, the views are scaled automatically. If a drawing sheet contains only one predefined view, the view uses the Custom Scale, if specified, or (if no scale is specified) the drawing sheet scale.
Empty Views You can insert Empty Views into drawing documents. Empty views are often used to contain sketches in drawings. To insert an empty view:
1.
Click Empty View
, or click Insert, Drawing View, Empty.
2.
Click in the graphics area to place the view. The Empty View PropertyManager appears.
3.
Specify a Custom Scale if necessary and click OK
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Chapter 11 Drawings
Derived Drawing Views Derived Drawing Views The following types of drawing views are derived from other views, either from standard views or from other derived views. Projected View Auxiliary View Detail View Crop View Broken-out Section Broken View Section View Aligned Section View Alternate Position View
Projected View Projected views are created with the following tools: Standard 3 Views. The Front view is a model view and the other two views are projected views, using First angle or Third angle projection as specified in Sheet Properties. Model View. When inserting an orthographic model view, the Projected View PropertyManager appears so you can insert projected views from any orthographic views on the drawing sheet. Projected View. Insert projected views from any orthographic view. You can create a projected view of an exploded assembly view. To create a projection view:
1.
Click Projected View
on the Drawing toolbar, or click Insert, Drawing View, Projected.
The Projected View PropertyManager appears. 2.
Select a view from which to project. The pointer shape changes to
3.
.
To display an arrow indicating the direction of projection, select Display View Arrow. Type a label to be displayed with the parent view and the projected view. To select the direction of projection, move the pointer to the appropriate side of the selected view. A preview of the view is displayed, snapped to the nearest projection. To override the snapping behavior, hold Ctrl as you move the preview. To resume the snapping behavior while dragging, release Ctrl. You can project to the left, right, above, or below (in this example, the user moved the pointer to the right of the selected view).
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4.
To place more than one Projected View, click Keep Visible
.
5.
When the view is where you want it to be, click to place the view.
The projection view is placed on the sheet, aligned to the view from which it was created. By default, you can move a projection view only in the direction of the projection. For information about changing the alignment of views, see View Alignment and Display. Projection Views are linked from the child view to the parent. Right-click the Projection View and select Jump to Parent View.
Projected View PropertyManager The Projected View PropertyManager opens when you create a Projected View in a drawing, or when you select an existing Projected View. Arrow Arrow. Select to display a view arrow indicating the direction of the projection. Label
. Type text to be displayed with both the parent view and the projected view.
Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values.
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Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for projected views. More Properties For an existing Projected View, click More Properties to open the Drawing View Properties dialog box.
Auxiliary View An Auxiliary View is similar to a Projected View, but it is unfolded normal to a reference edge in an existing view. Example of Auxiliary View The angled edge on the front view is selected for the Auxiliary View, which is at the upper right, with a view arrow labeled C.
You can create an auxiliary view of an exploded assembly view. To create an auxiliary view:
1.
Click Auxiliary View
on the Drawing toolbar, or click Insert, Drawing View, Auxiliary.
The Auxiliary View PropertyManager appears. 2.
Select a reference edge (not a horizontal or vertical edge, which would create a standard Projection View). The reference edge can be an edge of a part, a silhouette edge, an axis, or a sketched line. If you sketch a line, activate the drawing view first. NOTE: Auxiliary views are not available from entities of section or detail views of parts in the FeatureManager design tree. As you move the pointer, a preview of the view is displayed. You can control the alignment and orientation of the view as follows: o
o
3.
Alignment. To override the default alignment as you place the auxiliary view, hold Ctrl as you move the preview. To resume the snapping behavior while dragging, release Ctrl. Orientation. You can toggle the view orientation (front or back) by dragging the view across the reference edge. An arrow shows the view orientation, which is useful when the Show contents while dragging view option is cleared. After you place the view, you can toggle the view orientation by double-clicking the arrow or by selecting Flip direction in the PropertyManager.
Move the pointer until the view is where you want, then click to place the view.
For information about changing the alignment of views, see View Alignment and Display. The view arrow (or set of arrows, if you use the ANSI dimensioning standard) indicates the orientation of the projection.
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To remove the arrow, select the Auxiliary View. In the PropertyManager, select or clear the Display view arrow check box and enter a label if desired (maximum of two characters). Auxiliary Views are linked to their parent views. Right-click the Auxiliary View and select Jump to Parent View. The parent can be on the same sheet or another sheet. Center Marks in Auxiliary Views are oriented to the viewing direction such that one of the lines of the Center Mark is parallel to the view direction. If you used a sketched line to create an Auxiliary View, the sketch is absorbed so you cannot delete it inadvertently. You can delete sketch entities while editing the sketch. To edit a sketched line used to create an auxiliary view:
1.
Select the Auxiliary View.
2.
In the Auxiliary View PropertyManager, select Display view arrow.
3.
Right-click the view arrow and select Edit Sketch.
4.
Edit the sketched line.
5.
Select the line and click Rebuild
to update the view.
Auxiliary View PropertyManager The Auxiliary View PropertyManager appears when you create a new Auxiliary View in a drawing, or when you select an existing Auxiliary View. Arrow Arrow. Select to display a view arrow indicating the direction of the auxiliary view. Label . Type text to be displayed with both the parent view and the auxiliary view. Specify the label display in Tools, Options, Document Properties, View Labels. Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style.
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Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for auxiliary views. More Properties For an existing Auxiliary View, click More Properties to open the Drawing View Properties dialog box.
Detail View You create a Detail View in a drawing to show a portion of a view, usually at an enlarged scale. This detail may be of an orthographic view, a 3D view, or a Section View. You cannot create a Detail View from the following: •
a named view that shows the model with perspective turned on
•
another Detail View
•
a Crop View
Detail views expand in the FeatureManager design tree so that all components and features are available. You can create a detail view of an exploded assembly view. To create a detail view:
1.
Activate an existing view.
2.
Click Detail View
on the Drawing toolbar, or click Insert, Drawing View, Detail.
The Detail View PropertyManager appears and the Circle 3.
tool is active.
Sketch a circle. NOTE: To create a profile other than a circle, sketch the profile before clicking the Detail View tool. Using a sketch entity tool, create a closed profile around the area to be detailed. You can add dimensions or relations to the sketch entities to position the profile precisely relative to the model. NOTE: If you plan to create a Broken View, you are advised to relate the sketch to the model. As you move the pointer, a preview of the view is displayed.
4.
When the view is where you want it to be, click to place the view.
The note on the detail view includes the letter label and view scale, if the scale is different from the sheet scale. Detail views are not aligned to other views by default, and may be moved freely to any location on the drawing sheet. If you wish to remove any sketches that are imported to the drawing, edit the model and hide any sketches that interfere with the Detail View. Detail Views are linked to their detail circles. Right-click the circle and select Jump to Detail View, which can be on the same sheet or another sheet. Right-click the Detail View and select Jump to Parent View.
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Example of Detail View The active view on the left shows the sketched profile (a circle) and the profile label (A). The Detail View on the right shows the Detail View note, which displays the label (A) and the scale (1:1).
Detail View PropertyManager The Detail View PropertyManager appears when you create a new Detail View in a drawing, or when you select an existing Detail View or detail circle. The PropertyManager controls the following properties: Circle Options •
Style
. Select either Circle or Profile. If you select Circle, various circle styles are available.
•
Label . Edit the letter associated with the detail circle and detail view. To specify the label format, click Tools, Options, Document Properties, View Labels.
•
Font. To choose a font for the detail circle label other than the document's font, clear the Document's font check box and click Font. If you change the detail circle label font, a message appears asking if you wish to also apply the new font to the detail view label.
View Options •
Full outline. Select to display the profile outline in the detail view.
•
Pin position. Select to prevent the detail view from moving if the parent view changes size.
•
Scale hatch pattern. Select to scale the hatch pattern based on the scale of the detail view.
Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style.
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Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for detail views. More Properties For an existing Detail View, click More Properties to open the Drawing View Properties dialog box. Modifying a Detail View To change the position or size of a profile:
1.
Select the profile.
2.
Drag the center point to change the position, or drag a side to change the size. The Detail View changes as the profile changes.
To change the profile by editing the sketch.
1.
Right-click the profile sketch and select Edit Sketch.
2.
Edit the profile as needed to change the shape or size. The pointer changes to
3.
Click Rebuild
when it is on the detail profile.
to update the detail view.
To select the profile display:
If you use a shape other than a circle as the profile, you can choose to display either the profile or its circle in the parent view. 1.
Select the Detail View or detail circle. The Detail View PropertyManager appears.
2.
Under Circle Options, Style, choose either Profile or Circle. •
If you select Circle as the display, you can choose the Style of the detail note, and you can drag the note anywhere except inside the circle.
•
If you select Profile as the display, you can drag the note anywhere except inside the profile.
You can choose whether the circle or profile is displayed by default in a new Detail View. Click Tools, Options, System Options, Drawings. Select or clear the Display new detail circles as circles check box. To change the scale of the Detail View:
1.
Select the Detail View or detail circle.
2.
In the Detail View PropertyManager, select Custom Scale, enter a new scale ratio, and click OK
.
The Detail View scale is displayed in the note if its scale is different from the sheet scale. To change the Detail View note text:
Double-click the note and edit the text in place. Click outside the note to exit. - or Right-click the text and select Properties. The Note PropertyManager appears. Modify the text and the text properties, such as font, justification, and so on and click OK. The label text on the detail profile also updates. Changes in font do not apply to the profile label.
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To change the text of the label on the detail profile:
Double-click the label and edit the text in place. Click outside the label to exit. - or Select the detail circle or label. The Detail View PropertyManager appears. Under Circle Options, modify the text and font. The Detail View note text also updates. A message appears asking if you want to apply the font change to the Detail View as well. To pin Detail Views:
You can pin Detail Views, to prevent them from moving if the parent view changes size. Select the Detail View. In the Detail View PropertyManager, under View Options, select Pin position. Detail Circle Styles Per Standard
ISO, JIS, DIN, BSI - No Leader ANSI - Broken Circle GOST -
Broken Circle
With Leader
No Leader
Connected
Crop View You can crop any drawing view except a Detail View, a view from which a Detail View has been created, or an exploded view. Crop View can save steps because you do not create a new view. For example, instead of creating a Section View and then a Detail View, then hiding the unnecessary Section View, you can crop the Section View directly. You cannot create a Detail View from a Crop View. To crop a view:
1.
Activate an existing view.
2.
Draw a closed profile with a sketch tool such as a circle.
3.
Click Crop View
on the Drawing toolbar, or click Tools, Crop View, Crop.
The view outside the profile disappears.
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A circle is drawn on this Section View
After cropping, only the view inside the circle is displayed.
To edit a Crop View:
1.
Right-click the view and select Crop View, Edit Crop, or select the view and click Tools, Crop View, Edit Crop.
2.
Edit the profile.
3.
Click Rebuild
to update the view.
To remove a Crop View:
Right-click the view and select Crop View, Remove Crop, or select the view and click Tools, Crop View, Remove Crop. The crop is removed and the view returns to its uncropped state.
Broken-out Section A broken-out section is part of an existing drawing view, not a separate view. A closed profile, usually a spline, defines the broken-out section. Material is removed to a specified depth to expose inner details. Specify the depth by setting a number or by selecting an edge in a related view. Use reference geometry to specify depth for precise section planes. You cannot create a broken-out section on an exploded detail, section, or alternate position view. Example of Broken-out Section This example shows (1) wall thickness and shaft and (2) how the shaft is welded to the cap.
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To create a broken-out section:
1.
Click Broken-out Section Section.
on the Drawing toolbar, or click Insert, Drawing View, Broken-out
The Broken-out Section PropertyManager appears with the pointer active. You are prompted to sketch a closed spline.
showing that the spline tool is
If you want a profile other than a spline, create and select a closed profile before clicking the Brokenout Section tool. 2.
Sketch a profile.
3.
In the PropertyManager, set the depth.
4.
Click OK
.
To delete or edit a broken-out section:
Right-click the broken-out section in the graphics area (the pointer changes to when it is over a broken-out section) or in the FeatureManager design tree and select one of the following. •
Delete.
•
Edit Definition. In the Broken-out Section PropertyManager, change the depth, then click
•
OK . Edit Sketch. Select the sketch entity and edit it. Select the sketch entity again and click Rebuild
.
Broken-out Section PropertyManager The PropertyManager for a broken-out section controls the following properties: Depth. Specify in one of the following ways: •
Depth Reference . Select geometry, such as an edge or an axis, in the same or a related view. The entity name appears in the Depth Reference selection box.
•
Depth
. Enter a number in the Depth box.
Use reference geometry to specify depth for precise section planes. Preview. When selected, the broken-out section is displayed as you change the depth. When cleared, the broken-out section is applied when you exit from the PropertyManager. Auto hatching. For assemblies only. If selected, the software adjusts automatically for neighboring components to alternate crosshatch patterns in 90 degree increments. If there are still adjacent section faces with the same pattern, the pattern spacing is adjusted.
Broken View You can use a broken (or interrupted) view on the drawing of a long part. Broken views make it possible to display the part in a larger scale on a smaller size drawing sheet. Reference dimensions and model dimensions associated with the broken area reflect the actual model values. You can specify the gap between the break lines and the extension of the lines beyond the part geometry in Tools, Options, Document Properties, Detailing. The gap between the break lines is the gap when the break lines are first inserted, and also the gap after the view has been broken. You can specify the line font for the break lines in Tools, Options, Document Properties, Line Font. You can apply the Break View and Un-Break View commands to multiple views.
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Example of Broken View
Insert break lines into the view geometry.
Drag the break lines into position.
Break the view.
To create a Broken View:
1.
Select the drawing view and click Insert, Vertical Break (or Horizontal Break). Two break lines appear in the view. You can add more than one set of break lines to a view; however, all breaks must be in the same direction. You can add breaks only to an unbroken view.
2.
Drag the break lines with the
pointer to the places on the part where you want the breaks to occur.
3.
Right-click inside the highlighted boundary and select Break View. The part is displayed with a gap in the part geometry. In addition to model geometry, broken views also support cosmetic threads and axes.
NOTE: When you break the view, any sketch entities that are between the break lines are deleted. Dimensions that are between the break lines become dangling. To restore a broken view to its unbroken state:
Right-click the broken view (or multiple broken views), and select Un-Break View. To modify a broken view:
•
To change the shape of the break lines, right-click a break line and select a style from the shortcut menu.
•
To change the position of the break, drag the break lines.
•
To change the width of the break gap, click Tools, Options, Document Properties, Detailing. Under Break line, enter a new value for Gap. To display the new gap, Un-Break and then Break the view again.
NOTE: You can select an Area Hatch in a broken view only in its unbroken state. You cannot select an area hatch that crosses a break.
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Broken View Break Line Styles Broken View break lines can be in one of four styles.
Straight
Curved
Zig Zag
Small Zig Zag
Section Views in Drawings You create a Section View in a drawing by cutting the parent view with a section line. The section view can be a straight cut section or an offset section defined by a stepped section line. The section line can also include concentric arcs. NOTE: You can also create section views in models. You can create section views of section views. A new section is calculated from the original solid model, and the view updates if the model changes. You can show hidden edges in section views when the view is in Hidden Lines Removed mode. Section views expand in the FeatureManager design tree so that all components and features are available. You can add dimensions to section lines without editing the section line sketch. You can dimension between two section lines, or between a section line and another line or edge. To create a section view:
1.
Activate an existing drawing view.
2.
Click Section View
on the Drawing toolbar, or click Insert, Drawing View, Section.
The Section View PropertyManager appears, and the Line tool 3.
is active.
Sketch a section line. NOTE: To create a multi-line section view, or to use a centerline as the section line, sketch the section line before clicking the Section View tool. If the section line does not completely cut through the bounding box of the model in the view, you are asked if you want this to be a partial section cut. If you click Yes, the Section View is created as a partial section view. As you move the pointer, a preview of the view is displayed. By default, the view is aligned in the direction of the arrows on the section line. To override the default alignment as you place the view, press Ctrl. To return to the default alignment while dragging, release Ctrl. The orientation of the section view toggles as you drag the pointer over the section line. If the section line has multiple segments, the view is aligned to the sketch segment that was selected when you clicked the Section View tool.
4.
Click to place the view.
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In its default alignment, a section view can only move in the direction of the section arrows. For information about changing the alignment of views, see View Alignment and Display. Multiple section lines can have the same label. A warning message appears if the drawing standard you are using does not allow it. Section Views are linked to their section lines. Right-click the section line and select Jump to Section View, which can be on the same sheet or another sheet. Right-click the Section View and select Jump to Parent View. Example of Section View A section line is drawn horizontally across the activated view.
The Section View shows crosshatching on sectioned areas. The parent view now shows the direction arrows and labels.
Section View PropertyManager The Section View PropertyManager opens when you create a Section View in a drawing, or when you select an existing Section View. The PropertyManager controls the following properties: Line Options
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•
Flip direction
. Select to flip the direction of the cut.
•
Scale with model. Select for the section line to scale parametrically with the model if the model changes size. This can result in a section cut that is not what you intend.
•
Label
•
Font. To choose a font for the section line label other than the document's font, clear the Document's font check box and click Font. If you change the section line label font, you can apply the new font to the section view label.
. Edit the letter associated with the section line and section view.
View Options •
Partial section. If the section line does not completely cross the view, a message states that the section line is smaller than the view geometry and asks if you want it to be a partial section cut. o o
•
Yes. The section view is a partial section view and the check box is selected. No. The section view appears but is not cut. You can select the check box later to create a partial section view.
Display only surface. Only the surfaces cut by the section line appear in the section view. Complete section
•
Partial section
Display only surface
Auto hatching. Crosshatch patterns alternate between components in assemblies, or between bodies in multibody parts and weldments.
Display Style Use parent style. Clear to select style and quality settings different from those of the parent view. Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality. Model resolved.
•
Draft quality. Model lightweight, used for faster performance with large assemblies.
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Choose the scale for the view to be the same as the parent scale, the same as the sheet scale, or its own custom scale. For a custom scale, select Use custom scale and edit the values. Dimension Type Select either Projected (2D) or True (model value). Projected is set automatically for section views. More Properties For an existing Section View, click More Properties to open the Drawing View Properties dialog box.
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Chapter 11 Drawings
Modifying Section Views •
If a Section View in a Drawing needs to be updated (when a section line position or direction changes, for example), the view is marked with a crosshatch pattern. See Updating Views.
•
To change the length or location of the section line, the length of the leader, or the position of the label, select the line or label and drag it.
•
To edit the letter label on the section line, either: Double-click the letter label, edit in place, and click outside the label to exit. - or Select the section line and edit the label and its font in the Section View PropertyManager.
•
To edit the note text on the section view, double-click the text, edit in place, and click outside the label to exit. NOTE: To edit the properties of the section view note text, select the note and edit the properties in the Note PropertyManager.
•
To edit the sketch used to create the section line, right-click an entity of the sketch and select Edit Sketch.
•
Edit the sketch as needed. Then select one sketch entity and click Rebuild to update the section view. To change the cut direction as indicated by the arrows, double-click anywhere along the section line, or select the section line and select Flip Direction in the Section View PropertyManager.
•
To modify the crosshatch pattern, right-click a face, or hold Ctrl and select multiple faces, and select Properties. See Crosshatch Properties.
•
To modify the length of a centerline, drag the endpoints. Centerlines are automatically added where needed (holes, circular extruded bosses or cuts, and revolved features) in section views. You can specify the default distance for the centerline to extend beyond the model edge in Detailing Options. To remove centerlines, you can either delete them from the Section View, or you can turn the display of them on and off by clicking View, Axes.
Section Views of Assemblies When you create a Section (or Aligned Section) View of an assembly, you can exclude (leave uncut) selected components and set Auto hatching on the Section Scope tab of the Section View dialog box. To exclude components from a section view of an assembly:
1.
Activate a view, and create a section line as described in Section View or Aligned Section View.
2.
Click Section View or Aligned Section View View, Section or Aligned Section.
on the Drawing toolbar, or click Insert, Drawing
The Section Scope tab of the Section View dialog box appears. 3.
In the active drawing view, or in the same view in the FeatureManager design tree, click the components that you want to exclude from the section view. The selected components are listed in the Excluded components box. To remove a component from the list, select the component again, or select the component in the list and click Delete.
4.
If a selected component is used more than once in the assembly (for example, if it is a member of a pattern, or if it is used as a component of more than one sub-assembly):
5.
•
To exclude all the instances of the selected component, click the component name in the Excluded components list, and select the Don’t cut all instances check box. In the resulting view, all instances of the selected component will be left uncut.
•
To exclude only the selected instance, leave the Don’t cut all instances check box cleared. In the resulting view, only the selected instance will be uncut; all others will be cut.
Click OK. In the resulting section view, excluded components are not cut. They are shown in the view, or you can remove them from the view by setting the section line property Display only surface cut.
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To control auto hatching:
If you want the software to automatically adjust for neighboring components with the same crosshatch pattern, select the Auto hatching check box in the Section Scope dialog box. The angle used in the pattern automatically alternates in 90 degree increments. If there are still adjacent section faces with the same pattern, the pattern spacing is adjusted. If you do not use auto hatching, you can manually adjust the angle and spacing on adjacent components. See Crosshatch Properties. NOTE: A Detail View created from an assembly Section View inherits the crosshatch patterns of its parent view. Section Scope In a drawing, you can specify which components are to be left uncut in a section view of an assembly. The Section Scope dialog box appears when you create a section view in an assembly drawing. The Section Scope tab also appears in the Drawing View Properties dialog box for a section view. Section Scope controls the following items. Excluded components •
If you are creating a new section view, click the components to leave uncut in the parent drawing view on the sheet or in the FeatureManager design tree.
•
If you are editing an existing section view, click the components in the section view itself.
•
To remove a component from the list, click the component again, or click it in the Excluded components list and press Delete.
Don't cut all instances Specify what to do if the selected component is used more than once in the assembly (for example, if it is a member of a pattern, or if it is used as a component of more than one sub-assembly): •
Select. If you want to exclude all the instances of the selected component in the assembly, select the Don’t cut all instances check box. In the resulting view, all instances of the selected component are left uncut.
•
Clear. If you want to exclude only the selected instance, clear the Don't cut all instances check box. In the resulting view, only the selected instance are uncut; all others are cut.
Auto hatching •
Click Auto hatching if you want the software to automatically adjust for neighboring components with the same crosshatch pattern.
•
If you do not use Auto hatching, you can manually adjust the angle and spacing on adjacent components. See Area Hatch/Fill Properties.
Troubleshooting Section Views If a Section View is displayed with portions of the model uncut, and with the model in the dangling (brown) color, check for the following conditions: •
The section line may not extend completely across the model. Either extend the section line as needed, or use the Partial Section option. See Section Line Properties.
•
The cut may result in zero-thickness geometry that cannot be displayed correctly in the view. Modify the position of the section line to correct this problem.
•
There may be a problem with the model geometry. Use Tools, Check to identify the invalid geometry. For more information, see Check Entity.
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Modifying Section Line Properties You can make changes to a Section View or Aligned Section View in a drawing by editing the section line properties. You can set these properties before, during, or after creating the section view. To modify a section line before creating the view:
1.
Activate a drawing view and sketch a line.
2.
With the line selected, click Insert, Make Section Line.
3.
Select the section line. The Section View PropertyManager appears.
4.
Make any changes in the PropertyManager.
5.
Click Section View
or Aligned Section View
and place the view.
- or Click OK
to close the PropertyManager without creating a view.
NOTE: You can select the section line and create the view at any time. To modify a section line during creation of a section view:
Make any changes in the Section View PropertyManager, which appears when you click the Section View or Aligned Section View tool. To modify a section line after a section view is created:
1.
Select the section line or section view. The Section View ProprtyManager appears.
2.
Make any changes and click OK
.
Aligned Section View You can create an aligned section view in a drawing through a model, or portion of a model, that is aligned with a selected section line segment. The aligned section view is similar to a Section View, but the section line for an aligned section comprises two lines connected at an angle. Example of Aligned Section View The active view shows the section line, direction arrows, and labels. The resulting Aligned Section View is at the right.
To create an aligned section view:
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1.
Activate an existing drawing view.
2.
Click Centerline
3.
Sketch the section line. The section line should consist of two connected lines at an angle to each other.
4.
Select the segment of the sketched section line to which you want to align the view.
5.
Click Aligned Section View
or Line
or Tools, Sketch Entity, Centerline or Line.
on the Drawing toolbar, or click Insert, Drawing View, Aligned Section.
NOTE: If you are in an assembly, the Section View Section Scope dialog box appears. The Section View PropertyManager appears. You cannot change the angle of the line that you selected to align the view; however, you can change the position of the view. As you move the pointer, a preview of the view is displayed. By default, the view is aligned in the direction of the arrows on the selected segment of the section line. To override the default alignment as you place the view, press Ctrl. To return to the default alignment while dragging, release Ctrl. The orientation of the view flips as you drag the preview across the the section lline. You can also select Flip direction in the PropertyManager. The view is aligned to the sketch segment that was selected when you created the section line; the cut faces from the other segments are projected into the same plane. 6.
When the view is where you want it to be, click to place the view.
In its default alignment, an aligned section view can move only in the direction of arrows on the selected segment. For information about changing the alignment of views, see Drawing View Alignment and Display.
Alternate Position View You can superimpose one drawing view precisely on another with the Alternate Position View tool. The alternate position is shown with phantom lines. Alternate Position Views are often used to show the range of motion of an assembly. •
You can dimension between the primary view and the Alternate Position View.
•
The Alternate Position View is added to the FeatureManager design tree.
•
You can create more than one Alternate Position View in a drawing.
•
The Alternate Position View is not available in Broken, Section, Detail, or Crop views.
To insert an alternate position view:
1.
Click Alternate Position View Position.
on the Drawing toolbar, or click Insert, Drawing View, Alternate
The Alternate Position PropertyManager appears. You are prompted to select a drawing view in which to insert the alternate position. 2.
3.
Under Configuration, choose either: •
New configuration - to create a new Alternate Position configuration. Accept the default name or type a name of your choice.
•
Existing configuration - to choose an existing configuration in the assembly document. Select a configuration from the list.
Click OK
. The results are either:
•
New configuration - If the assembly document is not already open, it opens automatically. The assembly appears with the Move Component PropertyManager open and Free Drag activated. Continue to Step 4.
•
Existing configuration - The alternate position of the selected configuration appears in the drawing view, and the PropertyManager closes. The view is complete. No further steps are required.
4.
Use any of the Move Component tools to move the assembly components to the desired position.
5.
Click OK
to close the Move Component PropertyManager and return to the drawing.
The alternate position of the assembly configuration appears in the drawing view in phantom lines, and the Alternate Position PropertyManager closes.
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Example of an Alternate Position View
Alternate Position PropertyManager The Alternate Position PropertyManager opens when you insert an Alternate Position View into a drawing. You choose the Alternate Position configuration in the PropertyManager. Configuration •
New configuration - A default name appears in the box. You can accept the default name or type a name of your choice.
•
Existing configuration - Choose from existing assembly configurations that appear in the list.
Position Schematic PropertyManager The Position Schematic PropertyManager opens when you insert a schematic into a drawing document. You must have Microsoft Visio® Technical Edition installed on your system for this menu item to be available. To insert a Visio schematic into a drawing:
1.
Click Insert, Schematic. The Position Schematic PropertyManager opens.
2.
Drag-select a box in the graphics area to size and position the schematic.
3.
Under Schematic templates, select a template. NOTE: The PropertyManager lists the templates most commonly required in SolidWorks. To choose from the more extensive list in Visio, select Other from the SolidWorks list, or else make no selection.
4.
Click OK
to close the PropertyManager and activate Visio.
5.
Create a schematic in Visio.
Example of a Visio schematic in a SolidWorks drawing
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OLE Items in Drawings If any part of an active OLE item in a drawing is covered, the item does not redraw when it is uncovered. This behavior may occur, for example, when you move a stencil across an active Visio item. To redraw the OLE item and restore the drawing:
Deactivate the OLE item and reactivate it. - or Select one of the eight handles on the border of the OLE items.
Drawing View Update By default, all drawing views are updated automatically when the model changes. You can change this behavior to allow manual regeneration of drawing views. In manual view regeneration mode, you can update all the views at once when you are ready, or update them one by one. When the model changes, any drawing views that need to be updated are marked with a light gray crosshatch pattern. NOTE: You cannot activate or edit a view that needs to be updated. To manually update drawing views:
1.
Right-click the Drawing icon at the top of the FeatureManager design tree, and click Automatic view update. If there is no check mark, it indicates that manual view regeneration is enabled.
2.
To update all the views at once, either:
3.
•
Click Edit, Update All Views.
•
Click Edit, Rebuild or Rebuild
•
Right-click the Drawing icon in the FeatureManager design tree, and click Update All Views.
.
To update selected drawing views: •
Select the view, then click Edit, Update View, or click Update View on the Drawing toolbar. (Use Tools, Customize to add the Update View icon to your toolbar, if necessary.)
•
Right-click the view, and select Update View.
Press Ctrl to select more than one view at a time for updating.
Drawing View Alignment and Display Drawing View Alignment and Display Manipulating Views •
Drawing View Properties
•
Updating Views
•
Moving a Drawing
•
Moving Views
•
Aligning Views
•
Rotating Views
•
Copying and Pasting Views
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Chapter 11 Drawings
Hiding and Showing •
Hiding and Showing Views
•
Hiding and Showing Edges
•
Show Hidden Lines
•
Hide/Show Components
•
Hide Components Behind Plane
•
Hiding and Showing Sketches
Displaying •
Drawing View Display Modes
•
Component Line Font
•
Line Format
•
Layers
Manipulating Views Drawing View Properties The Drawing View Properties dialog box provides information about the drawing view and its associated model. To view and edit the Drawing View Properties:
1.
Right-click in a drawing view (but not on the model) and select Properties. - or From a view PropertyManager, click More Properties.
2.
Edit the following properties on the View Properties tab, or edit items on the Show Hidden Edges or Hide and Show Components tabs, and click OK.
View information. Displays the Name and Type of the view (read-only). Model information. The name of the model and the path of the referenced document are displayed (read-only). Model information is not available for Detached views when the model is not loaded. Configuration Information. Select one of the following: Use model’s "in-use" or last saved configuration. - or Use named configuration. To use a configuration that you previously created and named, select the configuration from the list. Show in exploded state. If the view contains an assembly with an exploded view defined, select this check box to display the exploded view. Bill of Materials (BOM). Linked to BOM. Selected automatically if the model in the view is linked to a Bill of Materials. The name of the BOM is displayed in the window. Align breaks with parent. If the view is a Broken View that was created from another broken view, select this check box to align the break gaps in the two views. Depending on the type of changes you have made, it may be necessary to click Update View Rebuild
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.
or
Multiple Views PropertyManager To set properties common to multiple drawing views:
1.
Select multiple drawing views in the graphics area.
2.
In the PropertyManager, set the properties described below and click OK
.
Display Style Select a display type: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded Select a display quality: •
High quality
•
Draft quality
Set options for drawing view display style in Tools, Options, System Options, Display Style. Scale Use parent scale. Available for related views (projected, auxiliary, section, detail, and so on) Use sheet scale. Use custom scale. Set a scale for the views. Dimension Type Select either Projected or True. Updating Views To control the update behavior of the views in an active drawing, specify the Automatic view update mode. If selected, drawing views update as you change the model. You can also set an option to specify whether views are updated when opening drawings. NOTE: You cannot activate or edit a drawing view that needs to be updated. To change the update mode in the current drawing:
Right-click the drawing icon at the top of the FeatureManager design tree, and select or clear Automatic view update. To update drawing views manually:
1.
Right-click the drawing icon at the top of the FeatureManager design tree and clear Automatic view update if it is checked.
2.
To update all the views at once, use one of these methods: •
Click Edit, Update All Views.
•
Click Rebuild
SolidWorks 2004 Reference Guide
or Edit, Rebuild to update any views that need to be updated.
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Chapter 11 Drawings
3.
To update selected drawing views, use one of these methods: •
Select the view, then click Update View on the Drawing toolbar, or click Edit, Update View. (Use Tools, Customize to add the Update View icon to the toolbar, if necessary.)
•
Right-click the view, and select Update View. You can select the view either in the FeatureManager design tree or on the drawing sheet for either method. You also can hold down Ctrl and select several views at once to update in this way.
To update automatically when opening drawings:
1.
Click Tools, Options, System Options, Drawings.
2.
Select Allow auto-update when opening drawings. NOTE: The automatic updating of views when opening drawings does not affect Automatic view update for the active drawing document.
Move Drawing You can move all of the entities of a drawing in relation to the drawing sheet. Entities that are on the drawing sheet (drawing views, annotations, and so on) or in the drawing sheet format are moved. To move drawing entities:
1.
Right-click the drawing name at the top of the FeatureManager design tree and select Move.
2.
Type a value in the X value or Y value box, and click Apply. All of the drawing entities move the specified distance in the X or Y direction.
3.
Click Close to exit the dialog box.
Moving Drawing Views To move a drawing view:
Press Alt, place the pointer anywhere in the view, and drag the view. - or Move the pointer over the boundary of a view to highlight the boundary, or select the view. When the move pointer
is displayed, drag the view to a new location.
Note the following restrictions: •
Standard 3 View. The alignment of the front view is fixed in relation to the other two views. When you move the front view, the other views also move. The other two views can move independently, but only horizontally or vertically, toward or away from the front view.
•
Auxiliary, Projected, Section, and Aligned Section views are aligned with the parent views from which they are created, and only move in the direction of the projection.
•
Broken views respect the alignment of the view before it was broken. Crop views and Alternation Position views retain the alignments of the original views.
Named, Detail, Relative to Model, and Empty views can be moved freely on the sheet and are not aligned to other views. Child views move relative to parent views. To retain exact positions between the views, press Shift while dragging.
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Aligning Views You can change the alignment of views that are not aligned by default, or views whose alignment you have broken. You can also break view alignments and return alignments to their defaults. To align one drawing view to another:
1.
Select a drawing view, and click Tools, Align Drawing View, Horizontal To Another View or Vertical To Another View. - or Right-click a drawing view, select Alignment, then select one of the following options: •
Align Horizontal by Origin
•
Align Vertical by Origin
•
Align Horizontal by Center
•
Align Vertical by Center The pointer changes to
2.
.
Select the view to which you want to align. The model origins or drawing view centers of the views are aligned along the chosen direction. The alignment is maintained if you move the reference view.
To align a drawing view to a model edge:
1.
Select a linear model edge in a drawing view.
2.
Click Tools, Align Drawing View, Horizontal Edge or Vertical Edge. The view rotates until the selected edge is oriented horizontally or vertically. If any views are projected from a view that you rotate this way, the projected views update to maintain their projection. For additional methods of rotating views, see Rotating Views.
To break a view’s alignment:
For views that are aligned, you can break the alignment and move the views independently. Right-click inside the view boundary (not on the model), and select Alignment, Break Alignment, or click Tools, Align Drawing View, Break Alignment. To return a view to its default alignment:
You can return a view whose alignment you have broken to its original alignment. Right-click inside the view boundary (not on the model), and select Alignment, Default Alignment or click Tools, Align Drawing View, Default Alignment. Rotating Views You can rotate a view to orient a selected edge either horizontally or vertically. You can also rotate a view around its center point to orient the view at any angle. To rotate a drawing view around a model edge:
1.
Select a linear model edge in a drawing view.
2.
Click Tools, Align Drawing View, Horizontal Edge or Vertical Edge. The view rotates until the selected edge is oriented horizontally or vertically. If there are any views projected from a view you change this way, they update to maintain their projection.
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To rotate a drawing view around its center point:
1.
Click Rotate View
on the View toolbar, or right-click the view and select View, Rotate View.
The Rotate Drawing View dialog box appears. 2.
Drag the view to the desired rotation. The view snaps to 45° increments, but you can drop the view at any angle. The angle appears in degrees in the dialog box. - or In the dialog box, type the angle in the Drawing view angle box, select or clear the Dependent views update to change in orientation check box, and click Apply to see the rotation.
3.
Click Close to close the dialog box.
To restore a view to its original rotation:
Right-click the view and select Alignment, Default Alignment. If the default alignment to another view was broken, this also restores the original alignment. Rotate Drawing View To rotate a drawing view:
1.
Select a drawing view (optional), and click Rotate View a view, and select View, Rotate View.
on the View toolbar. You can also right-click
The Rotate Drawing View dialog box appears. 2.
Rotate the view in one of these ways: •
Drag the view on the sheet. The view snaps to 45 degree increments, but you can drop the view at any angle.
•
Specify the Drawing view angle. (Select a view before entering an angle, if you did not pre-select a view.)
•
Use the left and right arrow keys. The increment value specified for the arrow keys (under Tools, Options, System Options, View Rotation) is used.
3.
Select Dependent views update to change in orientation if you also want to update any views that were created from the view you are rotating (projected views, for example).
4.
Select Rotate Center Marks with view if you want center marks to rotate with the view. You can rotate center marks in the Center Mark PropertyManager.
5.
Click Apply to update the views. You can rotate other views if needed, then click Close when you are finished.
6.
To restore the view to its original rotation, right-click the view and select Alignment, Default Rotation.
Copying and Pasting Views You can cut, copy, and paste drawing views from one sheet to another in the same drawing, and from one drawing document to another. You can also drag views from sheet to sheet within a drawing (but not to another drawing document). To perform these operations on multiple views at once, hold down the Ctrl key as you select the views. NOTE: To copy a Detail or Section View from one drawing to another, you must also copy the parent view. You can either copy the parent view first, or you can copy both the parent and the Detail or Section View at the same time. To cut/copy/paste a drawing view:
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1.
Select the view either on the sheet or in the FeatureManager design tree.
2.
Click Cut
or Copy
, or click Edit, Cut or Copy.
3.
Change to the target sheet or drawing document, click where you want to paste the view, and click Paste or Edit, Paste.
To move or copy views by dragging:
Select a view on the active drawing sheet, or select the view’s icon in the FeatureManager design tree. •
To move the view, hold down Shift, then drag the selected view or its icon, and drop it on the sheet icon for the target sheet.
•
To copy the view, hold down Ctrl as you drag and drop.
Hiding and Showing Hiding and Showing Views You can use Hide View to hide an entire view while working on a drawing. Once hidden, you use Show View to display that view again. When you hide a view that has dependent views (Detail, Section, or Auxiliary views), you are given the choice of hiding those views also. When you show either the parent view or a dependent view again, you are given the choice of showing the related view also. To hide/show views:
1.
Right-click the view on the sheet or in the FeatureManager design tree, and select Hide View. If the view has dependent views (Detail, Section, and so on), you are asked if you want to hide the dependent views as well. If the view was active when you hid it, the active view boundary (gray shadowed) is displayed. Otherwise, the view and boundary are invisible. To see where hidden views are placed on the sheet without displaying them, click View, Show Hidden Views. The boundaries of hidden views are displayed with an X.
The pointer changes to 2.
and the view boundary highlights when the pointer passes over a hidden view.
To show the view again, right-click the view, and select Show View. If the view has dependent views (Detail, Section, and so on), you are asked if you want to show the dependent views as well.
Hiding and Showing Edges To hide or show edges:
1.
Select an edge and click Hide Edge Edge.
on the Line Format toolbar, or right-click an edge and select Hide
The edge is removed from the display, but it still is highlighted when the pointer passes over it. 2.
To display the edge again, select the edge and click Show Edge Edge.
, or right-click the edge and select Show
If you cannot select the hidden edges, click Tools, Options, System Options, Drawings. Make sure that the Select hidden entities check box is selected. Showing or hiding an edge is a valid operation only if the edge would be shown in the view mode. For example, if the edge is hidden and the view mode is Hidden Lines Removed, you cannot show or hide the edge.
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Chapter 11 Drawings
Hiding and Showing Sketches You can show and hide model sketches in drawings. SolidWorks lists the sketches in the FeatureManager design tree but hides them in the graphics area by default. To show a sketch in a drawing:
Right-click the sketch in the FeatureManager design tree and select Show Sketch. NOTE: The sketch entities highlight in the graphics area when you point over the sketch name in the FeatureManager design tree. Drawing view with sketch hidden
Sketch shown
To hide a sketch in a drawing:
Right-click the sketch in the graphics area or in the FeatureManager design tree and select Hide Sketch. To show or hide dimensions of model sketches in drawings:
Right-click the sketch in the FeatureManager design tree (or in the graphics area if the sketch is shown) and select Show Dimensions or Hide Dimensions. When you insert model dimensions in a drawing, SolidWorks includes dimensions for all features and sketches. NOTE: SolidWorks does not insert dimensions for hidden, unabsorbed sketches. To insert dimensions for unabsorbed model sketches in a drawing:
1.
Right-click any unabsorbed sketches in the FeatureManager design tree and select Show Sketch.
2.
Click Model Items
3.
Hide the sketches or dimensions, or both, as necessary.
or Insert, Model Items, select Dimensions, and click OK.
Unabsorbed sketch with dimensions inserted
Show Hidden Edges You can show all the hidden lines of selected features and components in drawing documents. You can access this feature in two ways. To show or hide hidden edges from the shortcut menu:
Right-click a feature or component in the drawing view or in the FeatureManager design tree and select Show/Hide, Show Hidden Edges. If the hidden edges are visible, you can hide them again by right-clicking the feature or component and selecting Show/Hide, Hide Hidden Edges.
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To show or hide hidden edges in the Drawing View Properties dialog box:
1.
Right-click the drawing view and select Properties.
2.
Select the Show Hidden Edges tab.
3.
Select a feature or component from either the drawing view or the FeatureManager design tree to add it to the list of items to be shown with hidden lines.
4.
Click Apply to see the effect of your selection.
5.
To hide the hidden lines again, select an item from the list and press Delete. - or Select the feature or component in the drawing view or the FeatureManager design tree.
6.
Click OK to close the dialog box.
Hide/Show Components You can hide or show components in an assembly drawing. A quick selection method for hiding components is Hide Behind Plane. You can set an option in Tools, Options, System Options, Drawings to list hidden components automatically when you create a drawing view. New drawing views with the Automatic hiding of components on view creation check box selected display the list of hidden components on the Hide/Show Components tab in the Drawing View Properties dialog box. You can access Hide/Show Components in two ways. To show or hide a component from the shortcut menu:
Right-click a component in the drawing view or in the FeatureManager design tree and select Show/Hide, Hide Component. If the component is hidden, you can show it again by right-clicking the component in the FeatureManager design tree (not in the drawing view) and selecting Show/Hide, Show Component. To show or hide a component in the Drawing View Properties dialog box:
1.
Right-click the drawing view and select Properties.
2.
Select the Hide/Show Components tab.
3.
Select a component from either the drawing view or the FeatureManager design tree to add it to the list of items to be hidden.
4.
Click Apply to see the effect of your selection.
5.
To show the component again, select the component in the Hide/Show Components list and press Delete. - or Select the component in the FeatureManager design tree.
6.
Click OK to close the dialog box.
NOTE: You can hide or show surfaces in part and assembly documents without affecting their drawings. In a part or assembly document, right-click a surface and select Hide Surface Body. The surface remains visible in the associated drawing. To show the surface again, right-click the surface in the FeatureManager design tree and select Show Surface Body. Hide Behind Plane You can hide components of an assembly drawing behind a plane. This procedure is a quick selection method for Hide/Show Components. Only those components that are completely behind the plane are hidden. You can choose the direction to hide and the position of the plane. The X, Y, and Z coordinates of the plane distance are shown in the dialog box.
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Example of Hide Behind Plane The plane in the isometric view will hide components in the direction of the arrow. The plane and arrow are also displayed in the other views to aid in locating the components to be hidden.
The resulting isometric view.
To hide components behind a plane:
1.
In the FeatureManager design tree, right-click a plane under the view in which you want to hide components and select Hide Behind Plane. The Hide Behind Plane dialog box appears, and the plane and direction arrow are displayed in all views on the drawing sheet that contain the model.
2.
Change the distance of the plane in the Distance box to move the plane, if necessary. The X, Y, Z coordinates of the plane appear in the Plane point section, and the plane is displayed in the new location in all the views on the drawing sheet.
3.
Select the Reverse direction check box, if necessary.
4.
Click OK.
To show the components again:
1.
Right-click the view, and select Properties. The Drawing View Properties dialog box appears.
11-54
2.
Select the Hide/Show Components tab.
3.
Select all the items in the list that are behind the plane and press Delete.
4.
Click OK.
Displaying Component Line Font The Component Line Font dialog box lets you change the line font style of edges on each of the components in an assembly drawing. To change the font style of component edges:
1.
Right-click a component in a drawing view and select Component Line Font. The Component Line Font dialog box appears.
2.
Choose from the following Component Display Properties and click OK.
Use document defaults - when selected, other choices in the dialog box are ignored. Type of edge - select one or more type of edge (Visible Edges, Hidden Edges, and so on) from the list. Line style - select a style (Solid, Dashed, and so on) from the list. Line weight - select a weight (Normal, Thin, and so on) from the list. The line you select is displayed in the Preview box. NOTE: Click Reset to return Line style and Line weight to the defaults you set in Tools, Options, Document Properties, Line Font. Drawing view - choose to apply the changes to the drawing view From selection or to All views. Layer - if the component is in a layer, the name of the layer appears in the box. You can change the layer for the component by selecting a named layer from the list. NOTE: Selections for line style and line weight in the Component Line Font dialog box take precedence over those set in Layers properties. Drawing View Display Modes You can display drawing views in the following modes, from either the View toolbar or in the view PropertyManager: Wireframe Hidden Lines Visible Hidden Lines Removed Shaded With Edges Shaded When in Hidden Lines Visible or Hidden Lines Removed mode, you can select a style for Tangent Edge Display. Shaded mode is available for the following types of view: •
Model View
•
Standard 3 View
•
Projected View
•
Auxiliary View
•
Section View
•
Relative View
You can set the default display mode for drawings in Tools, Options, System Options, Display Style.
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Chapter 11 Drawings
Line Format You can specify the color, thickness, and style in drawings for: •
System settings for new sketch entities
•
Entities in layers
•
Properties of existing lines, edges, and sketch entities
You can specify the color for notes and other annotations in either layers or with the Line Color tool. The settings for the line formats are either: •
•
globally controlled - set in either: o
Layers
o
Tools, Options, System Options, Colors and Display Style
explicitly controlled - set by the Line Format tools
The following settings apply if the Default check box in a Line Format tool dialog box is: •
•
Selected o
Layer settings - if the entity is in a layer
o
System settings - if the entity is not in a layer
Cleared o
Line Format tool settings - set explicitly for the entity
When you add new sketch entities to a drawing, the line format follows the Layer settings. If no layer is active, the line format follows the system settings. For existing lines, edges, and sketch entities, the line format tool settings override layer specifications and system settings. Another method of setting line properties for assembly components in drawings is with Component Line Font. Format tools The tools on the Line Format toolbar change the following formats.
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•
Layer Properties. Set layer properties (Color, Thickness, and Style), move entities into layers, and select a layer for new entities.
•
Line Color. Choose a color from the palette, or select Default. You can toggle between the specified color and the system default colors with the Color Display Mode tool (below).
•
Line Thickness. Choose a thickness or Default from the menu. As you move the pointer over the menu, the thickness name (Thin, Normal, Thick, and so on) is displayed in the Status bar. Corresponding line weights for printing are defined in File, Print, Line weights.
•
Line Style. Choose a style or Default from the menu. As you move the pointer over the menu, the corresponding line style name (Solid, Dashed, Phantom, and so on) is displayed in the Status bar.
•
Color Display Mode. Click this tool to toggle between aesthetic colors (colors chosen in layers or with Line Color) and the system status colors (fully defined, under defined, and so on). Sketch endpoints and dangling dimensions are always in the system status color.
To specify the format for new sketch entities in the current and future drawings:
1.
Click outside the drawing sheet to activate the Line Format tools.
2.
Click a tool on the Line Format toolbar and select a format from the menu.
3.
Sketch entities of any type (lines, centerlines, circles, and so on) that you add to the drawing use the specified formats, until you select a different format.
To change the format of an existing line, edge, or sketch entity:
1.
Select the line, edge, or sketch entity you want to change. To select more than one entity at a time, hold Ctrl as you select.
2.
Click a tool on the Line Format toolbar and select a format from the menu. The new format is applied to the selected entities.
Tangent Edge Display Overview Tangent edges are transition edges between rounded or filleted faces in drawing views in Hidden Lines Removed or Hidden Lines Visible display modes. Tangent edges can be displayed as follows: •
Visible - a solid line
•
Use font - a line in the default font defined in Tools, Options, Document Properties, Line Font.
•
Removed - not displayed Visible
Use font
Removed
Tangent edges are always Visible in Isometric, Trimetric, and Dimetric oriented views. You can control tangent edge display in the following ways: •
Default - to set the display for all new drawing views, click Tools, Options, System Options, Display Style, and choose one of the options under Default display of tangent edges in new drawing views. In new installations, when you insert views into drawings, a dialog box appears so you can set the tangent edge display for the current view and future views.
•
Views - to set the display for an individual view in a drawing, right-click the view in either the graphics area or the FeatureManager design tree and select Tangent Edge, then choose one of the three tangent edge display modes.
Tangent Edge Display Select one of the display types as the default for tangent edges (transition edges between rounded or filleted faces in Hidden Lines Removed and Hidden Lines Visible display modes) for the current drawing view and for future views. •
Visible - a solid line
•
Use font - a line in the default font defined in Tools, Options, Document Properties, Line Font.
•
Removed - not displayed
As you select each button, the display is previewed in the drawing.
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The default in this dialog box is the default in the system options in Tools, Options, System Options, Display Style. Your choice in the dialog box becomes the new system option. You can control the default in either the dialog box or the system options. Don't ask me again. Select to prevent this dialog box from appearing each time you insert a drawing view. Layers You can create layers in a SolidWorks drawing document. You assign a line color, line thickness, and line style for new entities created on each layer. New entities are automatically added to the active layer. You can hide or show individual layers. You can move entities from one layer to another. •
Dimensions and annotations (including notes, area hatch, blocks, break lines, cosmetic threads, detail circles, section lines, and tables) can be moved onto layers; they use the color specified for the layer.
•
Sketch entities use all the properties of the layer.
•
Components, in either part or assembly drawings, can be moved onto layers. The Component Line Font dialog box includes a list for selecting a named layer for the component.
•
If you import a .dxf or .dwg file into a SolidWorks drawing, layers are created automatically. The layer information (names, properties, and entity locations) specified in the system where the .dxf or .dwg file originated is retained.
•
If you export a drawing with layers as a .dxf or .dwg file, the layer information is included in the file. When you open the file in the target system, the entities are on the same layers and have the same properties unless you use mapping to redirect the entities to new layers.
To create a drawing layer:
1.
In a drawing, click Layer Properties
on either the Layer toolbar or the Line Format toolbar.
The Layers dialog box appears. 2.
Click New, and enter the Name of a new layer. NOTE: If you save the drawing as a .dxf or .dwg file, the layer name may be changed in the .dxf or .dwg file as follows:
3.
•
All characters are converted to uppercase.
•
The name is truncated to 31 characters.
•
All spaces in the name are converted to underscores.
Specify the line format for entities on that layer as follows: •
To add a description, double-click in the Description column and type text.
•
To specify the line color, click the Color box, select a color, and click OK.
•
To specify the line style or thickness, click in the Style or Thickness column, and select the desired style or thickness from the list.
Active. An arrow
indicates which layer is active. To activate a layer, double-click beside the layer name.
Visible. A yellow lightbulb appears with any layer that is visible. To hide a layer, double-click its lightbulb. The lightbulb turns gray, and all the entities on the layer are hidden. To turn the layer back on, double-click the lightbulb again. Move. To move entities to the active layer, select the entities in the drawing and click Move. Delete. To delete a layer, select the layer name and click Delete.
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12 Detailing
Detailing Overview Detailing Overview You can add much of the necessary detailing of your models in part and assembly documents. This includes dimensions, notes, symbols, and so on. Then you can insert the dimensions and annotations from the model into a drawing. Once in the drawing, you can add reference dimensions, other annotations, and a bill of materials if required. Annotations and reference dimensions added in a drawing do not affect the part or assembly document. For drawings, sheet formats, and drawing views see Drawings.
Setting Detailing Options You can set options for various aspects of detailing. The options affect only the active document. To set detailing options:
1.
Click Tools, Options. On the Document Properties tab, select: •
Detailing - standards, trailing zeros, extension lines, and so on
•
Dimensions - text alignment, leaders, arrow styles and so on
•
Notes - text alignment, leaders, and borders
•
Balloons - balloon styles, sizes, and contents, and so on
•
Arrows - arrow sizes, styles, and attachments
•
Virtual Sharps - virtual sharp display styles
•
Annotations Display - display filter, text scale, and so on
•
Annotations Font - fonts for Note, Dimension, Detail, and so on
•
Tables - various controls for Hole Tables, Revision Tables, and Bills of Materials
•
View Labels - label content and format for Detail, Section, and Auxiliary view labels
2.
Change the options as necessary.
3.
Click OK to apply the changes and close the dialog box.
Inserting Model Items You can insert dimensions, annotations, and reference geometry from a model document (part or assembly) into a drawing. You can insert items into a selected feature, an assembly component, a drawing view, or all views. You can select a feature, component, or view in the graphics area or in the FeatureManager design tree. For directions, see Insert Model Items.
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Chapter 12 Detailing
Insert Model Items You can insert dimensions, annotations, and reference geometry from the model into the current drawing. You can insert items into a selected feature, an assembly component, a drawing view, or all views. When inserting into all views, dimensions and annotations appear in the most appropriate view. Features that appear in partial views, such as Detail or Section views, are dimensioned in those views first. To insert existing annotations or reference geometry into a drawing:
1.
Preselect views as follows: •
To annotate a single feature or assembly component, select the item.
•
To annotate a single drawing view, select the view.
•
To annotate all the views at once, do not select anything. NOTE: Dimensions are inserted for unabsorbed model sketches only if the sketch is visible in the drawing. To insert dimensions for an unabsorbed sketch, right-click the sketch in the FeatureManager design tree and select Show Sketch before inserting the dimensions. Dimensions belonging to an unabsorbed sketch are shown or hidden depending on the state of Show Sketch or Hide Sketch. You can also show or hide dimensions regardless of whether the sketch is shown or hidden. Right-click the sketch and select Show Dimensions or Hide Dimensions.
2.
Click Model Items
on the Annotation toolbar, or click Insert, Model Items.
The Insert Model Items dialog box appears. 3.
4.
Select the All types check box, or select individual types of items to insert: •
Annotations - Cosmetic thread (assemblies only), Datums, Datum targets, Dimensions, Geometric tolerances, Notes, Surface finish, Welds. If you select Dimensions, you have the option of also inserting Instance/Revolution counts if those dimensions exist in the part or assembly, Hole Wizard Profiles, and Hole Wizard Locations. Select Marked for drawing to insert only those dimensions that are marked in parts for drawings.
•
Reference Geometry - Axes, Curves, Planes, Surfaces, Routing points, Origins.
Choose other options as required: •
Layers - Select a layer from the Layers list (available if your drawing has layers) for the items to be inserted only in the specified layer.
•
Import from - If you have preselected a component or feature, you can select one of the following options: o o
o o
•
12-2
Entire model. Displays all of the selected item types that exist in the model. Selected component. If this drawing is of an assembly, displays the items that exist on the selected component only. Selected feature. Displays the annotations existing on the selected feature only. Only Assembly. When selected, annotations in the assembly are inserted. Annotations that were created in parts or subassemblies are not inserted. Reference dimensions created in the assembly, dimensions referring to mates, and dimensions referring to in-context features created in assemblies are inserted.
Include items from hidden features - To prevent the insertion of annotations that belong to hidden model items, clear the Include items from hidden features check box. Annotations on features that are completely hidden by other geometry are not inserted. The insertion operation is slower when the software filters out hidden features, but the resulting views do not contain inappropriate annotations.
•
Import items into all views - Change the selection of views if necessary. To insert dimensions into selected views, clear the Import items into all views check box, then click the desired views in the graphics area or FeatureManager design tree. The selected views are listed in the Import into views box. Click the views again to remove them from the list; right-click the drawing sheet, and select Clear selections to remove all the views from the list. NOTE: When Selected Feature or Selected Component is checked, annotations for the item are displayed only in the view where you selected the item. You cannot select a different view or all views.
•
5.
Eliminate duplicate model dimensions - When the Eliminate duplicate model dimensions check box is selected, duplicate dimensions are not inserted into drawings when model dimensions are inserted. The default for this check box follows the Eliminate duplicate model dimensions on insert option in Tools, Options, System Options, Drawings.
Click OK.
Attachment points of imported annotations can be dragged, but not re-attached to another edge, face, vertex, and so on. You can toggle the visibility of individual reference geometry items. Right-click the item, and select Hide or Show. Imported annotations display in the default Imported Annotations (Driving) or Imported Annotations (Driven) color; reference annotations (added in the drawing) are displayed in the default Imported Annotations (Driven) color. These colors are specified in Tools, Options, System Options, Colors.
Inserting Annotations into Drawings You can add all types of annotations to a drawing document. You can add most types in a part or assembly document, then insert them into a drawing document. However, there are some types, such as Center Marks, Area Hatch, and Blocks, that you can add only in a drawing document. Annotations behave like dimensions in all types of SolidWorks documents. You can add dimensions in a part or assembly document, then insert them into the drawing, or you can create dimensions in the drawing. When inserted into all views, annotations appear in the most appropriate view.
Inserting Dimensions into Drawings Dimensions in a SolidWorks drawing are associated with the model, and changes in the model are reflected in the drawing. Typically, you create dimensions as you create each part feature, then insert those dimensions into the various drawing views. Changing a dimension in the model updates the drawing, and changing an inserted dimension in a drawing changes the model. By default, inserted dimensions are black. This includes dimensions that are blue in the part or assembly document (such as the extrusion depth). Reference dimensions are gray and appear with parentheses. Dimensions are inserted only once for a part, even if the part shows in multiple instances in an assembly. Linear dimensions that have the same value and that could overlap or be parallel are not inserted. When you insert dimensions into all views, the dimensions appear in the most appropriate view. Features that appear in partial views, such as Detail or Section views, are dimensioned in those views first. When you insert dimensions into selected views, you can insert the dimensions for the entire model, or you can selectively insert the dimensions for one or more components (in an assembly drawing) or features (in a part or assembly drawing). Dimensions are placed only in the views where they are appropriate. Duplicate dimensions are not inserted automatically. Once a dimension has been inserted into one view, it is not inserted again into another view. You can delete a dimension from one view, then insert it into a different view, or you can move or copy it to another view.
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Chapter 12 Detailing
Inserting Reference Geometry into Drawings The reference geometry contained in a model is hidden by default in drawing views. When you insert reference geometry from the model, all entities of the selected types are shown. When you insert reference geometry into drawings, planes, axes, curves, and points are shown in gray. Surfaces are shown as visible lines (black). To toggle the display status of an individual reference geometry entity, right-click the entity in the FeatureManager design tree, and select Hide or Show.
Favorites You can define favorite styles, similar to paragraph styles in word processing documents, for dimensions and various annotations (Notes, Geometric Tolerance Symbols, Surface Finish Symbols, and Weld Symbols). With favorites, you can: •
Save any dimension or annotation property as part of a favorite.
•
Name favorites so that they can be referenced.
•
Apply favorite styles to multiple dimensions or annotations.
•
Add, update, and delete favorite styles.
•
Save and load favorite styles. You can also load styles saved from other documents and located in other folders.
The functionality of favorites includes: •
When adding a dimension or annotation, you can preselect an item that uses a favorite, and that favorite becomes the default for the new item. If you click a location first, no favorite is used for new items.
•
You cannot apply favorites to dimensions created by Hole Callouts.
•
When you insert dimensions from a part or assembly into a drawing with Insert Model Items, the dimensions' favorites belong to the original model. Therefore, you cannot assign drawing favorites to the inserted dimensions. You can load the part or assembly favorites into drawings. Changes to the favorites in the drawings change the favorites in the part or assembly document.
The extensions for favorites are: Dimensions
.sldfvt
Notes
.sldnotfvt
Geometric Tolerance Symbols
.sldgtolfvt
Surface Finish Symbols
.sldsffvt
Weld Symbols
.sldweldfvt
To add a favorite to a document:
1.
Select one or more dimensions or annotations.
2.
Edit the dimension or annotation properties in the PropertyManager or dialog box.
3.
Click Add or Update a Favorite
4.
In the dialog box, type a name under Enter a new name or choose an existing name and click OK.
.
To apply a favorite to a dimension or annotation:
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1.
Select one or more dimensions or annotations.
2.
In the PropertyManager or dialog box, select a favorite in Set a current Favorite.
To save a favorite:
1.
With a favorite displayed in Set a current Favorite, click Save a Favorite
.
2.
In the Save As dialog box, browse to the folder where you want to save the file, edit the file name if necessary, and click Save.
To load a favorite:
1.
Click Load Favorites
.
2.
In the Open dialog box, browse to the appropriate folder and select one or more files. You can select multiple favorite files by using Shift or Ctrl.
3.
Click Open. The loaded favorites appear in the Set a current favorite list.
To update a favorite style:
1.
Select a dimension or annotation with the favorite style.
2.
Edit the dimension or annotation properties.
3.
Click Add or Update a Favorite
4.
Select the favorite name from the list, select Update all annotations linked to this favorite, and click OK.
.
To break association with a favorite:
1.
Click Add or Update a Favorite
.
2.
Select the favorite name, select Break all links to this favorite, and click OK. Dimensions and annotations retain the properties previously applied by the favorite unless the items are reset to the document default (see below).
To delete a favorite:
1.
Select a style from Set a current Favorite.
2.
Click Delete a Favorite
.
The current favorite is set to
1.
Select dimensions or annotations with favorite styles.
2.
Click Apply the default attributes to selected items
.
The style is reset to
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Chapter 12 Detailing
Add or Update a Favorite Enter a new name or choose an existing name Type a name to add a new favorite to the current document. - or Choose a favorite from the list to apply one of the following actions. •
Update all annotations linked to this favorite. All annotations using the selected favorite style are updated with the changes to the selected annotation.
•
Break all links to this favorite. All links between the selected favorite and annotations are broken. The annotations retain the attributes previously applied by the favorite unless the annotations are subsequently reset to the document default.
Dimensions in Drawings Dimensions Overview Dimensions in a SolidWorks drawing are associated with the model, and changes in the model are reflected in the drawing. Model Dimensions. Typically, you create dimensions as you create each part feature, then insert those dimensions into the various drawing views. Changing a dimension in the model updates the drawing, and changing an inserted dimension in a drawing changes the model. Mark for Drawings. When creating dimensions in part sketches, you can specify whether the dimension should be included when inserting model dimensions into drawings. Right-click the dimension and select Mark for drawing. You can also specify that dimensions marked for drawings be inserted automatically into new drawing views. Click Tools, Options, Document Properties, Detailing and select Dimensions marked for drawings under Auto insert on view creation. Reference Dimensions. You can also add dimensions in the drawing document, but these are reference dimensions, and are driven; you cannot edit the value of reference dimensions to change the model. However, the values of reference dimensions change when the model dimensions change. Color. By default, model dimensions are black. This includes dimensions that are blue in the part or assembly document (such as the extrusion depth). Reference dimensions are gray and appear with parentheses by default. You can specify colors for various types of dimensions in Tools, Options, System Options, Colors and specify Add parentheses by default in Tools, Options, Document Properties, Dimensions. Arrows. Circular handles appear on dimension arrows when dimensions are selected. When you click on an arrowhead handle (on either handle if there are two for the dimension), the arrows flip outside or inside. When you right-click on a handle, a list of arrowhead styles appears. You can change the style of any dimension arrowhead individually by this method. Selection. You can select dimensions by clicking anywhere on the dimension, including dimension and extension lines and arrows. Hide and Show Dimensions. You can hide and show dimensions with Hide/Show Annotations on the Drawing toolbar or View menu. You can also right-click a dimension and select Hide to hide the dimension. Hide and Show Lines. To hide a dimension line or extension line, right-click the line and select Hide Dimensions Line or Hide Extension Line. To show hidden lines, right-click the dimension or a visible line and select Show Dimension Lines or Show Extension Lines. Angular Dimension Display. You can change a dimension from diameter to radius or linear display and vice versa in the Dimension Properties dialog box or on screen. On screen, right-click an angular dimension and select:
12-6
•
Display As Diameter
•
Display As Radius
•
Display As Linear
Slant. When you insert or select dimensions, handles appear so you can drag the dimension to slant the extension lines. See the section on Display Options for removing the slant. Display Options. Right-click a dimension and select Display Options. The choices available depend on the type of dimension and other factors and can include the following: •
Remove Slant
•
Center Dimension
•
Offset Text
•
Change Plane
•
Align Ordinate
•
Add to Ordinate
•
Jog
•
Re-Jog Ordinate
•
Show Parentheses
•
Show as Inspection
Link external dim text. You can right-click the top-level icon in a drawing FeatureManager design tree and select or clear Link external dim text to control whether text added to a dimension is displayed. Text added to a dimension in a drawing becomes an attribute of the dimension. The default is to have the option enabled.
Setting Dimensions Options You can set options for dimensions in the current document. You can also specify properties for specific dimensions in a document, either in the Dimension Properties dialog box or in the PropertyManager. To set options for the current document:
1.
Click Tools, Options, Document Properties, Detailing, Dimensions.
2.
Change selections, offset distances, arrows, and so on.
3.
Click OK.
To set properties in the Dimension Properties dialog box:
1.
Right-click a dimension and select Properties. The Dimension Properties dialog box appears. NOTE: You can select more than on dimension by holding Ctrl while clicking dimensions. Some properties are not available for multiple dimensions.
2.
Change units, precision, arrow style, and so on.
3.
Click OK.
To set dimension properties in the PropertyManager:
1.
In the drawing graphics area, select a dimension. - or Hold Ctrl to select multiple dimensions. The Dimension PropertyManager appears.
2.
Change the dimension tolerance, precision, arrow style, and so on. The changes appear in the graphics area.
3.
Click More Properties to open the Dimension Properties dialog box.
4.
Click OK
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or click in the graphics area to close the PropertyManager.
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Chapter 12 Detailing
Dimension PropertyManager In the Dimension PropertyManager, you can specify the display of dimensions. If you select multiple dimensions, only the properties that apply to all the selected dimensions are available. Dimension Favorite •
Apply the default attributes to selected dimensions the document defaults.
. Reset the selected dimension or dimensions to
•
Add or Update a Favorite
•
Delete a Favorite
•
Save a Favorite . Opens the Save As dialog box with favorite (.sldfvt) as the default file type to save an existing favorite.
•
Load Favorites . Opens the Open dialog box with favorite (.sldfvt) as the active file type. You can use Ctrl or Shift to select multiple files.
•
Set a current Favorite. Choose a favorite style from the list to apply to the selected dimension or dimensions, or to delete or save the favorite.
. Opens the Add or Update a Favorite dialog box.
. Deletes the selected favorite from the document.
Tolerance/Precision Tolerance Type . Select from the list (None, Basic, Bilateral, Fit, and so on). The list is dynamic. For example, types for chamfer dimensions are limited to None, Bilateral, and Symmetric. Maximum Variation
. Type in a value.
Minimum Variation
. Type in a value.
Primary Unit Precision value. Tolerance Precision
. Select the number of digits after the decimal point from the list for the dimension . Select the number of digits after the decimal point for tolerance values.
Classification . Available only for Fit, Fit with tolerance, or Fit (tolerance only) types. Classification can be User Defined, Clearance, Transitional, or Press. Select a classification from the list. When you select either Hole Fit or Shaft Fit (below), the list for the other category (Hole Fit or Shaft Fit) is filtered based on the classification. Hole Fit and Shaft Fit from the lists, or type any text.
. Available only for Fit, or Fit with tolerance, or Fit (tolerance only) types. Select
NOTE: Bilateral tolerances (Maximum Variation and Minimum Variation) and parentheses are available in the Fit with tolerance or Fit (tolerance only) type if you specify Hole Fit or Shaft Fit, but not both. Fit tolerance display. Available only for Fit or Fit with tolerance types. Choose from: Stacked with line display Stacked without line display Linear display Show parentheses. Parentheses are available for Bilateral, Symmetric, and Fit with tolerance tolerance types. When selected, parentheses bracket the tolerance values.
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Second Tolerance/Precision A second Tolerance/Precision section is available for Chamfer Dimensions. Fit and Fit with tolerance types are not available for chamfer dimensions. Dimension Text Text. The dimension appears automatically in the center text box, represented by
For some types of dimensions, additional text appears automatically. For example, a Hole Callout for a counterbore hole or a hole with blind depth displays the diameter and depth of the hole (represented by <MOD-DIAM>
Horizontal - Left Justify
•
Vertical - Top Justify
, Center Justify , Middle Justify
, Right Justify , Bottom Justify
Symbols. Click to place the pointer where you want a symbol. Click a symbol icon (for Diameter, Degrees, and so on) or click More to access the Symbol Library. The symbol is represented by its name in the text box, but the actual symbol appears in the graphics area. Chamfer Dimension Display. Choose from: Distance X Distance Distance
, or Chamfer
, Distance X Angle
, Angle X
(available only for chamfers with 45° angles, generally used in JIS standard).
Arrows Placement. Click Outside
, Inside
, or Smart
.
The type of arrows and leaders available depends on the type of dimension selected. For example, the following types are available for Chamfer Dimensions: Horizontal Text Horizontal, Underlined Text Angled Text Angled, Underlined Text Style. Select an arrow style from the list. The default style is the specified style for the dimensioning standard (ISO, ANSI, and so on). Layer In drawings with named layers, select a layer.
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Chapter 12 Detailing
Break Dimension Lines Break Dimension Lines. Select for the dimension extension lines to break when crossing other extension lines in drawings. You can choose for the extension lines to break only when crossing arrowheads. Click Tools, Options, Document Properties, Dimensions and select Break around arrow head only. For ANSI standard, the check box is selected by default. Use document's gap. Select to use the document default set in Tools, Options, Document Properties, Dimensions. Gap. Enter a value if you do not use the document's default. When the dimension lines are broken, they break around lines that are nearby. If a dimension is moved significantly, it may not break around the new nearby dimensions. To update the display, unbreak the dimension lines and then break them again. More Properties Click More Properties to open the Dimension Properties dialog box.
Symbol Inserts a symbol into a dimension, a note, a geometric tolerance symbol, and so on. The libraries include ANSI, GOST, ISO, JIS, hole, key, modifying, and flag symbols. Flag symbols contain: •
A letter or number
•
A period or no period
•
A border (a circle, a square, both a circle and a square, a triangle, or a rotated triangle)
To add a symbol to text:
1.
Select a library from the Symbol libraries list.
2.
Select a symbol name from the list, and click OK. The selected symbol appears in the preview box. The symbol is represented by its name in the Note text preview box, but the actual symbol appears in the drawing note.
To delete a symbol that currently appears in text:
In the Symbol dialog box, select No Symbol and click OK. For dimensions, you can delete symbols in the Dimension PropertyManager. For a Note, you can double-click the note and delete the symbol code in the on-screen editor.
Dimension Properties To modify the dimension properties, do one of the following:
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•
Right-click a dimension and select Properties.
•
Select multiple dimensions while holding down Ctrl, then right-click one of the selected dimensions, and select Properties. You can view and make changes to any properties that the selected dimensions have in common.
•
Select a dimension, or multiple dimensions. The Dimension PropertyManager appears. Click More Properties to open the Dimension Properties dialog box.
The following options are available for all dimensions: Value
Display as inspection dimension
Name
Read only
Full Name Units Font Arrow Style Arrows Precision
Display
Modify Text
Tolerance
Depending on the type of dimension (linear, radius, reference, and so on) or the type of document, the following options may be available: Driven
Diameter dimension
Specify Configs Display with parentheses
Foreshortened radius
Display as dual dimension
Dimension to inside of arc
Display with solid leader
Display as linear dimension
Use document's second arrow
First arc condition, Second arc condition
Display second outside arrow Display as chain dimension
Layer
Value The current value of the dimension. To change the value, either type a new value or use the arrows to increment the value. (Not available if you select multiple dimensions.) Name The name of the dimension (used in equations and design tables). To change the name, type a new name. (Not available if you select multiple dimensions.) Full Name The dimension name plus the name of the feature or sketch the dimension is associated with. (Read only. Not available if you select multiple dimensions.) Units Either select Use document’s units, as defined in the Dimension Options, or clear this check box and click Units to specify the unit type for the selected dimension. The available options depend on the type of dimensions that you selected. For example, an Angular Unit can be Deg, Deg/Min, Deg/Min/Sec, or Radians. A Length Unit can be Angstroms, Nanometers, Microns, Millimeters, Centimeters, Meters, Microinches, Mils, Inches, Feet, or Feet & Inches. For feet and inch units, you can choose Decimal or Fraction; if Fraction, you can specify the Denominator.
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Font Either select Use document’s font, as defined in the Dimensions Options, or clear this check box and click Font to select a new font type, style, and size for the selected items. Arrow Style You can change an arrow style in either the Dimension PropertyManager or the Dimension Properties dialog box. •
In the Dimension PropertyManager, under Arrows, select a style from the list.
•
In the Dimension Properties dialog box, under Arrow style, select or clear Use document's style. o
Select to use the style in Arrows Options.
o
Clear to choose a new style from the lists.
Two lists of arrow styles appear in the Dimension Properties dialog box. You can choose separate styles for each arrow when there are two arrows for a dimension. This feature supports the JIS dimensioning standard. Two lists appear in the Dimension PropertyManager only when separate styles are specified by the dimensioning standard. Arrows You can specify placement of arrows with respect to the dimension extension lines: Inside, Outside, Smart, or Document (uses the document defaults, as defined in the Detailing Options). Smart specifies that arrows automatically appear outside of extension lines if the space is too small to accommodate the dimension text and the arrowheads. Circular arrowhead handles
appear on dimension arrows when you select dimensions. The pointer changes to
when it is over the arrowhead handles. When you click on arrowhead handle (either handle if there are two for the dimension), the arrows flip outside or inside. You can change arrow styles. Display as inspection dimension Specifies whether to display the dimension as an inspection dimension.
Read only Specifies that the dimension cannot be changed. Dimension Precision Enter the number of decimal places for the precision of the dimension: •
Value
•
Tolerance
for the type of units: •
Primary Units
•
Alternate Units (in dual dimension display)
•
Angular Units
In the Dimension Options dialog box, all unit types are available. In the Dimension Properties dialog box, only those unit types that are appropriate for the selected dimensions are visible. In the Dimension PropertyManager, only the primary dimension and tolerance are visible. You can choose Same as nominal for the tolerance precision, so that if the precision of the dimension value changes, the precision of the tolerance changes with it. In the Dimension Properties dialog box and Dimension PropertyManager, (Document) after the precision indicates that the precision is the same as the document option.
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Dimension Display The Dimension Display dialog box controls the display of extension lines and leader lines. To access this dialog box, click Display in the Dimension Properties dialog box. •
Extension Lines. Select to display the first or second extension lines, or both.
•
Dimension Lines. Select to display the first or second dimension lines, or both.
•
Smart display of extension lines. Clear to enable manual placement of extension lines.
•
Use document's bend length. Clear so you can specify the dimension bent leader length. Type a value in the box.
•
Center between extension lines. Select so that dimensions are automatically centered between extension lines.
•
Dimension display. Select Use document's dimension display, or select one of the display styles available.
Driven Specifies that the dimension is driven by other dimensions and conditions, and cannot be changed. Display with parentheses Specifies whether to display the dimension as a reference dimension (with parentheses). Display as dual dimension Specifies that the dimension is displayed in both the document's unit system and the dual dimension units. Both units are specified in Tools, Options, Document Properties, Units. Display with solid leader Specifies the display of a solid line across the circle when its radial dimension uses outside arrows. Not available with ANSI standard.
Use document's second arrow Specifies that a diameter dimension (displayed as radial, not linear) with outside arrows follows the document default setting for use of a second arrow. To specify the document's default setting, click Tools, Options, and on the Document Properties tab click Dimensions. In the Arrows section, select the Display 2nd outside arrow (Radial) checkbox. To override the document default, clear the Use document's second arrow check box, then use the Display second outside arrow check box to turn the arrow display on or off. NOTE: This option is not visible in the DimensionProperties dialog box unless the selected dimension is a radial dimension.
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Display second outside arrow Specifies the display of a second arrow for a diameter dimension (displayed as radial, not linear) with Outside arrows. This is available only when the Use document's second arrow check box is cleared.
Second arrow ON
Second arrow OFF
Display as chain dimension Displays ordinate dimensions with an arrow from the base point to the dimension position. The measurement of the dimensions is from the base ordinate (the 0.0 mark). When you change this option for one member of a group of ordinate dimensions, the change is applied to all the members.
Option selected
Option cleared
Diameter dimension Specifies that the dimension on an arc or circle displays the diameter, not the radius. To convert a diameter dimension to a radius dimension, clear this checkbox. Foreshortened radius Specifies that the radius dimension line is foreshortened (broken) when the centerpoint of a radius is outside of the drawing or interferes with another drawing view.
To change the length or angle of the segments, click the dimension and drag the handles.
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Dimension to inside of arc Specifies that the dimension arrow is inside the arc. Use this option in combination with the Arrows setting (either Inside or Outside) to meet your drawing standards.
Dimension to inside ON Arrows set to outside
Dimension to inside OFF Arrows set to outside
Display as linear dimension Specifies the display of a diameter dimension as a linear dimension (not radial).
Linear
Radial
First arc condition, Second arc condition When you are dimensioning distances to arcs or circles, the following options are available: •
First Arc Condition specifies where on the arc or circle the distance is measured.
•
Second Arc Condition specifies where on the second item the distance is measured, when both items are arcs or circles.
In these examples, the First arc condition is Center, and the Second arc condition is set as noted.
Center (default)
Min (closest point)
Max (farthest point)
Layer To move the dimension to a different layer, select the name of the layer in the Layer list.
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Dimension Units/Chamfer Dimension Units Specify the Length Unit or Angular Unit for the selected dimensions. For Chamfer Dimensions, both Length Unit and Angular Unit are available. The available options depend on the type of dimension that you select. For some length dimensions, you can choose Decimal or Fractions. For Fractions, you can specify the Denominator and whether to round to the nearest fraction.
Dimensioning to Midpoints To dimension to a midpoint of a linear edge in a drawing:
1.
Click Smart Dimension
.
2.
Right-click the edge whose midpoint you want to dimension, and click Select Midpoint.
3.
Select the second entity to dimension, then click to place the dimension.
You can also dimension to midpoints when you are adding baseline dimensions or ordinate dimensions. Select the baseline or zero ordinate. Then follow Step 2 to dimension to midpoints as needed.
Reference Dimensions Reference dimensions show measurements of the model, but they do not drive the model and you cannot change their values. However, when you change the model, the reference dimensions update accordingly. Reference dimensions of features are suppressed when the features are suppressed. Reference dimensions are enclosed in parentheses by default. To prevent parentheses around reference dimensions, clear the Add parentheses by default check box in Tools, Options, Document Properties, Dimensions. You can control the color of reference dimensions in Tools, Options, System Options, Colors. Select Imported Annotations (Driven) and click Edit. You can use the same methods to add parallel, horizontal, and vertical reference dimensions to a drawing as you use to dimension sketches. For more information, see Dimensioning in Sketches. Ordinate Dimensions and Baseline Dimensions are both types of reference dimensions in drawings. Ordinate dimensions in sketches are driving dimensions. Reference dimensions are automatically hidden when a feature is suppressed. The dimensions are shown again when the feature is unsuppressed. To add a reference dimension:
1.
Select the drawing view.
2.
Click Smart Dimension
3.
Click the items you want to dimension.
on the Dimensions/Relations toolbar.
You can dimension to a silhouette edge. Point to the silhouette edge, and when the appears, click to dimension. 4.
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Click to place the dimension.
pointer
Parentheses Reference dimensions are shown in parentheses by default. To specify the default use of parentheses for all reference dimensions in the current document, click Tools, Options, Document Properties, Dimensions. Select the Add parentheses by default check box. To specify the use of parentheses on a particular dimension:
Right-click the dimension and select Properties. In the Dimension Properties dialog box, select or clear the Display with parentheses check box. - or Right-click the dimension and select Display Options, Show Parentheses. A check mark appears beside the menu item when the parentheses are shown.
Baseline Dimensions Baseline dimensions are reference dimensions. You cannot change their values or use the values to drive the model. Baseline dimensions are automatically grouped, and they are spaced at the distances specified in Tools, Options, Document Properties, Dimensions under Offset distances. To create a baseline dimension:
1.
Click Baseline Dimension
on the Dimensions/Relations toolbar, or click Tools, Dimensions, Baseline.
2.
Click the edge or vertex you want to use as a baseline.
3.
Click each of the edges or vertices you want to dimension.
4.
Click to place the dimensions.
If you select an edge, dimensions are measured parallel to the selected edge. If you select a vertex, dimensions are measured point-to-point from the selected vertex. Edge as baseline
Vertex as baseline
Ordinate Dimensions Ordinate dimensions are a set of dimensions measured from a zero ordinate in a drawing or sketch. In drawings, they are reference dimensions and you cannot change their values or use the values to drive the model. Ordinate dimensions are measured from the axis you select first. The type of ordinate dimension (horizontal, vertical, or angular) is defined by the orientation of the points you select.
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Example of Ordinate Dimensions Dimensioned to arc, with chain
Chain removed
Zero ordinate moved
Ordinate dimensions in a sketch
You can dimension to edges, vertices, and arcs (centers and minimum and maximum points). Ordinate dimensions are automatically grouped to maintain alignment. When you drag any member of the group, all the members move together. To disconnect a dimension from the alignment group, right-click the dimension, and select Break Alignment. You can drag the zero dimension to a new position, and all the ordinate dimensions update to match the new zero position. If adjacent dimensions are very close together, the leaders are automatically jogged as needed to prevent overlapping text. Drag handles are displayed at the bends when you select an ordinate dimension with a bent leader. You can remove the bend, or add a bend to a different ordinate dimension. You can specify that the leaders not be automatically jogged by clearing Automatically jog ordinates in Tools, Options, Document Properties, Dimensions. To create ordinate dimensions:
1.
Click Ordinate Dimension Ordinate.
on the Dimensions/Relations toolbar, or click Tools, Dimensions,
You can select Horizontal Ordinate Dimension or specify the direction of the dimensions.
Vertical Ordinate Dimension to
2.
Click the first item (edge, vertex, and so on) from which all others will be measured to be the base (the 0.0 dimension), and click again to place the dimension outside the model.
3.
Click the edges, or vertices, or arcs you want to dimension using the same ordinate. As you click each item, the dimension is placed in the view, aligned to the zero ordinate.
4.
Select another mode or another tool or press Esc to exit from the ordinate mode. Newly placed ordinate dimensions automatically jog to avoid overlapping text. The size of the jog is determined by the size of the text and the potentially overlapping area of the text.
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To modify ordinate dimensions:
You can modify ordinate dimensions using commands on the shortcut menu. Right-click an ordinate dimension, select Display Options, then choose from these options: •
Align Ordinate. Aligns all the dimensions along the ordinate with the 0.0 ordinate.
•
Add to Ordinate. Adds more dimensions later, along the same ordinate.
•
Jog. Bends the leader line of a dimension and allows you to reposition the dimension.
•
Re-jog Ordinate. Applies the automatic jogging algorithm to the selected ordinate dimensions.
•
Show Parenthesis. Adds parentheses around the selected dimensions.
•
Show as Inspection. Shows the selected dimensions as inspection dimensions.
To display as chain dimensions:
1.
Right-click an ordinate dimension and select Properties.
2.
Select the Display as chain dimension check box. All the dimensions along the ordinate are affected when you select or clear this check box.
Horizontal Ordinate Dimensions Creates horizontal ordinate dimensions in a drawing or sketch, measured horizontally from the entity you select first. To create horizontal ordinate dimensions:
1.
With a drawing or sketch active, click Horizontal Ordinate Dimension toolbar, or click Tools, Dimensions, Horizontal Ordinate.
on the Dimensions/Relations
2.
Click the first item from which all others will be measured, and click again to place the dimension.
3.
Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.
Vertical Ordinate Dimensions Creates vertical ordinate dimensions in a drawing or sketch, measured vertically from the entity you select first. To create vertical ordinate dimensions:
1.
With a drawing or sketch active, click Vertical Ordinate Dimension toolbar, or click Tools, Dimensions, Vertical Ordinate.
on the Dimensions/Relations
2.
Click the first item from which all others will be measured, and click again to place the dimension.
3.
Click an item to dimension, then click to place its dimension. Repeat this step until all the remaining items are dimensioned. The dimension tool remains in ordinate mode until you select another mode or another tool.
Parallel Dimensions To add parallel dimensions to a drawing:
1.
Click Smart Dimension
, or click Tools, Dimensions, Smart.
2.
Click the geometry to dimension. As you move the pointer around the model, a preview of the dimension is displayed. The position of the pointer relative to the attachment points causes the dimension to snap to the appropriate type (horizontal, vertical, linear, radial, and so on). When the preview shows the desired dimension type, you can lock the type by right-clicking.
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3.
Click to place the dimension. To override the snap behavior before selecting the points to dimension, select either Dimension or
Horizontal
Vertical Dimension (or click Tools, Dimensions, Horizontal or Vertical).
Chamfer Dimensions You can dimension chamfers in drawings. In addition to the usual dimension display properties, chamfer dimensions have their own options for leader display, text display, and X display. X display is the size of the X in a chamfer dimension with two numbers, such as 1 X 45° (Length X Angle), 45° X 1 (Angle X Length) or 1 X 1 (Length X Length). Example of Chamfer Dimensions Chamfer dimensions can be displayed with various types of text and leaders and sizes of X.
Tolerance types for chamfer dimensions are limited to None, Bilateral, and Symmetric. You can set document default for chamfer dimension leader display, text display, and X display in Tools, Options, Document Properties, Dimensions, Leaders. To insert chamfer dimensions into a drawing:
1.
Click Chamfer Dimension Chamfer. The pointer changes to
2.
on the Dimensions/Relations toolbar or click Tools, Dimensions,
.
Select the chamfered edge, select one of the lead-in edges, then click in the graphics area to place the dimension. You must select the chamfered edge first. However, the dimension does not appear until you subsequently select one of the lead-in edges. The Dimension PropertyManager appears, and the tool remains active for you to dimension other chamfers.
3.
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Click OK
to close the Dimension PropertyManager.
Dimension Leaders/Text By default, the display of dimension text with respect to the leaders follows the selected dimensioning standard. You can override the default display. To override the default alignment for dimension text:
1.
Select Override standard’s leader display.
2.
Choose display types in each column as described below, and click OK.
Linear, Radial, and Angular Dimensions •
Solid leader, text aligned with leader
•
Broken leader, horizontal text
•
Broken leader, text aligned with leader
Chamfer Dimensions •
•
•
Leader display: o
Horizontal Text
o
Horizontal, Underlined Text
o
Angled Text
o
Angled, Underlined Text
Text display: o
Distance X Distance
o
Distance X Angle
o
Angle X Distance
o
Chamfer (available only for angles of 45 degrees)
X display: o
Uppercase X
o
Lowercase x
Leader/Text Display for Chamfer Dimensions You can select chamfer dimension leader display, text display, and X display in this dialog box. To set the document's defaults, click Tools, Options, Document Properties, Dimensions, Leaders. Leader Display Use the display specified in the document properties options, or choose from: Horizontal Text Horizontal, Underlined Text Angled Text Angled, Underlined Text You can also select these display types in the Dimension PropertyManager.
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Text display Use the display specified in the document properties options, or choose from: •
1 X 1 (Distance X Distance)
•
1 X 45° (Distance X Angle)
•
45° X 1 (Angle X Distance)
•
C1 (Chamfer distance, available only for angles of 45°) You can also select these display types in the Dimension PropertyManager.
X Display Use the display specified in the document properties options, or choose from: •
X (Uppercase)
•
x (Lowercase)
Moving and Copying Dimensions Once dimensions are displayed in a drawing, you can move them within a view or to another view. When you drag a dimension from one place to another, the dimension reattaches to the model, as appropriate. You can only move or copy dimensions to a view where the orientation is appropriate for that dimension. •
To move a dimension within the view, drag the dimension to the new position.
•
To move a dimension from one view to another view, hold the Shift key as you drag the dimension into another view.
•
To copy a dimension from one view to another view, hold the Ctrl key as you drag the dimension into another view.
•
To move or copy several dimensions at once, hold the Ctrl key as you select
Aligning Dimensions To select a group of dimensions:
You can select a group of dimensions in a drawing view either by holding the left mouse button and dragging a box around the dimensions or by holding Ctrl while selecting them. The selected dimensions must be of the same type. You can align dimensions: •
Parallel/Concentric
•
Collinear/Radial See also Ordinate Dimensions.
To identify members of an aligned group:
Right-click the dimension you want to know about. •
If the selected dimension is a member of an aligned group, you can select Show Alignment to display a blue dot on each of the other members of the group.
•
If the selected dimension is not a member of an aligned group, the Show Alignment item does not appear in the shortcut menu.
To ungroup aligned dimensions:
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•
Right-click the dimension to ungroup, and select Break Alignment. The selected dimension is disconnected from the group, and may be moved freely; the other dimensions in the aligned group remain connected.
•
To break the entire group, select all the members of the group, then right-click one and select Break Alignment.
To center dimension text between extension lines:
•
Right-click a dimension (linear, radial, or angular), and select Display Options, Center Dimension.
•
If the text is inside the extension lines (or inside the circle, in the case of a radial or diameter dimension), it snaps to the center, and is locked in position between the extension lines. If the text is outside the extension lines, it remains outside.
•
To unlock the text position, right-click the dimension, and select Center Dimension again to toggle the option.
•
You can also drag the text toward the center of the extension lines to snap it to the center. When you center dimension text this way, its position is not locked between the extension lines, so you can move it freely.
To offset dimension text from its arrows:
•
Right-click a dimension (linear, linear radial, or angular), and select Display Options, Offset Text.
•
A leader is attached to the dimension text, and you can drag the text to a new location. When you select an offset dimension, a handle is displayed where the leader attaches to the arrows so you can move the arrows away from the model if needed.
•
To restore the dimension to its position between the arrows, right-click the dimension again, and select Offset Text again to toggle the option. Before Offset
Offset
Align Dimensions Parallel/Concentric In a drawing view, you can align selected linear, radial, or angular dimensions with uniform spacing. The selected dimensions must be of the same type. To align and group parallel dimensions:
1.
In a drawing view, hold Ctrl and select two or more dimensions that you want to align. You can also select the group of dimensions by holding the left mouse button and dragging a box around the dimensions.
2.
Click Align Parallel/Concentric
or Tools, Dimensions, Align Parallel/Concentric.
The dimensions are arranged with a uniform distance between the arrows. They also are grouped, and retain the parallel spacing when moved. Aligned Parallel
Aligned Concentric
To specify the distance between dimensions:
1.
Click Tools, Options, Document Properties, Dimensions.
2.
Under Offset distances, specify a value for From last dimension (B) (the distance between dimensions). The From model (A) value (the distance between the first dimension and the model) is not used with Align Dimensions Parallel/Concentric; it is used only with baseline dimensions.
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Align Collinear/Radial Dimensions In a drawing view, aligns and groups selected linear, radial, or angular drawing dimensions. The selected dimensions must be of the same type. To align and group dimensions to be collinear:
1.
In a drawing view, select a group of dimensions.
2.
Click
or Tools, Dimensions, Align Collinear/Radial.
The selected dimensions are arranged in a straight line. They also are grouped, and retain the linear arrangement when moved.
Aligned Collinearly
Aligned Radially
Dimension Extension Lines You can change the default attachment point of dimension extension lines, slant the extension lines, flip the direction of a leader, and drag extension lines between the center, minimum, and maximum attachment points of arcs and circles. You can specify in the Dimension PropertyManager that extension lines break when they cross other extension lines and specify in Tools, Options, Document Properties, Dimensions that the lines break only around dimension arrows. You can hide and show dimension lines and extension lines. Right-click a dimension line or extension line and select Hide Dimension Line or Hide Extension Line. To show hidden lines, right-click the dimension or a visible line and select Show Dimension Lines or Show Extension Lines. To change the attachment point of dimension extension lines:
1.
Select a dimension. Handles are displayed at the attachment end of the extension lines. The pointer changes to is over a handle.
2.
Drag a handle to the desired position or to a vertex (watch for the inferencing pointer
when it
).
If you choose a vertex, the default extension line gap is used. In sketches, the value of the dimension changes to reflect the new attachment point. In drawings, you can move attachment points only for reference dimensions, and the value is not updated. To return the extension line to its original position, right-click the dimension and select Display Options, Default Extension Snap.
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To slant dimension extension lines:
When you insert or select a dimension, handles appear so you can drag the dimension to slant the extension lines. Drag a handle at the end of the extension line nearest the arrow (the pointer changes to when it is over a handle that effects the slant). To return the dimension to its original position, right-click the dimension and select Display Options, Remove Slant. You can also drag the handle until the dimension snaps back to its original position.
To flip the direction of a dimension leader:
If a vertical dimension is displayed with horizontal text (in ANSI standard, for example), you can flip the direction of the leader. Select the dimension, then click the handle at the bend in the leader (the pointer changes to over the handle).
when it is
Example of Dimension Line Terminology
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Modify Text of Dimension You can modify the text of a dimension by adding prefix or suffix text and symbols. This functionality is also available in the Dimension PropertyManager. The dimension value is represented by
1.
Place the cursor in the Dimension Text box where you want to make changes. You can make the following changes: •
Add text before or after the dimension (in the middle box).
•
Add text or symbols above or below the dimension (in the upper or lower boxes).
•
Delete the dimension. If you delete or modify the dimension, a message warns that overriding the dimension value text
2.
To add a symbol, place the cursor in the text box where you want the symbol to appear. Click the symbol buttons on the left, - or Click Add Symbol. Select a library from the Symbol Libraries list. Select a symbol name from the list, and click OK. The symbol’s name is displayed in the Dimension Text box, but the actual symbol appears in the Preview box and in the drawing.
3.
To replace the dimension value if it was deleted, click Add Value.
4.
Click OK to return to the Dimension Properties dialog box. You can observe the resulting dimension text in the Preview box as you add text and symbols.
Modify Dimension You can change a dimension in a part, sketch, assembly, or drawing in the Modify dialog box. To change a dimension:
1.
Double-click a dimension. The Modify dialog box appears.
2.
Change the dimension value with the arrows or by typing in the dimension box. NOTE: You can use the dimension box as a calculator by entering values and arithmetic symbols directly.
3.
If the model has multiple configurations, you can apply the new value to This configuration only or to All configurations, or you can Specify configurations.
4.
Use the buttons as follows: Save the current value and exit the dialog. Restore the original value and exit the dialog. Rebuild the model with the current value. Rebuild is available in drawings if the model is not being edited in another document. Reset spin increment value. Mark dimension to be imported into drawing. Available only in part and assembly documents. When you Insert Model Items into a drawing, you can insert all dimensions or only those marked.
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Specify Configurations When you modify a dimension in a model with multiple configurations, you can specify the configurations to modify from the Modify or Dimension Properties dialog boxes. To modify a dimension in specified configurations from the Modify dialog box:
1.
Double-click the dimension to modify.
2.
In the Modify dialog box: a.
Change the dimension.
b.
Select Specify Configuration(s).
c.
Click Save
.
A dialog box appears. 3.
Select the configurations to modify. NOTE: Click Reset Selection to revert to the configuration that you modified.
4.
Click OK.
To modify a dimension in specified configurations from the Dimension Properties dialog box:
NOTE: This procedure applies only when you modify a sketch dimension. 1.
Right-click the dimension to modify and select Properties.
2.
In the Dimension Properties dialog box: a.
Change the dimension Value.
b.
Click Specify Configs. A dialog box appears.
3.
Click Specify configurations.
4.
Select the configurations to modify. NOTE: Click Reset Selection to revert to the configuration that you modified.
5.
Click OK.
6.
Click OK again to close the Dimension Properties dialog box.
Increment Linear Measure: Specifies the number of units added or subtracted when you click a spin box arrow to change a linear dimension value. Angular Measure: Specifies the number of degrees added or subtracted when you click a spin box arrow to change an angular dimension value. Select the Make Default check box to make your new specification the default for dimension increments.
Hide/Show Annotations Hide/Show Annotations allows you to toggle the visibility of individual annotations (dimensions and cosmetic threads) in a drawing. Hiding a dimension has a different effect than deleting it: •
If you hide a dimension, it is still present in the view. Therefore, it is not restored if you import dimensions again.
•
If you delete a dimension, it may be restored if you import dimensions again (if it does not already appear in another view).
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To hide or display dimensions:
1.
Click Hide/Show Annotations
on the Drawing toolbar, or click View, Hide/Show Annotations.
All dimensions and cosmetic threads are displayed; hidden dimensions and cosmetic threads are in gray.
2.
Click the dimensions and cosmetic threads that you want to show or hide. You can also right-click a dimension and select Hide. To show the dimension again, use the method described above.
Dimension Tolerance The Dimension Tolerance dialog box appears in both Dimensions Options and in the Dimension Properties dialog box. It controls the dimension tolerance values and the display of non-integer dimensions. The options available depend on the type of tolerance selected and whether you are setting options or applying the specifications to selected dimensions. A window previews the dimension and the tolerances. Tolerance type Select one of the following from the list: None, Basic, Bilateral, Limit, Symmetric, MIN, MAX, or Fit, Fit with tolerance, or Fit (tolerance only). Tolerance values Specify the Maximum Variation tolerance that you selected. Hole Fit
and/or Minimum Variation
values as appropriate for the type of
and Shaft Fit
Hole Fit and Shaft Fit are available only for Fit, Fit with tolerance, or Fit (tolerance only) types for Dimension Properties only. Specify a letter. NOTE: Tolerances and parentheses are available in the Fit with tolerance type if you specify Hole Fit or Shaft Fit, but not both. Font/Fit tolerance font Specify the font to use for the dimension tolerance text. For Fit and Fit with tolerance, Fit tolerance font is available for the Hole Fit and Shaft Fit text. •
Select Use dimension’s font if you do not want to change the font size for the dimension tolerance text.
•
To change the size of the dimension tolerance text, clear Use dimension's font and select either: o
Font Scale. Enter a number from 0 to 10.0 to scale the font.
o
Font Height. Enter a value to specify the font height.
Show parentheses Select for parentheses around the tolerances for Bilateral, Symmetric, or Fit with tolerance types. Linear tolerance or Angular tolerance Choose either Linear tolerance or Angular tolerance. The available options depend on the category you select.
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Fit tolerance display Choose either Stacked with line display
, Stacked without line display
, or Linear Display
.
Fit Tolerances Fit tolerances are available for dimensions in the Dimension PropertyManager. Fit tolerances are used typically for shafts in holes. Example of Fit Tolerances Hole dimension (top), Fit tolerance with Clearance and automatically calculated bilateral tolerance.
Shaft dimension (bottom), Fit tolerance with Clearance and automatically calculated bilateral tolerance.
Shaft dimension, both Hole and Shaft Fit tolerance type, Stacked with line display.
Hole dimension, Fit (tolerance only) type.
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Chapter 12 Detailing
Tolerance Types You can choose from the following types for showing Fit tolerances: •
Fit
•
Fit with tolerance
•
Fit (tolerance only)
Classification You can choose from the following classifications. The shaft and hole tolerances available are filtered to correspond to the classification. •
User Defined
•
Clearance
•
Transitional
•
Press
Hole Fit
and Shaft Fit
You can choose standard Fit tolerances from the hole and shaft lists. The software automatically checks whether the standard is appropriate for the dimension. When you select either a hole or a shaft Fit tolerance, the list for the other type is filtered to present only corresponding tolerances. The bilateral tolerances are also calculated automatically. NOTE: The Classification aid for selecting an appropriate Fit designation is either Hole Basis or Shaft Basis, depending on which Fit designation you choose first. As Hole Basis and Shaft Basis Fit classifications in the international standards are not fully bi-directional, you may get a different list of suggested Fit choices (or an empty list) depending upon the order in which you choose your designations. Hole Basis is preferred for most manufacturing processes Automatic Versus User Defined Tolerance The advantage of letting the SolidWorks software calculate the bilateral tolerance values for you is that if the dimension changes, the tolerances are updated automatically. To set tolerances manually, click the Hole Fit or Shaft Fit icon and type values in the Maximum Variation
and Minimum Variation
boxes.
Fit Tolerance Display For Fit or Fit with tolerance with both hole and shaft tolerances, you can select a display style. Stacked with line display Stacked without line display Linear display With Fit (tolerance only), the Fit standards are not displayed. Parentheses The Show parentheses check box is available for Fit with tolerance, but not for Fit or Fit (tolerance only).
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Annotations Annotations Overview Annotations behave like dimensions in each type of SolidWorks document. You can add annotations in a part or assembly document, then insert them to the drawing views, or you can create annotations in the drawing. For information on inserting annotations from models into drawings, see Inserting Model Items into Drawings. For information on setting options for annotations, see Annotations Options Overview. You can select annotations tools either from the Insert menu or from the Annotations toolbar.
The Align tools are available for aligning annotations. See Aligning Annotations.
You can change the arrowhead style on annotations by right-clicking the arrow to access a menu of styles. When you select an annotation, the geometry to which the annotation is attached is highlighted. You can select annotations by clicking any portion of them, including leaders and arrows. You can create multiple annotations without closing the dialog box or PropertyManager. This functionality applies to Notes, Surface Finish Symbols, Datum Feature Symbols, and Geometric Tolerancing. See Multiple Annotations. You can hide annotations and then show them again. For drawings, see Hide/Show Annotations. For parts and assemblies, click View, All Annotations to toggle the display.
Annotations Options Overview You can set options for annotations in various places. •
Annotations Display Options. Applies options to all annotations in the current document. Click Tools, Options, Document Properties, Annotations Display.
•
Annotation Properties. Contains the same options as Annotations Display. Right-click the Annotations folder
in the FeatureManager design tree and select Details.
•
Annotations Font Options. Sets separate fonts for various types of annotations (Note, Dimension, and so on). Click Tools, Options, Document Properties, Annotations Font.
•
Annotation Colors. Specifies colors for imported and non-imported annotations. Click Tools, Options, System Options, Colors.
The following types of annotations have their own options: •
Notes Options. Alignment, leaders, and borders for notes. Click Tools, Options, Document Properties, Notes.
•
Balloons Options. Style, size, text category, and leaders for balloons, and autoballoon layout. Click Tools, Options, Document Properties, Balloons.
•
Arrows. Size and style of arrows. Click Tools, Options, Document Properties, Arrows.
•
Virtual Sharps. Display of virtual sharps. Click Tools, Options, Document Properties, Virtual Sharps.
•
Tables Options. Various properties of hole, revision, and Bill of Materials tables. Click Tools, Options, Document Properties, Tables.
•
View Labels Options. Text and display of drawing view labels. Click Tools, Options, Document Properties, View Labels.
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Chapter 12 Detailing
Some annotations also have PropertyManagers or Properties dialog boxes for applying changes to individual annotations or a group of annotations. To access a PropertyManager, select the annotation. To access a Properties dialog box, right-click the annotation (or hold down Ctrl while selecting a group of annotations, then right-click one annotation) and select Properties.
Annotation Properties Lets you select the types of annotations that you want to display and set text scale and other annotations options. To select the types of annotations to display:
1.
In the FeatureManager design tree, right-click the Annotations folder,
, and select Details.
2.
In the Annotation Properties dialog box, specify a Display Filter by selecting the annotation types to display by default: Cosmetic threads
Geometric tolerances
Datums
Notes
Datum targets
Surface finish
Feature dimensions
Welds
Reference dimensions - or Select Display all types to show all kinds of annotations available for that part or view. 3.
Change the values in the Text scale edit box to change the scale of the text used in the annotations. NOTE: Always display text at the same size must be cleared, to specify a scale for the default size of annotation text.
4.
5.
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Select from the following options: •
Always display text at the same size. When checked, all annotations and dimensions are displayed at the same size regardless of zoom. Note that drawings have this option disabled and always zoom the text height.
•
Display items only in the view orientation in which they are created. When checked, any annotation is displayed only when the model is viewed in the same orientation as when the annotation was added. Rotating the part or selecting a different view orientation removes the annotation from the display.
•
Display annotations / Display assembly annotations. When checked, all annotation types that are selected in the Display filter are displayed. For assemblies, this includes not only the annotations that belong to the assembly, but also the annotations that are displayed in the individual part documents.
•
Use assembly’s setting for all components. When checked, the display of all annotations matches the setting for the assembly document, regardless of the setting in the individual part documents. Use this option along with Display assembly annotations to display different combinations of annotations.
•
If you use JIS dimensioning standards, specify the JIS surface finish size (1,2,3 characters) or Scale.
Click OK to accept your changes; click Cancel to exit the dialog without saving the changes.
Multiple Annotations The term multiple annotations refers to: •
Creating multiple instances of a type of annotation
•
Copying and pasting any combination of annotations and other entities
Multiple instances of an annotation You can create multiple instances of a type of annotation without closing the PropertyManager or dialog box. This functionality applies to: •
Notes
•
Surface Finish Symbols
•
Datum Feature Symbols
•
Geometric Tolerancing
To create multiple annotations:
1.
With nothing selected, click the appropriate tool from the Annotations toolbar, or click Insert, Annotations and select a tool from the menu. The PropertyManager or Properties dialog box for the tool appears.
2.
Type in text and select options as desired.
3.
With the PropertyManager or dialog box still open, click in the graphics area to place the annotation.
4.
•
Click as many times as necessary if you need to place multiple copies.
•
If the annotation has a leader, click once to place the leader, then click a second time to place the annotation.
•
To add a Multi-jog Leader to a Note, Geometric Tolerance Symbol, or Surface Finish Symbol, before placing the note or symbol, right-click and select Use Multi-jog Leader. Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point. To complete the leader and place the note or symbol, either double-click or right-click and select End Leader.
•
You can change text and other items in the dialog box for each instance of the annotation.
Click OK.
Combinations of annotations You can move or copy multiple annotations as follows: •
You can select any combination of annotations, dimensions, drawing views, and sketch entities. You can select items individually or by box selection.
•
You can cut and paste or drag multiple items in drawings, or you can use the Move or Copy tool. Any individual item can be moved, deleted, and so on at the new location.
•
When you paste multiple items, the paste point is the center of all the selected items. All pasted items retain their relative positions.
•
You can cut or copy items from one drawing sheet and paste them on another sheet.
•
You can cut or copy items that belong to different views. When pasted, the items are all attached to the active view.
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Chapter 12 Detailing
Aligning Annotations You can align annotations by inferencing or by using the Align tools. Inferencing You can control the snap behavior of detail items that you move. Click Tools, Options, System Options, Drawings. Under Detail Item Snapping, you have these options: •
Infer when dragging corner. When checked, you drag the selected item by the corner handles to infer to the corner of another detail item.
•
Infer when dragging center. When checked, you drag the center of the item to infer to the center of another detail item.
•
To ignore all inferences, and to prevent the display of inferencing lines, press the Alt key while dragging detail items.
To align an annotation with a neighboring annotation, drag the item (note, balloon, and so on) until inferencing lines appear. The item snaps to align with its neighbor. Align Tools You can access the Align tools in three ways: •
Click a tool button on the Align toolbar.
•
Click Tools, Align Annotation, and select a tool from the menu.
•
Select a group of annotations, right-click one of the annotations, select Align, and choose one of the options.
The Align tools are as follows:
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Leftmost
The left edges of all selected annotations line up at left edge of the leftmost one.
Rightmost
The right edges of all selected annotations line up at right edge of the rightmost one.
Uppermost
The top edges of all selected annotations line up at top edge of the uppermost one.
Lowermost
The bottom edges of all selected annotations line up at bottom edge of the lowermost one.
Space evenly across
The space is the largest space between selected annotations.
Space evenly down
The space is the largest space between selected annotations.
Center Horizontal
The centers of the annotations line up with the center of the leftmost annotation.
Center Vertical
The centers of the annotations line up with the center of the uppermost annotation.
Compact Horizontal
The edges of the annotations line up with each other in the horizontal direction. The leftmost annotation does not move.
Compact Vertical
The edges of the annotations line up with each other in the vertical direction. The uppermost annotation does not move.
Multi-jog Leaders You can use the Multi-jog Leader in drawings to create leaders with as many bends as required, or to create simple arrows or block diagrams. For example, a multi-jog leader can point a note to an entity in a drawing that is difficult to reach with a straight or bent leader. Some items to note about multi-jog leaders are as follows: •
You can attach multi-jog leaders to annotations, sketch entities, or model edges or faces, or you can insert a leader without attaching it to anything.
•
A preview of each segment of the leader appears as you move the pointer.
•
You can add jog points and branches to multi-jog leader segments.
•
You can start a multi-jog leader anywhere on a drawing sheet. You can end a leader anywhere on a drawing sheet by double-clicking. When a leader is not attached to an entity, the arrow at the endpoint follows the Unattached option in Tools, Options, Document Properties, Arrows. You can manually select a different arrow at the endpoint with a shortcut menu.
•
Multi-jog leaders inference to geometry. If you click a multi-jog leader point at an entity (for example, an edge or a face), the leader attaches to the entity with an smart arrow, and the leader is complete. To avoid inferencing and to prevent attaching to an entity, press Tab. The Tab key toggles between smart attachment and no attachment.
To add a multi-jog leader while creating an annotation:
1.
Click an annotation tool on the Annotation toolbar. NOTE: The annotations that currently support this method of inserting a multi-jog leader are Note, Surface Finish Symbol, and Geometric Tolerance Symbol.
2.
Edit properties in the annotation PropertyManager or dialog box.
3.
Before placing the annotation, right-click and select Use Multi-jog Leader.
4.
Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point.
5.
To complete the leader and place the annotation, either double-click or right-click and select End Leader.
Multi-jog leaders with other annotations •
You can attach a multi-jog leader to a dock point of an annotation (Note, Surface Finish Symbol, Geometric Tolerance Symbol, Weld Symbol, or Balloon).
•
Multi-jog leaders attached to annotations or sketch entities move with the annotations or entities.
•
When you specify a bent leader for an annotation, the length of the bent leader is set in Tools, Options, Document Properties, Dimensions. For documents in ANSI standard, bent leader is the default.
To create a multi-jog leader:
1.
Click Multi-jog Leader
on the Annotation toolbar, or click Insert, Annotations, Multi-jog Leader.
2.
Click the drawing sheet, at a dock point
3.
Move the pointer and click in the graphics area for each jog point.
4.
Complete the leader by clicking an entity such as an edge, or double-click the drawing sheet.
on an annotation, or at a point on a sketch entity.
To add a jog point:
Right-click a segment of the leader (the pointer changes to when it is over a segment) and select Add Jog Point. The jog point is added at the midpoint of the segment. You can drag the jog point. To delete a jog point:
Right-click the jog point (the pointer changes to Point.
SolidWorks 2004 Reference Guide
when it is over a jog point) and select Delete Jog
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Chapter 12 Detailing
To change the arrow at an endpoint:
Right-click the endpoint (the pointer changes to style from the menu.
when it is over an endpoint) and select an arrowhead
To add a branch:
Right-click a jog point and select Insert New Branch. Move the pointer and click to add segments to the branch. To delete a multi-jog leader:
Right-click anywhere along the leader and select Delete Leader, or select the leader and press Delete.
Notes A note can be free floating or placed with a leader pointing to an item (face, edge, or vertex) in the document. It can contain simple text, symbols, parametric text, and hyperlinks. The leader can be straight, bent, or multi-jog. To set Note options for the current document, click Tools, Options, Document Properties, Notes. To create notes:
1.
Click Note
on the Annotation toolbar, or click Insert, Annotations, Note.
The Note PropertyManager appears. 2.
Edit properties (arrows, leaders, font, border, and so on).
3.
Click in the graphics area to place the note. •
To add a Multi-jog Leader to the note, before placing the note, right-click and select Use Multijog Leader. Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point. To complete the leader and place the note, either double-click or right-click and select End Leader.
•
If the note has a leader, click first to place the leader, then again to place the note. A leader appears if you select Leader under Arrows/Leaders, or if you select Auto Leader and move the pointer near an object. See below for the procedure to add Multi-jog Leaders.
4.
Type the text.
5.
Click in the graphics area outside the note to complete the note.
6.
With the Note PropertyManager still open, repeat steps 2 through 5 to create as many notes as necessary.
7.
•
You can change text, properties, and formatting for each instance of the note.
•
To add multiple leaders, press Ctrl while dragging the note and before placing it. The note stops moving and a second leader appears. While still holding Ctrl, click to place the leader. Click as many times as necessary to place additional leaders. Release Ctrl and click to place the note.
Click OK
.
To create a note with a multi-jog leader:
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1.
Click Note
on the Annotation toolbar, or click Insert, Annotations, Note.
2.
Edit properties in the Note PropertyManager.
3.
Right-click in the graphics area and select Use Multi-jog Leader.
4.
Click in the graphics area to place the leader attachment point, then move the pointer and click in the graphics area for each jog point.
5.
To complete the leader and place the note, either double-click in the graphics area or right-click and select End Leader.
6.
Type the note text and click in the graphics area outside the note to complete the note.
To edit note text:
Double-click the note and edit the text in place. NOTE: During on-screen editing of notes, Pan, Zoom, and Rotate operations are not available. To edit note properties:
Select a note, or more than one note, and edit properties in the Note PropertyManager. NOTE: You can also right-click a note and select Properties to access the Note Properties dialog box. You can add more leaders to an existing note by holding down Ctrl and dragging a leader attachment point. Notes snap to a grid if the Display grid and Snap to points or Snap to angle options are selected. To set these options, click Tools, Options, Document Properties, Grid/Snap. Empty notes, which appear on screen as a box with an X
, do not appear in print previews or on printed pages.
Hyperlinks in Notes You can add an embedded hyperlink in a note, or you can add a floating hyperlink in any SolidWorks document. The hyperlink can be to a document on the Internet, on your local network, or on your own hard drive. If the link is to a web site, selecting the hyperlink launches a web browser, if one is not already running, and opens the associated URL (web site). If the link is to a SolidWorks document, clicking the link opens the document. If the link is to another type of document, such as a Word or Excel file, clicking the hyperlink launches the appropriate application, and opens the document. The actual path of a hyperlink embedded in a note does not appear in the note text. A hyperlinked note is displayed in blue; when the pointer moves over a note that contains a hyperlink, the pointer changes to a hand
, and the tooltip
indicates the path of the link. A floating hyperlink (one that is not attached to note text) displays the full path of the link (for example, HTTP://www.solidworks.com) in blue. NOTE: Because clicking a hyperlinked note activates the link, moving or editing a hyperlinked note can be difficult. Move the hyperlink pointer the note pointer
over the note until a box appears around the text. Point to a corner of the box. When
is displayed, drag the note to move it, or right-click the note to edit its properties.
To create an embedded hyperlink:
1.
Create a note, and click Insert Hyperlink while editing a note’s properties.
in the Note PropertyManager. You can also add a hyperlink
2.
Enter the path (or browse to the document) to which you want to link the note text. For a World Wide Web location, enter the website name in the format www.website.com. (You do not need to enter HTTP://)
3.
Click Use relative path for hyperlink if you want to the specify a directory path relative to the current location instead of the full pathname.
4.
Click OK to accept the path.
To create a floating hyperlink:
1.
Click Insert, Hyperlink.
2.
Enter the path (or browse to the document) and click OK. If you edit the properties of a floating hyperlink, you will see that it is a note, the text of which is $URL (a variable representing the path of the link).
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Chapter 12 Detailing
Note PropertyManager Use the Note PropertyManager to insert a Note, or to edit an existing note or balloon note. You can create a freefloating note or a note with a leader. •
You can place multiple notes without closing the Note PropertyManager. You can change the text and other properties for each note.
•
To edit text after creating a note, double-click the note and edit in place.
•
You can also edit note properties in the Note Properties dialog box.
Note Favorite In addition to the functionality described in Favorites, notes have two types of favorites: •
With text. If you type text in a note and save it as a favorite, the text is saved the with note properties. When you create a new note, select the favorite, and place the note in the graphics area, the note appears with the text. If you select text in the document and then select a favorite, the properties of the favorite are applied without changing the selected text.
•
Without text. If you create a note without text and save it as a favorite, only the note properties are saved.
Text Format Alignment. Choose Left Align Angle
, Center Align
, or Right Align
.
. Enter a value. A positive angle rotates the note counterclockwise.
Insert Hyperlink
. Click to include a Hyperlink in the note.
Link to Property
. Click to link a note to a document property.
Add Symbol . Place the pointer in the Note text box where you want the symbol to appear, then click Add Symbol. In the Symbol dialog box, select a library from the Symbol library list, then select a symbol name from the list, and click OK. The symbol’s name is displayed in the text box, and the actual symbol appears in the note. Use document's font. When selected, the text is in the font specified in Tools, Options, Document Properties, Notes. Font. When Use document's font is cleared, click Font to open the Choose Font dialog box and select a new font style, size, and effect. Block Settings The Block Settings section is available only when editing block definitions. Text appears in the Tag name box for notes with attributes imported from AutoCAD. You can also type tag names for notes created in the SolidWorks block definition editor. You can choose for a tag to be Read only, Invisible, or both. The Tag name and its attributes are shown in the Attributes editor, which you can access in the Block Instance PropertyManager. Border Style. Specifies the shape of the border (geometric shapes that enclose the text), or None. Size. Specifies either Tight Fit to the text, or a fixed number of characters.
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Leader Click Leader entity.
, No Leader
, or Auto Leader
Click Straight Leader , Bent Leader the shortcut menu as you create a note. Click a leader position of Leader Left
. Auto Leader inserts a leader if you attach the note to an
, or Underlined Leader
, Leader Right
, or Leader Nearest
Select an arrowhead style from Arrowhead Style. Smart Arrowhead (
to a face,
. You can add a Multi-jog Leader from
.
applies the appropriate arrowhead
to an edge, for example, depending on the detailing standard).
Select Apply to all to apply a change to all of the arrowheads of the selected note. If the selected note has multiple leaders, and Auto Leader is not selected, you can use a different arrowhead style for each individual leader. Layer In drawings with named layers, select a layer. Note Properties You can use the Note Properties dialog box to edit the properties of a Note or balloon note. After you have created a note and closed the Note PropertyManager, you can edit the text by double-clicking the note and editing in place, or by right-clicking the note and selecting Properties to open the Properties dialog box. You can also select a note and edit its properties in the Note PropertyManager. You can specify the following properties in the Note Properties dialog box. Note text/Balloon note text Type the text into the Note text box. For a parametric note, select a dimension on the drawing. If the note is a Balloon or Stacked Balloon, the title of the text section is Balloon note text. There are boxes for the type of text and the actual text for the Upper and Lower sections of the balloons. Add Symbol To add a symbol to the note text, place the pointer in the Note text box where you want the symbol to appear, then click Add Symbol. Select a library from the Symbol library list, then select a symbol name from the list, and click OK. The symbol’s name is displayed in the text box, and the actual symbol appears in the note. Layer To move the note to a different layer, select the name of the layer in the Layer list. Angle Type the text angle in the Angle box, or use the arrows to set the value. Text justification Text can be justified Left, Center, or Right. Text justification is not available for Balloons or Stacked Balloons. Stack Data For Stacked Balloons only. You can stack the balloons Up, Down, Left, or Right.
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Chapter 12 Detailing
Balloons per line For Stacked Balloons only. Set the number of balloons to stack in one line before starting the next line. Leader •
Choose one of the following: o o
o
Always show leaders. Automatic leaders. Adds a leader if you click an entity when you place the note; no leader if you click on the sheet or view. No leaders.
•
Style. If the selected note has a leader or if you select Always show leaders, you can choose the leader style to be Straight, Bent, or Underlined. NOTE: For balloons, the Underlined style is available under Border Style.
•
Display with bent leader. If the note is a balloon note and has a leader, you can choose the leader line to be bent.
•
Arrow style. When the Smart check box is selected, the arrow styles specified in Tools, Options, Document Properties, Detailing, Arrows are used. To choose a different arrow style, clear the check box and select a style from the list.
•
Leader anchor. Choose a default position: Closest, Left, or Right.
•
Apply to all arrowheads. If the selected note has multiple leaders, and Smart is not selected, you can use a different arrowhead style for each individual leader. To apply a change to all of the arrowheads of the selected note, select this check box.
Border •
Style. Specifies the shape of the border (various geometric shapes that enclose the text), or None.
•
Size. Specifies either Tight Fit to the text, or a fixed size to accommodate a specified number of characters.
Font •
If you want to use the font you selected in Tools, Options, Document Properties, Detailing, Notes for note text, leave the Use document’s font check box selected.
•
If you want to use a different font, clear the Use document’s font check box, and click Font to choose from various font styles and sizes.
Hyperlink Click Insert Hyperlink
if you want to include a Hyperlink in the note.
Link to Document Property Click Link to Property
if you want to link a note to a document property.
Tag For notes in Blocks only. Text appears in the Tag name box for notes with attributes imported from AutoCAD. You can also enter tag names for notes created in the SolidWorks block definition editor. You can choose for a tag to be Read Only, Invisible, or both. The Tag name and its attributes are shown in the Attributes editor, which you can access in the Block Instance PropertyManager.
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Multiple Leaders To create multiple leaders while generating a new annotation:
1.
After selecting the properties for the annotation, click in the graphics area to place the first leader.
2.
While dragging the annotation and before placing it, press Ctrl. The annotation stops moving and another leader is created.
3.
Click as many times as necessary to place additional leaders.
4.
Release Ctrl, drag the annotion into position, and click to place the annotation.
To add new leaders to an existing annotation:
1.
Select the annotation.
2.
Press Ctrl and drag a leader attachment point. A new leader is created.
Link to Property You can link the value of a document property, a custom property, or a configuration specific property to the text of a note. If the value of the property changes, the note text changes automatically. To link a note to a property:
1.
In the Note PropertyManager, click Link to Property - or In the Note Properties dialog box, click Link to Property
2.
3.
.
Select the place to link from: •
Current document
•
Model in view to which the annotation is attached (drawings only)
•
Model in view specified in sheet properties (drawings only)
•
Component to which the annotation is attached (assembly documents and part and assembly drawing documents)
View the list of available properties, which depends on your selection in step 2 and where the note is created. •
Part or assembly document. The list includes the properties of the model document, including any custom defined properties.
•
Drawing sheet or sheet format. The list includes the properties of the drawing document, including any custom defined properties.
•
Drawing view. The list includes the properties of the model document shown in the view. (If a view is selected when you insert the note, or if the note is attached to the model in a view, the note belongs to the view.)
NOTE: All documents have system-defined properties. Drawings have system-defined properties that you can use to customize a sheet format. For more information on document properties in notes, see Linking Notes to Document Properties 4.
To add a new custom property, or to edit an existing one, click File Properties, then edit the properties on the Summary Information – Custom and Configuration specific tabs.
5.
Select a system-defined or custom property from the list, and click OK.
The Note text shown in the dialog box is the name of the property in the form $PRP:"<property name>". In the document, the note text is the value assigned to the property.
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Chapter 12 Detailing
Prefixes for custom properties linked in notes are used as follows: Prefix
Evaluated from:
$PRP:
Current document
$PRPSHEET:
Model in the view specified in Sheet Properties. If the model specified in Sheet Properties for custom properties is Default, then for notes belonging to drawing views, the model in the drawing view to which the note belongs is used. For sheet and sheet format notes, the first view in the FeatureManager design tree is used. If a view is selected, the model for that view is used for all cases.
$PRPVIEW:
Model in the drawing view to which the note belongs
$PRPMODEL:
Component to which the annotation is attached
Links to dimensions are evaluated from the active document. If the appropriate document for custom properties cannot be located according to the designations above, the following rules apply: •
In edit sheet mode, all sheet format notes are blank. All sheet and drawing view notes show their property names.
•
In edit sheet format mode, all sheet format notes show their property names.
NOTE: When a note in a drawing is linked to a custom property or a dimension and then the property or dimension is deleted, the note displays ERROR!
Balloons You can create balloons in a drawing document. The balloons label the parts in the assembly and relate them to item numbers on the bill of materials (BOM). However, you do not have to insert a BOM in order to add balloons. If the drawing has no BOM, the item numbers are the default values that the software would use if you did insert a BOM. If there is no BOM on the active sheet, but there is a BOM on another sheet, the numbers from that BOM are used. To set the default BOM balloon properties, click Tools, Options, Document Properties, Balloons. If the default BOM balloon Style is Circular Split Line, you can choose what type of text to display in both the Upper and Lower portions of the balloon. For other styles, only Upper is available. Type of text can be Item Number, Quantity, or Custom. Balloons are automatically suppressed when the components they reference are suppressed. You can also add balloons in assembly documents. To import balloons from an assembly document into a drawing view, select Notes in the Insert Models Items dialog box. You can attach balloons to sketch entities. This is useful when sketches (with no extrusions) are combined to form an assembly and then taken into a drawing.
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If you change the Item Number in a balloon, the item number in the bill of materials also changes. To change an Item Number in a table-based BOM, clear Do not change item numbers in the Bill of Materials PropertyManager. To return to assembly order after changing item numbers, click Follow assembly order
.
To change an Item Number in an Excel-based BOM, you must clear the Row numbers follow assembly ordering check box on the Control tab of the Bill of Materials Properties dialog box. If the check box is selected (default), a message appears stating that the item number cannot be changed. You can also create stacked balloons. See Stacked Balloons. To insert balloons:
1.
Click Balloon
on the Annotations toolbar, or click Insert, Annotations, Balloon.
The Balloon PropertyManager appears. 2.
Edit the properties in the PropertyManager as needed, then click a component in a drawing view of an assembly, or click a component in an assembly model, to place the leader, then click again to place the balloon. A balloon containing an item number attaches to the part. If you specified the text to be Item Number, the number in the balloon corresponds to the item number in the bill of materials.
3.
Continue inserting as many balloons as needed. Edit the properties for each balloon in the PropertyManager before inserting the balloon.
4.
Click OK
.
To move the balloon or leader arrow, select and drag the balloon, or drag the leader by the handle.
To change the balloon properties:
Select the balloon and edit the properties in the Balloon PropertyManager. - or Right-click the balloon and select Properties. Make changes in the Note PropertyManager and click OK. To edit balloon text:
Double-click the balloon text and edit in place. To add multiple leaders to a balloon:
You can add more leaders to an existing balloon by holding down Ctrl and dragging a leader attachment point.
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Balloon PropertyManager The Balloon PropertyManager opens when you insert Balloons into a drawing or assembly document, or when you select an existing balloon. You can insert multiple balloons without closing the PropertyManager. Change the settings in the PropertyManager as necessary and click in the graphics area to place the balloons. The PropertyManager controls the following properties: Style Select a style for the shape and border of the balloon from the list. The style None displays the balloon text with no border. Size Select a size from the list, either a specified number of characters or Tight fit, which adjusts automatically to the text. Balloon text Select the type of text for the balloon, or for the upper section of a split balloon, from the list. •
Item Number - The Item Number in the Bill of Materials
•
Quantity - The quantity of this item in the assembly
•
Custom - The Custom Text box opens for you to type text
Lower text If you select the Circular Split Line style, this box is available to specify the text for the lower section. You have the same options as in the Balloon text section. More Properties When you select an existing balloon, you can click More Properties to open the Note PropertyManager.
Stacked Balloons Stacked balloons have only one leader for a set. You can stack the balloons vertically or horizontally. You can insert stacked balloons in drawings of assemblies and in assembly documents. To import balloons from an assembly document into a drawing view, select Notes in the Insert Model Items dialog box. To set default stacked balloon properties, click Tools, Options, Document Properties, Balloons. Under Stacked balloons, set Style and Size. Under Balloon text, choose the type of text: Item Number, Quantity, or Custom. You can insert a stacked balloon without selecting a component, so you can annotate an item that is part of an assembly but not actually modeled, such as glue or a liquid. If you change the Item Number in a stacked balloon, the item number in the bill of materials also changes. To change an Item Number in a table-based BOM, clear Do not change item numbers in the Bill of Materials PropertyManager. To return to assembly order after changing item numbers, click Follow assembly order . To change an Item Number in an Excel-based BOM, you must clear the Row numbers follow assembly ordering check box on the Control tab of the Bill of Materials Properties dialog box. If the check box is selected (default), a message appears stating that the item number cannot be changed.
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To insert stacked balloons:
1.
Click Stacked Balloon
on the Annotation toolbar or click Insert, Annotations, Stacked Balloon.
The Stacked Balloon PropertyManager appears, and the pointer changes to 2.
.
Select the point on the component where you want the balloon leader attached, then click again to place the first balloon. The leader and the first balloon appear.
3.
Continue to select components. A balloon is added to the stack for each component selected. As you add the stacked balloons, you can rightclick any balloon in the stack, select Stack Direction, and choose a new stack direction, or you can select the stack direction in the PropertyManager (Up
, Down
, Left
, Right
).
Each balloon is a separate note that you can select to delete or edit. 4.
Click OK
to close the PropertyManager.
To add balloons to the stack later:
Right-click one of the stacked balloons and select Add to Stack. To edit balloon text, do one of the following:
•
Double-click the balloon text and edit in place.
•
Select the balloon and edit the text in the PropertyManager.
•
Right-click the balloon, select Properties, and edit the text in the Note Properties dialog box.
To change the properties of the stacked balloons, do one of the following:
•
Select a balloon or balloons in the stack and change properties in the PropertyManager. For additional properties, click More Properties. Many properties are available in both the PropertyManager and the Note Properties dialog box.
•
Select a balloon or balloons, right-click a selected balloon and select Properties, and change the properties in the Note PropertyManager. Changes to properties apply only to selected balloons. To change all balloons in the stack, select all of them. Balloons stacked Right
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Chapter 12 Detailing
Stacked Balloon PropertyManager The Stacked Balloon PropertyManager opens when you insert a Stacked Balloon into a drawing or assembly document, or when you select an existing stacked balloon. The properties apply to the selected balloons. Balloon Settings Style. Select a style for the shape and border of the balloons from the list. If you select Circular Split Line, the Lower Text window opens for the lower half of the balloons. Size. Select a size from the list, either a specified number of characters or Tight fit, which adjusts automatically to the text. Balloon text. Select the type of text for the balloons, or for the upper section of split balloons, from the list. •
Item Number. The Item Number in the Bill of Materials
•
Quantity. The quantity of this item in the assembly
•
Custom. The Custom Text box opens for you to type text
Lower text. If you select the Circular Split Line style, this box is available to specify the text for the lower section. You have the same options as in the Balloon text section. Balloons per line. Set the number of balloons to stack in one line before starting the next line. Stack Right , Stack Left respect to its leader.
, Stack Down
, Stack Up
. Click for the direction of the stack with
Layer In drawings with named layers, select a layer. More Properties For existing stacked balloons, click More Properties to open the Note PropertyManager.
AutoBalloons Insert a set of balloons into one or more drawing views. Balloons are inserted into the appropriate views without duplicates. You can specify that balloons be inserted when creating new drawing views. Example of AutoBalloon
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Square
Circular
Top
Bottom
Left
Right
To insert balloons into a drawing view:
1.
Click AutoBalloon
on the Annotation toolbar, or click Insert, Annotations, AutoBalloon.
2.
Set properties in the AutoBalloon PropertyManager, then click OK
.
The balloons are placed outside the view border, and the leaders do not intersect. Once you close the PropertyManager, you cannot open it again. You can delete the balloons or undo the autoballoon command, then reinsert the balloons. You can drag a group of balloons or a single balloon. To specify that balloons be inserted into new drawing views:
1.
Click Tools, Options, Document Properties, Detailing.
2.
Under Auto insert on view creation, select Balloons, then click OK.
To specify the default layout for autoballoons:
1.
Click Tools, Options, Document Properties, Balloons.
2.
Under AutoBalloon Layout, select one of the formats, then click OK.
AutoBalloon PropertyManager Set the properties when inserting autoballoons into a drawing. Balloon Layout Select: Square Circular Top Bottom Left Right Ignore multiple instances. Applies a balloon to only one instance for components with multiple instances.
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Balloon Settings Sets the properties to apply to all the balloons. Layer In drawings with named layers, select a layer.
Center Marks You can place center marks on circles or arcs in drawings. The center mark lines can be used as references for dimensioning. Example of Center Marks
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Single center mark
Single center mark with extended lines
Extended lines in centerline font
Single center mark rotated 45°
Linear pattern with default size marks
Linear pattern with specified mark size
Linear pattern with extended lines
Linear pattern with connection lines
Circular pattern with extended lines
Circular pattern with base center mark
Circular pattern with circular lines
Circular pattern with radial lines
Some items to note about center marks are as follows: •
The axis of the circle or arc must be normal to the drawing sheet.
•
Center marks are available as single marks, in linear patterns, or in circular patterns. Linear patterns can include connecting lines. Circular patterns can include circular lines, radial lines, and base center marks. Display attributes include mark size, extended lines, and specifying the centerline font for the center mark lines.
•
You can set an option so that center marks are inserted automatically in new drawing views.
•
You can insert a center mark manually into one circle or arc in a pattern and then propagate center marks to all entities in the pattern.
•
Center marks propagate or insert automatically into patterns if the pattern is created from a feature and not a face or body.
•
You can rotate center marks individually, specifying the rotation in degrees. In the Rotate Drawing View dialog box, you can choose to have center marks rotate automatically when the view is rotated.
•
Center marks in Auxiliary Views are oriented to the viewing direction such that one of the lines of the center mark is parallel to the view arrow direction.
To set options for center marks:
1.
Click Tools, Options, Document Properties, Detailing.
2.
Under Center marks, type a value for Size and select or clear the check boxes for Extended lines and Centerline font.
3.
Under Auto insert on view creation, select or clear the check box for Center marks. When selected, center marks are inserted automatically into all appropriate circles and arcs in new drawing views.
4.
Click OK.
To insert center marks manually:
1.
Click Center Mark
on the Annotation toolbar, or click Insert, Annotations, Center Mark.
The Center Mark PropertyManager appears and the pointer changes to 2.
Choose from the Options, Display Attributes, and Angle.
3.
Click the model edges or silhouettes of circles or arcs.
.
NOTE: You cannot apply a center mark to an ellipse or a torus. 4.
If you selected Linear Pattern to all entities in the pattern.
5.
Click OK
or Circular Pattern
, click Propagate
to apply center marks
.
To edit center marks:
1.
Select a center mark (the pointer changes to
when it is over a center mark).
2.
Edit the center mark properties in the Center Mark PropertyManager.
3.
Click OK
.
To dimension to center marks:
You can dimension to the horizontal lines, the vertical lines, or the circular edges to generate vertical, horizontal, or angular dimensions. You can dimension between two center marks, or between a center mark and another entity.
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Example of Center Mark Dimensions
Example of Center Mark Fonts The default center mark font is typical for ANSI standard.
The centerline font used for center mark lines is typical for ISO standard.
Center Mark PropertyManager You can control the following properties for center marks in the Center Mark PropertyManager. The properties available vary depending on the type of center mark selected. Options Single Center Mark. Insert a center mark into a single circle or arc. You can change the Display Attributes and rotation Angle of the center mark. Linear Center Mark. Insert center marks into a linear pattern of circles or arcs. You can select Connection lines and Display Attributes for linear patterns. Circular Center Mark. Insert center marks into a circular pattern of circles or arcs. You can select Circular lines, Radial lines, Base center mark, and Display Attributes for circular patterns. Example Display Attributes Clear Use document's defaults to change the following attributes:
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•
Mark size. Enter a value. Set the default in Tools, Options, Document Properties, Detailing.
•
Extended lines. Display extended axis lines, with a gap between the center mark and the extended lines.
•
Centerline font. Display the center mark lines in the centerline font.
Angle Displays the current angle of a single center mark. If the center mark is rotated because the view is rotated, the rotation angle appears here. Enter a new value if desired. Not available for linear or circular pattern center marks. Layer In drawings with named layers, select a layer.
Centerline Annotations You can insert centerlines into drawing views automatically or manually. The SolidWorks software avoids duplicate centerlines. Example of Centerline Annotations To insert centerlines throughout a feature, select one face.
To insert a centerline in one feature, select a face. To insert centerlines in selected features, press Ctrl and select multiple faces. To insert centerlines in all appropriate features, select the view in either the graphics area or the FeatureManager design tree. To insert a centerline from the middle of the left side to the middle of the right side, select the top and bottom edges.
To insert centerlines automatically into drawing views:
1.
In a drawing document, click Tools, Options, Document Properties, Detailing.
2.
Under Auto insert on view creation, select Centerlines.
3.
Click OK.
4.
Insert a drawing view. Centerlines appear automatically in all appropriate features.
To insert centerlines manually:
1.
In a drawing document, click Centerline Centerline.
on the Annotations toolbar, or click Insert, Annotations,
The Centerline PropertyManager appears. NOTE: You can select either the tool or an entity first.
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2.
Select one of the following: •
Two edges (parallel or non-parallel)
•
Two sketch segments (except splines)
•
A face (cylindrical, conical, toroidal, or swept)
•
A drawing view in the graphics area (except isometric orientation)
•
A feature, component, or drawing view in the FeatureManager design tree
•
Insert Component Centerline in the component shortcut menu in the graphics area (assembly drawings only) Centerlines appear in all appropriate segments of the selected entities.
3.
Click OK
.
Hole Callouts Hole callouts are available in drawings. If you change a hole dimension in the model, the callout updates automatically. Hole callouts use Hole Wizard information when a hole has been created by the Hole Wizard. The default formats for the Hole Wizard types are stored in installation directory\lang\
The same hole callout, but defined by geometry.
The axis of the hole must be normal to the drawing sheet. To add hole callouts in a drawing:
1.
Click Hole Callout The pointer changes to
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on the Annotation toolbar, or click Insert, Annotations, Hole Callout. .
2.
Click the edge of a hole. A Hole Callout is inserted and the Dimension PropertyManager appears. The callout contains a diameter symbol and the dimension of the hole diameter. If the depth of the hole is known, the callout also contains a depth symbol and the dimension of the depth. If the hole is created in the Hole Wizard, the callout contains additional information (the dimensions of a countersink or number of hole instances, for example).
3. 4.
Click in the graphics area to place the hole callout. Edit the callout in the Dimension PropertyManager. You can specify precision, select an arrow style, or add text (for example, the number of places where the hole occurs). However, you should retain the dimensions and symbols for the size and type of hole. If the hole has been created by the Hole Wizard, you can also click Variables in the Dimension PropertyManager to access a list of Hole Wizard variables to insert into the hole callout. If you attach a hole callout to a tapped hole in ANSI inch standard and the current drawing units are millimeters, the drill diameter and hole depths are reported in mm but the thread description retains the ANSI inch size designation. You might want to replace the thread description with other variables from the Hole Callout Variable dialog box.
5.
Repeat steps 2 through 4 to insert additional hole callouts, then click OK
.
To edit the properties of a hole callout:
Select the callout and make the changes in the Dimension PropertyManager. If you manually change a portion of the callout text, you might break that portion's link with the model. SolidWorks displays a warning message if you are about to break a link. To toggle between Hole Wizard and geometry definitions:
1.
Right-click the hole callout and select Display Options, Define by Geometry.
2.
To return to the Hole Wizard definition, right-click the hole callout and select Display Options, Define by Hole Wizard. These menu items are available only when holes have been created using the Hole Wizard.
Hole Callout Variables You can choose a hole callout variable from the list of Hole Wizard variables. The variable is inserted in the hole callout text where the pointer is located in the Dimension Text section of the Dimension PropertyManager. The variable name (for example,
If you select a variable from the list that is not appropriate for the hole for which you are editing the hole callout, a value of zero is displayed in the hole callout.
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Cosmetic Threads A cosmetic thread represents the inner diameter of a thread on a boss or the outer diameter of a thread on a hole and can include a hole callout.
The properties and functionality of cosmetic threads include:
•
You can represent threads on a part, assembly, or drawing, and you can attach a thread callout note. You can add cosmetic threads to conical holes. If the conical thread does not end at a flat face, it is trimmed by the curved face.
•
A cosmetic thread differs from other annotations in that it is an absorbed feature of the item to which it is attached. For example, the cosmetic thread on a hole is in the FeatureManager design tree under the Hole feature, along with the sketches used to create the hole.
•
When the pointer is over a cosmetic thread, the pointer changes to
•
Cosmetic threads in part documents are inserted automatically into drawing views if the drawing document is in ANSI standard. A copy of any present thread callout is also inserted. Thread callouts are not used in ISO, JIS, or other standards, but you can show them with Insert Callout on the shortcut menu (see the next paragraph). To insert cosmetic threads from assembly documents into drawings, click Insert, Model Items and select Cosmetic Threads. In ANSI drawings, one copy of a cosmetic thread callout is also imported into a sheet.
•
In drawings, Insert Callout appears in the shortcut menu. If a cosmetic thread callout is defined in the part but is not displayed in the drawing, you can display the callout by selecting this menu item. A leader attaches to the thread by default. The callout is a note. You can edit the callout as you would edit any note.
•
If you add a cosmetic thread while working in a drawing view, the part or assembly is updated to include a Cosmetic Thread feature.
•
You can attach notes to both the circular faces and silhouette edges of cosmetic threads. You can dimension both the circular cosmetic thread and the linear dimension of the sides in drawings. You can dimension the silhouette edge of a cosmetic thread to a sketch entity. You cannot dimension cosmetic threads in part or assembly documents.
•
A cosmetic thread that is created in a part cannot be deleted from a drawing, but it can be hidden and shown. To hide or show a cosmetic thread, right-click the cosmetic thread and select Hide or Show.
•
The visibility of cosmetic threads follows the visibility of the owner feature. When you change display mode, add features to the Show Hidden Edges list, or hide a component, the visibility of cosmetic threads changes automatically.
•
You can reference patterned cosmetic threads.
•
You can display cosmetic threads on assembly feature holes. The cosmetic thread appears only on the last component cut by the hole.
•
For tap and pipe tap holes, you can add cosmetic threads in the Hole Wizard.
.
NOTE: For tapped holes with cosmetic threads created in the Hole Wizard, the hole diameter is the diameter of the tap drill. For tapped holes without cosmetic threads, the hole diameter is the outer diameter of the thread. •
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For shaded display of cosmetic threads, click Tools, Options, Document Properties, Annotations Display. Under Display filter, select Shaded cosmetic threads.
To insert cosmetic threads:
1.
On a cylindrical feature (a boss, a cut, or a hole), select the circular edge where the thread begins. If the feature is a conical hole, select the major diameter. If the feature is a conical boss, select the minor diameter. You can also select the feature after you click the tool.
2.
Click Cosmetic Thread
on the Annotations toolbar, or click Insert, Annotations, Cosmetic Thread.
3.
Set the properties in the Cosmetic Thread PropertyManager.
4.
Click OK
.
To edit a cosmetic thread:
1.
In a part or assembly document, right-click the Cosmetic Thread feature and select Edit Definition.
2.
Make the necessary changes in the Cosmetic Thread PropertyManager, and click OK
.
To specify the line style and weight for cosmetic threads in the active drawing document:
1.
Click Tools, Options. On the Document Properties tab, select Line Font.
2.
In the Type of edge section, select Cosmetic Thread.
3.
Choose a Style and Thickness from the lists. The Preview box shows the results.
Cosmetic Thread PropertyManager Specify the following properties when inserting a cosmetic thread in a part or drawing. Thread Settings Circular Edges
. Select a circular edge in the graphics area.
End Condition. The cosmetic thread extends from the edge selected above to the end condition: •
Blind. A specified depth. Specify the depth below.
•
Through. Completely through the existing geometry.
•
Up to Next. To the next entity that intercepts the thread.
Depth
. Enter a value when the End Condition is Blind.
Minor Diameter, Major Diameter, or Conical Offset entity type with the cosmetic thread.
. Sets the diameter for the dimension corresponding to the
Thread Callout. Type text to appear in the thread callout. Layer In drawings with named layers, select a layer.
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Surface Finish Symbols You can specify the surface texture of a part face by using a surface finish symbol. You can select the face in a part, assembly, or drawing document. For ISO and related drafting standards, you can specify Display symbols per 2002 in Tools, Options, Document Properties, Detailing to display surface finish symbols per 2002 standards. To insert a surface finish symbol:
1.
Click Surface Finish
2.
Set the properties in the PropertyManager.
3.
Click in the graphics area to place the symbol.
4.
on the Annotations toolbar, or click Insert, Annotations, Surface Finish Symbol.
•
Multi-jog Leader. Before placing the symbol, right-click and select Use Multi-jog Leader to add a multi-jog leader. Click in the graphics area to place the arrow end of the leader, then move the pointer and click to add each jog point. To complete the leader and place the symbol, either doubleclick or right-click and select End Leader.
•
Multiple instances. Click as many times as necessary to place multiple copies.
•
Editing each instance. You can change text and other items in the dialog box for each instance of the symbol.
•
Leaders. If the symbol has a leader, click once to place the leader, then click a second time to place the symbol.
•
Multiple leaders. While dragging the symbol and before placing it, press Ctrl. The note stops moving and a second leader is added. While still holding Ctrl, click to place the leader. Click as many times as necessary to place additional leaders. Release Ctrl and click to place the symbol.
Click OK
.
Drag You can drag a surface finish symbol with a leader to any location. If you attach a leaderless symbol to an edge, then drag it off the model edge, an extension line is created.
Edit To edit a surface finish symbol, select the symbol. Rotate You can rotate surface finished symbols attached to sketch entities by 180°. Right-click the symbol and select Rotate by 180. Rotate by 180 is not available for model edges or faces, it is not available in ANSI standard, and the symbol must not have a leader. Multiple Leaders You can add more leaders to an existing symbol by holding down Ctrl and dragging a leader attachment point.
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Surface Finish PropertyManager Edit properties of surface finish symbols. Surface Finish Favorite Symbol Select a symbol style. The symbols available vary depending on the drafting standard specified. For ISO and related standards, the symbols available also vary depending on whether you select display of surface finish symbols using 2002 standards. Specify both options in Tools, Options, Document Properties, Detailing. Basic Machining Required Machining Prohibited Local All Around JIS Basic JIS Grind JIS No Machining If you select JIS Basic or JIS Grind, several surface textures are available. Symbol Layout For ANSI symbols and symbols using ISO and related standards prior to 2002, specify: •
Maximum Roughness
•
Minimum Roughness
•
Material Removal Allowance
•
Production Method/Treatment
•
Sampling Length
•
Other Roughness Values
•
Roughness Spacing
•
Lay Direction
For symbols using ISO and related standards from 2002, specify: •
Manufacturing Method
•
Texture Requirement 1
•
Texture Requirement 2
•
Texture Requirement 3
•
Machining Allowance
•
Surface Lay and Orientation
For JIS symbols, specify: •
Roughness/Ra
•
Roughness Rz/Rmax
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Format Use document font. To specify a different font for the symbol and text, clear and click Font. Select: Upright Rotated/Perpendicular Leader Select a leader style: Leader No Leader Auto Leader Straight Leader Bent Leader Select an Arrow Style. Layer In drawings with named layers, select a layer.
Datum Feature Symbols You can attach a datum feature symbol to the following items: •
In a part or assembly, on a planar model surface or on a reference plane
•
In a drawing view, on a surface that appears as an edge (not a silhouette) or on a section view surface
•
A geometric tolerance symbol frame
To insert datum feature symbols:
1.
Click Datum Feature Symbol Symbol.
on the Annotations toolbar, or Insert, Annotations, Datum Feature
2.
Edit the options in the Datum Feature PropertyManager.
3.
Click in the graphics area to place the attachment and then the symbol.
4.
Continue inserting as many symbols as needed.
5.
Click OK
.
If you drag a datum feature symbol off the model edge, an extension line is added. To edit a datum feature symbol, select the symbol. NOTE: If you use ANSI dimensioning standards, you can display datum feature symbols in the 1982 style. To select this option for the active document, click Tools, Options, Document Properties, Detailing. In the Dimensioning standard section, select ANSI from the list, then select the Display datums per 1982 check box.
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Datum Feature PropertyManager The PropertyManager controls properties of datum feature symbols. Settings Label
. The text appears in the datum feature box.
Use document style. The document style follows the standard (ANSI, ISO, and so on) specified in Tools, Options, Document Properties, Detailing. Clear to select a different style of box and attachment. Each style of box has a different set of attachment styles.
Square
Round (GB)
Filled Triangle
Perpendicular
Filled Triangle With Shoulder
Vertical
Empty Triangle
Horizontal
Empty Triangle With Shoulder Layer In drawings with named layers, select a layer.
Datum Targets You can attach a datum target and symbol to a model face or edge in any document. To create a datum target and symbol:
1.
Click Datum Target
on the Annotations toolbar, or click Insert, Annotations, Datum Target.
2.
Set the properties in the PropertyManager.
3.
Click in the graphics area to place the target and then the symbol. You can insert multiple symbols.
4.
Click OK
.
To move the datum target symbol (the balloon, the crosshatch area, or the point), select the symbol and drag the item. To edit the datum target symbol, select the symbol. In a drawing, you can dimension to the center of a datum target area. Activate the view, then click either the symbol or the area to add the dimension.
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Datum Target PropertyManager Attach a datum target and associated symbol to a model face or edge. Settings Target symbol. Select the target symbol style: Target symbol Target symbol with area size outside No target symbol Target area. Select the target area display: X target area Circular target area Rectangular target area Do not display target area Target area size Datum references
. Specify Width and Height (for rectangles) or Diameter (for X's and circles). . Specify up to three references.
Leader Select a leader style: Bent, solid leader Bent, dashed leader Straight, solid leader Straight, dashed leader Select an Arrow style. Layer In drawings with named layers, select a layer.
Geometric Tolerancing The SolidWorks software supports the ANSI Y14.5 Geometric and True Position Tolerancing guidelines.
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•
You can place geometric tolerancing symbols, with or without leaders, anywhere in a drawing, part, assembly, or sketch, and you can attach a symbol anywhere on a dimension line.
•
A geometric tolerance symbol can have any number of frames.
•
The pointer changes to dimension.
•
You can add multiple symbols without closing the dialog box.
•
You can display multiple leaders. The leaders can be straight, bent, or perpendicular.
•
When you drag the leader of a geometric tolerance symbol off a model edge, an automatic witness line is created.
when it is near the handle of an arrow of a geometric tolerancing symbol on a
Example of Geometric Tolerance Symbols Multiple frames
Perpendicular leaders
Automatic witness line
To create geometric tolerancing symbols:
1.
Click Geometric Tolerance
, or click Insert, Annotations, Geometric Tolerance.
2.
Type in values and select symbols. As you add items, a preview is displayed. For more information on the options available (Geometric Characteristic Symbols, Material Condition Symbols, Projected tolerance zone, and so on), see Geometric Tolerance Properties. For information on leader, arrow, anchor, and font options, see Geometric Tolerance Options.
3.
4.
Click to place the symbol. •
To add a Multi-jog Leader to the symbol, before placing the symbol, right-click and select Use Multi-jog Leader. Click in the graphics area to place the leader attachment point, then move the pointer and click to add each jog point. To complete the leader and place the symbol, either doubleclick or right-click and select End Leader.
•
Click as many times as necessary to place multiple copies.
•
If the symbol has a leader, click once to place the leader, then click a second time to place the symbol.
•
You can change text and other items in the dialog box for each instance of the symbol.
•
While dragging the symbol and before placing it, hold down Ctrl. The note stops moving, but the leader continues, lengthening the leader. While still holding Ctrl, click to place the leader. Click as many times as necessary to place additional leaders. Release Ctrl and click to place the symbol.
Click OK to close the dialog box.
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You can drag the symbol any place in the document. To edit an existing symbol, double-click the symbol, or right-click the symbol and select Properties. You can add more leaders to an existing symbol by holding down Ctrl and dragging a leader attachment point. Geometric Tolerance Properties You can specify the properties and insert Geometric Tolerance symbols. Feature control frames 1.
In the first Feature Control Frame, click GCS (Geometric Characteristic Symbol). In the Symbols dialog box, choose a Symbol library, select a symbol, and click OK. As you make each selection, a preview is displayed.
2.
Enter a tolerance value in the Tolerance 1 box, and click
to include a Diameter symbol.
3.
Click MC to choose the material condition symbol for Tolerance 1, and click OK.
4.
Repeat steps 2 and 3 for Tolerance 2.
5.
Enter datum names and material condition symbols for the Primary, Secondary, and Tertiary datums.
6.
For additional frames, increment the number in Frames and repeat steps 1 through 5 for each frame.
Composite frame. To create a composite frame, select Composite Frame and enter values and material condition symbols. Between two points. Select if the tolerance value applies to a measurement between two points or entities, and type the labels of the points in the boxes. Projected tolerance zone To enter a Projected Tolerance Zone (PTZ) height, select Show PTZ and enter a value in the Height box. The value appears in the first frame’s tolerance box. GTol Favorite Layer In drawings with named layers, select a layer. Additional Properties To specify styles for leaders, arrows, anchors, and fonts, click Options. Geometric Tolerance Options You can specify properties for leaders, arrows, and fonts of the selected geometric tolerance symbol. Attached leader •
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Choose one of the following: o
Always show leaders.
o
Automatic leaders. Adds a leader if you click an entity; no leader if you click on the sheet or view.
o
No leaders.
•
Display with bent leader. With this selected, you can also select an All Around leader.
•
Perpendicular leaders.
•
All Around. Indicates that the profile tolerance extends all the way around the feature to which the tolerance applies.
Arrow Select Smart to use the default arrow style (specified in Tools, Options, Document Properties, Detailing) for the type of item the symbol is attached to. To select a different arrow style, clear this check box and select an arrow style from the Arrow list. Anchor Choose the location of the leader anchor from Closest, Left, or Right sides. Font Select Use document’s font to use the default font, or clear the check box and click the Font button to choose from various font styles and sizes. Click OK to return to the Geometric Tolerance Properties dialog box.
Dowel Pin Symbols You can add dowel pin symbols to holes (circular edges or sketched circles) in drawings. The symbol conforms to the size of the selected hole. Example of Dowel Pin Symbols Dowel pin symbols are added to holes of various sizes. The symbol in green is flipped 90°.
Following are some restrictions on dowel pin symbols: •
The face containing the hole must be normal to the plane of the currently active view.
•
You cannot move dowel pin symbols with Copy or Cut and Paste operations.
To insert dowel pin symbols into a drawing:
1.
Click Dowel Pin Symbol edge.
, or click Insert, Annotations, Dowel Pin Symbol, and select a circular
- or Select one or more circular edges and click Dowel Pin Symbol Pin Symbol.
or click Insert, Annotations, Dowel
Dowel pin symbols appear in the selected holes, and the Dowel Pin Symbol PropertyManager appears. You can continue to select circular edges to insert additional dowel pin symbols. 2.
Under Display Attributes, select Flip symbol if desired. The dowel pin symbols currently selected rotate 90°. NOTE: To flip a dowel pin symbol after it has been inserted, right-click the symbol (the pointer changes to when it is over the symbol) and select Flip Symbol.
3.
Click OK
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Weld Symbols When you create a weld bead in an assembly, a weld symbol is created automatically on the weld bead component, representing the parameters you specify. You can also construct weld symbols independently in a part, assembly, or drawing document. When creating or editing a weld symbol, you can: •
Add secondary weld fillet information to the weld symbol for certain types of weld (Square or Bevel, for example).
•
Choose a Leader anchor of None and add a Multi-jog Leader later.
•
Choose the text font for each weld symbol.
To insert a weld symbol:
1.
Click a face or edge where you want to indicate a welded joint.
2.
Click Weld Symbol
on the Annotations toolbar, or click Insert, Annotations, Weld Symbol.
The Weld Symbol Properties dialog box appears for ISO, BIS, DIN, JIS, and GB standards. Different dialog boxes appear for ANSI and GOST standards. 3.
Type in values and select symbols and options. A preview is displayed. Click OK to close the dialog box and place the symbol.
To edit a weld symbol:
Double-click the symbol - or Right-click the symbol and select Properties. Weld Symbol Properties You can create weld symbols in part, assembly, and drawing documents. The Dimensioning standard in Tools, Options, Document Properties, Detailing must be set to ISO, BSI, DIN, JIS, or GB for this dialog box, or ANSI or GOST to access dialog boxes for weld symbols in those standards. Many of the properties are available both above and below the weld symbol line and are described in order from the line. A preview of the symbol is displayed in the graphics area.
Peripheral. Adds Field/Site. Adds
to indicate that the weld is applied all around the contour. to indicate that the weld is applied in the field or on-site.
Weld symbol. Click and select a symbol from a symbol library. Other options become available, depending on the symbol chosen. Type dimensions to the left and right of the Weld symbol button. Specification process. Type text in the large box at the right, in any number of lines, to appear in the tail of the symbol. Contour. Applies a contour shape above the symbol. 2nd fillet. The 2nd fillet is available for only certain weld symbols (Square or Bevel, for example). Type dimensions in the fields to the left and right of the check box. Symmetric. Properties on one side of the symbol line also appear on the other side.
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Stagger. Fillet weld symbols above and below the line are staggered. Identification line on top. Moves the dashed identification line above the symbol line. Font. To specify a font for text and size of symbols, clear Use document's font and click Font. Leader anchor. Anchor the leader to the specified location on the weld symbol. Layer. In a drawing with named layers, choose a layer from the list. Weld Symbol Favorite. ANSI Weld Symbol Properties You can create ANSI weld symbols in part, assembly, and drawing documents. The Dimensioning standard in Tools, Options, Document Properties, Detailing must be set to ANSI. Many of the properties are available both above and below the weld symbol line and are described in order from the line. A preview of the symbol is displayed in the graphics area.
Around. Adds Field/Site. Adds
to indicate that the weld is applied all around the contour. to indicate that the weld is applied in the field or on-site.
Weld Symbol. Click and select a symbol from a symbol library. Other options become available, depending on the symbol chosen. Type dimensions to the left and right of the symbol. Specification process. Type text in the box, in any number of lines, to appear in the tail of the symbol. Contour. Select None, Flat, Convex, or Concave. Finishing method. Select None, Chipping, Grinding, Hammering, Machining, Rolling, or Unspecified.
Stagger weld. Fillet weld symbols above and below the line are staggered. 2nd fillet. Type dimensions. Root opening. Type a dimension. Arrow. Offset text. Groove angle. Type an angle in degrees. Inside. Text placed inside the weld symbol. Joint with spacer. Choose None or one of the types (Double V Groove Spacer and so on). Font. To specify a font for text and size of symbols, clear Use document's font and click Font. Leader anchor. Anchor the leader to the specified location on the weld symbol. Layer. In a drawing with named layers, select a layer from the list. Weld Symbol Favorite.
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GOST Weld Symbol Properties You can create GOST weld symbols in part, assembly, and drawing documents. The Dimensioning standard in Tools, Options, Document Properties, Detailing must be set to GOST. Field. Adds Around. Adds
to indicate that the weld is applied in the field. to indicate that the weld is applied all around the contour.
Other Side. Move the arrow from the upper
to the lower
side of the leader.
Leader anchor. Anchor the leader to the specified location on the weld symbol. Layer. In a drawing with named layers, choose a layer from the list. Solder. Adds Glue. Adds
to the symbol leader. to the symbol leader.
Weld Text. Type the weld dimensions and specifications. •
The box on the left contains the text that appears on the bent leader; the other two boxes contain the text that appears above and below the horizontal leader.
•
Place the cursor in the text box where you want one of the following symbols and click the symbol button. Fillet
Stagger Check
Heat
Not all around
Smooth
Diameter
Stagger Chain
Number
Surface Finish Symbol. To add surface finish information to the symbol, under SF Symbol, select Top or Bottom to place the symbol above or below the horizontal leader. Enter the information in the Surface Finish Symbol dialog box, and click OK. To modify the surface finish information, click Details for the side you want to modify. Font. To specify a font for text and size of symbols, clear Use document's font and click Font. Weld Symbol Favorite.
Area Hatch/Fill You can apply a crosshatch pattern or solid fill to a model face or to a closed sketch profile. Area hatch can be applied only in drawings. Some characteristics of area hatch include the following: •
If you choose the area hatch to be solid fill, the default color of the fill is black. You can change the color with the Line Color
tool on the Line Format toolbar.
•
You can include area hatch in blocks.
•
You can move area hatch into layers.
•
You can select an area hatch in a Broken View only in its unbroken state; you cannot select an area hatch that crosses a break.
•
When the pointer is over an area hatch or fill, the pointer changes to
.
To set options for Area Hatch/Fill, click Tools, Options, System Options, Area Hatch/Fill.
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Example of Area Hatch/Fill and Crosshatch Area hatch on model face and in sketched profile.
Solid fill on model face.
Crosshatch in section view.
Solid fill in section view.
To add area hatch or solid fill to a model face or sketched profile:
1.
In a drawing document, select a model face, or select a segment of a closed sketch profile.
2.
Click Area Hatch/Fill
on the Drawing toolbar, or click Insert, Area Hatch/Fill.
The Area Hatch/Fill dialog box appears. 3.
Choose from the selections in Properties, Layer, Pattern, Scale, and Angle. You can clear Always show dialog on creation to prevent the dialog box from appearing whenever you insert area hatch.
4.
Click OK. The area hatch or solid fill appears in the model face or sketched profile. You can change the shape and size of a sketch profile and the area updates to fill the modified profile. To delete an area hatch, select it in the graphics area and press Delete. Sketched profiles are not deleted when the area hatch is deleted.
To edit an area hatch or solid fill:
1.
Right-click the area hatch and select Properties. The Area Hatch/Fill dialog box appears.
2.
Edit the properties and click OK.
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Area Hatch/Fill Properties You can change the properties of crosshatch, area hatch, and solid fill in drawings with this dialog box. The pattern is displayed in the Preview window. The properties available vary depending on the type of hatch or fill selected. To open the dialog box:
Right-click a crosshatch, area hatch, or solid fill and select Crosshatch Properties. - or Select a face or closed sketch profile and click Area Hatch/Fill Insert, Area Hatch/Fill.
on the Drawings toolbar, or click
To set default options:
•
To set default options for area hatch or solid fill, click Tools, Options, System Options, Area Hatch/Fill.
•
To set default options for crosshatch, click Tools, Options, Document Properties, Material Properties. You can set the Material Properties options only in part documents.
Properties. Select None, Solid, or Hatch. •
Pattern, Scale, and Angle are available only for Hatch.
•
The default color of the solid fill is black. You can change the color of the fill by selecting the fill in the graphics area and clicking Line Color
•
on the Line format toolbar.
To remove crosshatch, select None.
Pattern. Select a material from the list. Layer. Select an existing layer from the list. Scale. Set a value for the scale of the pattern. Angle. Set a value for the angle of the pattern. Material crosshatch. Uses the pattern, scale, and angle for the material specified in the part document. Apply To. If the crosshatch is on a section face, select one of the following levels: •
View. All instances in the currently active section view (lowest priority, overrides only the document default).
•
Component. All section faces on the currently selected component in an assembly.
•
Region. The currently selected surface only (highest priority, overrides all other specifications).
Always show dialog on creation. Clear to prevent the dialog box from appearing whenever you insert area hatch or solid fill.
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Blocks You can make, save, edit, and insert blocks for drawing items that you use often, such as standard notes, title blocks, label positions, and so on. Blocks can include text, any type of sketch entity (except points), balloons (except stacked balloons), imported entities and text, and area hatch. You can attach blocks to geometry or to drawing views, and you can insert them into sheet formats. Blocks can be used only in drawing documents. Example of Blocks
Title block
First angle and third angle projection
Routing schematic symbols
Blocks have the following forms: •
Definition. named in the FeatureManager design tree. If the block definition is edited, the new version appears in subsequent instances. If you link to an external file while editing the block definition, the changes are automatically applied to any instances of the block in the current document.
•
Instance. inserted into the graphics area based on a definition. Changes in properties of a block instance apply only to the selected instance.
Saving blocks is optional. You can make, edit, copy, and move blocks within a drawing document without saving the blocks to file. Pointers When the pointer is over block entities, the pointer changes to
. When the pointer is over blank spaces in a
block, the pointer changes to . • When you right-click an entity in the block instance, you access the shortcut menu for the block. •
When you right-click a space within the block instance, you access the shortcut menu for the drawing sheet.
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Base Points Blocks have a base point. When you insert or paste a block, the block instance is located so that its base point is at the insertion or paste point. Block instances are scaled and rotated about their base points. When you select a block instance, the base point is displayed in blue . You can change the position of a block base point in the block definition editor. Leaders Block leaders have an anchor point (the end anchored to the block) and an attachment point (the end attached to a model or the drawing sheet). You can add a leader to a block instance, and you can drag the leader anchor point anywhere within the block.
Note leaders that are attached to a model are frozen when included in a block. Leaders on notes within blocks do not adjust to attach to any model or sketch entity. Layers You can move sketch entities and annotations onto layers before making blocks. You can also move them onto layers in the block editor. If you change properties of layers while in the block editor, the changes apply to all entities in the layers, not just the entities in the block. Selecting a layer in the Insert Block PropertyManager or Block Instance PropertyManager applies to the block leader and arrow. To specify a default path for locating blocks:
1.
Click Tools, Options, System Options, File Locations.
2.
Under Show folders for, select Blocks from the list, then click Add.
3.
In the Browse For Folder dialog box, browse to the desired folder, then click OK. The list can include more than one directory; the first path in the list is displayed by default in the Open dialog box when you insert a block.
To create a new block in the block definition editor:
1.
In a drawing document, click Tools, Block, New. The block definition editor opens, with a temporary drawing sheet in the graphics area and the Block Definition PropertyManager in the left panel.
2.
Create the block definition with sketch tools and the Note tool. You can apply and edit Block Settings (Tag name, Read only, and Invisible) to notes as you create or edit them in the block definition editor. When editing the properties of a block instance, you can change the Value (text) of a note that has not been specified to be Read only.
3.
Close any sketches or PropertyManagers and click OK block to the FeatureManager design tree.
to close the block definition editor and add the
The block name appears under the Blocks folder in the FeatureManager design tree. You can edit the block name in the FeatureManager design tree. The block name appears in the list of available blocks when you insert a block instance (see below). You can also save the block to file (see below).
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To create a new block from entities in a drawing:
1.
In a drawing, sketch the entities that make up the block. To add text, use the Note tool.
2.
Box-select all the entities.
3.
Click Tools, Block, Make. If you select entities for the block that belong to one view, the block belongs to the view. If you select entities for the block that belong to more than one view, the block then belongs to the sheet. If you link a note to a system or custom property, the block stores the system variable ($PRPMODEL, for example) that identifies the entity to which the note is attached and resolves the link when block instances are attached to the model, view, sheet, or document. It also stores and later resolves the system or custom variable name ("SW-Created Date", for example). The block name appears under the Blocks folder in the FeatureManager design tree. You can edit the block name in the FeatureManager design tree. The block name appears in the list of available blocks when you insert a block instance (see below). You can also save the block to file (see below).
4.
Click OK
.
To move or copy a block:
To move a block, select the block and drag it. To copy a block, press Ctrl while dragging the block. To save a block:
Right-click the block and select Save to File. - or Select the block and click Tools, Block, Save to File. The Save As dialog box appears. The default extension for block files is .sldblk. The SolidWorks software still supports .sldsym for inserting blocks and editing blocks, but all new blocks saved to external files use the .sldblk extension. NOTE: Properties of the block (scale and rotation angle) are saved in the file. To insert a block into a drawing:
1.
Click Insert Block
, or click Insert, Block.
The Insert Block PropertyManager appears. NOTE: You can also drag a block from the Blocks folder in the FeatureManager design tree into the graphics area. 2.
Under Source, do one of the following: Select a block Name from the list of blocks in the drawing document. - or Click Browse and browse to an external file that contains a block definition. You can insert files with extensions .sldblk, .sldsym, .dwg, and .dxf. If desired, select Create external reference to file to link the definition in the document to the file definition.
3.
Click in the graphics area as many times as necessary to place as many copies of the block as you want. The block is positioned so that the block base point is at the point in the graphics area where you click. The block base point snaps to grid points if Snap to points is enabled in Tools, Options, Document Properties, Grid/Snap, and to sketch entities and annotations. If you press Esc while inserting blocks, all instances created in the current operation are lost.
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4.
Click OK
.
You can edit block notes either for all instances or for each instance individually. Edit the text in the Block Definition PropertyManager to apply the change to all instances. To enable editing of each instance, give the note a tag name in the definition and then edit the note attribute in the Block Instance PropertyManager. You cannot doubleclick a block note to edit it on screen. To edit the properties of a block instance:
1.
Select a block instance in the graphics area.
2.
The Block Instance PropertyManager appears.
3.
Specify a leader, scale, rotation angle, and text display. Click Attributes to edit the values of notes.
4.
Click OK
.
To edit a block definition:
1.
Select the block definition in the FeatureManager design tree and click Tools, Block, Edit Definition. - or Right-click the block definition in the FeatureManager design tree, or right-click a block instance in the graphics area, and select Edit Definition. The block appears on a temporary sheet and the Block Definition PropertyManager opens.
2.
You can add, delete, and edit entities in the graphics area. In the Block Definition PropertyManager, you can edit the name of the block, change the base point position, and link the block definition to a file.
3.
Click OK
to save changes and remake the block.
To explode a block:
1.
Right-click the block in the graphics area and select Explode. - or Select the block and click Tools, Block, Explode.
2.
To remake the block, select the entities to include and click Tools, Block, Make. The name of the new block appears in the FeatureManager design tree with the next sequence number. If you explode a block that is on a layer, the entities retain their old colors when you move them to a new layer. To reset the colors so that the entities inherit the color of the new layer, first select the entities, click Line Color
on the Line Format toolbar, select Default, and click OK.
To change the position of the block base point:
1.
Edit the block definition (see above). The base point of the block is identified in the graphics area of the block definition editor by
2.
. The
pointer changes to . Drag the base point to any position in the editor's graphics area. - or Under Base Point in the Block Definition PropertyManager, enter relative values in the X Coordinate and Y Coordinate
boxes.
The original base point position is identified by 3.
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Click OK
.
.
To change the position of the leader attachment point and leader anchor point:
1.
Select a block instance.
2.
In the Block Instance PropertyManager, under Arrow/Leader, select Display leader. NOTE: The block must have a leader in order for you to change the position of the leader attachment point and anchor point. The leader attachment point appears by default at the lower left corner of the block, on top of the anchor point.
3.
In the graphics area, select the leader attachment point (the pointer changes to point) and drag it anywhere on the drawing sheet.
when it is over the
The leader anchor point is now visible. 4.
Select the leader anchor point (the pointer changes to another position within the block.
when it is over the point) and drag the point to
Insert Block PropertyManager The Insert Block PropertyManager appears when you insert a block instance into a drawing. To insert a block:
1.
Click Insert Block
on the Annotation toolbar, or click Insert, Block.
2.
Select a block under Source, or browse to a block file.
3.
Specify the properties described below, then click in the graphics area to place the block.
4.
Repeat steps 2 and 3 as many times as necessary, then click OK
.
Source Select the block to insert by one of the following methods: •
Name. Select a block name from the list of blocks in the document.
•
Browse. Browse to a block file (.sldblk, .sldsym, .dwg, .dxf).
Location As you move the pointer, the coordinates of the block base point appear in the X Coordinate
and Y Coordinate
boxes. Click in the graphics area to place the block. You can enter values for X Coordinate and Y Coordinate for the last block inserted.
Blocks snap to grid if snap is enabled in Tools, Options, Document Properties, Grid/Snap, and to sketch entities and annotations. If the block has a leader, place the leader first, then the block. Block Display Block Scale . Enter a positive non-zero number. If you enter an invalid number (zero or negative), the scale is reset to the previous valid number. Block Rotation
. Enter a value in degrees. A positive value rotates the block counterclockwise.
Leader Display leader. Select to attach a leader to the block. Bent leader. Select to add a horizontal segment at the block end of the leader. Arrowhead Style. Select a style from the list.
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Layer In drawings with named layers, select a layer that applies to the block leader and arrow. Block Instance PropertyManager You can control block leaders, arrows, scale, rotation angle, and text display while you insert a block instance or for an existing block instance. Block Display Block Scale . Enter a positive non-zero number. If you enter an invalid number (zero or negative), the scale is reset to the previous valid number. Block Rotation
. Enter a value in degrees. A positive value rotates the block counterclockwise.
Text Display Select one of the following for display of note text: •
Normal. Notes are displayed based on their visibility settings.
•
All. All text is displayed, regardless of visibility settings.
•
None. No text is displayed.
Attributes. Click to edit values of note attributes. Leader Display leader. Select to attach a leader to the block. Bent leader. Select to add a horizontal segment at the block end of the leader. Arrowhead Style. Select a style from the list. Layer In drawings with named layers, select a layer that applies to the block leader and arrow. Move sketch entities and annotations onto layers in the block definition, or before making the block. Attributes You can edit the values of Block attributes in this editor. Changes apply to the current instance of the block. Attributes can be created automatically when you import blocks from AutoCAD files, or manually when you assign a Tag name (and specify Invisible or Read Only, or both) when you insert a note into a block definition. NOTE: Attributes in SolidWorks drawings can have multi-line values (note text). However, if you plan to export blocks to AutoCAD, you should use only single-line values. To access the editor, select a block instance in a drawing document and click Attributes in the Block Instance PropertyManager. The following columns appear in the editor: •
Name. The name of the attribute (Tag name in the Note PropertyManager).
•
Value. The value, or text, of the attribute. You can edit the value if the attribute is not Read Only.
•
Invisible. This column contains an X if the attribute is invisible (information only).
•
Read Only. This column contains an X if the attribute is read only (information only). NOTE: Values that are linked to file properties or custom properties display the link path and variable name ($PRP:"SW-File Name", for example) during editing but show the values of the properties (WIDGET, for example) when block instances are inserted into drawings.
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Block Definition PropertyManager Edit the block definition and specify the properties described below. To access the block editor:
•
Right-click the name of the block in the FeatureManager design tree and select Edit Definition.
•
Right-click a block instance in the graphics area and select Edit Definition.
•
Select the name of the block in the FeatureManager design tree and click Tools, Block, Edit Definition.
•
Select a block instance in the graphics area and click Tools, Block, Edit Definition. The block is displayed on a temporary sheet in the graphics area and the Block Definition PropertyManager opens.
The block is in exploded form in the definition editor. When you click OK definition is automatically remade.
to exit from the editor, the block
You can move sketch entities and annotations onto layers. Changes you make to layer properties while in the block editor apply to all entities in the layer, not just the block entities. Block Name Type to edit the block name. The name appears in the FeatureManager design tree. Base Point Drag the base point (designated by
, initially at the lower left corner of the block) to a new relative position or
enter values for its relative X Coordinate was opened is identified by
and Y Coordinate
. The position of the base point when the editor
.
When you insert a block in a drawing graphics area, the block instance is located so that its base point is at the insertion point. External Reference If you selected the Create external reference to file check box in the Open dialog box when you inserted the block into the drawing document from a file, Link to file is selected automatically and the file name appears in the box. If you select Link to file after you open the block definition editor, the local definition updates to reflect any changes in the selected file definition. When you exit from the definition editor, the local definition is still linked to the specified file and reflects any subsequent changes to the file definition. When Link to file is selected, you cannot edit the block definition. To edit the file definition, select the file name in the FeatureManager design tree and click Tools, Block, Edit File.
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Tables Annotation Tables Tables are available on the Annotation toolbar for: •
Bills of Materials
•
Hole Tables
•
Revision Tables
•
Weldment Cut Lists
All tables have the following functionality: •
Drag with the pointer
•
Snap to an anchor point that you can set
•
Snap to lines, points, and vertices in the sheet format
•
Use standard or custom templates
•
Add columns and rows and adjust their dimensions
•
Select and delete tables, columns, and rows
•
Split or merge tables
•
Merge or split cells
•
Sort the contents of columns
•
Zoom to selection
•
Control color in layers
Selecting the title bar selects the whole table for such operations as dragging, formatting, and adjusting column width or row height. To drag a table:
1.
In the table PropertyManager, clear Attach to anchor.
2.
Hold Alt and drag the table from anywhere inside the table - or Drag the table title bar.
To snap a table to sheet format entities:
1.
Drag the table toward a vertical or horizontal line, a point, or a vertex in the sheet format.
2.
As the edge of the table snaps to the line or point, release the pointer.
To add a column or row to a table:
In the column or row where you want to add the new column or row, right-click and select Insert: •
Column Right
•
Column Left
•
Row Above
•
Row Below
To adjust column width or row height:
Drag a border - or Select one or more columns or rows (or select the whole table by the title bar), right-click and select Formatting, Column Width or Row Height, then type a number in the dialog box.
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To select or delete a table, column, or row:
Right-click in the table and choose Select or Delete, then Table, Column, or Row. To split a table:
Right-click in the table and select Split: •
Horizontally Above
•
Horizontally Below
•
Vertically Left
•
Vertically Right
To merge a table that has been split, right-click in a section of the table and select Merge. To merge or split cells:
1.
Select the cells.
2.
Right-click and select Merge or Split.
To sort columns in a Bill of Materials:
1.
Right-click in the Bill of Materials and select Sort.
2.
Select options in the Sort dialog box, then click OK.
To sort a column in a hole table or weldment cut list:
Right-click in a column and select Sort, Ascending or Descending. Editing Tables •
If you edit items in a table, automatic controls do not change them. To edit text, double-click the text and edit on screen. The Note PropertyManager appears, allowing you to format the text in addition to editing it.
•
If the cell value is parametrically linked to a part or assembly document, a message warns you that editing the value will sever the link. To restore the link in the future, delete the user-defined text from the cell.
PropertyManagers Each table has PropertyManagers for: •
Table Properties
•
Table Format
•
Column Properties
•
Cell Properties
Buttons for the other PropertyManagers appear at the bottom of each PropertyManager, as appropriate.
Table Anchors Each type of annotation table has its own anchor point in a drawing sheet format. To set a table anchor point:
1.
In the FeatureManager design tree, expand
Sheet Format for the active drawing sheet.
2.
Right-click the anchor you want to set and select Set Anchor. Choose from: Bill of Materials Anchor Hole Table Anchor Weldment Cut List Anchor Revision Table Anchor
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3.
Click in the graphics area to specify the anchor point. You are in Edit Sheet Format mode.
4.
Right-click in the graphics area and select Edit Sheet.
In the table PropertyManagers, select the corner of the table to attach to the anchor point.
Table Templates Standard templates for Bills of Materials, Hole Tables, Revision Tables, and Weldment Cut Lists are available in
File Name Extension
Bill of Materials Hole Table Revision Table Weldment Cut List
.sldbomtbt .sldholtbt .sldrevtbt .sldwldtbt
Custom templates contain headings and formatting, but not table contents. The table PropertyManagers remember the last used template. To change the location of table templates:
1.
Click Tools, Options, System Options, File Locations.
2.
Under Show folders for, select: •
BOM Templates
•
Hole Table Templates
•
Revision Table Templates
•
Weldment Cut List Templates
3.
Click Add, browse to a folder, and click OK.
4.
Repeat steps 2 and 3 as necessary, then click OK.
To save a custom template:
1.
Insert a table into a drawing.
2.
Customize the table.
3.
Right-click in the table and select Save as template.
4.
In the Save As dialog box, type in the template name, browse to a folder, and click Save.
To use a custom template:
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1.
When inserting a table, under Table Template in the PropertyManager, click Browse for template.
2.
In the Select Template dialog box, browse to a template, then click Open.
Custom Table Templates You can customize standard table templates to save for future use. To customize a table template:
1.
2.
3.
Open a model that contains the characteristics needed for the template: •
Components
•
Custom properties
Insert a table. In the table PropertyManager, specify one of the standard templates shipped with the SolidWorks software; for example: •
bom-standard.sldbomtbt for a Bill of Materials
•
standard hole table--letters.sldholtbt for hole table
•
standard revision block.sldrevtbt for a revision table
•
cut list.sldwldtbt for a weldment cut list
Edit the table as described below, then save the table as a template.
To add a column:
1.
Right-click in a table column and select Insert, Column Right or Column Left.
2.
In the Column PropertyManager, select from the list of Column Properties. To select a custom property, the property must be available in the model documents. For properties in the various types of tables, see the Column PropertyManager topic for Bill of Materials, hole tables, revision tables, or weldment cut lists.
3.
Edit the column Title.
To add a row:
Right-click in a table row and select Insert, Row Above or Row Below. See Annotation Tables for procedures to adjust column width or row height, split or merge a table or cells, sort columns, and so on.
Table Format PropertyManager Specify formatting for a Bill of Materials, Hole Table, Revision Table, or Weldment Cut List. To specify formatting for a table:
1.
In one of the table PropertyManagers (Table, Column, or Cell), click Table Format.
2.
Specify the formatting described below, then click OK
.
Header Title. Edit the table header title if Display title is selected. Display title. Displays the text in Title in a header row across the width of the table. Position. The header can be at the Top
or the Bottom
of the table.
Border Click Box Border
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, Grid Border
, or All Borders
, then select a corresponding thickness.
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Text Format Table text format for the document is set in Tools, Options, Document Properties, Annotations Font. You specify formatting for individual tables in this PropertyManager and override formatting for individual cells in the Table Cell PropertyManager. •
Click Left Justify
, Center Justify
, or Right Justify
to justify text horizontally.
•
Click Top Justify
, Middle Justify
, or Bottom Justify
•
Use document's font. When selected, the text is in the font specified for Tables in Tools, Options, Document Properties, Annotations Font.
•
Font. When Use document's font is cleared, click Font to open the Choose Font dialog box and select a new font style, size, and effect to apply to the table. You can specify a different font for cells.
to justify text vertically.
Layer In drawings with named layers, select a layer. Table Properties Click to access the table properties. Cell Properties Click to access the Table Cell PropertyManager. Column Properties Click to access the table column properties. BOM Contents In a Bill of Materials, click to access the Bill of Materials Contents dialog box.
Table Cell PropertyManager Specify formatting for one or more cells in a Bill of Materials, Hole Table, Revision Table, or Weldment Cut List. Table text format is set in the Table Format PropertyManager. You override formatting for individual cells in this PropertyManager. To specify formatting for cells:
1.
Select one or more cells in a table - or Click Cell Properties in another table PropertyManager.
2.
Specify the formatting described below, then click OK
.
Text Format
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•
Click Left Justify
, Center Justify
, or Right Justify
to justify text horizontally.
•
Click Top Justify
, Middle Justify
, or Bottom Justify
•
Click Rotate
•
Use table's font. When selected, the text is in the font specified in the Table Format PropertyManager.
•
Font. When Use table's font is cleared, click Font to open the Choose Font dialog box and select a new font style, size, and effect for the selected cells.
to justify text vertically.
to rotate the text in 90° increments counterclockwise.
Column Properties Click to access the table column properties. Table Properties Click to access the table properties. Table Format Click to access the Table Format PropertyManager.
Bill of Materials You can insert Bills of Materials into assembly drawings. A drawing can contain a table-based Bill of Materials or an Excel-based Bill of Materials, but not both. The table-based Bill of Materials is based on SolidWorks tables and includes: •
Templates
•
Anchors
•
Quantities for configurations
•
Whether to keep items that have been deleted from the assembly
•
Zero quantity display
•
Excluding assembly components
•
Following assembly order
•
Item number control
Example of Bill of Materials
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You can specify a starting Item Number, but the increment is always a single integer (1, 2, 3 ..., or 100, 101, 102 ..., for example). You can change the text in any cell by double-clicking and editing on screen, but if you edit data generated by SolidWorks (Item Number, Quantity, and so on), you break the link between the data and the Bill of Materials. To set options for a Bill of Materials in the active document:
1.
Click Tools, Options, Document Properties, Tables.
2.
Set options under Bill of Materials Table, then click OK.
To insert a Bill of Materials into a drawing document:
1.
Click Bill of Materials
on the Annotation toolbar, or click Insert, Tables, Bill of Materials.
2.
Select a drawing view to specify the model.
3.
Set the properties in the Bill of Materials PropertyManager, then click OK
4.
If you did not select Attach to anchor, click in the graphics area to place the table.
.
To exclude assembly components from Bills of Materials:
1.
In the assembly document, right-click the component and select Properties.
2.
In the Component Properties dialog box, select Exclude from bill of materials, then click OK.
To sort columns in a Bill of Materials:
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1.
Right-click anywhere in the Bill of Materials and select Sort.
2.
In the Sort dialog box, choose up to three columns to sort by, select other options, then click OK.
Bill of Materials PropertyManager Specify properties for Bills of Materials. To specify properties for Bills of Materials:
1.
Click Bill of Materials
on the Annotation toolbar, or click Insert, Tables, Bill of Materials.
2.
Specify the properties described below, then click OK
.
Table Template Click Browse for template insertion.
to choose a standard or custom template. This option is available only during table
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. BOM Type Select: •
Top level only. List parts and sub-assemblies, but not sub-assembly components.
•
Parts only. Does not list sub-assemblies. Lists sub-assembly components as individual items.
•
Indented assemblies. Lists sub-assemblies. Indents sub-assembly components below their sub-assemblies without item numbers.
Configurations Lists quantities in the Bill of Materials for all selected configurations. Select configurations manually, or click Select all configurations
or Unselect all configurations
.
Part Configuration Grouping Display as one item number. If a component has multiple configurations, all the configurations appear with the same item number. Use this option with BOM Type set to Top level only. To see the configuration name in the PART NUMBER column, go to the part document. On the Configuration tab, right-click each configuration, and select Properties. Under Part number displayed when used in a bill of materials, select Configuration Name. Keep Missing Item If components have been deleted from the assembly since the Bill of Materials was created, you can keep the components listed in the table. If missing components are still listed, the text for the items can appear with strikethrough display.
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Zero Quantity Display If an assembly component does not appear in a configuration, displays the zero quantity with a dash (-), a zero (0), or a blank cell. Item Numbers Start at. Type a value for the beginning of the item number sequence. The sequence increases by single digits. Click Follow assembly order for the item numbers to follow the order in which the assembly appears in the FeatureManager design tree. For components with multiple instances, the first instance appears in the order of the FeatureManager design tree, and subsequent instances increment the quantity. Click Do not change item numbers to keep the item numbers with their components when reordering rows (manually in BOM Contents, by sorting, or when you click Follow assembly order, for example). BOM Contents Click to access the Bill of Materials Contents dialog box. Table Format Click to access the Table Format PropertyManager. Cell Properties Click to access the Table Cell PropertyManager. Column Properties Click to access the Bill of Materials Column PropertyManager. Bill of Materials Contents In this display of the Bill of Materials contents, you can move rows up or down, and you can group and ungroup rows. To edit Bill of Materials Contents:
1.
In the Bill of Materials, Column Properties, Cell Properties, or Table Format PropertyManager, click BOM Contents.
2.
Edit properties as described below, then click Apply.
3.
Click OK.
Show balloon state Toggle row visibility Row up
. The icon shows whether the component has a balloon . Click the icon to hide
or Row down
or show
or not
.
the row.
. Select a row and click to move the row up or down.
To keep the item number with its component when reordering rows, click numbers in the Bill of Materials PropertyManager.
Do not change item
Group and Ungroup . Select two or more rows to group the components under one item number. To dissolve the group, select a member and click Ungroup.
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Bill of Materials Column PropertyManager Specify the columns to be included in a Bill of Materials and their position in the table. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To edit Bill of Materials column properties:
1.
2.
Access the PropertyManager by one of the following methods: •
Add a new column to the Bill of Materials
•
Click at the head of a column when the pointer changes to
•
Click Column Properties in another Bill of Materials PropertyManager (Cell, Table Properties, Table Format)
Specify the properties described below, then click OK
.
Column Properties For the selected column, choose one of the following column types, listed with its header title. You can edit the header in the Title box below. •
Item Number. ITEM NO.
•
Part Number. PART NUMBER
•
Quantity. QUANTITY
•
User Defined. Select a document property under Custom Property.
Custom Property. Document's custom properties, available when you specify User Defined under Column Properties. Use Title Summary. In Part Number, use the data in the Title field of File, Properties, Summary Information in part documents. Title. Edit the text of the column header. Column position. Click Move Column Left
or Move Column Right
to move the selected column.
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Bill of Materials PropertyManager. Table Format Click to access the Table Format PropertyManager. BOM Contents Click to access the Bill of Materials Contents dialog box. Bill of Materials Sort To sort the columns of a Bill of Materials:
1.
Right-click anywhere in the Bill of Materials table and select Sort.
2.
Edit the options as described below, then click OK.
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Sort by Select the name of a column and either Ascending or Descending for the primary sort. Then by Select the name of a column and either Ascending or Descending for a secondary sort. Then by Select the name of a column and either Ascending or Descending for a tertiary sort. Group items Assemblies, Parts, Other. Select one or more category to sort rows within the category. If you select more than one category, order them by selecting one and clicking Up or Down. Other is user-defined data (oil or grease, for example). Item numbers Do not change item numbers. Select to keep the item numbers with the configuration row.
Hole Tables Hole tables in drawing documents measure the positions of selected holes from a specified origin datum. The software labels each hole with a tag that corresponds to a row in the table. Non-circular holes such as rectangles and slots are recognized as holes. The table lists the X and Y coordinates of the entities, but you must enter the size. In addition to the functionality for all tables, you can specify in options and in the Hole Table PropertyManager: •
Tags to be alphabetic or numeric
•
Tag leaders to be visible
•
Cells with the same tags to be combined
•
Cells for holes of the same size to be combined
•
Precision of hole locations
Example of Hole Tables
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To set options for hole tables in the active document:
1.
Click Tools, Options, Document Properties, Tables.
2.
Set the options under Hole Table, then click OK.
To create a hole table:
1.
Click Hole Table
on the Annotation toolbar, or click Insert, Tables, Hole Table.
2.
In the graphics area, select a vertex to specify the origin datum. You can select an X axis and Y axis to define a vertex for the datum. You can also drag the origin datum into position after you place the table.
3.
Select hole edges, or select a model face to include all the holes on the face.
4.
In the PropertyManager, select a template or anchor, then click OK
5.
If you did not select Attach to anchor, click in the graphics area to place the table.
.
To edit the origin datum:
Select the datum in the graphics area - or Right-click the hole table in the FeatureManager design tree and select Edit datum definition. To add holes to a table:
Right-click the hole table in the FeatureManager design tree and select Add holes.
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To format hole tags:
1.
Select one or more tags.
2.
In the Note PropertyManager: •
Under Text Format, specify justification, angle, and font.
•
Under Border, select a border style and size.
•
Under Leader, select a leader and arrow. Apply to all applies to all the arrows on the selected tags. To see a preview leader without adding a visible leader, hold the pointer over the tag for a few seconds. The leader and arrow appear in red.
• 3.
Under Layer, in drawings with named layers, select a layer.
Click OK
.
Hole Table Add Holes To add holes to an existing hole table:
1.
Right-click the table in the FeatureManager design tree and select Add Holes.
2.
Select edges of holes or faces containing holes, then click OK
.
Hole Table PropertyManager Specify properties for existing hole tables. For new hole tables, see Hole Table Insert PropertyManager. To specify properties for hole tables:
1.
2.
Access the PropertyManager by one of the following methods: •
Right-click anywhere in the table and select Properties.
•
Right-click the table in the FeatureManager design tree and select Properties.
•
In another PropertyManager (Cell, Column, or Table Format), click Table Properties.
Specify the properties described below, then click OK
.
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. Alpha/Numeric Control Specify the tags identifying the holes to be letters or numbers. Scheme Combine same tags. Combines rows with holes in the same pattern, which also combines holes with the same sizes. The columns of location values are removed. Combine same sizes. Available only if Combine same tags is cleared. Merges cells for holes of the same size. The columns of location values remain.
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Hole Location Precision Specify the number of significant digits for the hole location values. Visibility Select to hide any or all of the following: •
Hide origin indicator
•
Hide hole centers
•
Hide hole tags
Table Format Click to access the Table Format PropertyManager. Hole Table Axis PropertyManager To edit the hole table origin datum:
1.
Select the hole table origin datum in the graphics area. The pointer changes to
when it is over the origin datum.
2.
Edit the axis labels, font, and layer.
3.
To edit the position of the datum, click Edit datum definition.
4.
Click OK
.
You can drag the origin datum to a new location in the graphics area. The location values in the table update. Hole Table Insert PropertyManager Specify properties for new hole tables. For existing hole tables, see Hole Table PropertyManager. To specify properties for new hole tables:
1.
Click Hole Table
on the Annotation toolbar, or click Insert, Tables, Hole Table.
2.
Specify the properties described below, then click OK
.
Table Template Click Browse for template insertion.
to choose a standard or custom template. This option is available only during table
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor.
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Datum During insertion, Origin is ready for you to select a vertex. To define the origin with an X axis and Y axis, click X Axis Direction Reference and select a horizontal model edge in the graphics area, then click Y Axis Direction Reference and select a vertical model edge. After the table has been created, you can drag the datum origin to another position. The location values in the table update. To edit the origin datum, select it in the graphics area, or right-click in the FeatureManager design tree and select Edit datum definition. Holes Select individual hole edges, or select a model face to include all the holes in the face. After the table has been created, right-click the hole table in the FeatureManager design tree and select Add Holes. Hole Table Column PropertyManager Specify the columns to be included in a hole table and their position in the table. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To edit hole table column properties:
1.
2.
Access the PropertyManager by one of the following methods: • •
Add a new column to a hole table. Click at the head of a column when the pointer changes to
•
Click Column Properties in another hole table PropertyManager.
Specify the properties described below, then click OK
.
.
Column Properties For the selected column, choose one of the column types, listed with its header title. You can edit the header in the Title box below. •
X. XLOC
•
Y. YLOC
•
Hole. TAG
•
Quantity. QUANTITY
•
Size. SIZE
•
Custom. Type a header under Title.
Title. Edit the text for the column header. Column position. Click Move Column Left
or Move Column Right
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Hole Table PropertyManager. Table Format Click to access the Table Format PropertyManager.
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to move the selected column.
Revision Tables Insert a revision table into a drawing to track document revisions, including revision symbols. In addition to the functionality for all tables, you can select: •
Revision symbol shapes
•
Alphabetic or numeric sequence The latest revision also appears under REV in the lower-right corner of a sheet format.
To set options for revision tables in the active document:
1.
Click Tools, Options, Document Properties, Tables.
2.
Set the options under Revision Table, then click OK.
To insert a revision table:
1.
Click Revision Table
on the Annotation toolbar, or click Insert, Tables, Revision Table.
2.
Set the properties in the Revision Table PropertyManager, then click OK
.
To add a revision to the table:
Right-click in the revision table and select Revisions, Add Revision.
Revision Symbols You can add revision symbols (the revision letter or number enclosed in a circle, triangle, square or hexagon) to the drawing. •
If you select Enable symbol when adding new revision under Options in the Revision Table PropertyManager, you can click in the graphics area to place symbols when you add a revision to the table.
•
If you clear Enable symbol when adding new revision or to add a symbol later, right-click in a row of the revision table and select Revisions, Add Symbol, then click in the graphics area to place symbols.
•
If you edit revision text, the symbols update.
Alphabetic or Numeric Control You can choose either letters or numbers for revisions in Tools, Options, Document Properties, Tables. If you switch from one to the other, you can change the revisions already in the table, or you can leave them unchanged and continue with future revisions in the new format. Any revision text you edit remains unchanged by automatic operations.
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Note Linked to Revision Level You can link a note (generally at the lower left in the Sheet Format) to the revision letter so that it is synchronized. To synchronize the revision in a note:
1.
With no revision table in the drawing, right-click in the graphics area and select Edit Sheet Format.
2.
Click Note
3.
In the PropertyManager, click Link to Property
4.
In the dialog box, click File Properties.
5.
In the Summary Information dialog box, select the Custom tab and do the following:
on the Annotation toolbar and click in the graphics area to place the note. .
a.
Under Name, select Revision (type Revision if it does not appear in the list).
b.
Place the pointer in the Value field and press the space bar.
c.
Click Add.
d.
Click OK.
6.
In the Link to Property dialog box, under Use custom property from, select Revision from the list, then click OK.
7.
Right-click in the graphics area and select Edit Sheet.
8.
Insert a revision table. The note displays the latest revision level.
Revision Table PropertyManager Specify properties for revision tables. Table Template Click Browse for template insertion.
to choose a standard or custom template. This option is available only during table
Table Anchor Set the Anchored corner to: Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. Revision Symbol Shapes Select a border shape for revision symbols: Circle Triangle Square Hexagon
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Options Enable symbol when adding new revision. Allows you to click in the graphics area to place revision symbols when you add a revision to the table. Table Format Click to access the Table Format PropertyManager. Revision Table Column PropertyManager Specify the columns to be included in a revision table and their position in the table. The columns are populated with data from the document's properties. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To edit revision table column properties:
1.
2.
Access the PropertyManager by one of the following methods: •
Add a new column to a revision table
•
Click at the head of a column when the pointer changes to
•
Click Column Properties in another revision table PropertyManager.
Specify the properties described below, then click OK
.
Column Properties For the selected column, choose one of the column types, listed with its header title. You can edit the header in the Title box below. •
Zone. ZONE
•
Revision. REV.
•
Description. DESCRIPTION
•
Date. DATE
•
Approved. APPROVED
•
Custom Properties. Select a document property under Properties.
Properties. Document's custom properties, available when you specify Custom Properties under Column Properties. Title. Edit the text for the column header. Column position. Click Move Column Left
or Move Column Right
to move the selected column.
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Revision Table PropertyManager. Table Format Click to access the Table Format PropertyManager.
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Excel-based Bill of Materials Bill of Materials Overview Applies to Excel-based Bills of Materials. A drawing can contain an Excel-based Bill of Materials or a tablebased Bill of Materials, but not both. You can insert a bill of materials (BOM) into the drawing of an assembly. If you add or delete components in the assembly, the bill of materials automatically updates to reflect the changes if you select the Automatic update of BOM option under Tools, Options, Document Properties, Detailing. Such changes include adding, deleting, or replacing components, changing component names or custom properties, and so on. •
If you do not select Automatic update of BOM, you must delete and re-insert the BOM to update it NOTE: To insert a bill of materials in a drawing, you must have Microsoft Excel 97 or later installed on your computer.
•
Rows in bills of materials are combined when all fields (except for Item Number) are the same. However, bills of materials in drawings created in releases prior to SolidWorks 2000 are not automatically updated to combine rows.
•
You can insert balloons or stacked balloons that label the parts in an assembly and relate them to item numbers in the bill of materials.
•
If you change the Item Number in a balloon, the item number in the bill of materials also changes.
•
SolidWorks includes several BOM templates in the following directory: \install_directory\lang\english.
•
You can embed dimensions and mass property parameters into values of custom properties in part documents. You can then include the custom properties in a bill of materials. The values in the BOM update automatically if the part dimensions or mass properties change.
To hide a bill of materials:
Right-click the bill of materials in the graphics area or in the FeatureManager design tree and select Hide Bill of Materials. NOTE: To show the bill of materials again, right-click the bill of materials in the FeatureManager design tree (expand the drawing view if necessary) and select Show Bill of Materials.
Bill of Materials Templates Applies to Excel-based Bills of Materials. The default template, Bomtemp.xls, contains columns for ITEM NO., QTY., PART NO., and DESCRIPTION. The SolidWorks software populates the columns in the default template automatically. Other templates supplied with the software add the following columns to the default format. BOM template file name
Columns added to default format
Bomtemp-Material.xls
MATERIAL
Bomtemp-StockSize.xls
STOCK SIZE
Bomtemp-Vendor.xls
VENDOR NO
Bomtemp-Weight.xls
WEIGHT
Bomtemp-All.xls
VENDOR NO, WEIGHT, STOCK SIZE, MATERIAL
You must add the custom properties into the parts of your assembly in order to take advantage of the additional columns in these templates.
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Bill of Materials - Inserting Applies to Excel-based Bills of Materials. You can insert a bill of materials into the drawing of an assembly. If you add or delete components in the assembly, the bill of materials automatically updates if you have selected the Automatic update of BOM option under Tools, Options, Document Properties, Detailing. NOTE:To insert a bill of materials into a drawing, you must have Microsoft Excel 97 or later installed on your computer. To insert a bill of materials:
1.
With a drawing view selected, click Insert, Bill of Materials.
2.
In the Select a BOM Template dialog box, select an Excel template for the BOM and click Open. NOTE: The default BOM template is in install_folder\lang\english\bomtemp.xls.Several other BOM templates are available in the same directory. You can customize the templates by adding columns or changing the text formatting. You can also create new templates to meet your company’s standards.
3.
In the Bill of Materials Properties dialog box, select properties from the Configuration, Contents, and Control tabs.
4.
Click OK.
A bill of materials is displayed that lists the components of the assembly.
Bill of Materials - Configuration Applies to Excel-based Bills of Materials. The Configuration tab in the Bill of Materials Properties dialog box specifies basic display properties of a bill of materials. The other tabs available in the dialog box are Contents and Control. The software remembers your selections from session to session. The Configuration tab controls the following properties. •
Use summary info title as part number. If you assigned a part identifier number in the title box of the Summary Info for the part, you can use that identifier in the bill of materials.
•
Use the document’s note font when creating the table. When selected, the BOM uses the text font specified for notes, under Tools, Options, Document Properties, Detailing, Notes, Font. Otherwise, the font specified in the BOM template is used.
•
Choose one of the following to specify the way to list sub-assemblies and their components in the bill of materials: o
o
o
Show parts only. Select this option to list only parts in the bill of materials. Subassemblies are not listed; their components are listed as individual items. Show top level subassemblies and parts only. Select this option to list parts and subassemblies in the bill of materials. Each subassembly type is an item; the individual subassembly components are not listed. Show assemblies and parts in an indented list. Subassemblies are listed as items; subassembly components are shown below the subassembly to which they belong, but without item numbers.
•
Anchor point. Select or clear Use table anchor point. The standard templates supplied with the software include an anchor point for placing the BOM in a specific location on the sheet. To use the point, select this option, then select which corner of the BOM table to make coincident with the point (top left, bottom right, and so on). If you do not use the anchor point, the BOM is placed on the sheet near the selected view.
•
Add new items by extending top border of table. New components are always added at the bottom of the table, and the rest of the table shifts upward. The last row of the table remains in the same position on the drawing sheet. This option applies only when you do not use an anchor point.
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Bill of Materials - Contents Applies to Excel-based Bills of Materials. The Contents tab in the Bill of Materials Properties dialog box specifies which items appear in the bill of materials, and allows you to reverse the order of the list. The other tabs available in the dialog box are Configuration and Control. The Contents tab controls the following properties: •
Select which items to include in the table. A green check mark in the ITEM NO. column means that the item is displayed in the table. Clear the check mark to hide the item. This has the same effect as hiding the row in the Excel worksheet.
•
To move the header row to the bottom of the table, and to list the items in order from bottom to top, clear the Display labels at top check box.
•
To sort the items alphanumerically by a column (for example, to sort by part number), hold down the Ctrl key, and click the box at the top of the column. The item numbers are re-assigned so that the first line is still Item 1, and the remaining item numbers are in order. NOTE: If you do not hold down the Ctrl key, the item number for each line stays with the original item, resulting in a list with item numbers out of order.
Bill of Materials - Control Applies to Excel-based Bills of Materials. The Control tab in the Bill of Materials Properties dialog box specifies how row numbers are assigned, what happens when a component is deleted, and how to split long BOM tables. The other tabs available in the dialog box are Configuration and Contents. The Control tab controls the following properties: Row numbers •
Row numbers follow assembly ordering. Select to use the item numbers assigned by the software. Clear to assign the item numbers in Excel, and override the system-defined item numbers. NOTE: When you select this check box: o o
•
Any sorting other than by Item No. is not preserved in the Bill of Materials. If you try to change an item number in a balloon, a message appears stating that you cannot change the item number.
Reserve row numbers for missing components. Specify what happens if a component is removed from the assembly. o o
No. The rows for the removed components are deleted from the table. Yes. Specify how the row is displayed: Display with zero quantity, Hide, or Display with strike through text.
Split Tables •
Split tables into multiple sections. Select to allow the table to split.
•
Table height before splitting. Specify a value for the height.
•
Split direction for new sections. Select Left or Right from the list. If the BOM exceeds the height you specify, the table splits and continues in another column to the Left or Right.
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Bill of Materials - Edit Text Applies to Excel-based Bills of Materials. To edit text in a bill of materials (BOM):
1.
Double-click the BOM, or right-click the BOM and select Edit Bill of Materials. While the bill of materials is active, it is displayed with shaded borders, and row and column headers. Excel toolbars replace the SolidWorks toolbars.
2.
Edit the worksheet as needed, using Excel functions. You can perform these kinds of edits: •
Edit the cells in the Item No. column or the Description column. Before you edit the Item No. column, you must clear the Row numbers follow assembly ordering check box on the Control tab of the Bill of Materials Properties dialog box. See the previous section for more information.
•
If you edit text in the Qty. or Part No. columns, these changes will be lost the next time that the BOM updates for any reason.
•
To edit linked properties, Automatic Update of BOM in Tools, Options, Document Properties, Detailing must not be selected. If this option is selected, the linked properties are reset to the values in the Summary Info dialog box when you rebuild the drawing.
•
Rename the column headers. Type the new text in the header cell or in the Formula Bar. Do not edit the text in the Name box.
•
Add columns, before the cell marked $$END, and rows (but not above the header row). You can include rows for bulk items, such as oil or adhesive.
•
Change the order of the columns. Insert a new column, cut and paste the existing columns until they are arranged as needed, then delete the empty column.
•
Hide columns. Right-click the lettered cell at the top of the column, and select Hide. If the BOM includes a column that you do not want to display, do not delete it; hide it instead.
•
Hide rows. Right-click the numbered cell at the left of the row, and select Hide. This has the same effect as clearing the check mark beside the item on the Contents tab of the Bill of Materials Properties dialog box.
•
Do not delete rows to remove them from the table. If you delete a row in Excel, the row is replaced the next time the BOM is updated.
•
You cannot delete or hide the header row.
•
Change the text alignment (left, right, center) by column.
•
Adjust the column width or row height.
•
Change the text font.
•
Some editing operations apply to an entire row or column in the table. To select an entire row, click the numbered cell at the left of the row. To select an entire column, click the lettered cell above the column. NOTE: The following types of cell formatting are not supported in a bill of materials: cell shading (colors and patterns), borders, text orientation (text at an angle), wrap text, merge cells.
3.
Click outside the worksheet to return to the drawing.
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Chapter 12 Detailing
Bill of Materials - Part No. Column Applies to Excel-based Bills of Materials. You can display a name other than the document name in the part number column of the BOM. For example, you can use a stock number specified by your company, or the configuration name for a part or sub-assembly that has more than one configuration. To do so, it may be necessary to edit the Advanced properties of the configuration. To specify the name to use in the Part No. column:
1.
In the part or sub-assembly document, click the Configuration tab change to the ConfigurationManager view.
2.
Right-click the configuration you want to edit, and select Properties.
3.
In the Configuration Properties dialog box, under Part number displayed when used in a bill of materials, select one of the following:
4.
•
Document name.
•
Configuration name.
•
User-specified name. Type a name in the box.
at the lower left of the window to
If you always want a sub-assembly to be listed as a single component in the bill of materials, select the Don’t show child components in BOM when used as sub-assembly check box. When cleared, child components are listed individually in the BOM, when Show parts only or Show assemblies and parts in an indented list is selected in the Bill of Materials Properties dialog box.
5.
Click OK.
Bill of Materials - Multiple Configurations Applies to Excel-based Bills of Materials. You can specify how to list component configurations in a BOM. When multiple configurations of the same component are used in an assembly, there are some additional considerations. •
In the Item No. column, you can list the configurations as a separate entries with individual item numbers, or you can group all the configurations as a single entry with one item number.
•
In the Part No. column, you can display a user-defined name, the configuration name, or the document name for each item.
In the component document, you need to perform certain steps to achieve the desired results. The steps vary, depending on how you create the configurations If you use a design table to create configurations:
Item No.
Part No.
Procedure
each configuration as a separate item
use-defined names
Use $PARTNUMBER in the table, with a different value for each configuration
configuration names
This is the default. Design tables automatically set the Advanced Configuration Properties to use the configuration name.
a user-defined name
Use $PARTNUMBER in the table, with the same value for each configuration
the document name
Use $PARTNUMBER in the table, with the document name for all configurations
all configurations as a single item
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If you create configurations manually:
Item No.
Part No.
Procedure
each configuration as a separate item
use-defined names
Under Advanced Configuration Properties, click Use name below, and specify a different value for each configuration.
configuration names
Under Advanced Configuration Properties, click Use name below. The configuration name is the default.
a user-defined name
1 Use the default Advanced Configuration Properties (Use document name selected). 2 Click File, Properties, and enter a Title in the Summary Information dialog box. 3 When you create the BOM, select Use summary information title as part number.
the document name
This is the default for the Advanced Properties (Use document name selected).
all configurations as a single item
To edit the Add Configuration/Configuration Properties, right-click the configuration name, and select Properties. When the Configuration Properties are not defined in the same way for all the configurations of the components, the following order of precedence applies: •
User-defined name or configuration name (if Use name below is selected)
•
Summary Information Title (if the option is selected, and if Title is defined for the component)
•
Document name
Bill of Materials - Save as Excel File Applies to Excel-based Bills of Materials. To save a bill of materials as an Excel file:
1.
Click the bill of materials on the drawing sheet.
2.
Click File, Save As. The Save as type is set to Excel Files (*.xls) by default.
3.
Enter a file name, and click Save.
You can use the saved bill of materials in Excel, or as an OLE object in other applications. The saved file is not linked to the bill of materials in the drawing; edits to one do not affect the other.
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Chapter 12 Detailing
Bill of Materials - Custom Properties Applies to Excel-based Bills of Materials. You can add more information such as Material, Vendor_Number, Cost, and so on to the open part or sub-assembly document by clicking File, Properties, and selecting the Custom tab or the Configurations specific tab. (See Summary Info - Custom and Configuration Specific for information about specifying properties.) SolidWorks provides several templates for bills of materials in the directory \install_directory\lang\english. Columns in the templates are populated automatically as follows: Property
Automatically populates
ITEM NO. QTY. PART No.
In all templates supplied
DESCRIPTION MATERIAL STOCK SIZE VENDOR WEIGHT
1) When the column appears in the selected template, and 2) you add the property to the Custom or Configuration Specific information in the part or assembly document
custom properties
1) When you add a custom column to a BOM or template, and 2) you add the property to the Custom or Configuration Specific information in the part or assembly document
Custom properties can include model dimensions and mass properties, which update automatically in the BOM if they are changed in the model. To add custom columns to the bill of materials:
1.
Open the BOM template file. To add the columns to the default BOM template, open install_directory\lang\english\Bomtemp.xls. To create a new BOM template, it is a good idea to make a copy of the default template, then open the copy.
2.
Insert a new column where you want the information to appear. The new column must be to the left of the column marked $$END.
3.
Enter the column heading for the property you want to display in that column, and press Enter. The name appears in the Formula Bar in the Excel toolbar. This column heading does not need to match the custom property name.
4.
Click the cell to select it, then click Insert, Name, Define and type in the name of the property that you want to appear in this column. This cell name replaces the default alphanumeric cell name that appears in the Name Box in the Excel toolbar whenever you click a cell. The cell name is listed in the Names in workbook list for the selected cell. This name must match the name of the property from the part or sub-assembly document, and must not contain any spaces.
5.
Click Add, then click OK. When you add a bill of materials to a drawing, it now includes the added column. The cells are populated with the values of the custom properties of the document, or the values of the configuration specific properties for the item. NOTE: Do not change the cell names in the Name Box for the default columns in the BOM template. You can change the text in the column heading, but not the cell name.
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13 Import/Export
Importing and Exporting Files This section describes these SolidWorks file import and export topics: •
ACIS®
•
Parasolid® text and binary
•
Autodesk Inventor®
•
•
CADKEY®
•
Pro/ENGINEER®
•
CATIA®Graphics
•
Solid Edge®
•
DXF 3D
•
STEP
•
DXF™/DWG
•
STL
•
eDrawings
•
TIFF™
•
Highly Compressed Graphics
•
Unigraphics®
•
HOOPS®
•
VDAFS
•
IGES
•
Viewpoint®
•
JPEG
•
VRML
•
Mechanical Desktop®
•
ZGL Files
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Chapter 13 Import/Export
Importing/Exporting SolidWorks Documents You can import files to the SolidWorks software from other applications. You can export SolidWorks documents to a number of formats for use with other applications. The following table displays the data translation methods available for SolidWorks documents: Parts Application
Assemblies
Import
Export
Import
Export
ACIS
X
X
X
X
Autodesk Inventor
X
CADKEY
X
CATIA Graphics
X
DXF/DWG
X
DXF 3D
X
X
X
Highly Compressed Graphics
X
X
HOOPS
X
X
X
X
X
Mechanical Desktop
X
Parasolid
X
X
X
X
X
Solid Edge
X
STEP
X
X
X
X
STL
X
X
X
X
TIFF
X
X
X
X
Unigraphics
X
VDAFS
X
ZGL
X
X
X
X
X X X X X
X X
X X
NOTE: X = This option is available. A blank box = This option is not available.
13-2
X
X
X
X
X
X
Pro/ENGINEER
VRML
X
X X
X
Viewpoint
X X X
JPEG
Export
X
X
X
Import
X
eDrawings
IGES
Drawings
X
Importing Documents Before you import a document to the SolidWorks software, make sure that you have the import options set for your purposes. To import a file from another application:
1.
Click Open
or File, Open.
The Open dialog box appears. 2.
In the Files of type list, click the desired format.
3.
Browse to the desired file, and click Open. The selected file is opened. If there are surfaces in the file, they are read as follows: •
If there are blanked surfaces, they are imported and added to the FeatureManager design tree as surface features.
•
If the attempt to knit the surfaces into a solid succeeds, the solid appears as the base feature (named Imported1) in a new part file. You can add features (bosses, cuts, and so on) to this base feature, but you cannot edit the base feature itself.
•
If the surfaces represent multiple closed volumes, then one part is made for each closed volume. An assembly file also is made that includes the imported parts positioned relative to the assembly origin, according to how the surfaces are defined in the imported file. For ACIS files, if the imported ACIS file consists of surfaces only, then only surfaces are created even though they represent multiple closed volumes, regardless of the import options you choose. If the ACIS file consists of data about multiple solid bodies, parts or surfaces are created, depending on the import options you choose.
•
If the attempt to knit the surfaces fails, the surfaces are grouped into one or more surface features (named Surface-Imported1, 2, ...) in a new part file.
•
If you import a .dxf or .dwg file, the DXF/DWG import wizard appears.
Importing Geometry You can import surfaces, solids, sketches, curves, and graphics models (CATIA CGR, STL, or VRML files only) from ACIS, CATIA CGR, IGES, Parasolid, STEP, STL, VDAFS, or VRML files as reference geometry into part documents. To import the geometry from another application:
1.
In a part document, click Imported Geometry Imported.
on the Features toolbar, or click Insert, Features,
The Open dialog box appears. 2.
Browse to the desired file, and click Open. NOTE: For ACIS, IGES, STEP, STL, VDAFS, or VRML files, you can click Options to set the import options One or more features are imported, and the Imported features are added to the part. The features are positioned relative to the origin, using the coordinates in the imported file. NOTE: Wireframe geometry and curves are ignored when importing surfaces as reference geometry.
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Chapter 13 Import/Export
Editing Imported Features You can replace an imported feature with geometry from a new file. To edit a feature created from an imported document:
1.
In the FeatureManager design tree, right-click the feature created from the imported document, and select Edit Feature. The Open dialog box appears.
2.
In the Files of type list, select the desired format.
3.
Browse to select the desired file to import. The file name appears in the File name box.
4.
5.
Select the Match faces and edges check box, if desired. This does the following: •
Propagates the dependencies of the old faces and edges in the old body, such as sketches or features, to the new faces and edges in the new body.
•
Ensures you get the correct results when you open a file that has imported features.
Click Open. An imported solid is replaced only if the data in the new document can be successfully knitted into a body. A surface feature is replaced with the first surface in the new document, and subsequent surfaces in the new file are added to the model. NOTE: You can edit only features that were created from an IGES, STEP, ACIS, VRML, Parasolid, or VDAFS file.
If you had added features to the imported body before selecting Edit Feature, SolidWorks attempts to rebuild these features whenever possible. For example, this STEP file contains an imported feature. You need to add a feature to the imported body. 1. Select the bottom face of the imported body. 2.
Click Chamfer
.
The Chamfer PropertyManager appears. 3.
Under Chamfer Parameters, make the desired settings and click OK . The imported body now shows the additional chamfer feature on the bottom face.
4.
Right-click Imported1 in the FeatureManager design tree and select Edit Feature. A message box appears warning that this feature has a parent/child relation or is being referenced.
5.
Click OK. The Open dialog box appears.
6.
Select the STEP file and click Open. The STEP file opens with the imported body. The chamfer feature that you added to the imported body is rebuilt. You did not have to rebuild this feature that you had added to the imported body before selecting Edit Feature.
13-4
Open - Match Faces and Edges of Imported Features The Match faces and edges check box appears in the Open dialog box when you edit the definition of an imported feature. To edit the definition of an imported feature:
1.
Open a file containing an imported feature.
2.
In the FeatureManager design tree, right-click the imported feature, and select Edit Feature. The Open dialog box appears.
3.
Browse to select the edited file to import. The file name appears in the File name box.
4.
5.
Select the Match faces and edges check box. This does the following: •
Propagates the dependencies of the old faces and edges in the old body, such as sketches or features, to the new faces and edges in the new body.
•
Ensures you get the correct results when you open a file that has imported features.
Click Open. The file opens and the imported features are correctly displayed.
Import Diagnosis Use the Diagnosis tool to diagnose and repair gaps and bad faces on imported features. Use the Diagnosis tool when you have: •
An imported solid or surface body that has rebuild errors.
•
An imported surface that was not able to knit into a solid body. If you try to fix gaps but all the gaps cannot be healed, try fixing the faces to fix the gaps.
To view and fix gaps:
1.
Right-click the Imported feature in the FeatureManager design tree and select Diagnosis. The Import Diagnosis PropertyManager appears.
2.
In the PropertyManager, under Gaps, click Diagnose. The PropertyManager reports the number of gaps found.
3.
View and fix the gaps using the View/Close Gaps tools.
4.
Click OK
.
To diagnose and fix or simplify faces:
1.
Right-click the Imported feature in the FeatureManager design tree and select Diagnosis.
2.
In the PropertyManager, under Faces, click Diagnose.
3.
Faces that are faulty or require simplification highlight in the graphics area and appear in the Faces to be
4.
fixed/removed . Move the pointer over a face in the list to display a tooltip that reports the problem with that face.
5.
Click Fix to simplify that face. The diagnosis automatically finds faulty faces and spline curves/surfaces that can be simplified to analytical ones for operations such as sheet metal creation and assembly mating.
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Chapter 13 Import/Export
To simplify entities with a tolerance greater than 1.0e-8 meters and less than 1.0e-5 meters, you must manually select the relevant faces, then click Fix. The example has some plane-like and cylinder-like faces, but they are not in analytical forms. 1.
Select the two faces in the graphics area.
2.
Click Fix. If two faces are meant to be one (for example, the two halves of a cylindrical face), the two faces merge.
The diagnosis performs an in-depth check on all the entities in a model. The number of faults or faulty faces may differ from those found by the more generic Tools, Check command. This detailed check is required to heal the faulty entities. 3.
Click OK
.
If the imported body still shows rebuild error markers even though a body check and the Import Diagnosis PropertyManager report no surface problems, the body is probably valid. Click Rebuild clear the rebuild error markers.
to
Import Diagnosis PropertyManager The Import Diagnosis PropertyManager appears when you import a file, right-click the imported body, and select Diagnosis. The PropertyManager controls the following properties: Gaps •
Diagnose. Checks the imported body for gaps and reports the number of gaps found.
View/Close Gaps •
Next. Views the next gap. An arrow
points to the gap or gap edge in the graphics area.
•
Previous. Views the previously viewed gap.
•
Healing Preview. Zooms in to the next or previous gap and displays a preview of the proposed fix.
•
Accept (Available only when Healing Preview is selected). Accepts the fix for the currently viewed gap. The number of gaps found updates.
•
Close All. Fixes all gaps and updates the number of gaps found.
Faces
13-6
•
Diagnose. Checks the imported body for bad faces. Diagnosis reports the problem and faces under Faces to be fixed/removed.
•
Faces to be fixed/removed . Reports the bad faces found when you click Diagnosis. Hover over the face name for a tooltip that describes the problem with the face. You can manually select faces in the graphics area to add to this list. You can also select multiple faces to merge.
Click the selected face in Faces to be fixed/removed to view normal to that face. Click the selected face in the list again to flip the face 180 degrees and view it from the opposite direction. This is useful when manually fixing faces. •
Fix. Fixes the bad faces.
•
Remove. Removes the bad faces. You can use surface creation functionality to try to create new surfaces to fill gap, then try to knit again.
•
All selected. Fixes all faces listed in Faces to be fixed/removed individually or manually.
. Clear this option to fix faces
General Import Options You can set the general import options when you import IGES, STEP, SAT (ACIS), VDAFS, or Inventor Part files. To set the general import options:
1.
Click Open
or File, Open.
The Open dialog box appears. 2.
Set Files of type to IGES (*.igs,*.iges), STEP AP203/214 (*.step,*.stp), ACIS (*.sat), VDAFS (*.vda), or Inventor Part (*.ipt) , then click Options. The Import Options dialog box appears with General selected on the File Format tab. If you move the pointer over General, a tooltip displays the file formats that the General item controls.
3.
Select from the following options: •
Surface/solid entities. Imports surface and solid entities. You must also select one of the following options: Try forming solid(s). Tries to form solids. Additionally, you can select the following option: • B-REP mapping. Attempts to import the model by directly mapping topologies using boundary representation (BREP) data. In general, this mode is faster than knitting, especially for complex models. If you select the Try forming solid(s) option, but do not select the B-REP mapping option, the SolidWorks application attempts to knit the surfaces into solid(s). o Knit surface(s). Imports as surfaces and attempt to knit the imported surfaces. o Do not knit. Imports as surfaces and prevent surfaces from knitting. Free point/curve entities. Imports free points and free curve entities. You must also select one of the following options: o
•
Import as sketch(es). Imports data as 2D and 3D sketch data. If you want to import free curves, SolidWorks strongly recommends you select this option, for performance reasons. Free points and 2D sketches import as 2D sketches. 2D curves, 3D curves, and 3D sketches import as 3D sketches. o Import as 3D curves. Imports data as 3D curves data. 2D and 3D curves import as curves. Free points and 2D sketches import as 2D sketches. Import multiple bodies as parts (STEP and ACIS files only). Imports a multibody part as an assembly document. The multiple bodies are imported as part documents contained in the assembly. With this option cleared, the multibody part imports as a part document that contains multiple imported bodies. o
•
•
Perform full entity check and repair errors. Checks and repairs errors (default is selected). With this option selected, import performance is slower because the software spends more time checking and repairing the model entities wherever possible. If the quality of the imported data is good, you may not have to select this option.
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Chapter 13 Import/Export
•
Customize curve tolerance. Customizes the tolerance when you import models with very small entities (smallest values on the order of 1.0e-6 to 1.0e-7 meters). With this option cleared, SolidWorks uses internal tolerance settings which are too large to properly import and display these small models. Enter the desired tolerance in the box.
•
Unit. Set the units of measure for the imported file. You must select one of the following options: File specified unit. Use the units of measure from the imported file. Document template specified unit. Use the units specified in the SolidWorks template files under Tools, Options, System Options, Default Templates. IGES - Show IGES levels. Displays the IGES-In Surfaces, Curves, and Levels dialog box if there are curves or different levels (or layers) in the IGES file. o o
• •
STEP - Map configuration data. Applies to STEP files only. Imports STEP file configuration data plus geometric data. Leave this option cleared to import only geometric data.
4.
Click OK to return to the Open dialog box.
5.
Select the file to open, then click Open to import the file as a SolidWorks document.
STL and VRML Import Options You can set the import options when you import STL or VRML files as SolidWorks documents. The VRML translator supports explicit normals, crease angle smooth shading, and color per vertex, which results in smooth blending of colors. To set the STL and VRML import options:
1.
Click Open
or File, Open.
The Open dialog box appears. 2.
Set Files of type to STL (*.stl) or VRML (*.wrl) and click Options. The Import Options dialog box appears with STL/VRML selected on the File Format tab.
3.
Select from the following options: •
Import as o
Graphics Body. Imports data as graphical data only. The translator does not attempt to create any features. The graphics icon
appears in the FeatureManager design tree with the file
type, for example, STL Graphics1. Solid Body. Attempts to import data as solid bodies. In many cases (especially complex models) some of the data does not knit into a usable solid, in which case the translators import that data as surface bodies. Therefore, in the FeatureManager design tree, you can potentially see a Solid Bodies folder, a Surface Bodies folder, imported solid body features, and imported surface body features. o Surface Body. Imports data as surfaces. The Surface Bodies folder and the imported surface body features appear in the FeatureManager design tree. Unit. Select the unit of measure for the SolidWorks document. The available units are Millimeters, Centimeters, Meters, Inches, and Feet. The translator does not convert units during import. For example, if the unit of measure of the original document is meters and you import the document with the unit Millimeters, an edge that measures 1 meter in the original document will measure 1 millimeter in the imported document, not 1000 millimeters. o
•
•
13-8
Import texture information (applies only when you select import as Graphics Body). Imports texture information, which if contained in the file, results in a high-quality, realistic-looking image. Choosing to not import texture information may improve performance.
4.
Click OK to return to the Open dialog box.
5.
Select the file to open, then click Open to import the file as a SolidWorks document.
Exporting Documents and Setting Options When you export a document from the SolidWorks application, you can set the options for the new file you create. The options vary, depending on the type of file. To export a SolidWorks document as another file type:
1.
Select one of the following: •
The face or surface of a part in the graphics area
•
A solid body or surface body from the Solid Bodies FeatureManager design tree
•
The components of an assembly
or Surface Bodies
folder in the
NOTE: If you do not select any entities, the entire part or assembly is exported. 2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to the desired file type, then click Options. The Export Options dialog box appears with the desired file type selected on the File Format tab.
4.
Set the appropriate options for the target file type. See the target file type below for the available options: •
ACIS (*.sat)
•
DXF/DWG (*.dxf, *.dwg)
•
eDrawing (*.eprt, *.easm, or *.edrw)
•
IGES (*.igs)
•
Parasolid (*.x_t, *.x_b)
•
STEP (*.step)
•
STL (*.stl)
•
Tif (*.tif)
•
VDAFS (*.vda)
•
VRML (*.wrl)
5.
In the File name box, type a name. The extension for the selected format is added automatically when you save the document.
6.
Click Save. NOTES: •
If you export an assembly that contains lightweight parts, the Resolve Lightweight Parts dialog box appears. You must resolve any lightweight parts before you can export an assembly.
•
If you export an assembly that contains hidden or suppressed parts, a message box appears asking if you want to resolve these parts. To export these parts, you must resolve them.
•
If you select any faces, surfaces, solid bodies or surface bodies of a part, the Export dialog box appears verifying if you want to export only the selected objects. Click Selected face(s) to export only the selected faces, Selected bodies to export only the selected bodies, or All bodies to export all solid bodies.
ACIS Export Options You can set the export options when you export SolidWorks part or assembly documents as ACIS files. To set the ACIS export options:
1.
Open the SolidWorks document that you want to export as an ACIS file.
2.
Click File, Save As. The Save As dialog box appears.
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Chapter 13 Import/Export
3.
Set Save as type to ACIS (*.sat), then click Options. The Export Options dialog box appears with ACIS selected on the File Format tab.
4.
5.
Select from the following options: •
Solid/Surface geometry. Exports the geometry as all solids and surface bodies.
•
3D curves. Exports the solid and surface bodies as wireframe entities. All 3D curves (composite curves, 3D wires, imported curves, and so on) are also saved.
•
Export sketch entities (available only when you select 3D curves). The Export sketch entities item is available as an option for 3D curves. Select this check box to export all the items in 3D curves, plus all 2D and 3D sketches in the document.
•
Version. Select the type supported by the target system.
•
Units. Select the default units of length to use for ACIS files.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
DXF/DWG Export Options You can set the export options when you export SolidWorks drawing documents as DXF or DWG files. To set the DXF or DWG export options:
1.
Open the SolidWorks drawing document that you want to export as a DXF or DWG file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Dxf (*.dxf) or Dwg (*.dwg), then click Options. The Export Options dialog box appears with DXF/DWG selected on the File Format tab.
4.
5.
Select from the following options: •
Version. Select the type supported by the target system. The SolidWorks DXF and DWG translators support all AutoCAD® versions up to and including AutoCAD 2002.
•
Fonts. Select either TrueType or AutoCAD STANDARD only. If you select AutoCAD STANDARD only, the drawFontMap.txt mapping file is used. See AutoCAD Font Support for details.
•
Line styles. Select AutoCAD Standard Styles to map SolidWorks line fonts to the original AutoCAD stock line types. Line font weight is mapped to the closest AutoCAD line weight value. AutoCAD line weight value mapping is only supported for AutoCAD Version setting R2000 and higher. Select SolidWorks Custom Styles to use the SolidWorks line styles.
•
Custom Map SolidWorks to DXF. Implements mapping. See DXF/DWG Mapping.
•
Don't show mapping on each save. Prevents the SolidWorks To DXF/DWG Mapping dialog box from appearing every time you save a drawing with Custom Map SolidWorks to DXF selected. The map file specified in the Map file box is used.
•
Map file. Select a previously saved map file, or browse to the desired file.
•
1:1 Scale output. Exports the drawing using a model geometry scale of 1:1 and enable the Base scale list. The paper or sheet scale is not normally used when you enable this option.
•
Base scale. Refers to the basis used for the 1:1 scale output of the geometry, based on the various drawing view scales on the sheet. If you have a view selected, the view scale and count values for this selected view appear in the Base scale list. If no view is selected, the view scale with the highest count is displayed by default. Count indicates the number of occurrences of this scale in the drawing document.
Click OK, then click Save to export the document. If you selected the 1:1 Scale output check box, the drawing document is saved with a model geometry scale of 1:1 for the chosen views, with the remainder of the sheet scaled accordingly.
13-10
eDrawings Export Options You can set the export options when you export SolidWorks documents as eDrawing files. To set the eDrawings export options:
1.
Open the SolidWorks document that you want to export as an eDrawing file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to eDrawing (<eDrawing file type>), then click Options. NOTE: The eDrawings translator automatically displays the appropriate eDrawing file type based on the open document: eDrawing (*.edrw) for drawings, eDrawing (*.eprt) for parts, or eDrawing (*.easm) for assemblies. The Export Options dialog box appears with EDRW/EPRT/EASM selected on the File Format tab.
4.
5.
Select from the following options: •
Okay to measure this eDrawing. Select this check box to enable measurement of the geometry in this eDrawing file. Recipients of this eDrawing file can measure the geometry in the eDrawings Viewer.
•
Compress this eDrawing. Select this check box to compress the eDrawing file size. File compression may decrease the quality of some shaded images.
•
Allow export to STL for parts and assemblies. Select this check box to allow recipients of the eDrawing file to save it as an STL file from the eDrawings Viewer.
•
Save shaded data in drawings. For SolidWorks drawings only. Select this check box to save the shaded data from the SolidWorks drawing document in the published eDrawing file.
Click OK, then click Save to export the document.
IGES Export Options You can set the export options when you export SolidWorks part or assembly documents as IGES files. To set the IGES export options:
1.
Open the SolidWorks document that you want to export as an IGES file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to IGES (*.igs), then click Options. The Export Options dialog box appears with IGES 5.3 selected on the File Format tab.
4.
Select from the following options: •
Output as o
o
IGES solid/surface entities. Exports the data as solid or surface entities. Select Trimmed Surface (type 144) to convert the faces of the part, assembly, or the selected surfaces to trimmed surfaces in the IGES file. Select Manifold Solid B-rep Object (type 186) to export boundary representation (BREP) data to the IGES file. IGES Wireframe (3D curves). Converts the solid body to a 3D wireframe representation in the IGES file. Unlike surfaces or faces, you cannot export individually selected model edges to an IGES file. Select either B-Splines (Entity type 126) or Parametric Splines (Entity type 112) depending on the entity types required by the target system. For more information, see the IGES 3D Curves table.
NOTE: If you select both of the above options, the model is exported as both trimmed surfaces and 3D curves.
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Chapter 13 Import/Export
•
Surface representation/System preference. The IGES entity types that compose the trimmed surfaces depend on the export format chosen. The Surface representation table shows the IGES entity types that compose the trimmed surfaces.
•
Export 3D Curve features. Includes 3D curve features in the exported file.
•
Export sketch entities. Includes sketch entities in the exported file. All 2D and 3D sketch entities are included.
•
Use high trim curve accuracy. Exports using high trim curve accuracy; the file size is larger than if the check box is cleared. This setting affects files exported both with Trimmed surfaces and with 3D curves. High trim curve accuracy can sometimes help if the target system has trouble importing the IGES file, or cannot knit the surfaces into a useful solid.
•
IGES assembly structure o
o
• 5.
Save all components of an assembly in one file (assemblies only). Saves all assembly components, sub-assemblies, and sub-assembly components in one file. Otherwise, the assembly components and the sub-assembly components are saved as individual IGES files in the same directory. Flatten assembly hierarchy (assemblies only). Flattens the assembly to one level of only part bodies. A flattened file contains a top-level assembly and a series of parts that contain imported features.
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
Surface Representation Surface Representation
Exported IGES Entity Types
STANDARD
144, 142, 128, 126, 122, 120, 110, 102, 100
NURBS
144, 142, 128, 126, 110, 102, 100
ALIAS
144, 142, 128, 126, 122, 120, 110, 102, 100
ANSYS
144, 142, 128, 126, 110, 102, 100
COSMOS
144, 142, 128, 126, 110, 102, 100
MASTERCAM
144, 142, 128, 126, 110, 102, 100
SURFCAM
144, 142, 128, 126, 110, 102, 100
SMARTCAM
144, 142, 128, 126, 110, 102, 100
TEKSOFT
144, 142, 128, 126, 110, 102, 100
ALPHACAM
144, 142, 128, 126, 110, 102, 100
MULTICAD
144, 142, 128, 126, 110, 102, 100
NOTE: If the system you are exporting to is not listed, refer to the documentation for that system to see which entities are supported, and choose an appropriate setting.
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Parasolid Export Options You can set the export options when you export SolidWorks part or assembly documents as Parasolid files. To set the Parasolid export options:
1.
Open the SolidWorks document that you want to export as a Parasolid file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Parasolid (*.x_t) or Parasolid Binary (*.x_b), then click Options. The Export Options dialog box appears with Parasolid selected on the File Format tab.
4.
5.
Select from the following options: •
Version. Select the type supported by the target system.
•
Flatten assembly hierarchy (assemblies only). Flattens the assembly to one level of only part bodies. A flattened file contains a top-level assembly and a series of parts that contain imported features.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
STEP Export Options You can set the export options when you export SolidWorks part or assembly documents as STEP files. To set the STEP export options:
1.
Open the SolidWorks document that you want to export as a STEP file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to STEP AP203 (*.step) or STEP AP214 (*.step), then click Options. The Export Options dialog box appears with STEP selected on the File Format tab.
4.
Select from the following options: •
Output as o o
o
•
Solid/Surface geometry. Exports the geometry as solids and surface bodies. 3D curves. Exports the solid and surface bodies as wireframe entities. All 3D curves (composite curves, 3D wires, imported curves, and so on) are also saved. Export sketch entities (available only with 3D curves selected). Exports all the items in 3D curves, plus all 2D and 3D sketches in the document.
Set STEP configuration data (available only when exporting to STEP AP203 (*.step) file types). Displays the STEP Configuration Data for Export dialog box. NOTE: If you select 3D curves or Export sketch entities, you can only open the exported STEP files in SolidWorks 2001Plus or later.
• 5.
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document. If you selected Set STEP configuration data, the STEP Configuration Data for Export dialog box appears, as described in step 4. NOTE: Because you cannot group the sketch elements together in a STEP file, when you open the exported STEP file in SolidWorks: •
All lines and splines are imported into a single 3D sketch.
•
Circles, ellipses, and parabolas are imported into individual 2D sketches.
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Chapter 13 Import/Export
STL Export Options You can set the export options when you export SolidWorks part or assembly documents as STL files. To set the STL export options:
1.
Open the SolidWorks document that you want to export as an STL file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to STL (*.stl), then click Options. The Export Options dialog box appears with STL selected on the File Format tab.
4.
Select from the following options: •
Output as o Select either Binary or ASCII as the file format. Binary files are smaller than ASCII files, but they are not supported in some other systems. Select the type supported by the target system. o Unit. Select the unit of measure.
•
Resolution. Controls the tessellation of non-planar surfaces for Stereolithography (STL) output. A lower deviation setting produces a more finely tessellated STL file. Files generated with higher accuracy settings (increased tessellation) are larger in size and slower to generate. o o
Coarse or Fine. Select one of these preset resolutions. Custom. Move the Deviation and Angle slider controls to adjust the resolution or type values for deviation Tolerance and angle Tolerance. If you click Custom: •
Move the Deviation slider to adjust the deviation Tolerance, which controls whole-part tessellation. Lower numbers generate files with greater whole-part accuracy.
•
Move the Angle slider to adjust the angle Tolerance, which controls smaller detail tessellation. Lower numbers generate files with greater small-detail accuracy, but those files take longer to generate. As you move the two sliders, the corresponding concentric circles adjust accordingly. The circles show, approximately, how the tessellation will vary as a result of the settings. (See the Preview option below.)
o
o
5.
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Show STL info before file saving. Displays a SolidWorks dialog box (when you click Save in the Save As dialog box) that contains the following information: Triangles (number), File Size, File Format, and the directory path and file name. Preview. Displays a faceted model preview in the graphics area and display the Triangles (number) and File size information in the Export Options dialog box.
•
Do not translate STL output data to positive space. Makes exported parts maintain their original position in global space, relative to the origin.
•
Save all components of an assembly in a single file (assemblies only). Saves the assembly and each of its components in a single .stl file.
•
Check for interferences (assemblies only). Performs an interference check on an assembly document prior to saving. Export of an assembly with coincident or interfering bodies to a single .stl file produces a file that may be unsuitable for some rapid prototyping systems. It is recommended that you check for interference between the components prior to saving the assembly document. For more information, see Interference Detection.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
TIFF Export Options You can set the export options when you export SolidWorks documents as TIFF files. To set the TIFF export options:
1.
Open the SolidWorks document that you want to export as a TIFF file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Tif (*.tif), then click Options. The Export Options dialog box appears with TIF selected on the File Format tab.
4.
Select from the following options: •
Image type. Select either RGB full color, or Black & white (bilevel) image.
•
Compression scheme. Select the type supported by the target system: o
Uncompressed.
o
Packbits. Results in the smallest color image.
o
•
Capture type. Select either Screen capture or Print capture. o o
5.
Group 4 Fax. Results in the smallest file size of the three formats, but can only be used for a black and white image. Screen capture. Captures the image at the resolution of the screen display. Print capture (drawings only). Enables the options under For drawings. Capture the image at a user-defined DPI (dots per inch) and Paper size. The drawing Width and Height information update automatically. Select the Scale to fit check box to scale the drawing automatically, or set the scale manually in the Scale box.
Click OK, then click Save to export the document.
VRML Export Options You can set the export options when you export SolidWorks part or assembly documents as VRML files. To set the VRML export options:
1.
Open the SolidWorks document that you want to export as a VRML file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to VRML (*.wrl), then click Options. The Export Options dialog box appears with VRML selected on the File Format tab.
4.
Select from the following items: •
Output as o
o
5.
Version. Select the type supported by the target system. VRML 97 is also called VRML version 2.0. Unit. Select the unit of measure.
•
Quality. Advises you that the resolution of the exported VRML file depends on the current display resolution. To change the current display resolution, click Tools, Options, Document Properties, Image Quality and adjust the options.
•
Save all components of the assembly in a single file (assemblies only). Includes each assembly and sub-assembly component in one file.
•
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Click OK, then click Save to export the document.
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Chapter 13 Import/Export
Exporting Multibody Documents When you export a multibody part document as another file type, you have the option to export selected solid bodies or all solid bodies. To export a multibody part document:
1.
With a multibody part document open, select at least one face or solid body in the graphics area, or one solid body from the Solid Bodies
folder in the FeatureManager design tree, and click Save As.
The Save As dialog box appears. 2.
Set the Save as type to the desired file type and click Save. The Export dialog box appears. NOTE: If you select a solid body, the Selected face(s) option in the Export dialog box is unavailable.
3.
4.
Click one of the following: •
Selected face(s). Exports only the selected faces.
•
Selected bodies. Exports only the selected bodies.
•
All bodies. Exports all solid bodies.
Click OK to export the multibody part document.
Print3D Print3D is a web portal linked to the SolidWorks software. You can contact rapid part and prototype vendors to request price quotes and place orders for the current part document through the Print3D web portal. Print3D automates the prototype request process, eliminating the need to save parts as STL files, FTP parts to vendors, or perform other operations. To access the Print3D web portal:
1.
Open a part document for which you want to get a price quote or place an order.
2.
Click File, Print3D. The Print3D web portal opens in your browser. A list of rapid part and prototype vendors is displayed in the web portal. You can also access the Print3D web portal from the Save As dialog box. Select STL (*.stl) in Save as type and click Try Print3D.
3.
13-16
Click any of the following: •
What is Print3D? Explains the Print3D process and contains basic technical definitions of rapid prototyping processes and materials.
•
Print3D button. Leads you to a web-based quote and order process controlled by the vendor, which may involve a web form or wizard. Follow the on-screen instructions to complete the process.
•
Tell me more. Displays more information about a vendor and its offerings.
File Types ACIS Files (*.sat) The ACIS™ translator supports import and export of body and face colors, curves, and wireframe geometry. You can export the entity attribute information of faces and edges to ACIS files, and this information is retained in the ACIS file. If you import that same ACIS file back into SolidWorks, for entity attribute information of faces, you can select any import options and the faces retain the entity attribute information. However, if you import edges, you must select the B-Rep mapping check box in the Import Options dialog box to retain the entity attribute information for the edges. Import The ACIS translator imports ACIS part or assembly files as SolidWorks part or assembly documents. If the units of length are not explicitly specified in the ACIS file, a dialog box gives you the opportunity to specify the units. Files created with early versions of the ACIS modeler do not contain information about the units of length. The default import mode is knitting. SolidWorks supports import of generic named attributes (integer, position, real, string, and vector) associated with bodies and faces from ACIS (.sat) files. These attributes are displayed as features in the FeatureManager design tree. Their values are accessible only through the SolidWorks Application Programming Interface (API). Export The ACIS translator exports SolidWorks part or assembly documents as ACIS files. When you export parts, you can export faces or bodies as separate ACIS files. You can select to export individual parts or subassemblies from an assembly tree, limiting export to only those parts or subassemblies. If you select a subassembly, all of its components are automatically selected. The ACIS translator does not support assembly hierarchy. Version Information The ACIS translator supports all SAT versions up to and including version 8.0.
Autodesk Inventor Files The Inventor Part translator imports Autodesk Inventor® part files as SolidWorks part documents. The imported part files contain only geometry; features are not imported. The Inventor Part translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box. To open an Autodesk Inventor part:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to Inventor Part (*.ipt) and click Options. The Import Options dialog box appears with General selected on the File Format tab.
3.
Set the import options, then browse to the desired file and click Open.
Version Information The Inventor translator supports all Autodesk Inventor versions up to and including Autodesk Inventor 5.3.
CADKEY Files The CADKEY® translator imports CADKEY part and assembly files as SolidWorks part or assembly documents. All CADKEY files have the same .prt file extension. The CADKEY translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box.
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Chapter 13 Import/Export
To open a CADKEY file:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to CADKEY (*.prt).
3.
Browse to the desired file, and click Open.
Version Information The CADKEY translator supports import of surface or solid entities from CADKEY version 19 part or assembly files.
CATIA Graphics Files The CATIA® Graphics (CGR) translator is integrated into the SolidWorks software and is always available as a file type in the Open and Save As dialog boxes. Import The CATIA Graphics translator imports CGR files as SolidWorks part documents. CGR files contain only graphical information and are for viewing only. System Requirements: Windows NT® or Windows 2000 or above. To open a CGR file in SolidWorks:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to Catia Graphics (*.cgr).
3.
Browse to the desired file and click Open.
Export The CATIA Graphics translator exports SolidWorks part or assembly documents as CATIA graphics files that users can view in CATIA, CATweb, and DMU Navigator. To export a SolidWorks document as a CGR file:
1.
With a SolidWorks part or assembly document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to Catia Graphics (*.cgr).
3.
Type the file name in the File name box, and click Save.
Version Information The CATIA Graphics translator supports CATIA version 5, release 1 through release 9.
DXF 3D Files The DXF 3D translator extracts ACIS information from a DXF file, if that information exists in the file, and imports it into a SolidWorks part document. If a DXF file contains multiple bodies or an assembly, SolidWorks creates an assembly document. Note the following translator limitations: •
It is not a 2D to 3D converter.
•
It does not import 2D or wireframe data from DXF files.
The DXF 3D translator is integrated into the DXF/DWG translator in the SolidWorks software and is always available when you select DXF (*.dxf) under Files of type in the Open dialog box.
13-18
To open a DXF 3D part:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to DXF (*.dxf).
3.
Browse to the desired file, and click Open. The Conversion Unit dialog box appears.
4.
Select the unit in which the original model was created, or click Other and type the scale in the Unit Scale box.
5.
Click OK.
Version Information The DXF 3D translator supports DXF 3D files including, but not limited to, versions AutoCAD® R14 and above.
DXF/DWG Files (*.dxf, *.dwg) Bitmaps stored in DXF/DWG files in AutoCAD®'s native bitmap format are not supported. You can copy and paste entities from an AutoCAD DXF or DWG file into SolidWorks part, assembly, and drawing documents. You can insert DXF or DWG files directly into the current SolidWorks part or drawing document with the Insert, DXF/DWG tool. The menu item activates the DXF/DWG Import Wizard at the appropriate dialog box, with simplified options to help you insert these files. The DXF/DWG translator supports the import and export of hole tables. Import The DXF/DWG translator imports DXF or DWG files, including Mechanical Desktop files, as SolidWorks part or drawing documents, according to the option settings in the DXF/DWG Import Wizard. This translator also imports DXF 3D files without the wizard. In a drawing document, you can import the geometry to the drawing sheet or the drawing sheet format. Entities in either paper space or model space are imported. When you import drawings, the most popular AutoCAD SHX or True Type fonts are supported, even though you may not have the fonts installed. See AutoCAD Font Support. If you import a DXF or DWG file that contains a large number of blocks (more than 200), you are prompted to enable the Explode Blocks option. Explode the blocks to improve import performance. The DXF/DWG translator imports: •
AutoCAD Mechanical annotations, known as proxy entities, (such as surface finish symbols or GTOL frames) and automatically drawn objects (such as cams and springs) when you import DXF or DWG files as SolidWorks drawing documents. The translator converts these imported items to equivalent SolidWorks objects, or creates them as blocks of primitive geometry, as appropriate.
•
Associative and non-associative crosshatches as area hatches.
•
XREFs in AutoCAD DWG files.
•
DWG files with multiple sheets.
When you import DWG files, you can now see a thumbnail image of the file in the Preview panel of the Open dialog box. Previews appear for DWG files created by both SolidWorks and AutoCAD. In AutoCAD, the bitmap preview option must be enabled when the file is last saved. The Open dialog box remembers the Preview check box state from the last time you opened a DWG file. The SolidWorks software fully supports the import of AutoCAD block definitions and instances with properties and attributes. When you import AutoCAD DWG files saved in paper space (layout mode) as SolidWorks drawing documents, the DXF/DWG Import Wizard converts each AutoCAD viewport into a separate SolidWorks drawing view. Drawing view data is selectable if you activate the drawing view.
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Chapter 13 Import/Export
Data that does not belong to a viewport is imported to the drawing sheet. Drawing sheet data is selectable if you activate the drawing sheet. If Dynamic drawing view activation is enabled, you must lock sheet focus to select drawing sheet data. The DXF/DWG translator alerts you to problems encountered when importing a DXF or DWG file. To import an AutoCAD 2004 DXF or DWG file, you must save the file in AutoCAD 2004 as "AutoCAD 2000/ LT2000." SolidWorks warns you if you try to import AutoCAD 2004 DXF or DWG files that are not saved in this format. You can import entire DWG sheets as view only SolidWorks drawing sheets, which allows the direct display of the original DWG entities inside SolidWorks drawing documents. You can view, pan, zoom, and print these sheets. Select View only in the DWG Import - Drawing Layer Mapping dialog box to import DWG sheets as view only sheets. Export The DXF/DWG translator exports only drawing documents as .dxf or .dwg files. When you export a drawing as a .dxf or .dwg file, the drawing's sheet scale is used for the new file. All entities (such as edges, annotations, and assembly components) on layers are exported to the assigned layer. SolidWorks crosshatch patterns are translated into AutoCAD hatch patterns when you export SolidWorks documents as DXF or DWG files. The SolidWorks software translates the SolidWorks crosshatch patterns as non-associative hatch definitions, and preserves the layer and color of the original crosshatch. The SolidWorks application also supports crosshatch export when you map layers with a mapping file. You have the option to map only those items whose layers are not otherwise defined when you export SolidWorks drawing documents as DXF or DWG files. All entity types that you can assign to AutoCAD layers through the mapping file support layering in the SolidWorks drawing format. The DXF/DWG translator supports line thickness, hidden sketches, and auto-centerlines. Version Information The DXF/DWG translator supports importing and exporting of OLE objects through DXF/DWG files of version 13 and higher. DXF/DWG View Only You can import entire DWG sheets as view only SolidWorks drawing sheets, which allows the direct display and printing of the original DWG entities inside SolidWorks drawing documents. You can view, pan, zoom, and print these sheets. Only view-related controls are available. The View only functionality improves import and viewing performance. If you have a large schematic drawing to include as a reference in a SolidWorks drawing document, View only eliminates the need to convert the schematic drawing document entities. When you print the SolidWorks drawing, the printed document contains all the items from the view only sheet. When you open a SolidWorks drawing document that contains view only DWG data, the DXF/DWG View Only PropertyManager appears and (VIEW ONLY) appears in the SolidWorks title bar. To import a DWG file as view only:
1.
Open a DWG file. The DXF/DWG Import Wizard appears.
2.
3.
In the DXF/DWG Import - Drawing Layer Mapping dialog box: a.
Select Import to drawing.
b.
Select View only to import the current sheet only, or View only all to import all sheets in the DWG file.
Click Next to set options in the DXF/DWG Import - Document Settings dialog box, or click Finish to accept all settings and import the DWG file. The DWG file opens and the DXF/DWG View Only PropertyManager appears.
13-20
4.
Set the values in the PropertyManager to manage link references. Use the PropertyManager to enable and manage the external reference between the view only sheet and its source DWG file.
5.
Click OK
.
DXF/DWG View Only PropertyManager The DXF/DWG View Only PropertyManager appears when you import a DWG file as a drawing and select View only or View only all in the DWG Import - Drawings Layer Mapping dialog box. The PropertyManager controls the following properties: Link to. Enables linking of the view only sheet in the SolidWorks drawing document (*.slddrw) to its source DWG file. When you select this option, if the DWG source file has been modified since the *.slddrw file was created, the view only sheet appearance updates accordingly. Folder. Displays the path to the linked source DWG file. . Click to browse to a new DWG file to display as view only. The path is displayed in the Folder box. Update. Click to manually update the link and the view only display after you browse to the source DWG file in the Folder box. Inserting DXF/DWG Files You can insert DXF or DWG files directly into the current SolidWorks drawing or part document with the Insert, DXF/DWG tool. The menu item activates the DXF/DWG Import Wizard at the appropriate dialog box, with simplified options to help you insert these files. When you insert DXF or DWG files into SolidWorks drawing documents, the SolidWorks software inserts a new sketch on the current sheet. When you insert DXF or DWG files into SolidWorks part documents, the SolidWorks software inserts a new sketch, and the software prompts you to select a plane or face for the sketch if you have not selected one. For example, you can insert a DXF file as a sketch into a SolidWorks part document, then use the inserted sketch to modify the part. To insert a DXF file into a SolidWorks part document:
1.
Open the SolidWorks part document into which you want to insert a DXF file.
2.
Select a face on the part. NOTE: The file is inserted as a sketch onto the face or plane you select.
3.
Click Insert, DXF/DWG. The Open dialog box appears.
4.
Open the DXF file you want to insert. The DXF/DWG Import Wizard opens to the Part Document Options dialog box, with the appropriate options selected.
5.
Click Finish to accept the default settings.
The DXF file entities are inserted into the SolidWorks part document as a sketch on the selected face. Now you can use the inserted sketch to modify the part. 6.
Click Extruded Cut
SolidWorks 2004 Reference Guide
on the Features toolbar, or Insert, Cut, Extrude.
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Chapter 13 Import/Export
7.
8.
Under Direction1, do the following: •
Set End Condition to Through All.
•
Select the Flip side to cut check box, if necessary, to make sure you create the desired part.
Click OK
.
The imported DXF sketch creates the cut on the SolidWorks part, resulting in the finished part document. Copying and Pasting from AutoCAD to SolidWorks You can copy and paste entities from an AutoCAD DXF or DWG file into SolidWorks part, assembly, and drawing documents. In the SolidWorks drawing document, the lines, arcs, notes, annotations, and so forth that you paste are attached to either a drawing view or the sheet, whichever is active. The pasted entities inherit scaling, grouping, visibility, and other properties from the drawing view or sheet. In SolidWorks part and assembly files, you must select a planar face onto which you paste the entities as a sketch. To copy and paste entities from AutoCAD to a SolidWorks drawing document:
1.
In AutoCAD, open a DXF or DWG file. This example shows a DWG file. Select the entities inside the box, then click Edit, Copy.
2.
In SolidWorks, open the SolidWorks drawing document into which you want to paste the entities. Click inside the sheet in the graphics area where you want to paste the entities.
3.
Click Edit, Paste to paste the entities onto the active sheet.
AutoCAD file entities
AutoCAD file entities pasted into SolidWorks document
Imported DXF/DWG Entities Entities that are imported from a .dxf or .dwg file can appear to be dimensioned and to be related to one another. To actually add the dimensions and relations, you must attach the dimensions and constrain all of the entities. You can then create a sketch in a part or assembly from the imported entities. Attach Dimensions You can attach the dimensions to the nearest reasonable sketch entities all at once. To attach dimensions:
With an imported .dxf or .dwg drawing document active, click Tools, Dimensions, Attach Dimensions.
13-22
Constrain All You can set relations on the sketch entities of an unconstrained imported .dxf or .dwg file. To solve relations in an imported drawing:
Click Tools, Relations, Constrain All. The SolidWorks software adds all the apparent relations and reports the number of relations that are added. Sketch from Drawing You can transfer entities from a drawing to an open sketch in a part or assembly. To insert sketch entities from a drawing:
1.
Open a sketch in a part or assembly.
2.
Click Insert, Customize Menu, and select Sketch from Drawing to activate this menu item.
3.
Click Insert, Sketch from Drawing.
4.
Make your drawing the active window and drag-select the sketch entities. The sketch entities must lie entirely within the drawing view border.
5.
Make your part or assembly the active window, and notice the sketch entities have been inserted into the open sketch.
DXF/DWG Mapping You can map selected SolidWorks entities or colors to different layers or colors in a .dxf or .dwg file. You create map files in the SolidWorks software to assign selected items to designated layers or colors in the .dxf or .dwg file. To create a map file:
1.
Open the SolidWorks drawing document for which you want to create a map file.
2.
Click File, Save As. The Save As dialog box appears.
3.
Set Save as type to Dxf (*.dxf) or Dwg (*.dwg), then click Options. The Export Options dialog box appears with DXF/DWG selected on the File Format tab.
4.
5.
Do the following: a.
Select the Custom Map SolidWorks to DXF check box.
b.
Click to clear the Don’t show mapping on each save check box.
c.
Click OK to close the Export Options dialog box.
Type a name for the drawing file in the File name box, then click Save. The SolidWorks To DXF/DWG Mapping dialog box appears.
6.
Define the layers then map the entities, or map the colors you want to map in the .dxf or .dwg file. Select the Keep existing SolidWorks drawing layers for entities check box to apply the mapping file settings only to those entities whose layers are not defined and to preserve existing SolidWorks drawing file layers in the exported file. If you do not select this option, the mapping file definitions overwrite all of the current SolidWorks drawing file layers.
7.
Click OK to save the SolidWorks drawing with mapping applied to the document.
See also Define Layers, Map Entities, or Color Mapping. To save a map file:
1.
Click Map File Settings in the SolidWorks To DXF/DWG Mapping dialog box. The Map File Settings dialog box appears.
2.
Select the Save map file check box, and clear the Load map file check box.
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Chapter 13 Import/Export
3.
Type a path and name for a new map file in the box, or browse to an existing file.
4.
Click OK.
To use a previously saved map file:
1.
Click Map File Settings in the SolidWorks To DXF/DWG Mapping dialog box. The Map File Settings dialog box appears.
2.
Select the Load map file check box, and clear the Save map file check box.
3.
Browse to an existing file, and click OK. NOTE: Previously saved map files can contain information for each of the mapping tabs. Review all tabs prior to saving the SolidWorks drawing document.
eDrawings eDrawings lets you animate and view models and drawings. It also allows you to create a document convenient for sending to others. Two tools are available on the eDrawings 2004 toolbar: •
Animate an eDrawing 2004 . Also available by clicking View, Modify, Animate. Begins continuous animation of the model in shaded mode. To stop the animation, click the Animate an eDrawing 2004 tool again, or click View, Modify, Animate again.
•
Publish an eDrawing 2004 . Also available by clicking File, Publish eDrawing 2004. Opens the eDrawings Viewer, which has tools for viewing, shading, animating, hyperlinking, and arranging drawing views. NOTE: If the eDrawings 2004 toolbar is not visible, click View, Toolbars, eDrawings 2004.
You can: •
Create eDrawing files from SolidWorks part, assembly, and drawing documents.
•
Open SolidWorks documents in the eDrawings Viewer.
•
Save eDrawing data to SolidWorks documents in the eDrawings Viewer.
You can view any SolidWorks document from SolidWorks 97Plus and later. If the document does not contain eDrawings data, in the SolidWorks application: •
Select Save eDrawings data in SolidWorks document in Tools, Options, System Options, General before you save the document -or-
•
Select Save eDrawing data in the Save As dialog box
Saving the eDrawings data in the SolidWorks document enables functionality in the eDrawings Viewer, such as: •
13-24
Configurations o
Component names in the Component tree
o
Multiple configurations (only the last saved configuration is visible)
•
Explode in assembly documents
•
Hole information for Measure
•
Hyperlinks in drawing views
•
Mass properties
•
OLE objects
•
Shaded information and animation in drawing documents
To save a SolidWorks document as an eDrawing file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
In the Save as type list, select one of the following: •
eDrawing (*.eprt). Part documents.
•
eDrawing (*.easm). Assembly documents.
•
eDrawing (*.edrw). Drawing documents. NOTE: SolidWorks displays the correct eDrawing file type based on the SolidWorks document type.
3.
Click Save to create the eDrawing file.
eDrawings Professional With the optional eDrawings Professional tools, you can: •
Mark up files
•
View cross sections
•
Measure dimensions
•
Move assembly components
•
View exploded views
•
Display mass properties
For more information, click Help, eDrawings Help Topics in the eDrawings Viewer, or visit the web site at www.solidworks.com/edrawings.
Saving Drawing Sheets in eDrawing Files If a SolidWorks drawing document has multiple sheets, when you publish an eDrawing file, you can select which sheets to save to the eDrawing file. If you publish multiple sheets, the file size and the time required to save the eDrawing file may increase. NOTES: •
You must have eDrawings Professional installed to choose the sheets to save. If you have the free eDrawings Viewer, all the sheets are published with the eDrawing file.
•
You must select the eDrawings2004 check box under Tools, Add-Ins to display the eDrawings toolbar and to publish eDrawing files.
To save sheets when you publish eDrawing files:
1.
Open the SolidWorks document containing multiple sheets that you want to publish as an eDrawing file.
2.
Click Publish an eDrawing 2004
on the eDrawings toolbar, or click File, Publish eDrawing 2004.
The Sheets to Save to eDrawing dialog box appears. 3.
4.
Select one of the following: • Current sheet. Save the current sheet only. •
All sheets. Save all sheets.
•
Selected sheets. Select the sheets to save from the list displayed below.
Click OK to publish the eDrawing file. A progress bar reports the publication process. The eDrawings Viewer opens and lists the selected sheets on the Sheets tab in the eDrawing Manager
5.
To display a different sheet in the graphics area, double-click the sheet on the Sheets tab, or click the tab with the sheet name below the graphics area.
6.
In the eDrawings Viewer, click Save
SolidWorks 2004 Reference Guide
to save the eDrawing file with the sheets.
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Chapter 13 Import/Export
Saving Configurations in eDrawing Files If a SolidWorks part or assembly document has multiple configurations, when you publish an eDrawing file, you can select which configurations to save to the eDrawing file. If you publish multiple configurations, the file size and the time required to save the eDrawing file may increase. NOTES: •
You must have eDrawings Professional installed to choose the configurations to save. If you have the free eDrawings Viewer, only the active configuration is published with the eDrawing file.
•
You must select the eDrawings2004 check box under Tools, Add-Ins to display the eDrawings toolbar and to publish eDrawing files.
To save configurations when you publish eDrawing files:
1.
Open the SolidWorks document containing multiple configurations that you want to publish as an eDrawing file.
2.
Click Publish an eDrawing 2004
on the eDrawings toolbar, or File, Publish eDrawing 2004.
The Configurations to Save to eDrawing dialog box appears. 3.
4.
Select one of the following: •
Current configuration (default). Save the current configuration only.
•
All configurations. Save all configurations.
•
Selected configurations. Select the configurations to save from the list displayed below.
Click OK to publish the eDrawing file. A progress bar reports the publication process. The eDrawings Viewer opens with images of the saved configurations displayed on the Configurations tab. You can click the images to display the different configurations.
5.
In the eDrawings Viewer, click Save
to save the eDrawing file with the configurations.
Highly Compressed Graphics Files The Highly Compressed Graphics (HCG) translator exports SolidWorks documents as Highly Compressed Graphics files. HCG files, used by CATIA® in CATweb, are optimized for transmission over the Web. You can export only parts and assemblies with the HCG translator. The exported files contain graphical information only; you cannot edit these files. The HCG translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as an HCG file:
1.
With a SolidWorks part or assembly document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to HCG (*.hcg).
3.
Type the file name in the File name box, and click Save.
Version Information The HCG translator exports SolidWorks documents as CATIA version 5, release 9 files.
13-26
HOOPS Files The HOOPS translator exports SolidWorks part or assembly documents as HOOPS (.hsf) files. HOOPS files are streaming graphics files that download details piece by piece to a web page, which is helpful when you display large files. You can view HOOPS files over the Internet using the HOOPS viewer. See www.hoops3d.com for information about the HOOPS viewer. NOTE: The exported files contain graphical information only; you cannot edit these files. The HOOPS translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as a HOOPS file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to HOOPS HSF (*.hsf).
3.
Type the file name in the File name box, and click Save.
Version Information The HOOPS translator exports SolidWorks documents as HOOPS version 8.0 files.
IGES Files (*.igs, *.iges) The following IGES entity types are supported for import and export, except where noted. The IGES translator can import and export IGES surfaces and BREP solids. The IGES error file information is merged into the IGES report file (.rpt). Import If there is wireframe geometry in an imported file, the software reads the IGES data and forms curves for the IGES wireframe entities. The 2D geometry is imported into a sketch rather than imported as reference curves. If you want the software to try to form a solid from imported IGES data, export the solid or surfaces from the source system as trimmed surfaces (Entity type 144) or as untrimmed surfaces (Entity types 128, 122, 120, 118, 114). Also, set the number of significant digits (precision) as high as possible to ensure accurate translation. You can import 3D curves in an IGES file as 3D sketch entities. In the Import Options dialog box, select the Free point/curve entities check box and click Import as sketch(es). The IGES translator supports colors when you import curves. You can select the levels to import for IGES files that contain multiple levels. Select the Show IGES levels option in the Import Options dialog box to display the IGES-In Surfaces, Curves, and Levels dialog box. Export The IGES translator exports SolidWorks part and assembly documents as IGES files. Parts and surfaces exported to IGES format retain their part or surface color, and are displayed in color when in Shaded mode. You can export both surfaces and solids in the same IGES file. If you export a SolidWorks assembly document that has hidden or suppressed components to IGES format, a dialog box appears asking if you want to resolve these components. •
Click Yes, and all the components, including the hidden or suppressed ones, are exported.
•
Click No, and the hidden or suppressed components are not exported.
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Chapter 13 Import/Export
IGES Entity Types
13-28
IGES Entity Type
Entity Name
514
Shell Entity
510
Face Entity
508
Loop Entity
504
Edge Entity
502
Vertex Entity
416
External reference entity
408
Singular subfigure instance entity
406 Form 12
External reference file
402 Form 7
Group entity
314
Color definition entity
308
Subfigure definition entity
198
Toroidal Surface
196
Spherical Surface
194
Right Circular Conical Surface
192
Right Circular Cylindrical Surface
190
Plane Surface
186
Manifold Solid B-Rep Object Entity
144
Trimmed (parametric) surface
143 Import only
Bounded Surface
142
Curve on a parametric surface
140 Import only
Offset surface
128
Rational B-spline surface
126
Rational B-spline curve
124
Transformation matrix entity
123
Direction entity
122
Tabulated cylinder
120
Surface of revolution
118 Import only
Ruled surface
116
Point
114 Import only
Parametric spline surface
112
Parametric spline curve
110
Line
108
Plane
106 form 12 Import only
Copious Data—3D Piecewise linear curve
106 form 11 Import only
Copious Data—2D Piecewise linear curve
104 Import only
Conic arc
102
Composite curve
100
Circular arc
IGES Levels If there are curves in the IGES file or if there are different levels (or layers) in the IGES file, the IGES-In Surfaces, Curves, and Levels dialog box appears. Levels are sometimes used by other systems to separate assembly components or to separate IGES entity types. To select the desired entities and levels:
1.
Select Include surfaces to import any surfaces in the file, if applicable.
2.
Select Include curves to import any curves in the file, if applicable.
3.
Select the levels to include:
4.
•
Include all levels. All levels are imported to level zero.
•
Include levels. Only the specified levels are imported to level zero.
Click OK to exit the IGES-In Surfaces, Curves, and Levels dialog box or click Cancel to abort the import process.
IGES 3D Curves Type of 3D Curve
Exported IGES Entity Types
B-splines (entity 126)
126, 110, 102*, 100
Parametric splines (entity 112)
112, 110, 102*, 100
JPEG Files The JPEG translator takes a snapshot of anything displayed in the graphics window of a SolidWorks part, assembly, or drawing document, and exports it as a .jpg file. A .jpg file is an image file that you can open in most image viewers. The .jpg file displays only the information from the graphics window; toolbars and other areas of the SolidWorks window do not appear. The JPEG translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as a JPEG file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to JPEG (*.jpg).
3.
Type the file name in the File name box, and click Save.
Mechanical Desktop Files The MDT translator imports part and assembly information from Mechanical Desktop® (MDT) files as SolidWorks part or assembly documents. You must have MDT installed on your desktop, but it does not have to be running, to use the MDT translator. NOTE: If you import large assemblies from MDT, SolidWorks recommends you do the following: •
Start Mechanical Desktop and open the MDT file inside the MDT application before you import the file into the SolidWorks application.
•
Set the MDT temporary files path to a drive where you have sufficient space (1GB minimum).
•
Increase the paging file size to appropriate limits. This is relevant mainly for low configuration systems.
MDT files can contain a combination of part, assembly, and drawing files. The MDT translator provides different conversion options, depending upon the contents of the MDT file. The MDT translator supports import of MDT assembly relations.
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Chapter 13 Import/Export
The MDT translator supports the following items during import: •
Large MDT assembly files, in excess of 130MB in size, depending on the complexity of the data.
•
All types of mates, including point-to-point and line-to-line mates
•
MDT combined features, which are sometimes referred to as toolbodies
•
MDT tapped hole features (cosmetic thread annotation)
•
MDT design tables (Design Variable Tables - Global Variable Sheets)
•
MDT Work Features (Work Planes, Work Axes, and Work Points)
•
MDT pattern features, which creates multiple disjoint bodies
The MDT translator is integrated into the DXF/DWG translator in the SolidWorks software, and is always available when you select DXF (*.dxf) or DWG (*.dwg) under Files of type in the Open dialog box. Version Information The MDT translator supports the following MDT versions: •
MDT4.0 or higher (MDT4.0 with Windows 2000 or Windows® XP is not supported)
•
MDT5.0 only with Windows 98, Windows 2000, or Windows NT (Windows 98 must have MDT5.0 Service Pack 1 or later)
•
MDT 6.0 only with Windows® 98, Windows® 2000, Windows® Me, Windows NT® 4.0 (with Service Pack 5 or later), or Windows® XP Professional.
To open an MDT file:
1.
Click File, Open. The Open dialog box appears.
2.
Set Files of type to DXF (*.dxf) or DWG (*.dwg).
3.
Browse to the desired file, and click Open. The MDT File Import dialog box appears. NOTE: If you do not have Mechanical Desktop installed, the DXF/DWG Import Wizard appears instead of the MDT File Import dialog box.
4.
Do one of the following: •
To import the MDT file as a part document using the MDT translator: 1.
Click Import as a part with MDT translator, then click OK. The DXF/DWG Import - Document Settings dialog box appears with the most appropriate options automatically selected. You can change the options if desired.
2.
Select from the following options: •
Units of imported data. Select the unit in which the imported model was created.
•
MDT Options, Component Import Options. Click one of the following options: o o
•
Use Geometry Import. Imports one solid part that you cannot directly edit.
MDT Options, If file with the same name exists. Click one of the following options: o
13-30
Use Feature Import. Imports individual features that you can edit.
Use existing. Uses the existing SolidWorks file and does not import the new part or assembly file.
o
Overwrite. Overwrites the existing SolidWorks file.
o
Save with new name. Prompts you to save the file with a new name.
3.
Adjust the following Preview box options to change the preview displayed as desired: •
4.
Select from the following viewing options: o
Previous view
o
Zoom to Fit
o
Rotate
o
Select a view from the pulldown menu
, Zoom to Area
, Zoom In/Out
, Pan
•
White background. Select this check box to display the model with a white background color.
•
Import this sheet. Select this check box to import drawing views.
•
Model tab. Select this tab to display the part data of the imported model. This tab is selected by default when you import MDT files as parts.
Click Finish to import the MDT file as a part document. The Mechanical Desktop to SolidWorks Converter dialog box reports on the conversion process. The MDT translator imports the MDT file as a SolidWorks document.
•
To import the MDT file as a drawing document using the DXF/DWG translator (MDT does not need to be installed in this case): 1.
Click Import as a drawing with the DXF/DWG translator, then click OK. The DXF/DWG Import - Drawing Layer Mapping dialog box appears with the most appropriate options automatically selected. You can change the options if desired.
2.
Select from the following options: •
Import to drawing. Imports the MDT file as a drawing and creates two sheets, one with the model outline and another with the drawing data. This option is selected by default when you import MDT files as drawings.
•
Import to part. Imports the MDT file as a part, creating one part with 3D solid data and a sheet.
•
Show Layers. Select one of the following options: o
o
o
All selected layers. Shows all the layers being imported to either the drawing sheet or the sheet format. If a layer is not selected, the entities on that layer are ignored for import and not included in the drawing, as shown in the preview image. Layers selected for drawing sheet. Shows the subset of layers whose entities are imported to the drawing sheet. Layers selected for sheet format. Shows the subset of layers whose entities are imported to the sheet format. Drawing sheet layers and sheet format layers are mutually exclusive; entities cannot be directed to both the drawing sheet and the sheet format at the same time.
NOTES:
3.
•
The layers themselves are always present in the resulting drawing. Depending on the option you selected, the layer entities may be ignored, and the initial status of the layer may be off.
•
These options allow you to direct or redirect entities by layer to either the drawing sheet or the sheet format, or to completely block out the entities of a specific layer.
Adjust the following Preview box options to change the preview displayed as desired: •
SolidWorks 2004 Reference Guide
Select from the following viewing options:
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Chapter 13 Import/Export
4.
o
Previous view
o
Zoom to Fit
o
Rotate
o
Select a standard view from the pulldown menu
, Zoom to Area
, Zoom In/Out
, Pan
•
White background. Select this check box to display the model with a white background color.
•
Import this sheet as. This check box is selected by default when you import MDT files as drawings. The name of the selected sheet appears in the box to the right. You can rename the sheets you import and the new names appear in the new SolidWorks document.
•
Model tab. Select this tab to display a preview of the model space from the imported model. This tab is selected by default when you import MDT files as drawings.
•
Layout tab. Select this tab to display a preview of the drawing layout and to display the tab name in the box next to Import this sheet as. The tabs match the tabs shown when you have the DXF or DWG file open inside the AutoCAD application.
Do one of the following: •
Click Finish to accept the remaining default options and import the MDT file as a part document.
•
Click Next to set the document settings. The DXF/DWG Import - Document Settings dialog box appears.
5.
Set the following options: •
Input file properties. Set the Data units. You can set the units to Angstroms (1.0e-10 meters), Nanometers (1.0e-9 meters), Microns (1.0e-6 meters), Microinches (1.0e-6 inches), or Mils (1.0e-3 inches), in addition to the standard Feet, Inches, and Meters units.
•
Output file properties. Set the following options: o
o
Width. Sets the width of the drawing sheet.
o
Height. Sets the height of the drawing sheet.
o
Geometry scaling. Sets the scale for the imported drawing. The default is 1:1.
•
Geometry positioning. Sets the position of the geometry on the sheet. Click one of the following:
o o
13-32
Document template. Sets a document template for the imported entities. If Paper size, Width, and Height are specified in the sheet format of the template, these settings update accordingly. This template information is saved in the registry for DXF files, and used in future DXF file imports, unless you change the template.
•
o
6.
Paper size. Sets the drawing sheet size. Select User Defined to specify the Width and Height.
Move entities onto the sheet. Moves the lower left corner of the imported drawing to the origin of the SolidWorks drawing sheet. Center in sheet. Centers the imported drawing in the drawing sheet. Position (default). Specifies where to place the origin position of the imported drawing on the SolidWorks drawing sheet. Input X and Y coordinates to place the origin of the imported drawing.
Click Finish to import the MDT file as a drawing document.
Parasolid Files (*.x_t, *.x_b) •
Data exported to or imported from Parasolid format retains its color when displayed in Shaded mode.
•
Component names in assemblies are retained for both import and export.
•
The Parasolid translator does not support the import or export of point data.
•
The Parasolid translator supports import and export of curves and wireframes.
Import •
The Parasolid translator imports Parasolid text files or binary files as SolidWorks documents.
•
The Parasolid translator imports files with the extension .x_t, .x_b, .xmt_txt, or .xmt_bin.
Export The Parasolid translator exports SolidWorks part or assembly documents as Parasolid text files or binary files. Binary files are smaller than text files, but binary files are not supported in some target applications. Select the type supported by the target application. If you export a SolidWorks assembly document that has hidden or suppressed components to a Parasolid text or binary file, a dialog box appears asking if you want to resolve these components. •
Click Yes, and all the components, including the hidden or suppressed ones, are exported.
•
Click No, and the hidden or suppressed components are not exported.
Version Information The Parasolid translator supports all Parasolid versions up to and including version 15.0.
PDF Files This add-in module exports SolidWorks part, assembly, and drawing documents as Portable Document Format (PDF) files. Save as PDF is not available on Windows® Me. To deactivate or reactivate the PDF translator:
1.
Click Tools, Add-Ins.
2.
Select or clear Save As PDF.
To export a SolidWorks document as a PDF file:
1.
With a SolidWorks document open, click File, Save As.
2.
In the dialog box, select PDF (*.pdf) in Save as type.
3.
Type the file name File name, and click Save.
Pro/ENGINEER Files The Pro/ENGINEER translator imports Pro/ENGINEER® files into SolidWorks and exports SolidWorks documents as Pro/ENGINEER files. The Pro/ENGINEER translator is integrated into the SolidWorks software and is always available as a file type in the Open and Save As dialog boxes. NOTE: Pro/ENGINEER accepts only ASCII characters in its file names. When you save a SolidWorks document as a Pro/ENGINEER file, any non-ASCII characters are replaced by an underscore (_).
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Chapter 13 Import/Export
Importing Pro/ENGINEER Files into SolidWorks The Pro/ENGINEER translator imports Pro/ENGINEER part or assembly files as SolidWorks part or assembly documents. The attributes, features, sketches, and dimensions of the Pro/ENGINEER part are imported. If all of the features in the file are not supported, you can choose to import the file as either a solid body or a surface model. The Pro/ENGINEER translator supports import of free curves, wireframes, and surface data. When importing an assembly, you can control how to import individual components. Sub-assemblies are supported as well. You can import Pro/ENGINEER surface-trim and surface-extend features into SolidWorks. These features are read in from the Pro/ENGINEER file and mapped to SolidWorks. Some known limitations are as follows: •
Version Information - Versions 17 through 2001 of Pro/ENGINEER are supported. Pro/ENGINEER Wildfire™ files are not supported.
•
Assembly features are not supported.
Exporting SolidWorks Documents as Pro/ENGINEER Files The Pro/ENGINEER translator exports part or assembly documents as Pro/ENGINEER part or assembly files. Version Information - The exported files are saved as Pro/ENGINEER version 20 files. More Information Click the links below for details about these topics: •
Importing Pro/ENGINEER assembly files into SolidWorks
•
Exporting SolidWorks part or assembly documents as Pro/ENGINEER files
Importing Pro/ENGINEER Part Files Into SolidWorks To import a Pro/ENGINEER part file into SolidWorks:
1.
Click File, Open.
2.
In the Open dialog box, set Files of type to ProE Part (*.prt;*.prt.*;*.xpr).
3.
Browse to the desired file, and click Open. The Pro/ENGINEER To SolidWorks Converter dialog box appears.
4.
Set these options: •
Import geometry directly. Imports a model without features, either as a solid or surfaces. o
o
5.
BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid. Knitting. Attempts to knit surfaces during import. Select the Try forming solid model(s) check box to try to form solids using Knitting mode. Otherwise, the models are imported as surface bodies.
•
Analyze the model completely. Determines the number of features that SolidWorks can recognize and import.
•
Import material properties
•
Import sketch/curve entities
Click OK. If you select Import geometry directly, SolidWorks imports the model. If you select Analyze the model completely, SolidWorks parses the imported file and redisplays the Pro/Engineer to SolidWorks Converter dialog box with the following options:
13-34
6.
•
Features. Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.
•
Body. Attempts to import the model as a solid using Knitting. The Attempt to correct invalid feature check box has no effect if you click Body.
•
Generate translation report. If you select Features, generates a report that includes the features plus the recognition and import status.
Select Feature or Body to import the part. If you selected Generate translation report, the Translation Report dialog box appears.
7.
8.
Click one of the following: •
•
Copy. Copies the translation report to the clipboard so you can paste it into another file.
Close the dialog box to import the part.
Importing Pro/ENGINEER Assembly Files Into SolidWorks To import a Pro/ENGINEER assembly file into SolidWorks:
1.
Click File, Open.
2.
In the Open dialog box, set Files of type to ProE Assembly (*.asm;*.asm.*;*.xas).
3.
Browse to the desired file, and click Open. The Pro/ENGINEER To SolidWorks Converter dialog box appears.
4.
Set these options: •
Component Import Options section. Select one of the following: o
Use feature import for all parts. Imports all component parts as features.
o
Use body import for all parts. Imports all component parts as bodies.
o
•
5.
•
BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid.
•
Knitting. Attempts to knit surfaces during import.
Prompt for each part. Prompts you to import each component part individually as a feature or a body.
If same name SolidWorks file is found section. Select one of the following: o
Use Existing. Uses the existing SolidWorks file and does not import the new file.
o
Overwrite. Overwrites the existing SolidWorks file.
o
Save with new name. Saves the file with a new name automatically.
•
Import material properties
•
Import sketch/curve entities
Click Import. SolidWorks converts and imports the file. If you selected Prompt for each part in the Component Import Options section, SolidWorks redisplays the Pro/ENGINEER To SolidWorks Converter dialog box.
6.
Set these options: •
Import geometry directly. Imports a model without features, either as a solid or surfaces. o
SolidWorks 2004 Reference Guide
BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid.
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Chapter 13 Import/Export
o
7.
Knitting. Attempts to knit surfaces during import. Select Try forming solid model(s) to try to form solids using Knitting mode. Otherwise, the models are imported as surface bodies.
•
Analyze the model completely. Determines the number of features that SolidWorks can recognize and import.
•
Import material properties
•
Import sketch/curve entities
Click OK. If you select Import geometry directly, SolidWorks imports the model. If you select Analyze the model completely, SolidWorks parses the imported file and redisplays the Pro/Engineer to SolidWorks Converter dialog box with the following options:
8.
•
Features. Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.
•
Body. Attempts to import the model as a solid using Knitting. The Attempt to correct invalid feature check box has no effect if you click Body.
•
Generate translation report. If you select Features, generates a report that includes the features plus the recognition and import status.
Select Feature or Body to import the model component. If you selected Generate translation report, the Translation Report dialog box appears.
9.
Click one of the following: •
•
Copy. Copies the translation report to the clipboard so you can paste it into another file.
10. Close the dialog box. SolidWorks imports the component. The Pro/ENGINEER to SolidWorks Converter dialog box prompts you to import the next component. 11. Continue importing components until you have imported the entire assembly.
Exporting SolidWorks Documents as Pro/ENGINEER Files To export a SolidWorks document as a Pro/ENGINEER file:
1.
Click File, Save As. The Save As dialog box appears.
2.
3.
Set the Save as type box to one of the following: •
ProE Part (*.prt)
•
ProE Assembly (*.asm)
Click Save. The SolidWorks to Pro/ENGINEER Converter dialog box informs you of the progress, and the file is saved. If you export an assembly document that is referenced by other open documents, a message appears directing you how to proceed. Click OK to save the file. See Saving an Assembly and its Components for more information.
Solid Edge Files The Solid Edge translator imports the Parasolid information of Solid Edge® parts or assemblies into SolidWorks part or assembly documents. Only the Parasolid information is extracted, not the proprietary feature information. The Solid Edge translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box.
13-36
To open a Solid Edge part or assembly:
1.
Click File, Open. The Open dialog box appears.
2.
3.
Set Files of type to one of the following: •
Solid Edge Part (*.par)
•
Solid Edge Assembly (*.asm)
Browse to the desired file, and click Open.
Version Information The Parasolid translator imports Parasolid information from Solid Edge parts up to and including the most current version of Solid Edge.
STEP Files (*.step) The STEP translator supports import and export of body, face and curve colors of STEP AP214 files. The STEP AP203 standard does not have any color implementation. Import The STEP translator imports: •
STEP files as SolidWorks part or assembly documents.
•
Body geometry, body, face, and curve colors, and topology information from an AP214 STEP file.
•
Wireframe geometry from STEP AP203 and AP214 files.
•
STEP configuration data. You have the option to import this data by selecting the Map configuration data check box under STEP in the Import Options dialog box.
Export •
The STEP translator exports SolidWorks part or assembly documents to STEP files.
•
You can select to export individual parts or subassemblies from an assembly tree, limiting export to only those parts or subassemblies. If you select a subassembly, all of its components are automatically selected. If you select a component, its ascendants are partially selected, preserving the assembly structure.
•
SolidWorks supports exporting the unit of length of a part or assembly document to a STEP AP203 or AP214 file.
•
You can set export options in the STEP Export Options dialog box.
Version Information •
•
STEP Application Protocol AP203 is supported for both import and export. o
For import, Conformance Classes 1, 2 (surface data only), 4, 5, and 6 of AP203 are supported.
o
For export, Conformance Classes 1, 4, and 6 are supported.
STEP Application Protocol AP214 is supported for both import and export.
STL Files (*.stl) You can assign a unit of measure to a model for both import and export. Import The STL translator imports STL files as SolidWorks part documents. SolidWorks assembly files that you export as STL files import into SolidWorks as part documents. You have the option to import STL files as graphical data, solids, or surfaces. When you import STL files as graphical data, you can select the Import texture information check box to import texture information if this data exists.
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Chapter 13 Import/Export
Export The STL translator exports SolidWorks part and assembly documents as STL files. Click Try Print3D to open the Print3D web portal linked to the SolidWorks software. Print3D automates the prototype request process, eliminating the need to save parts as STL files. You can contact rapid part and prototype vendors to request price quotes and place orders for the current part document through the Print3D web portal.
TIFF Files (*.tif) Import You can insert a TIFF image as a background into part or assembly documents. See Inserting TIFF Files for more information. NOTE: The SolidWorks application does not support LZW format compression for TIFF files. Export The TIFF translator exports any SolidWorks document as a TIFF image. You can capture the image as it appears on a normal view (screen), or you can capture the image as it appears on a print preview. For drawing documents, you can select the sheet size and scale factor.
Inserting TIFF Files You can import a TIFF image and use it as a background of a part or assembly. The SolidWorks application does not support LZW format compression for TIFF files. To import a TIFF file:
1.
In a part or assembly document, click Insert, Customize Menu, and select Picture to activate this menu item.
2.
Click Insert, Picture.
3.
In the Open dialog box, browse to the desired file, and click Open. The selected file opens as a background image of your part or assembly. You can import RGB Full Color and Black & White (Bilevel) images, and you can also import Grayscale and Palette images from other systems.
To turn the display of the TIFF image on or off:
1.
Click View, Display, Customize Menu, and select Picture to activate this menu item.
2.
Click View, Display, Picture. When the Picture option is selected, the image is displayed; when the Picture option is cleared, the image is hidden.
To delete a TIFF image from a document:
1.
Click View, Modify, Customize Menu, and select Picture to activate this menu item.
2.
Click View, Modify, Picture, Delete.
To replace one TIFF image with another:
13-38
1.
Click View, Modify, Customize Menu, and select Picture to activate this menu item.
2.
Click View, Modify, Picture, Replace.
3.
In the Open dialog box, browse to the TIFF file that you want to use as a replacement, and click Open.
Unigraphics II Files The Unigraphics translator imports the Parasolid information of a Unigraphics® II part or assembly into a SolidWorks part or assembly document. Only the Parasolid information is extracted, not the proprietary feature information of a Unigraphics II part. You can import Unigraphics II compressed files. The Unigraphics translator is integrated into the SolidWorks software and is always available under Files of type in the Open dialog box. To open a Unigraphics part or assembly:
1.
Click File, Open.
2.
In the Open dialog box, set Files of type to UGII (*.prt).
3.
Browse to the desired file, and click Open. If the file contains multiple bodies, the Unigraphics to SolidWorks Converter dialog box appears.
4.
5.
Select an import option: •
Multibody as separate parts. Imports the multiple bodies as parts contained in an assembly document.
•
Multibody in the same part. Imports the multiple bodies as imported bodies contained in a part document.
Click OK.
Version Information You can import parts and assemblies from Unigraphics II version 10 and higher.
VDAFS Files (*.vda) VDAFS is a neutral file format for the exchange of surface geometry. Import Options The VDA translator imports VDAFS part files as SolidWorks part documents. Export Options The VDA translator exports SolidWorks part documents as VDAFS files. You can set the following option: •
Output coordinate system. Select a coordinate system to apply for export. If you select -- default --, no transformation matrix is applied.
Viewpoint Files This add-in module exports SolidWorks part or assembly documents to Viewpoint (.mts) files. You can view Viewpoint files over the Internet using the Viewpoint viewer. The Viewpoint files contain the compressed geometry of the model. The Viewpoint (MTS) translator also creates an .mtx file, which is in XML. This is the animation and attribute file of the model. The exported files contain graphical information only; you cannot edit these files. To deactivate or reactivate the Viewpoint translator:
1.
Click Tools, Add-Ins.
2.
Select or clear the SolidWorks MTS check box from the list of installed compatible software products.
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Chapter 13 Import/Export
To export a SolidWorks document as a Viewpoint file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to Viewpoint MTX/MTS (*.mts).
3.
Type the file name in the File name box, and click Save.
Version Information The Viewpoint translator exports SolidWorks documents as Viewpoint version 3.0.11 files.
VRML Files (*.wrl) VRML files can display 3D graphics over the Internet. Import The VRML translator imports all VRML files as SolidWorks part documents. SolidWorks assembly files that you export as VRML files import into SolidWorks as part documents. The VRML translator attempts to knit the VRML polygons into a solid. There are no contoured surfaces in the imported file; all surfaces are planar. This import option is intended as a last resort for importing data into SolidWorks. In many cases (especially complex models) the data does not knit into a usable solid, and is useful for viewing purposes only. You have the option to import VRML files as graphical data, solids, or surfaces. When you import VRML files as graphical data, you can select the Import texture information check box to import texture information if this data exists. Export The VRML translator exports SolidWorks part or assembly documents as VRML files. When you export as a VRML file, the SolidWorks software takes the View, Display, Section View option into account. If Section View is on, only the visible geometry is exported to the VRML file. This is different from the way the software behaves when you save documents as IGES, STEP, Parasolid, or ACIS files. When you export SolidWorks documents as VRML files, you can choose the version to export, VRML 1.0 or VRML 2.0 (VRML 97). Version Information The VRML translator supports all versions of VRML files up to and including VRML version 2.0 (VRML 97).
ZGL Files The ZGL translator exports SolidWorks part or assembly documents as RealityWave's ZGL file format. After you export the document, you must save the ZGL file into a RealityWave® database (VizStream Server). This converts the ZGL file into RealityWave’s streaming format that you can view over the Internet with the RealityWave viewer. The exported files contain graphical information only; you cannot edit these files. The ZGL translator is integrated into the SolidWorks software and is always available under Save as type in the Save As dialog box. To export a SolidWorks document as a ZGL file:
1.
With a SolidWorks document open, click File, Save As. The Save As dialog box appears.
2.
Set Save as type to RealityWave ZGL (*.zgl).
3.
Type the file name in the File name box, and click Save.
Version Information The ZGL translator exports SolidWorks documents as RealityWave version 2.0 files.
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14 Library Features and the Feature Palette Window
Library Features and the Feature Palette Window A library feature is a frequently used feature, or combination of features, that you create once and then save in a library for future use. You can create commonly used features, such as holes or slots, in common sizes, and save them as library features to use whenever you need them. You can use several library features as building blocks to construct a single part. This can save time, and it can help ensure consistency in your models. The Feature Palette™ window helps you organize and use library features, sheet metal forming tools, piping components, and other commonly used parts. The Feature Palette window gives you quick access to the items you use most, by simply dragging them into the SolidWorks window. This topic describes: •
Creating and editing library features
•
Adding library features to parts
•
Organizing library features, forming tools, piping components, and other parts in the Feature Palette window
•
Inserting palette items in parts and assemblies
•
Palette Features and Library Features - Similarities and Differences
Palette Features and Library Features - Similarities and Differences Similarities between palette features and library features: •
You create a palette feature in the same way as a library feature.
•
The palette feature is displayed as a library feature in the FeatureManager design tree of the target part.
•
You can dissolve a palette feature the same way as a library feature.
Differences between palette features and library features: •
When you add a palette feature to a part, you can simply drag the feature roughly where you want it to be, then place it precisely by re-attaching and modifying any locating dimensions saved in the feature.
•
You can edit the dimensions of the palette feature as you insert it into the part.
•
Not all library features are suitable for use in the Feature Palette window. A palette feature is limited to one mandatory reference (one face, plane, edge, or vertex) on the target part. See Mandatory References.
•
Library features that have multiple mandatory references (such as draft features that depend on the selection of several faces) cannot be added through the Feature Palette window.
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Chapter 14 Library Features and the Feature Palette Window
You can also use the Feature Palette window to add parts to an assembly. You can organize parts in logical groups, and you can see a miniature graphical view of each palette part. You can add fittings to piping assemblies by dragging them from the Feature Palette window. For more information, see SolidWorks Piping Help Topics. The Feature Palette window is also used to apply forming tools to sheet metal parts. Forming tools are special parts that punch, stretch, or shape the sheet metal part, to create embossments, lances, flanges, louvers, ribs, and so on. Limitations In library features, you cannot have relations to silhouette edges or axes.
Mandatory References A palette feature is limited to one mandatory reference on the target part. The limitation of a single mandatory reference does not mean that a palette feature can consist of only one feature. As long as the parent feature uses a single reference, the palette feature can include multiple child features. To examine the parent/child relationships, right-click the feature, and select Parent/Child. To determine if a library feature is suitable for use in the Feature Palette, insert it as a library feature in a target part (see Adding a Library Feature to a Part). If there is only one mandatory reference listed, you can use the library feature as a palette feature. Feature Limitations Because of the limitation of a single reference, lofts, sweeps, and shape features are allowed only in certain cases: •
For lofts, the single mandatory reference is the sketch plane of one of the profiles. This must be the face or plane where you drop the feature. Additional sketch planes must be offset from this plane, or from each other. The library feature must include the planes.
•
For sweeps, the sweep path is the single mandatory reference. This must be a model edge. The sketch plane for the sweep section must be a Normal to Curve plane, with the model edge as the curve (when you select the edge, click near the vertex where the plane should be placed). Include this plane in the library feature. Then, when you drop the palette feature in the target part, drop it on the edge that is the sweep path, near the appropriate vertex.
•
For shape features, the shape must not be constrained to any entities. The definition can include only variations in Pressure, Bend, and Stretch (on the Controls tab of the Shape Feature dialog box).
Library Features Library Features A library feature can contain one or more features. Most feature types are supported, some with certain limitations. You can edit a library feature once it has been inserted into a part. After a library feature is added to a part, there is no associativity between the target part and the library feature part. If you edit a library feature part, the change is not propagated to parts that contain the library feature. Usually, library features consist of features added to a base feature, but not the base feature itself. Because you cannot have two base features in a single part, you cannot insert a library feature that includes a base feature into a part that already has a base feature. However, you can create a library feature that includes the base feature and insert it in an empty part. NOTE: A base feature is either the first solid feature or a solid feature not attached to another feature. You can only add a library feature to a part, or while editing a part in the context of an assembly. You cannot add a library feature to an assembly itself.
14-2
This section describes: •
Creating a Library Feature
•
Adding a Library Feature to a Part
•
Editing a Library Feature
•
Adding Color to a Library Feature
•
Dissolving a Library Feature
Creating a Library Feature To create a library feature, you first create a base feature, then create the features that you want included in the library feature on the base. Library features have the .sldlfp extension. NOTES: •
A base feature is either the first solid feature or a solid feature not attached to another feature.
•
You cannot create a library feature part (*.sldlfp file) from a multibody part document.
To create a library feature:
1.
Open a new part, sketch a profile, and create a base feature.
2.
Create the features you want to have in the library feature. Dimension the features to the base if you want to use the dimensions to locate the library feature when you place it on the target part.
3.
In the FeatureManager design tree, select the features you want to save as the library feature. This library feature has three features: a boss, a hole, and a fillet.
To select more than one feature, hold down the Ctrl key while you select. To select several features in a row, click the first feature, hold down the Shift key, then click the last feature.
Do not select the Base feature unless you plan to insert the library feature into an empty part. 4.
Base
Click File, Save As. The Save As dialog box appears.
5.
From the Save as type list, select Lib Feat Part (*.sldlfp). Enter a name and click Save. The part icon beside the part name in the FeatureManager design tree changes to the library feature icon and each feature that is included is marked with a letter L.
,
NOTE: To create a library feature from an existing part, open the part, select those features that you want to use in your library feature, and save them as a library feature part (*.sldlfp). You can create a library feature part that excludes some of the features of the source part, or one that contains all the features in the source part (with the exception of the base feature). It is important to note that excluding some features may cause rebuild errors in the library feature part because of unresolved dependencies.
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Chapter 14 Library Features and the Feature Palette Window
Adding a Library Feature to a Part There are two ways to add a library feature to a part: •
Place the library feature in the Feature Palette (available for most, but not all types of features), then drag and drop the feature into the part. See Feature Palette Window.
•
Use Insert, Features, Library Feature (for those types of features that are not supported in the Feature Palette).
To add a library feature to a part:
1.
With the target part open, click Insert, Features, Library Feature. The Open dialog box appears.
2.
Browse to the directory where the library feature is located, and select the library feature file (.sldlfp).
3.
Click Open. Two windows and a dialog box appear, and tile automatically: •
the library feature window
•
the target part window
•
the Insert Library Feature dialog box
In the Insert Library Feature dialog, there is at least one Mandatory reference, and there may be Optional references also.
4.
•
A Mandatory reference is preceded by an exclamation point ;
•
An Optional reference is preceded by a question mark references.
. Dimensional references are optional
To locate the library feature on the target part, click a Reference entity (Plane, Edge, Face, or Vertex) that is listed as Mandatory on the target part. The ex,clamation point in the Reference list changes to a check mark
5.
.
Select any optional references. As you click each item in the Reference list, notice that the corresponding entity is highlighted in the library feature window. Select the corresponding entity in the target part window. To deselect an entity, either double-click the check mark or click Deselect All.
6.
Click OK.
The library feature is added to the target part.
14-4
Insert Library Feature Wizard 1.
Select the entity on the target part that corresponds to the Reference item listed as Mandatory.
2.
If you are placing a library feature that includes a Base feature in an empty part, select the plane where you want to place the library feature. (You cannot add a library feature that includes a Base feature to a part that already has a Base feature.) NOTE: A base feature is either the first solid feature or a solid feature not attached to another feature.
3.
As you click each item in the Reference list, the entity is highlighted in the library feature window. Select the corresponding entity in the target part window.
4.
Select entities for Reference items listed as Optional, if desired. If you select the wrong entity, double-click the item in the Reference list to deselect it, or click Deselect All.
5.
When you are satisfied, click OK.
Editing a Library Feature You can change which features are included as part of a library feature in the library feature part document (.sldlfp): •
To add another feature, right-click the feature to add, and select Add To Library.
•
To remove a feature, right-click the feature, and select Remove From Library.
•
You can edit an existing library feature and save it with a new name (and .sldlfp extension) to create additional, similar library features.
After the library feature is inserted into a part, you can edit a library feature in the following ways: •
Use the same techniques that you would use to edit any SolidWorks feature, such as Edit Sketch or Edit Feature.
•
Move the library feature to a different location on the target part, by modifying the locating dimensions. Double-click the library feature icon in the FeatureManager design tree to display the dimensions.
Change Dimensions After inserting a feature from the Feature Palette, you can modify its dimensions. To modify the inserted feature's dimensions:
1.
In the Change Dimensions dialog box, click a Name or Value. The dimension appears on the model.
2.
Double-click the Value, and enter a new value.
3.
Click Apply to see the changes.
4.
When you are satisfied with the dimension values, click Finish.
Adding Color You can apply color to a library feature either in its own document or in a target part. To change the color of library features:
1.
Click Tools, Options, and on the Document Properties tab, select Colors.
2.
In the Model\Features colors box, select Library Feature.
3.
Click the Edit button and select a color from the color palette (or create a custom color), and click OK.
4.
Click OK. •
In a library feature document (.sldlfp), all the features that are included in the library feature use the new color.
•
In a target part, all inserted library features use the new color.
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Chapter 14 Library Features and the Feature Palette Window
Dissolving a Library Feature After the library feature is inserted into a part, you can dissolve (break down) a library feature into the individual features it contains. To break down a library feature into the features it contains:
In the FeatureManager design tree, right-click the library feature icon, and select Dissolve Library Feature from the shortcut menu. The library feature icon is removed, and each of the features it contains is listed individually in the FeatureManager design tree.
Feature Palette Window Feature Palette Window The Feature Palette window gives you quick access to the features and parts you use most often. It helps you organize features and parts in a way that suits your specific needs. This section describes: •
Displaying the Feature Palette Window
•
Organizing Feature Palette Items
•
Creating a Palette Item
•
Thumbnail Graphics
•
Working with Palette Items and Folders
•
Palette Parts as Derived Parts
•
Adding Palette Items to Documents: Parts and Assemblies
•
Applying a Palette Forming Tool to a Sheet Metal Part
Feature Palette Window Overview The Feature Palette window gives you quick access to the parts, assemblies, and library features you use most often. The Feature Palette window has several default folders. Each folder contains a group of palette items, displayed as thumbnail graphics. Palette items can include parts (.sldprt files), assemblies (.sldasm files), sheet metal forming tools (.sldprt files), and library features (.sldlfp files). To display the Feature Palette window:
Click Tools, Feature Palette. The palette stays open, and on top of the SolidWorks window, while you work. If the palette is displayed when you exit the SolidWorks software, it will be displayed when you start the SolidWorks software the next time. You can display the folder icons and the thumbnail graphics of palette items in two sizes. To change the size, right-click a blank area of the Feature Palette window, and select View, Large Icons or Small Icons. To dismiss the palette, click the X in the upper right corner of the Feature Palette window, or click Tools, Feature Palette again to remove the check mark from the item in the menu. To navigate in the Feature Palette window:
When you display the Feature Palette window, it opens at the top level, or Palette Home. To specify the folders that appear at Palette Home, see Organizing Feature Palette Items and File Locations. To open a folder, double-click it. The window controls include a dropdown history list of the last folders opened (up to 16), and these buttons (similar to the controls in Internet Explorer):
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Go Backward
Back up through the list of folders
Go Forward
Go ahead through the list of folders
Reload
Refresh the palette window after changing the contents
Home
Return to Palette Home
Displaying the Feature Palette Window The Feature Palette window has several default folders. Each folder represents a directory; each palette item contained in that directory is displayed as a thumbnail graphic. Palette items can include parts, assemblies, sheet metal forming tools (.sldprt files), and library features (.sldlfp files). •
To display the Feature Palette window, click Tools, Feature Palette. The Feature Palette window stays open, and on top of the SolidWorks window, while you work. If the Feature Palette window is displayed when you exit SolidWorks, it will be displayed when you start SolidWorks the next time. See Organizing Feature Palette Items and File Locations for information on how to specify the folders displayed in the Feature Palette window.
•
To dismiss the Feature Palette window, either click in the upper-right corner of the window, or click Tools, Feature Palette again to remove the check mark from the item in the menu.
•
You can display the folder icons and the thumbnail graphics of palette items in two sizes. To change the size, right-click a blank area of the window, and select View, Large Icons or View, Small Icons.
Navigating in Feature Palette Window When you display the Feature Palette window, it opens at the top level, or Palette Home. To open a folder, doubleclick it. These toolbar controls are similar to the controls in Internet Explorer. •
Back
•
Forward
•
Reload
•
Home (to Palette Home)
•
The history list, with the names of the last folders opened (up to 16).
Organizing Feature Palette Items The Feature Palette window has several default folders. You can create and name new folders to suit your specific needs, and you can place items in each folder according to the way you want to organize the contents. The SolidWorks software includes some palette items to get you started. They are stored in these folders by default: •
install_directory\data\Palette Assemblies\folder_name
•
install_directory\data\Palette Features\folder_name
•
install_directory\data\Palette Parts\folder_name
•
install_directory\data\Palette Forming Tools\folder_name
If you chose a different path for the data directories when you installed SolidWorks, these folders are placed in the path you specified instead.
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Chapter 14 Library Features and the Feature Palette Window
Folders •
You add individual items to a folder by placing parts, assemblies, forming tools (.sldprt) or library feature parts (.sldlfp) in the appropriate folder.
•
A folder can contain individual palette items, and other folders. You can have as many folders, and as many levels of folders, as you want.
•
You can store palette items anywhere you want; the folders do not have to be located in the default path. You can have folders on different disk drives on your system, or on different computers on a network.
To specify which folders appear at the Palette Home level:
1.
Click Tools, Options, and on the System Options tab, select File Locations.
2.
From the Show folders for list, select the type of file for which you are defining a folder list: Palette parts, Palette assemblies, Palette features, or Palette forming tools. The first time you edit the Folders list, the default paths for the palette folders are already listed. These folder lists are always used, whether the Search file locations for external references check box under Tools, Options, System Options, External References is selected or not (this check box applies only to the Documents folder list). You can have more than one folder in the Palette Home for each type of item.
3.
•
To add a new path to the list, click the Add button. In the Browse for Folder dialog box, locate the path, and click OK.
•
To delete a path from the list, select the path in the Folders list, and click the Delete button.
•
To change the order of the list, select a path in the Folders list and use the Move Up or Move Down buttons to rearrange the list. Folders appear in the Palette Home in the order of the list.
Click OK. If you change the paths while the Feature Palette window is open, click Reload the paths.
to update
The icons in the Feature Palette window identify the type of item that the folder contains (with large icons only).
Creating a Palette Item There are several ways to add items to the Feature Palette window. Move or copy existing parts, assemblies, forming tools (.sldprt) or library feature parts (.sldlfp) into the appropriate folder, using Windows Explorer utilities. •
Drag the item from an open part or assembly document.
•
Drag a document from Windows Explorer.
•
Drag a hyperlink to a palette item from the Internet Explorer (version 4.0 or later).
To add a palette item from an open document:
1.
Create and save a new part, assembly, forming tool, or library feature part, or open an existing document (.sldprt or .sldlfp).
2.
Display the Feature Palette window, and navigate to the folder where you want to store the palette item.
3.
Drag the part from the graphics area, or the part icon from the top of the FeatureManager design tree of the active document, and drop it on the Feature Palette window. The Save As dialog box appears.
4.
Either accept the current name, or enter a new name, and click Save.
To add a palette item from Windows Explorer:
14-8
1.
Display the Feature Palette window, and navigate to the folder where you want to store the palette item.
2.
In Windows Explorer, navigate to the folder that contains the palette item.
3.
Drag the file from the Explorer window and drop it in the Feature Palette window.
To add a palette item from a hyperlink in Internet Explorer:
1.
Display the Feature Palette window, and navigate to the folder where you want to store the palette item.
2.
In Internet Explorer (version 4.0 or later), navigate to a location that contains hyperlinks to SolidWorks palette items. For example, on the SolidWorks web site, in the Gallery, Model Library section, navigate to the Solid Modeling Library page. You may also be able to obtain SolidWorks palette items from third-party vendors.
3.
Drag a hyperlink from the Internet Explorer window, and drop it in the Feature Palette window. The document is saved in the specified folder. NOTE:You can also just open a hyperlinked item, without adding it to the palette. To open the document, drag it to an empty area of the SolidWorks window. Then you can decide if you want to add the item to the palette, save it to a different folder, or close it without saving.
See also Forming Tools when using the Feature Palette window with sheet metal parts.
Thumbnail Graphics When you save a palette item, the thumbnail graphic reflects the view when the document is saved. Be sure to orient the part or assembly so that the thumbnail graphic looks the way you want it to look. To make it clear which features are included in a palette feature, consider changing the color in the library feature part. Thumbnail graphics use a palette of 16 colors; if the color you choose for the feature is not available, the software replaces it with a similar color in the thumbnail graphic. See Adding Color. NOTE: In the target part, palette features that consist of more than one feature use the color specified for Library Features under Tools, Options, on the Document Properties tab, select Colors. Palette features that consist of a single feature are automatically dissolved when you add them. Therefore they use the color specified for the individual feature type. Another way to emphasize the features is to select them, then click Zoom to Selection before you save the library feature part. That way, the thumbnail graphic provides a close-up view of the included features.
Working with Palette Items and Folders To copy a palette item:
Hold down the Ctrl key, then drag a palette item within the Feature Palette window. You can only copy an item this way in the same folder. The new item is named Copy of
You can rename the palette items and the folders, except the folders at the Palette Home level. Click-pauseclick the name in the Feature Palette window, and enter a new name. To edit a palette item:
1.
Right-click the item in the palette window, and select Edit Palette Item. – or – Drag the item from the Feature Palette window and drop it in an empty area of the SolidWorks window (not an empty area of a document window). The part (.sldprt) or library feature (.sldlfp) document is opened in a new window.
2.
Edit the document as needed, then Save. The palette updates automatically to reflect the changes. NOTE: The thumbnail graphic reflects the newly saved view. Be sure to orient the part or assembly so that the graphic looks the way you want it to look.
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Chapter 14 Library Features and the Feature Palette Window
To change the contents of a palette folder:
1.
In Windows Explorer, navigate to the directory you want to modify.
2.
Add, move, or delete the files as needed, using Windows file management commands.
3.
Click Reload
on the toolbar in the Feature Palette window to update the folders.
To delete a palette item:
Click the item in the Feature Palette window, and press Delete. The item is removed from the window, and the file is deleted from the corresponding folder. To delete a palette folder:
1.
Exit SolidWorks.
2.
Navigate to the directory to delete, move the contents to a new location, if necessary, then delete the directory.
Palette Parts as Derived Parts You can use the Feature Palette window to create a derived part, based on the selected palette part. 1.
With an empty part document open, click Tools, Feature Palette, then navigate to the folder that contains the desired part.
2.
Drag the part from the Feature Palette window and drop it into the part window.
3.
When you are asked if you want to create a derived part: •
Click Yes if you want to create a derived part (a part that has another part as its first feature). See Derived Parts for more information.
•
Click No if you want to edit the palette part itself. The palette part is opened in the current window.
Adding Palette Items to Documents Adding a Palette Feature to a Part Try using either Hidden Lines Removed or Hidden Lines Visible view mode, in order to see the preview and dimensions easily. To add a palette feature to a part:
1.
With a part open, click Tools, Feature Palette, and navigate to the folder that contains the feature.
2.
Drag the feature from the Feature Palette window, observing the preview as you drag. Drop the feature in the general area of the face where you want the feature to be placed. NOTE: You can also drag a hyperlink to a library feature part (.sldlfp) from Internet Explorer (4.0 or later) and drop it on the face of the part. If you want to save the hyperlinked palette feature for future use, be sure to also drag a copy into the palette, or into an empty area of the SolidWorks window, then save it. Otherwise, no local copy of the document is saved. Hyperlinked library feature parts have the same limitations and behaviors as library feature parts in the Feature Palette window. The Edit This Sketch dialog box appears, and remains open while you position the sketch.
3.
14-10
Click Zoom to Selection
to get a closer view of the feature.
4.
Click Modify Sketch on the Sketch toolbar, and move or rotate the sketch as needed. See Modify Sketch for more information. If the feature has locating dimensions, they are left dangling, and are displayed in brown.
5.
Re-attach the dangling dimensions. Select a dimension, then drag the red handle on the dimension line. The pointer has the shape until it is over a suitable entity for re-attachment. When you release the handle over an edge or vertex, the dimension re-attaches and the handle turns green. You can also add geometric relations to control the position of the sketch.
6.
Adjust the values of the locating dimensions. (Double-click the dimension, change the value, and press Enter.) You can also adjust the locating dimensions in the next step, or later, by editing the appropriate sketch.
7.
Click Next in the Edit This Sketch dialog box. The Change Dimensions dialog box appears. The Name and Value of each available dimension is displayed. If the dimensions are named in the part where you created the library feature, those names are used. Otherwise, the default dimension names D1 through Dn are used. Some dimensions of the feature may be unavailable, because they are specified as Internal Dimensions. See Dimension Access.
8. To display a feature dimension on the model, click either the Name or Value. To modify a dimension, double-click the Value, and enter a new value. Click Apply to see the changes.
9.
When you are satisfied with the dimension values, click Finish. If the palette item consists of more than one feature, a library feature icon appears in the FeatureManager design tree. If the palette item consists of a single feature, the item is automatically dissolved, and the appropriate icon for the feature type appears in the FeatureManager design tree. In either case, the name of the feature is the name of the item in the Feature Palette window.
Edit This Sketch 1.
Click Modify Sketch
2.
Re-attach any dangling dimensions (displayed in brown). Select a dimension, drag the red handle on the dimension line, and drop it on a suitable entity for re-attachment (edge or vertex).
3.
Adjust the values of the locating dimensions. You can either do this now (by double-clicking and editing the dimensions), or later.
on the Sketch toolbar, and move or rotate the sketch as needed.
NOTE: If the palette feature does not include dimensions that locate the feature on the face, you can use the
4.
Dimension tool Click Next.
SolidWorks 2004 Reference Guide
now to position the feature.
14-11
Chapter 14 Library Features and the Feature Palette Window
Edit Dimension Access For some types of features, such as sheet metal forming tools and library features, you may want to prevent other users from changing certain dimensions. You can also edit dimension access to reduce the clutter of unnecessary dimensions in the display. When you drag one of these features into a part document (from the Feature Palette window, or from Windows Explorer, or from a hyperlink in Internet Explorer), the dimensions are displayed, and they are available for editing. You can control the access to each dimension, to prevent other users from making unwanted changes when they use these features. To control dimension access:
1.
Right-click the part icon at the top of the FeatureManager design tree, and select Edit Dimension Access. In the Dimension Access dialog box, there are two lists: User dimensions (those that may be edited) and Internal dimensions (those that may not).
2.
Specify which dimensions are visible and available: •
To move a dimension from one list to the other, click the name, then click the left
or right
arrow button. As you click each name, the dimension is displayed in the model. • 3.
To move all the dimensions, use the double arrow button
.
Click Finish. When you insert an item that has restricted dimension access, only the User dimensions are visible and available for editing. The Internal dimensions are not displayed, and they are not available for editing. To make them visible and available again, repeat this procedure in the target part, after adding the library feature.
Internal Dimensions For some types of parts, such as sheet metal forming tools and library feature parts, you may want to prevent other users from changing certain dimensions. When you drag one of these items into a part document (from the Feature Palette window, or from Windows Explorer, or from a hyperlink in Internet Explorer), the dimensions are displayed, and available for editing. To prevent other users from making unwanted changes when they use these items, you can control the access to each dimension. Adding a Palette Part to an Assembly To add a palette part to an assembly:
1.
With the assembly open, click Tools, Feature Palette, and navigate to the folder that contains the desired part.
2.
Drag the part from the Feature Palette window and drop it into the assembly window.
3.
If the part has multiple configurations, the Select a configuration dialog box appears, with a list of the configurations in the part. Select the configuration you want, and click OK.
If you defined a mate reference in the part, you can create some types of mates automatically when you drop the part in the assembly. For more information, see Mate Reference. If you are editing a piping sub-assembly, you can drag fittings (T-junctions, flanges, and so on) from the Feature Palette window and drop them on vertices in the sketch. For more information, see SolidWorks Piping Help Topics.
14-12
15 Sheet Metal
Sheet Metal Sheet metal parts are generally used as enclosures for components or to provide support to other components. You can design a sheet metal part on its own without any references to the parts it will enclose, or you can design the part in the context of an assembly that contains the enclosed components. This chapter introduces the SolidWorks sheet metal functionality and describes: •
Designing Sheet Metal with Sheet Metal-Specific Features
•
Designing a Solid Body, Then Converting it to a Sheet Metal Part
•
Comparing Sheet Metal Design Methods
•
Other Sheet Metal Topics: o
Adding and Editing Bends
o
Bend Allowance and Bend Deduction
o
Flattening Bends in a Sheet Metal Part
o
Adding and Editing Auto Reliefs
o
Inserting Rips
o
Making Lofted Bends
o
Creating Sketched Bends
o
Adding Hems
o
Creating Jogs
o
Breaking Corners
o
Mirroring a Sheet Metal Part
o
Creating Flat Pattern Configurations
o
Using Forming Tools with Sheet Metal
o
Creating Drawings of Sheet Metal Parts
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Chapter 15 Sheet Metal
Designing Sheet Metal with Sheet Metal Features Base Flange A base flange is the first feature in a new sheet metal part. When you add a base flange feature to a SolidWorks part, the part is marked as a sheet metal part. Bends are added wherever appropriate, and sheet metal specific features are added to the FeatureManager design tree. Some additional items to note about a base flange feature: •
The Base-Flange feature is created from a sketch. The sketch can be a single open, a single closed, or multiple-enclosed profiles.
•
There can be only one base flange feature in a SolidWorks part.
•
The thickness and bend radius of the Base-Flange feature become the default values for the other sheet metal features.
To create a Base-Flange feature:
1.
Create a sketch that meets the requirements above. Alternatively, you can select the Base-Flange feature before you create a sketch (but after you select a plane). When you select the Base-Flange feature, a sketch opens on the plane.
2.
Click Base-Flange/Tab
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Base Flange.
The controls on the Base Flange PropertyManager update according to your sketch. For example, the Direction 1 and Direction 2 boxes do not appear for a sketch with a single closed profile. 3.
If necessary, under Direction 1 and Direction 2, set the parameters for the End Condition and Depth
4.
Under Sheet Metal Parameters:
5.
6.
•
Set a value for Thickness
•
Select Reverse direction to thicken the sketch in the opposite direction.
•
Set a value for Bend Radius
.
to specify the sheet metal thickness.
.
Under Bend Allowance, select a bend allowance type. •
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
•
If you selected Bend Table, select a bend table from the list, or click Browse to browse to a bend table file.
Under Auto Relief, select a relief type. If you selected Rectangular or Obround: •
Select Use relief ratio and set a value for Ratio. - or -
• 7.
Clear Use relief ratio and set a value for Relief Width
Click OK
and Relief Depth
.
.
Examining the FeatureManager Design Tree A Base Flange feature creates three new features in the FeatureManager design tree: Sheet-Metal1. Contains the default bend parameters. To edit the default bend radius, bend allowance, bend deduction, or default relief type, right-click Sheet-Metal1 and select Edit Feature. Base-Flange1. Represents the first solid feature of the sheet metal part. Flat-Pattern1. Flattens the sheet metal part. It is suppressed by default as the part is in its bent state. Unsuppress the feature to flatten the sheet metal part.
15-2
When Flat-Pattern1 is: •
suppressed, all new features are inserted above it in the FeatureManager design tree
•
unsuppressed, all new features are inserted below in the FeatureManager design tree and are not shown in the folded part
Edge Flange The Edge Flange feature adds a flange to your sheet metal part at an edge that you select. Here are some items to note about an edge flange feature: •
The selected edge must be linear.
•
The thickness is automatically linked to the thickness of the sheet metal part.
•
One sketch line of the profile must lie on the selected edge.
To create an edge flange feature:
1.
In an open sheet metal part, click Edge Flange Metal, Edge Flange.
on the Sheet Metal toolbar, or click Insert, Sheet
The Edge-Flange PropertyManager appears. 2.
In the graphics area, select the edge where you want to place the feature. The selected edge appears in the Edge
3.
box.
In the Edge-Flange PropertyManager, do the following: •
Under Flange Parameters, click Edit Flange Profile to edit the sketch of the profile.
•
To use something other than the default bend radius, clear the Use default radius check box and set Bend Radius
to the desired bend radius.
4.
Under Angle, set the Flange Angle
.
5.
Under Flange Length, set the Length End Condition and its corresponding parameters. For example, if you select Blind, you must set the Length Virtual Sharp
and Outer Virtual Sharp
or Inner
to determine where the length is measured from. You can also click Reverse Direction
to change the direction of the edge flange. 6.
Under Flange Position, do the following: •
Set the bend position to Material Inside
•
Bend from Virtual Sharp . See Bend Positions for a description of each of these selections. To remove extra material in neighboring bends, select the Trim side bends check box.
•
, Material Outside
, Bend Outside
, or
To offset the flange from the sheet metal body, select the Offset check box. Then, set the Offset End Condition and its corresponding parameters.
7.
To use something other than the default bend allowance, select the Custom Bend Allowance check box, and set a bend allowance type and value.
8.
If you want relief cuts added automatically, select the Custom Relief Type check box, then select the type of relief cut. If you select Rectangular or Obround, then you must specify a Relief Ratio.
9.
Click OK
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.
15-3
Chapter 15 Sheet Metal
Profile Sketch You can edit the profile sketch of an edge flange. The profile sketch has the following requirements: •
One sketch line of the profile must lie on the edge you selected when creating the Edge Flange. This sketched line does not have to be the same length as the selected edge.
•
The profile can be a single open, a single closed, or multiple-enclosed profiles.
To edit the profile sketch:
1.
When editing an edge flange feature, click Edit Flange Profile under Flange Parameters. The Profile Sketch dialog box appears.
2.
In the graphics area, drag one of the sketch entities of the Edge Flange preview to modify the sketch. Additionally, you can use the tools on the Sketch Tools toolbar to modify the sketch. For example, you can add a circle to the sketch to place a hole in the Edge Flange.
3.
Click Back to accept the changes to the profile sketch and to continue editing the Edge Flange feature. - or Click Finish to accept the changes to the profile sketch and to create the Edge Flange feature. - or Click Cancel to cancel the change to the profile sketch and close the Edge Flange PropertyManager.
Miter Flange A miter flange feature adds a series of flanges to one or more edges of a sheet metal part. Some items to note about a miter flange feature: •
The sketch for a miter flange must adhere to the following requirements: o
The sketch can contain lines or arcs. If you use an arc to create a miter flange, the arc cannot be tangent to the thickness edge. The arc can be tangent to the long edges, or by putting a small sketch line between the arc and the thickness edge. Click here for an example of creating a sketch for a miter flange with arcs.
o
o
The Miter Flange profile can contain more than one continuous line. For example, it can be an L-shaped profile. The sketch plane must be normal to the first edge where the Miter Flange is created. Click here for instructions to create a sketch for a miter flange.
•
The thickness is automatically linked to the thickness of the sheet metal part.
•
You can create a miter flange feature on a series of tangent or non-tangent edges. Click here for an illustration of each.
•
Instead of creating a miter flange across the entire edge of a sheet metal part, you can specify an offset of the flange.
To create a miter flange feature:
1.
15-4
Create a sketch that meets the requirements above. Alternatively, you can select the Miter Flange feature before you create a sketch (but after you select a plane). When you select the Miter Flange feature, a sketch opens on the plane.
2.
Click Miter Flange on the Sheet Metal toolbar, or click Insert, Sheet Metal, Miter Flange. The first edge for the Miter Flange feature is selected and a preview of the Miter Flange appears in the graphics area.
3.
In the graphics area, select the edges to miter for Along Edges
.
To select all of the edges tangent to the selected edge, click Propagate midpoint of the selected edge. 4.
Under Miter Parameters: •
To use something other than the default bend radius, clear Use default radius and set a value for Bend Radius
5.
that appears at the
.
•
Set the Flange position to Material Inside , Material Outside See Bend Positions for a description of each of these selections.
, or Bend Outside
•
Select Trim side bends to remove extra material in neighboring bends.
•
Set Gap distance
.
to use something other than the default gap.
If necessary, specify the offset distances for a partial miter flange: •
Under Start/End Offset set a value for Start Offset Distance
and End Offset Distance
•
. (If you want the miter flange to span the entire edge of the model, set these values to zero.) Select Custom Relief Type, and select a Relief type of: Rectangular, Tear, or Obround. If you selected Rectangular or Obround: Select Use relief ratio and set a value for Ratio.
o
- or Clear Use relief ratio and set a value for Relief Width
o
•
6.
and Relief Depth
.
To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value.
Click OK
.
The miter flange is added to the sheet metal part.
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Chapter 15 Sheet Metal
Miter Flange - Arc Sketches
Valid sketch: Arc is tangent to long edge
Valid sketch: Line is coincident to thickness edge, and arc is tangent to line
Invalid sketch: Arc is tangent to thickness edge
Miter Flange - Sketch Creation The sketch for a Miter Flange must adhere to the following: •
The sketch can contain only lines or arcs.
•
The Miter Flange profile can contain more than one continuous line. For example, it can be an L-shaped profile.
•
The sketch plane must be normal to the first edge where the Miter Flange is created.
To create a sketch for a Miter Flange feature:
1.
Select the first edge in the series of edges where you want to create a Miter Flange feature. Make sure to click the edge near the endpoint at the start of the series of edges.
2.
Click Line on the Sketch toolbar, or click Tools, Sketch Entities, Line. A sketch opens normal to the selected edge. The origin of the sketch is at the endpoint of the edge that is closest to where you clicked in step 1.
3.
Sketch the profile of the Miter Flange. Make sure that one line starts at the endpoint of the edge where the sketch origin is located. Back to Miter Flange.
15-6
Miter Flange - Edge Selection Before Miter Flange
After Miter Flange
Tangent Edges
Non-tangent Edges
Bend Positions In a Miter Flange, Edge Flange, Sketched Bend, Hem, or Jog, you have to select a bend position. The following table explains your choices. Bend Position
Preview
Material Inside . The top of the shaded preview of the flange coincides with the top of the fixed sheet metal entity.
Material Outside . The bottom of the shaded preview of the flange coincides with the top of the fixed sheet metal entity.
Bend Outside . The bottom of the shaded preview of the flange is offset by the bend radius.
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Chapter 15 Sheet Metal
Bend from Virtual Sharp . This preserves the dimension to the original edge and will vary the bend material condition to automatically match with the flange's end condition.
No preview available. Bend Centerline . The bend line is placed such that it equally splits the bend region in the flattened part. This is available only for Sketched-Bend features.
Trim Side Bends To remove extra material in neighboring bends, select the Trim side bends check box. Extra material appears when one of the bends of a Miter Flange touches an existing bend. The cut that trims the neighboring bends is automatically sized, and cannot be edited. Here is an example, using an Edge Flange feature: This is the preview of an Edge Flange feature. Notice the bend region of the blue preview touches the bend of the L-shaped base flange.
This is the end result without the Trim side bends check box.
This is the end result with the Trim side bends check box.
15-8
Sheet Metal Tab A Tab feature adds a tab to the sheet metal part. The depth of a Tab feature is automatically set to the thickness of the sheet metal part. The direction of the depth automatically coincides with the sheet metal part to prevent a disjoint body. Here are some additional items to note about a Tab: •
The sketch can be a single closed, multiple closed, or multiple-enclosed profile. The illustration shows a single tab feature that adds two tabs to the sheet metal part. The sketch must be on a plane or planar face that is perpendicular to the direction of thickness of the sheet metal part. You can edit the sketch, but you cannot edit the definition. This is because the depth, direction, and other parameters are set to match the parameters of the sheet metal part.
•
•
To create a Tab feature in a sheet metal part:
1.
Create a sketch on a plane or planar face that meets the above requirements.
2.
Click Base-Flange/Tab on the Sheet Metal toolbar, or click Insert, Sheet Metal, Tab. The tab is added to the sheet metal part. The tab's depth and direction are automatically set to match the parameters of the Base Flange feature.
Sketched Bend You can add bend lines to the sheet metal part while the part is in its folded state with a sketched bend feature. This allows you to dimension the bend line to other folded-up geometry. Some items to note about a sketched bend feature: •
Only lines are allowed in the sketch. You can add more than one line per sketch.
•
The bend line does not have to be the exact length of the faces you are bending. A Sketched Bend feature is commonly used with a Tab feature to bend the tab.
SolidWorks 2004 Reference Guide
15-9
Chapter 15 Sheet Metal
To create a Sketched Bend feature:
1.
Sketch a line on a planar face of the sheet metal part. Alternatively, you can select the Sketched Bend feature before you create a sketch (but after you select a plane). When you select the Sketched Bend feature, a sketch opens on the plane.
2.
Click Sketched Bend on the Sheet Metal toolbar, or click Insert, Sheet Metal, Sketched Bend.
3.
In the graphics area, select a face that does not move as a result of the bend for Fixed Face
4.
.
Click a Bend position of Bend Centerline Inside
, Material Outside
, Material
, or Bend Outside
5.
Set a value for Bend Angle, and click Reverse Direction
6.
if necessary. To use something other than the default bend radius, clear
7.
8.
.
Use default radius and set Bend Radius . To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value. Click OK
.
Hem The Hem tool adds a hem to your sheet metal part at a selected edge. Here are some additional items to note about the Hem tool: •
The selected edge must be linear.
•
Mitered corners are automatically added to intersecting hems.
•
If you select multiple edges to add a hem, the edges must lie on the same face.
To create a hem feature:
1.
In an open sheet metal part, click Hem
2.
In the graphics area, select the edges where you want to add a hem. The selected edges appear in Edges
3.
15-10
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Hem.
.
In the PropertyManager, under Edges: •
Select Material Inside
•
Click Reverse Direction
or Bend Outside
to specify where to add the material.
to create the hem on the opposite side of the part.
4.
Under Type and Size: a.
b.
Click a hem type:
o
Closed
o
Open
o
Tear Drop
o
Rolled
o
Length
o
Gap Distance
o
Angle
o
Radius
Set: (closed and open hems only) (open hem only)
(tear drop and rolled hems only) (tear drop and rolled hems only)
5.
Under Miter Gap, set Rip Gap if you have intersecting hems. Mitered corners are automatically added to intersecting hems, and you can set the gap between these hems.
6.
To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value.
7.
Click OK
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Chapter 15 Sheet Metal
Closed Corner You can create a Closed Corner feature to extend one face of a Butt rip so it overlaps the other face of the Butt rip. This is shown as follows:
Corner with Butt rip
Corner with Closed Corner feature
Here are some additional items to note about a Closed Corner feature: •
You can close more than one corner at a time. Select the faces for all of the rips that you want to close.
•
You can select only planar faces to close. The planar faces must be perpendicular to each other.
•
A closed corner cannot be applied in some cases where flange angles are not 90°.
To close a corner:
1.
Create a sheet metal part with a Base-Flange and a Miter-Flange, so that one corner looks like the illustration at right.
2.
Click Closed Corner on the Sheet Metal toolbar, or click Insert, Sheet Metal, Closed Corner. The Closed Corner PropertyManager appears.
3.
Select one of the planar faces on the corner, like the one that is highlighted, as the Faces to Extend
4.
Select a Corner type of Butt or Underlap
5.
Click OK
, Overlap
. .
The face is extended to close the corner.
15-12
. ,
Designing a Solid Body, then Converting it to Sheet Metal Bend Types Three types of bends are available when converting a solid body to a sheet metal part. These bends are: sharp bends, round bends, and flat bends. Sharp Bends A sharp bend is created by adding bends to a model that has sharp corners and a uniform thickness.
Round Bends A round bend can be created by adding bends to a model that has filleted or rounded corners and a uniform thickness. Round bends can also be created from cylindrical and conical faces.
Flat Bends A flat bend is created from a bend line sketched in the flattened sheet metal part. These lines are sketched in Flat-Sketch1 under Process-Bends1 in the FeatureManager design tree. The lines across the model in the illustration below on the left are sketched bend lines.
Creating a Sheet Metal Part Using Sharp Bends When bending sheet metal, you may want to create sharp bends instead of round bends. To create a sheet metal part with sharp bends:
1.
Create a part by sketching the part profile, then extruding a thin-feature part.
2.
Click Insert Bends
or Insert, Sheet Metal, Bends.
The Bends PropertyManager appears.
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15-13
Chapter 15 Sheet Metal
3.
Under Bend Parameters: •
Select the fixed face on the model. The fixed face remains in place when the part is flattened. The name of the face is displayed in the Fixed Face or Edge
•
Type the Bend Radius
box.
.
4.
Under Bend Allowance, select from the following options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
5.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
6.
If you want relief cuts added automatically, select the Auto Relief check box, then choose the type of relief cut. If you choose Rectangular or Obround, then you must specify a Relief Ratio. NOTE: The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
7.
Click OK
.
A bent sheet metal part is created whose dimensions in the flattened state reflect the specified bend allowance and radius values.
Creating a Sheet Metal Part Using Round Bends When bending sheet metal, you can create round bends instead of sharp bends. To create a sheet metal part with round bends:
1.
Create a thin feature part. In the Extrude PropertyManager, under Thin Feature: a.
Select Auto-fillet corners.
b.
Set a value for Bend Radius
to determine the inner bend radius.
2.
Click OK
.
3.
Click Insert Bends
4.
In the PropertyManager, under Bend Parameters, set the following:
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Bends.
a.
Fixed Face or Edge . In the graphics area, click a fixed face on the model. The fixed face remains in place when the part is flattened.
b.
Bend Radius . Set the value to zero, because the radius is propagated from the Bend Radius under Thin Feature.
5.
Under Bend Allowance, select from: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
6.
If you selected K-Factor, Bend Allowance, or Bend Deduction, set a value.
7.
If you want relief cuts added automatically, select Auto Relief, then choose the type of relief cut. If you choose Rectangular or Obround, set a Relief Ratio. The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
8.
Click OK
.
A bent sheet metal part is created whose dimensions in the flattened state reflect the specified bend allowance and radius values.
15-14
Creating Sheet Metal Parts with Conical Faces Parts with conical faces can also be made of sheet metal. To create a sheet metal part with conical faces:
1.
2.
Create a thin feature part with one or more conical faces: •
Any adjacent planar and conical faces must be tangent.
•
At least one end face of any conical face must have at least one linear edge.
Click Insert Bends
or Insert, Sheet Metal, Bends.
The Bends PropertyManager appears. 3.
Under Bend Parameters: •
Select a linear edge on an end face of a conical face as the fixed edge. - or Select a planar face tangent to the conical face as the fixed face. The fixed edge remains in place when the part is flattened. The name of the edge is displayed in the
• 4.
Fixed Face or Edge
box.
Set the Bend Radius
.
Under Bend Allowance, select from the following bend allowance options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction. NOTE: If creating a sheet metal part with one or more conical faces, you must select K-Factor as the type of bend allowance.
5.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
6.
If you want relief cuts added automatically, select the Auto Relief check box, then choose the type of relief cut. If you choose Rectangular or Obround, then you must specify a Relief Ratio. NOTE: The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
7.
Click OK
.
NOTE: Only parts with exact analytic conical faces can be unfolded. Oblong or non-right angle cones are not supported. As a test, try to insert an axis on the conical face. If you can insert an axis, the model is an exact cone. If you cannot insert an axis, then the model is not an exact cone and cannot be unfolded. However, sheet metal parts created with the Lofted Bends feature avoid this limitation and unfold appropriately.
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Chapter 15 Sheet Metal
Adding Walls to a Sheet Metal Part You cannot add walls to cylindrical or conical faces on sheet metal parts. To add a wall to a sheet metal part:
1.
Open a sketch on the face of a sheet metal part where the new wall will be attached.
2.
Select a linear edge of a planar face on the model to attach the wall to, and click Convert Entities the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities.
3.
Drag the vertices near existing bends a small distance away from the bends to allow for the bend radius.
4.
Click Extruded Boss/Base
5.
In the PropertyManager, under Direction 1:
on the Features toolbar, or click Insert, Boss/Base, Extrude.
a.
Select Blind in End Condition.
b.
Set a value for Depth
.
6.
Under Thin Feature, set Thickness
7.
Click OK
to the same value as the base part.
.
If a message appears warning of a disjoint body, click Reverse Direction click OK
15-16
on
again.
under Thin Feature, then
Sheet Metal Features When you click Insert Bends part.
or Insert, Sheet Metal, Bends, two distinct stages are applied to the sheet metal
•
The part is flattened and a bend allowance is added. The developed length is calculated, based on the bend radius and bend allowance.
•
The flattened part is restored to the folded state to create the bent version of the part.
Three features appear in the FeatureManager design tree that are specific to sheet metal operations. These three features represent a process plan for the sheet metal part: Sheet-Metal contains the definition of the sheet metal part. This feature stores the default bend parameter information (thickness, bend radius, bend allowance, auto relief ratio, and fixed entity) for the entire part. Flatten-Bends represents the flattened part. This feature contains information related to the conversion of sharp and filleted corners into bends. Each bend generated from the model is listed as a separate feature under Flatten-Bends. Bends generated from filleted corners, cylindrical faces, and conical faces are listed as RoundBends; bends generated from sharp corners are listed as SharpBends. The Sharp-Sketch listed under Flatten-Bends is the sketch that contains the bend lines of all sharp and round bends generated by the system. This sketch cannot be edited but can be hidden or shown. Process-Bends represents the transformation of the flattened part into the finished, formed part. Bends created from bend lines specified in the flattened part are listed under this feature. Flat-Sketch, listed under Process-Bends, is a placeholder for these bend lines. This sketch can be edited, hidden, or shown. Features listed after the Process-Bends icon in the FeatureManager design tree do not appear in the flattened view of the part.
Importing a Sheet Metal Part to SolidWorks If you have a sheet metal part with bends from another CAD system, you can import these parts, then convert them to SolidWorks sheet metal. The imported parts must be of uniform thickness to fold and unfold properly. To convert an imported part into a SolidWorks sheet metal part:
1.
Import a document into SolidWorks. See Importing Documents for more information.
2.
Click Insert Bends
3.
In the graphics area, select a face for Fixed Face or Edge
4.
Click OK
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Bends. .
.
The part converts to a SolidWorks sheet metal part. The FeatureManager design tree contains Sheet-Metal1 , Flatten-Bends1 , and Process-Bends1 features. The part can now be flattened and bent as a sheet metal part by toggling the suppression state of the Process-Bends feature.
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Chapter 15 Sheet Metal
Comparing Sheet Metal Design Methods Comparing Sheet Metal Design Methods You can better understand the features available in SolidWorks by comparing methods of creating sheet metal parts. There are two ways to create a sheet metal part: •
Build a part, then convert it to sheet metal.
•
Create the part as a sheet metal part using sheet metal-specific features. This eliminates extra steps because you create a part as sheet metal from the initial design stage.
Design a Sheet Metal Part from a Solid When you create a sheet metal part, you generally design the part in the folded state. This allows you to capture the design intent and the dimensions of the finished part. To create a sheet metal part of uniform thickness:
1.
Open a new part, and sketch a rectangle.
2.
Create a Base-Flange by clicking Base-Flange/Tab or Insert, Sheet Metal, Base Flange. The sheet metal features appear in the FeatureManager design tree.
3.
Now that the base for your part is created, add walls that bend from the base with a miter flange.
4.
or If you want to make a cut across a bend, click Unfold Insert, Sheet Metal, Unfold. This flattens the individual bends.
5.
Sketch a closed profile across the flattened bend, and Extrude the cut Through All.
6.
To restore the part to the bent state, click Fold Sheet Metal, Fold.
or Insert,
When you create a part initially out of sheet metal you use two features: Base-Flange and Miter Flange. However, if you build a solid, then convert it to sheet metal, you need more features: Base Extrude, Shell, Rip, and Insert Bends. It is much faster to create a part as sheet metal instead of creating a part, then converting it to sheet metal.
15-18
Design a Part from a Solid, Then Convert it to Sheet Metal It is possible to create a solid part, then convert it to sheet metal to add the bends and sheet metal features. To create a part of uniform thickness and convert it to sheet metal:
1.
Create a block with the Base-Extrude tool. Make the block 50mm on all sides.
2.
Shell the block to 1mm so the part is of uniform thickness. In Faces to Remove, select the faces as shown.
3.
To bend the part, rip the block between the edges of the tabs or Insert, Sheet Metal, Rip. Select the by clicking Rip edge to rip as shown.
4.
Convert the part to sheet metal by clicking Insert Bends or Insert, Sheet Metal, Bends.
5.
If you want to make a cut across a bend, drag the Rollback Bar before the Process-Bends feature in the FeatureManager design tree.
6.
Sketch a closed profile across one of the bends.
7.
Extrude the cut Through All.
8.
To restore the part to the bent state, drag the rollback bar to the bottom of the FeatureManager design tree.
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Chapter 15 Sheet Metal
Design a Sheet Metal Part from the Flattened State You may want to design a sheet metal part from the flattened state. In this case, you create a sheet metal part, then insert bend lines on which to fold the part. To create a sheet metal part from the flattened state:
1.
Open a new part.
2.
Create a sketch as shown. You do not have to dimension the part.
3.
Create a Base-Flange by clicking Base-Flange/Tab or Insert, Sheet Metal, Base Flange. The sheet metal features appear in the FeatureManager design tree.
4.
To bend the sheet metal part, sketch lines on the part as shown.
5.
Bend the part by clicking Sketched Bend , or Insert, Sheet Metal, Sketched Bend. The part bends at the sketched lines.
To add features that appear in the folded model:
There is no need to drag the rollback bar in order to add any additional tabs, cuts, or other features to the folded model. Instead, you can add features directly in the folded state; the features appear above the FlatPattern feature in the FeatureManager design tree. Designing a part with sheet metal-specific features uses fewer features and editing tools, and eliminates the use of the rollback bar. The sheet metal-specific features make it easier and faster to create a sheet metal part than designing a part, then converting it to sheet metal. SolidWorks includes sheet metal-specific features so you can create a part as sheet metal without having to convert it to sheet metal.
Design a Part from the Flattened State, Then Convert it to Sheet Metal It is possible to create a flattened part, then convert it to sheet metal to add the bends and sheet metal features. To create a flattened part and convert it to sheet metal:
15-20
1.
Open a new part.
2.
Create a sketch as shown. You do not have to dimension the sketch.
3.
Create a Base-Extrude feature that forms the flattened part.
,
4.
Convert the part to sheet metal by clicking Insert Bends or Insert, Sheet Metal, Bends.
5.
Bend the sheet metal part by adding bend lines to the FlatSketch. Sketch three lines on the Flat-Sketch as shown.
6.
Close the sketch. The sheet metal part bends on the lines you sketched.
7.
Once the sheet metal part is in its folded state, you can still add features to the part by dragging the Rollback Bar before the Sheet-Metal features in the FeatureManager design tree. This insures that the new features appear in both the bent and flattened states.
Reasons to Build a Part, then Convert it to Sheet Metal There are a few instances where it is to your advantage to build a part, then convert it to sheet metal. •
Imported Solid Bodies. If you import a sheet metal file with bends from another CAD system, the bends are already in the model. Using Insert Bends SolidWorks sheet metal part.
•
is your best option for converting the imported file to a
Conical Bends. Conical bends are not supported by the sheet metal-specific features, such as Base Flange, Edge Flange, and so on. Therefore, you must build the part using extrusions, revolves, and so on, then convert it to add bends to a conical sheet metal part.
Combining the Different Sheet Metal Design Methods Parts that are originally created as sheet metal have different features than parts that are created, and then converted to sheet metal. However, you can add sheet metal-specific features to parts converted to sheet metal. As soon as you add a sheet metal-specific feature, (a Miter Flange
, an Edge Flange
, and so on), the following occurs:
•
Flat-Pattern1
is added to the FeatureManager design tree, and suppressed.
•
Bends for new sheet metal features are stored under each individual feature instead of under Flatten-Bends1 or Process-Bends1
. Additionally, all pre-existing and new bends are listed under the Flat-Pattern1
feature. To flatten the part, unsuppress Flat-Pattern1
SolidWorks 2004 Reference Guide
rather than suppressing Process-Bends1
.
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Chapter 15 Sheet Metal
Other Sheet Metal Topics Bend Allowance and Bend Deduction Bend Allowance and Bend Deduction Options You can specify the bend allowance or bend deduction values for your part. Select from the following options: Bend Table K-Factor Bend Allowance Bend Deduction Bend Allowance and Bend Deduction You can choose either bend allowance or bend deduction calculations to determine the flat length of sheet stock to give the desired dimension of the bent part. Bend Allowance Calculations The following equation is used to determine the total flat length when bend allowance values are used: Lt = A + B + BA where: •
Lt is the total flat length
• •
A and B are shown in the illustration BA is the bend allowance value
Bend Deduction Calculations The following equation is used to determine the total flat length when bend deduction values are used: Lt = A + B - BD where:
15-22
•
Lt is the total flat length
• •
A and B are shown in the illustration BD is the bend deduction value
K-Factor K-Factor is a ratio that represents the location of the neutral sheet with respect to the thickness of the sheet metal part. When you select K-Factor as the bend allowance, you can specify a K-Factor bend table. The SolidWorks application also comes with a K-Factor bend table in Microsoft Excel format. This is located in
where: BA = bend allowance R = inside bend radius K = K-Factor, which is t / T T = material thickness t = distance from inside face to neutral sheet A = bend angle in degrees (the angle through which the material is bent)
Bend Table Overview You can specify the bend allowance or bend deduction values for a sheet metal part in a bend table. The bend table also contains values for bend radius, bend angle, and part thickness. There are two types of bend tables that you can use: •
A text file with the .btl extension
•
An embedded Excel spreadsheet
A comparison of the two methods is shown as follows: Text File
Excel Spreadsheet
When you share your part with a colleague, you must remember to share your bend table as well.
When you share your part with a colleague, your bend table is automatically included because it is embedded.
Text tables can be edited in a variety of applications.
Excel spreadsheets can be edited in Microsoft Excel only.
NOTES: •
It is recommended that you use the Excel spreadsheet unless you have legacy bend tables from SolidWorks 2000 or earlier.
•
If you edit a bend table that has multiple bend thickness tables, the radii and angles must be the same. For example, if you insert a new bend radius value into a bend table with multiple bend thickness tables, you must insert the new value in all of the tables.
You can edit a bend table in a separate Excel window. Click Edit, Bend Table, Edit Table in New Window.
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Chapter 15 Sheet Metal
Bend Table - Text File A sample bend table for sheet metal operations is provided in
All bend table types (bend deduction, bend allowance, and k-factor).
•
All units of measure (meters, millimeters, centimeters, inches, and feet). Set the unit of measure in the Units row of the bend table.
A few items to note about bend tables in a text file: •
The sample bend table is provided only for informational purposes. The values in this table do not represent any actual bend allowance values.
•
If the thickness of the part or bend angle falls between values in the table, the software interpolates the values to calculate the bend allowance.
Bend Table - Excel Spreadsheet New bend tables that you create for SolidWorks are stored in an embedded Excel spreadsheet. You add bend table values into the cells of the spreadsheet, ensuring that the table is read properly by the SolidWorks software. Bend tables made in Microsoft Excel now support the following: •
All bend table types (bend deduction, bend allowance, and k-factor).
•
Multiple angles in a single bend table file.
To create a bend table:
1.
In a part, click Insert, Sheet Metal, Bend Table, New. If you get a message that says inserting a bend table may cause the developed length of the flat pattern to change, click Yes.
2.
In the dialog box: a.
Select an item in Units to set the unit of measurement.
b.
Select an item in Type to set the bend allowance or bend deduction.
c.
Type a path for File name, or click Browse to locate a path where you want to save the bend table.
d.
Click OK.
An embedded Excel window, containing the bend table spreadsheet, appears in the SolidWorks window. The bend table spreadsheet contains default radius, thickness, and angle values.
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3.
Type the bend allowance or bend deduction values to the spreadsheet, depending on your choice for Type in step 2.
4.
Click outside the table, but within the SolidWorks graphics area, to close the spreadsheet.
Bend Allowance Value You can specify an explicit bend allowance for any sheet metal bend by entering the value when you create the bend. NOTE: By definition, the bend allowance is the arc length of the bend as measured along the neutral axis of the material.
Bend Deduction Value You can specify an explicit bend deduction for any sheet metal bend by entering the value when you create the bend. NOTE: By definition, the bend deduction is the difference between the bend allowance and twice the outside setback.
Using Forming Tools with Sheet Metal Forming Tools Forming tools act as dies that bend, stretch, or otherwise form sheet metal. The SolidWorks software includes some sample forming tools to get you started. They are stored in
Base feature. Used as a temporary parent feature on which the boss feature is created.
•
Boss feature. Used as the actual forming tool.
After you create the boss feature, you delete the base feature.
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Chapter 15 Sheet Metal
To create a forming tool:
1.
Open a new part.
2.
Sketch a profile for the base feature on the horizontal plane centered on the origin. By default, the horizontal plane is the Top Plane. A typical profile for the base feature is a rectangle. Make sure the profile is big enough to accommodate the boss feature (forming tool). When you apply a forming tool to a sheet metal part, the origin lies where you drop the forming tool.
3.
Extrude the profile for the base feature upwards as shown.
4.
Create the boss feature below the horizontal plane. The boss feature can be an extrude or a revolve.
5.
Add additional features to the forming tool such as extrudes, revolves, fillets, chamfers, and so on. NOTES: The horizontal plane is the stopping surface of the forming tool. Therefore, the entire forming tool must lie below the stopping surface. The minimum radius of curvature of the forming tool must be greater than the thickness of the sheet metal part to which it is applied. To determine the minimum radius of curvature of the forming tool, click Tools, Check.
6.
Remove the base feature of the forming tool, so only the form feature remains: a.
Open a sketch on the bottom face of the base feature, and click Convert Entities
b.
.
Make an Extruded Cut and select Through All in End Condition.
7.
Indicate which faces of the forming tool create openings on sheet metal parts.
8.
Create a positioning sketch, if necessary.
9.
Save the part.
10. Add the tool to the Feature Palette window.
15-26
Creating Openings on Forming Tools Some types of form features, such as louvers and lances, create openings on sheet metal parts. To indicate which forming tool faces create openings, change the color of these faces to red. To create an opening on a forming tool:
1.
Right-click the face designed to create an opening, and select Properties under Face.
2.
In the dialog box, set Red to 255, Green to 0, and Blue to 0.
3.
Click OK.
4.
Click Rebuild
.
Create a Positioning Sketch for Forming Tool To edit the position of a form feature on a sheet metal part, you can create a positioning sketch on the top face of the forming tool. When you apply the forming tool to the sheet metal face, you use the positioning sketch to locate the form feature on the face of the sheet metal part. To create a positioning sketch for a forming tool:
1.
Open a sketch on the top face of the boss feature on the forming tool.
2.
Create a profile to locate the form feature on the sheet metal part. One method to create a profile is to click Convert Entities Sketch Tools, Convert Entities.
3.
Close the sketch, and rename the sketch if desired.
4.
To hide the positioning sketch so that it does not appear in the thumbnail graphic of the forming tool in the Feature Palette window, right-click the sketch in the FeatureManager design tree, and select Hide.
on the Sketch toolbar, or click Tools,
Working with Palette Items and Folders To copy a palette item:
Hold down the Ctrl key, then drag a palette item within the Feature Palette window. You can only copy an item this way in the same folder. The new item is named Copy of
You can rename the palette items and the folders, except the folders at the Palette Home level. Click-pauseclick the name in the Feature Palette window, and enter a new name. To edit a palette item:
1.
Right-click the item in the palette window, and select Edit Palette Item. - or Drag the item from the Feature Palette window and drop it in an empty area of the SolidWorks window (not an empty area of a document window). The part (.sldprt) or library feature (.sldlfp) document is opened in a new window.
2.
Edit the document as needed, then Save. The palette updates automatically to reflect the changes. NOTE: The thumbnail graphic reflects the newly saved view. Be sure to orient the part or assembly so that the graphic looks the way you want it to look.
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Chapter 15 Sheet Metal
To change the contents of a palette folder:
1.
In Windows Explorer, navigate to the directory you want to modify.
2.
Add, move, or delete the files as needed, using Windows file management commands.
3.
Click Reload
on the toolbar in the Feature Palette window to update the folders.
To delete a palette item:
Click the item in the Feature Palette window, and press Delete. The item is removed from the window, and the file is deleted from the corresponding folder. To delete a palette folder:
1.
Exit SolidWorks.
2.
Navigate to the directory to delete, move the contents to a new location, if necessary, then delete the directory.
Applying Forming Tools to Sheet Metal Parts You can only insert forming tools from the Feature Palette window and you can apply them only to sheet metal parts. A sheet metal part has the Sheet-Metal feature in the FeatureManager design tree. To apply a palette forming tool to a sheet metal part:
1.
In an existing sheet metal part, click Tools, Feature Palette, and navigate to the folder that contains the forming tools.
2.
Drag the forming tool from the Feature Palette window to the face you want to deform, but do not drop it yet. The face where you apply the forming tool corresponds to the stopping surface of the tool itself. By default, the tool travels downward. The material is deformed when the tool strikes the face where it is dropped. To toggle the direction of travel and strike the opposite side of the material, press the Tab key. Notice the preview as you toggle the direction.
3.
Drop the feature where you want it applied. If the forming tool includes an optional positioning sketch, that sketch is displayed when you drop the tool on the face.
4.
Locate the positioning sketch by dimensioning, adding relations, or modifying the sketch. As you add dimensions, the positioning sketch moves as a single entity. The absorbed sketch in the feature controls only the location of the feature, not its dimensions.
5.
In the Position form feature dialog box, click Finish. The forming tool is applied to the face, and the feature is added to the FeatureManager design tree with the name of the forming tool.
More Sheet Metal Topics Using Auto Reliefs The software automatically adds relief cuts wherever needed when inserting bends if you select Auto Relief. The software supports the following types of relief cuts: •
Rectangular
•
Tear
•
Obround
If you want to automatically add Rectangular or Obround reliefs, you must specify the Relief Ratio. Tear reliefs are of the minimum size required to insert the bend and flatten the part.
15-28
Relief Ratio The distance d represents the width of the Rectangular or Obround relief cut and the depth by which the side of the Rectangular or Obround relief cut extends past the bend region. The distance d is determined by the following equation: d = (relief ratio) * (part thickness) The bend region is represented by the dark gray area of the diagram.
The value of the relief ratio must be between 0.05 and 2.0. The higher the value, the larger the size of the relief cut added during insertion of bends. Changing Auto Reliefs You can change the type and size of a relief cut for a feature bend. A feature bend is different from an individual bend, in that the feature bend is an actual sheet metal feature. For example, when you have a Sketched Bend in the FeatureManager design tree, the Sketched Bend feature is the sheet metal feature, and SketchBend is the individual bend that is absorbed in the Sketched Bend feature. To change the type and size of a relief cut for a feature bend:
1.
In the FeatureManager design tree, right-click the feature bend you want to edit, and select Edit Feature.
2.
In the PropertyManager, select Custom Relief Type.
3.
Under Custom Relief Type: •
Set a relief cut in Auto Relief Type.
•
If you selected Rectangular or Obround, change the values for Relief Width Depth
4.
Click OK
and Relief
, or select Use relief ratio and set a value for Relief Ratio.
.
Edit Auto Reliefs You can edit auto relief cuts in sheet metal parts. For more information, select from the following: •
Edit a single auto relief
•
Edit all auto reliefs
NOTE:You cannot edit relief cuts in sheet metal parts created in versions prior to SolidWorks 99. Edit All Auto Reliefs You can change the type of auto reliefs automatically added to the bend regions in sheet metal parts. You cannot edit relief cuts in sheet metal parts created in versions prior to SolidWorks 99. To change the type of relief cut for all bends:
1.
Right-click the Sheet-Metal feature in the FeatureManager design tree and select Edit Feature.
2.
In the PropertyManager, under Auto Relief, change the type of relief cut.
3.
If you select Rectangular or Obround, specify the Relief Ratio.
4.
Click OK
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.
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Chapter 15 Sheet Metal
Rip Creates a rip feature along the selected model edges. A rip feature is commonly used in sheet metal parts, but you can add a rip feature to any part. To create a rip feature:
1.
2.
Create a part of uniform thickness with adjacent planar faces that form one or more linear edges or a chain of linear edges.
Click Rip
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Rip.
The Rip PropertyManager appears. 3.
On the model, select the internal linear edges to rip. Note the arrows that appear on each selected edge. By default, rips are inserted in both directions. To insert a rip in only one direction, click the name of the edge listed under Edges to Rip, and click Change Direction. The rip direction toggles every time you click Change Direction to one direction, then the other direction, then back to both directions.
4.
To change the gap distance, clear the Use default gap check box, and type a value in the Rip Gap
5.
Click OK
Both directions:
One direction:
15-30
.
box.
Bends The Bends PropertyManager allows you to create a sheet metal part. When you use the Insert Bends tool, you must create a solid body, then use Insert Bends to convert the part to sheet metal. Alternatively, you can create a part directly out of sheet metal with a Base-Flange. To convert a part to sheet metal:
1.
In a part made of uniform thickness, click Insert Bends Sheet Metal, Bends.
on the Sheet Metal toolbar, or click Insert,
The Bends PropertyManager appears. 2.
Under Bend Parameters, do the following: •
Select a Fixed Face or Edge
•
Set the Bend Radius
.
.
3.
Under Bend Allowance, select from the following options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
4.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
5.
If you want relief cuts added automatically, select the Auto Relief check box, then select the type of relief cut. If you select Rectangular or Obround, then you must specify a Relief Ratio.
6.
If desired, select an edge to rip under Rip Parameters •
Click Change Direction if you want to reverse the direction of the rip.
•
Clear the Use default gap check box if you want to set a gap distance, and type the value in the Rip Gap
7.
, and do the following:.
Click OK
box. .
The bends are added, and the part is converted to sheet metal. Edit Bends You can edit the bend parameters for a single bend, for a group of bends, or for your entire sheet metal part. The bend parameters include the default bend radius, and the bend allowance or bend deduction values. Select from the following: •
Edit a single bend.
•
Edit a group of bends.
•
Edit all the bends in your sheet metal part.
Reorder Bends You can reorder the bends in a sheet metal part in which bends have been inserted. To reorder bends in relation to each other:
1.
Right-click Flat-Pattern1 in the FeatureManager design tree, and select Reorder Bends. If you created the sheet metal part with the Insert Bends feature, right-click Process-Bends1, and select Reorder Bends.
2.
In the dialog box, click a bend name in the list, then click Move Up or Move Down to change the bend order.
3.
Repeat step 2 to move additional bends.
4.
Click OK.
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Chapter 15 Sheet Metal
Flattening Sheet Metal Bends You can flatten the bends in a sheet metal part in the following ways: •
To flatten the entire part, if the Flat-Pattern1 feature is present, unsuppress Flat-Pattern1, or click Flattened on the Sheet Metal toolbar. The bend lines are shown by default when you unsuppress Flat-Pattern1. To hide the bend lines, expand Flat-Pattern1, right-click Bend-Lines, and select Hide. When you flatten the entire part in this manner, corner treatments are applied to create a clean, flattened sheet metal part.
•
To flatten the entire part, if the Process-Bends1 feature is present, suppress Process-Bends1, or click Flattened
•
on the Sheet Metal toolbar.
To flatten one or more individual bends, add an Unfold
feature.
For faster system performance, only unfold the bends that you need for the task that you are performing. For example, when you add a cut across a bend, only unfold that one bend. No Bends You can roll back all bends from a sheet metal part in which bends have been inserted so that you can make additions, such as adding a wall. This is available only in sheet metal parts with Flatten-Bends1 and Process-Bends1 features. To roll back all bends from a sheet metal part:
Click No Bends on the Sheet Metal toolbar to roll back the bends up to Sheet-Metal1. The bend radius and bend allowance are rolled back. (The part is not flattened.) To restore all bends to the part:
Click No Bends
again.
Sheet Metal - Default Bend Parameters The presence of the Sheet-Metal1 feature in the FeatureManager design tree indicates that you have a sheet metal part. The Sheet-Metal1 feature contains the default bend parameters. To edit the default bend radius, bend allowance or bend deduction, or default relief type:
1.
Under Bend Parameters: •
On the model, select a linear edge on an end face of a cylindrical or conical face, or select a planar face for Fixed Face or Edge . The edge or face remains in place when the part is flattened. This step is not necessary if you start your sheet metal part from a Base Flange feature.
•
15-32
Set the Bend Radius
.
2.
Under Bend Allowance, select from the following: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
3.
If you selected K-Factor, Bend Allowance, or Bend Deduction, set a value.
4.
If you want relief cuts added automatically, select Auto Relief, then select the type of relief cut. If you selected Rectangular or Obround, then you must set a Relief Ratio.
5.
Click OK
.
Mirroring Sheet Metal Parts When you mirror a sheet metal part, many of the bends are mirrored as well. The only bends that are not mirrored are those that are normal to and coincident to the mirror plane; those bends are extended. To mirror a sheet metal part:
1.
In an existing sheet metal part, click Insert, Pattern/Mirror, Mirror. NOTE: If a message appears that says sheet metal features cannot be mirrored individually, click OK. The Mirror PropertyManager appears.
2.
Select a plane of symmetry or a planar face as the Mirror Face/Plane . Use Select Other from the shortcut menu if necessary.
3.
Select a body as the Bodies to Mirror
4.
Click OK
.
.
The entire part is mirrored as well as the sheet metal bends.
5.
Expand Mirror1 in the FeatureManager design tree and notice the new bends that include the mirrored geometry.
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Chapter 15 Sheet Metal
Cut Across Sheet Metal Bends You can make cuts across bend lines. To cut across sheet metal bends:
1.
In an existing sheet metal part, click Unfold
or Insert, Sheet Metal, Unfold.
The Unfold PropertyManager appears. 2.
In the graphics area: a.
Select a face as the fixed face. The selected face appears in the Fixed face
b.
box.
Select the bend you want to cut across. The selected bend appears in the Bends to unfold
3.
Click OK
box.
.
The selected bend only is unfolded. 4.
Sketch a closed profile across the flattened bend, and Extrude the cut Through All.
5.
To restore the part to the bent state, click Fold Metal, Fold.
or Insert, Sheet
The Fold PropertyManager appears. 6.
In the graphics area: a.
Select a face as the fixed face. The selected face appears in the Fixed face
b.
box.
Select the bend you want to fold. - or Click Collect All Bends to fold all bends. The selected bends appear in the Bends to fold
7.
Click OK
.
The selected bends fold.
15-34
box.
Normal Cut When adding a cut to a folded sheet metal part, you can select the Normal cut check box to ensure that the cut is created normal to the sheet metal thickness. The Normal cut check box is selected by default for sheet metal features, and is located in the Cut-Extrude PropertyManager. The effect of a Normal cut is illustrated below:
Sketch for cut
Without Normal cut
With Normal cut
Break Corner/Corner-Trim The Break Corner tool cuts away material from a folded sheet metal part on an edge or a face. The Corner-Trim tool cuts material away from a flattened sheet metal part on an edge or a face. If you use the Corner-Trim tool when your sheet metal part is in Flattened suppresses the feature when the part is folded.
mode, the SolidWorks software
To create a break corner or corner-trim on a sheet metal part:
1.
Create a sheet metal part.
2.
Click Break-Corner/Corner-Trim Corner.
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Break
The Break Corner PropertyManager appears. If the part is flattened, the Corner-Trim PropertyManager appears. 3.
Under Break Corner Options select from: •
Corner Edges and/or Flange Faces . In the graphics area, click the corner edges or flange faces to break. You can select corner edges, flange faces, or both. A preview of the break corner appears in the graphics area. The preview is not an exact representation of the geometry.
•
Preview of Break Corner/Corner-Trim
Internal corners only (flattened sheet metal parts only). Applies a corner trim to internal corners, as shown.
Preview of internal corners
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Chapter 15 Sheet Metal
4.
•
Break type. Click Chamfer
•
Distance
•
Radius
(straight edges) or Fillet
(round edges).
. Set a value for the chamfer distance. . Set a value for the fillet radius.
Under Relief Options (flattened sheet metal parts only) select from: •
Corner edges cuts.
. In the graphics area, click the corner edges to which you want to apply relief
A preview of the relief cuts appears in the graphics area. The preview is not an exact representation of the geometry. •
Relief type. Select a relief type to apply to the corner edge. If you select Circular or Bend Waist, set the Radius
5.
Click OK
. If you select Square, set the Side length
.
.
The selected corners are broken.
Chamfered break corners
Filleted break corners
example of corner edge Jog The Jog tool adds material to a sheet metal part by creating two bends from a sketched line. Some additional items to note about the Jog tool:
15-36
•
The sketch must contain only one line.
•
The line does not need to be horizontal or vertical.
•
The bend line does not have to be the exact length of the faces you are bending.
To create a jog feature on a sheet metal part:
1.
Sketch a line on the face of a sheet metal part where you want to create the jog. Alternatively, you can select the Jog feature before you create a sketch (but after you select a plane). When you select the Jog feature, a sketch opens on the plane.
2.
Click Jog on the Sheet Metal toolbar, or click Insert, Sheet Metal, Jog.
3.
In the graphics area, select a face for Fixed Face
4.
Under Selections, to edit the bend radius, clear Use default radius, and type a new value for Bend Radius
.
.
5.
6.
Under Jog Offset: •
Select an item in End Condition.
•
Set a value for Offset Distance
•
Select a Dimension position: Outside Offset
•
. Select Fix projected length if you want the face of the jog to stay the same length.
Under Jog Position, select: Bend Centerline Bend Outside
. , Inside Offset
, Material Inside
, or Overall Dimension
, Material Outside
, or
.
7. 8.
Set a value for Jog Angle . To use something other than the default bend allowance, select Custom Bend Allowance, and set a bend allowance type and value.
9.
Click OK
.
Example of Fixed Projected Length In this example, the original length of the tab is preserved if you select the Fix projected length check box. If you clear the Fix projected length check box, no material is added to the tab to make the jog.
Original part
SolidWorks 2004 Reference Guide
Fix projected length selected
Fix projected length cleared
15-37
Chapter 15 Sheet Metal
Lofted Bend You can create a lofted bend in sheet metal parts. A lofted bend, similar to a loft feature, uses two sketches that are connected by a loft. The Base-Flange feature is not used with the Lofted Bend feature. Example of a Lofted Bend
Begin with two open profile sketches.
Use Lofted Bends to create a solid feature.
Lofted bend is complete.
The SolidWorks software contains several pre-made sheet metal parts created with lofted bends. These parts are located in
When a lofted bend is represented with a lofted surface (B-spline), as is created by a square to circle profile, it cannot use K-Factor or Bend Allowance in the sheet metal calculations.
•
When a lofted bend is represented as a conical or cylindrical bend, such as a loft between concentric circular arcs, then it behaves in the same way as a cylindrical or conical bend in that it uses K-Factor or Bend Allowance to calculate the bends.
•
Lofted bends cannot be mirrored.
To create a lofted bend:
1.
Create two separate open profile sketches. Both sketches must conform to the following: • • •
The sketches must be open profiles. The profile openings should be aligned for flat-pattern accuracy. The sketches cannot have sharp edges.
2.
Click Lofted Bend on the Sheet Metal toolbar, or click Insert, Sheet Metal, Lofted Bends.
3.
In the graphics area, select both sketches. Make sure to select the points from which you want the path of the loft to travel. The sketch names appear under Profiles PropertyManager.
15-38
in the
4.
Examine the path preview. If necessary, click Move Up or Move Down to adjust the order of the profiles, or re-select the sketches to connect different points on the profiles.
5.
Set the Thickness for the sheet metal part.
6.
Click Reverse Direction
7.
Click OK
, if necessary.
.
Bend Deviation When you create a lofted bend, you can examine the surface area and curve lengths of the bend. These items are located in the Bend Deviation PropertyManager. To examine bend deviation:
1.
In the FeatureManager design tree: •
Right-click Flat-Pattern1 and select Unsuppress.
•
Click
•
Right-click Flatten-
to expand Flat-Pattern1.
The graphics area callouts display the bend deviation values for each edge. The bend deviation plane for the Bend Surface Area is the plane or face where the sketch is located. For example, if the material is extruded toward the inside of the model, bend deviation is measured from the outside face. The Bend Deviation PropertyManager appears, and displays the following: •
Under Bend Surface Area: o
Folded. Surface area of the lofted bend when in the folded state.
o
Flat. Surface area of the lofted bend when in the flattened state.
o
Deviation. Flat value minus the Folded value.
o
•
Under Curve Lengths: o
2.
Click OK
SolidWorks 2004 Reference Guide
Percentage change (%). Deviation value divided by the Folded value, multiplied by 100. Max deviation only. When selected, this shows the maximum deviation of the curve only.
.
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Chapter 15 Sheet Metal
Creating Sheet Metal Parts with Cylindrical Faces Parts with cylindrical faces can be made of sheet metal if they meet the following criteria: •
Any adjacent planar and cylindrical faces must be tangent.
•
At least one end face of any cylindrical face must have at least one linear edge.
To create a sheet metal part with cylindrical faces:
1.
Sketch an open contour arc. The arc can also be tangent to a line.
2.
Click Base-Flange/Tab
or Insert, Sheet Metal, Base Flange.
The Base Flange PropertyManager appears. 3.
4.
15-40
Under Direction 1: •
Select an End Condition from the list.
•
Set the Depth
.
Under Sheet Metal Parameters: •
Set the Thickness
.
•
If necessary, select the Reverse direction check box to extend the feature in the opposite direction from that shown in the preview.
•
Set the Bend Radius
.
5.
Under Bend Allowance, select from the following bend allowance options: Bend Table, K-Factor, Bend Allowance, or Bend Deduction.
6.
If you selected K-Factor, Bend Allowance, or Bend Deduction, type a value.
7.
If you want relief cuts added automatically, select the Auto Relief check box, then choose the type of relief cut. If you choose Rectangular or Obround, then you must specify a Relief Ratio. NOTE: The options and values you specify for bend radius, bend allowance, and auto relief are shown as the default settings for the next new sheet metal part that you create.
8.
Click OK
.
The cylinder is now a sheet metal part.
NOTE: Only parts with exact analytic cylindrical faces can be unfolded. As a test, try to insert an axis on the cylindrical face. If you can insert an axis, the model is an exact cylinder. If you cannot insert an axis, then the model is not an exact cylinder and cannot be unfolded. However, sheet metal parts created with the Lofted Bends feature avoid this limitation and unfold appropriately. Creating Drawings of Sheet Metal Parts When you create a drawing of your sheet metal part, a flat pattern is automatically created. Drawings of sheet metal parts can also contain views of the bent sheet metal part. To create a drawing of a flat pattern:
1.
Open a new drawing.
2.
In the Model View PropertyManager, under Part/Assembly to Insert, select an item in Open documents, or click Browse to locate a sheet metal part. If the PropertyManager does not appear, click Model View Insert, Drawing View, Model.
3.
Click Next
4.
Under Orientation, select Flat Pattern in View Orientation
5.
Click in the drawing to place the view.
on the Drawing toolbar, or click
. .
A flat pattern configuration is created automatically with the bend lines visible. The bend region lines are not shown. 6.
Click OK
.
If you want to toggle the suppression of additional features in a flat pattern, create a part configuration of a flat pattern, then select a drawing view for it. To toggle the visibility of the bend lines in a flat pattern view:
1.
In the drawing window, expand Drawing View in the FeatureManager design tree to show the Flat-Pattern feature. Expand the Flat-Pattern feature.
2.
Right-click Bend-Lines and select Show or Hide.
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Chapter 15 Sheet Metal
To toggle the visibility of the bend region lines in a flat pattern view:
1.
Right-click the drawing view in the drawing sheet.
2.
Select Tangent Edge, Tangent Edges Visible or Tangent Edges Removed. - or Select Tangent Edge, Tangent Edges With Font to show bend region lines in the specified document Line Font. If the bend region lines do not appear, go back to the part window and right-click Flat-Pattern in the FeatureManager design tree. Select Edit Feature, and clear Merge faces. You may have to rebuild the drawing to see the tangent edges.
Flat Pattern The Flat-Pattern1 feature is intended to be the last feature in the folded sheet metal part. All features before Flat-Pattern1 in the FeatureManager design tree appear in both the folded and flattened sheet metal part. All features after Flat-Pattern1 appear only in the flattened sheet metal part. Some items to note about the flat-pattern feature: •
New features in folded part. When Flat-Pattern1 is suppressed, all features that you add to the part automatically appear before this feature in the FeatureManager design tree.
•
New features in flattened part. You flatten the entire sheet metal part by unsuppressing Flat-Pattern1. To add features to the flattened sheet metal part, you must first unsuppress Flat-Pattern1.
•
Reorder features. You cannot reorder sheet metal features to go below Flat-Pattern1 in the FeatureManager design tree. So, you cannot order a cut with the Normal cut option underneath Flat-Pattern1.
•
Modify parameters. You can modify the parameters of Flat-Pattern1 to control how the part bends, to enable or disable corner options, and to control the visibility of the bend region in the flattened sheet metal part.
To modify the parameters of the Flat-Pattern1 feature:
1.
Right-click Flat-Pattern1 in the FeatureManager design tree, and select Edit Feature.
2.
In the PropertyManager, under Parameters: •
In the graphics area, select a face that does not move as a result of the feature for Fixed face
•
Select Merge faces to merge faces that are planar and coincident in the flat pattern.
.
When selected, no lines are shown in the bend regions. • 3.
Select Simplify bends to straighten curved edges in the flat pattern.
Under Corner Options: •
Select Corner Treatment to apply smooth edges in the flat pattern.
•
Select Add Corner-Trim to apply relief cuts in the flat pattern. When selected, you can choose from: o
Break corners. Cuts away material from an edge or a face. Click Chamfer
o
as the Break type and set the Distance or Radius Relief type. Sets the relief type for any relief cuts needed.
o
Radius or Side length. Set the Radius
15-42
Click OK
.
or Side length for the Relief type.
Ratio to thickness. Sets the relief type radius to a specified ratio of the sheet metal thickness. When selected, set the Ratio of radius/distance to sheet metal thickness.
o
4.
or Fillet
.
Merge Faces When you select the Merge faces check box, no lines are shown in bend regions of the flat pattern. Here is an example of merged faces:
Merge faces selected
Merge faces not selected
Simplify Bends When you select the Simplify bends check box, curves are straightened out in the flat pattern. When this option is not selected, complex edges remain in the flat pattern. Here is an example of simplified bends:
Simplify bends selected
Simplify bends not selected
Corner Treatment When you flatten a sheet metal part by unsuppressing the Flat-Pattern feature, corner treatments are automatically applied to create a clean, flattened sheet metal part. The corner treatments are applied so the flat pattern is correct for manufacturing. To turn off corner treatments, right-click Flat-Pattern1, and select Edit Feature. In the PropertyManager, clear Corner Treatment. Here is an example of corner treatments:
Model with a miter flange
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Chapter 15 Sheet Metal
Flattened model without a corner treatment (using the Unfold
Flattened model with a corner treatment
feature)
Add Corner-Trim
Circular relief type
Square relief type
Bend waist relief type
Creating a Sheet Metal Flat Pattern Configuration You can create a configuration in a sheet metal part that shows the flattened part. To ensure that all features are shown in a flat pattern, you should create the flat pattern configuration after the entire design pattern of the part is complete. To create a flat pattern configuration:
1.
In a sheet metal part, create a new configuration.
2.
In the FeatureManager design tree: Right-click Flat-Pattern and select Unsuppress. - or Select Process-Bends and all of the features after it. Click Edit, Suppress, This Configuration to suppress all of the selected features.
15-44
Unfold/Fold With the Unfold and Fold tools, you can flatten and bend one, more than one, or all of the bends in a sheet metal part. This combination is useful when adding a cut across a bend. First, add an Unfold feature to flatten the bend. Next, add your cut. Lastly, add a Fold feature to return the bend to its folded state. For faster system performance, unfold and fold only the bends that you need for the task that you are performing. To add an Unfold feature:
1.
In a sheet metal part, click Unfold
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Unfold.
2.
In the graphics area, select a face that does not move as a result of the feature for Fixed face
3.
Select one or more bends as the Bends to unfold appropriate bends in the part.
4.
Click OK . The selected bends unfold.
.
, or click Collect All Bends to select all the
To add a Fold feature:
1.
In a sheet metal part, click Fold
on the Sheet Metal toolbar, or click Insert, Sheet Metal, Fold.
2.
In the graphics area, select a face that does not move as a result of the feature for Fixed face
3.
Select one or more bends as the Bends to fold bends in the part.
4.
Click OK
.
, or click Collect All Bends to select all the appropriate
.
The selected bends fold.
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Chapter 15 Sheet Metal
15-46
16 Weldments
Weldments Toolbar The Weldments toolbar provides tools for creating weldment parts. Weldment Structural Member Gusset End Cap Fillet Bead Trim/Extend
Weldments - Structural Members When you add the first structural member to an existing layout sketch, adding the structural member defines the model as weldment feature. The weldment feature sets up a design functionality environment. It is not a feature in the same context as a fillet is a feature in the SolidWorks environment. When you insert a weldment feature, it activates the multibody environment by clearing the Merge result check box in the PropertyManager of features that add material. The weldment feature also acts as a placeholder for common custom properties that are inherited by all cut list items. All structural members include the following attributes: •
Structural members use profiles, for example an angle iron.
•
Profiles are identified by Type, Size, and Standard (iso and ansi inch). Each profile Type includes multiple sizes.
•
Structural members can include multiple segments, but all segments can use only one profile.
•
Multiple structural members, each with a different profile, can belong to the same weldment part.
•
Two structural members can only share a single point.
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Chapter 16 Weldments
Structural Member1
Structural Member2
You need to create a new structural member to add the vertical structural members to the top square structure. •
Structural members appear in the FeatureManager design tree as Structural Member1, Structural Member2, and so on. Bodies created by the structural members appear under Solid Bodies
.
•
You can create your own profiles (Type, Size, and Standard), and add them to the existing library of weldment profiles.
•
Weldment profiles are located in:
•
Structural members allow you to specify the pierce point of the profile, relative to the sketch segment used to create the structural member.
•
You can select structural members under Solid Bodies
, and create cut lists used in drawings.
To add structural members:
1.
Create a sketch.
Using linear sketch entities, you can create multiple 2D sketches with planes, create a 3D sketch, or combine 2D and 3D sketches.
16-2
2.
Click Structural Member
on the Weldments toolbar, or click Insert, Weldments, Structural Member.
3. 4.
To add multiple structural members, in the PropertyManager, click Keep Visible In the PropertyManager, under Selections:
.
•
Click in Standard and select iso or ansi inch.
•
Click in Type and select a Profile Type.
•
Click in Size and select a Profile.
•
To create the first structural member, select the first set of linear sketch entities in the graphics area as the Path segments.
As you select the structural members, Settings appears. Under Settings you can: •
Apply a corner treatment, or clear Apply corner treatment to specify a corner treatment later. For example, you can apply the corner treatment when you trim the structural members. You can also modify the corner treatment, allowing you to specify multiple corner treatments per structural member.
5.
•
Change Rotation Angle so that the structural member turns by a set number of degrees relative to the adjacent structural member.
•
Click Locate Profile to change the pierce point between the adjacent structural members. The default pierce point is the sketch origin.
Click OK
.
This clears Path segments, and allows you to apply additional, consecutive structural members. 6.
Select the second set of structural members. If necessary, you can apply a different Standard, Type, and Size.
7.
Click OK
to clear the Path segments, and to create additional structural members.
Weldments - Pierce Points (Locate Profile) The pierce point defines the location of the profile, relative to the sketch segment used to create the structural member. The default pierce point is the sketch origin in the profile library feature part. Any vertex or sketch point specified in the library feature profile can also be used as a pierce point.
Same profile with three different pierce points selected.
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Chapter 16 Weldments
To change a pierce point:
1.
Open an existing weldment part with structural members.
2.
Select a structural member in the FeatureManager design tree, and click Edit Feature.
3.
In the PropertyManager, under Settings, click Locate Profile. The system zooms in to the appropriate area. The graphics area displays the intersection between the last profiles you joined, using the default pierce point.
4.
Select any of the pierce points on the profile, or a sketch point that you added.
5.
Click OK
Rectangular tube profile with 11 pierce points. The pierce point is located at the default.
.
Weldments - Corner Treatments
No corner treatment
End Miter
End Butt1
End Butt2
Weldments - Change Corner Treatment You can change the corner treatment between adjacent structural members. To change a corner treatment:
1.
Right-click a structural member in the FeatureManager design tree and select Edit Feature.
2.
Select any of the points where structural members intersect.
The intersection point changes.
16-4
3.
Click the corner you want to modify. The Corner treatment pop-up toolbar appears.
4.
Click the corner treatment you want to apply, and click
End Trim 5.
End Miter
Click OK
End Butt1
.
End Butt2
.
Weldments - Trim and Extend You can trim structural members with planar faces so they butt up correctly in the weldment part. •
To trim a structural member with a planar face, such as a square tube, select one structural member as the Bodies to be Trimmed and another structural member as the Trimming Boundary.
•
To trim a structural member with a non-planar face, such as a pipe, use other trim tools such as Extruded Cut
.
1 - Bodies to be Trimmed 2 - Trimming Boundary
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Chapter 16 Weldments
To trim structural members with planar faces:
1.
Click Trim/Extend
2.
In the PropertyManager, under Corner Type, select a corner type.
End Trim
on the Weldments toolbar, or click Insert, Weldments, Trim/Extend.
End Miter
End Butt1
End Butt2
3.
Under Bodies to be Trimmed, select a structural member in the graphics area for Bodies.
4.
Under Trimming Boundary: •
Click Planar Face or Bodies. Selecting Planar Face as the Trimming Boundary is normally more efficient and offers better performance.
•
5.
Select an adjacent structural member in the graphics area as Face/Bodies.
Click OK
.
You should trim all corners in a weldment model.
16-6
Weldments - Adding Gussets Gussets reinforce the area between two, intersecting structural members with planar faces. There are two types of gussets:
•
Triangular Profile Triangular Profile Under Supporting Faces: •
Select Faces
. Select adjacent planar faces from two intersecting structural members.
•
Flip Profile D1 and D2 Parameters Profile Distance2.
. Flip the values between Profile Distance1 and
Under Profile: Set a value for Profile Distance1, and for Profile Distance2. Thickness. Set a Gusset Thickness thickness (inner, both, or outer side).
Inner Side
Both Sides
, and specify a side to the
Outer Side
Under Parameters: Locate a profile relative to the left and right edges of the structural member. Or, specify an offset distance from the edge to locate the gusset.
Profile Locates at Start Point
Profile Locates at Mid Point
Profile Locates at End Point
All location profiles shown above use Inner Side thickness.
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Chapter 16 Weldments
•
Polygonal Profile Polygonal Profile Under Supporting Faces: •
Select Faces . Select adjacent planar faces from two, intersecting structural members.
•
Flip Profile D1 and D2 Parameters . Flip the values between Profile Distance1 and Profile Distance2. Under Profile: Set values for Profile Distance1, Profile Distance2 and Profile Distance3. Select d4 to set a value for Profile Distance4. d4 defines the distance between the structural member and the vertex. - or Click a to set Profile Angle. a defines the angle between the two edges in the polygon that are adjacent to the structural members. Thickness. Set Gusset Thickness thickness (inner, both, or outer side).
Inner Side
Both Sides
, and specify a side to the
Outer Side
Under Parameters: Locate a profile relative to the left and right edges of the structural member. Or, specify an offset distance from the edge to locate the gusset. Click Flip Offset Direction
Profile Locates at Start Point
to change the offset direction.
Profile Locates at Mid Point
All profile locations shown above use Inner Side thickness.
16-8
Profile Locates at End Point
To add gussets:
1.
Click Gusset
2.
To add multiple gussets, in the PropertyManager, click Keep Visible
3.
Under Supporting Faces, select two adjacent, planar faces for Select Faces.
4.
Under Profile, click Triangular Profile or Polygonal Profile. •
on the Weldments toolbar, or click Insert, Weldments, Gusset. .
Set values for the appropriate profile distances. - or With Polygonal Profile, click a to set a Profile Angle.
•
• 5.
o
Inner Side
o
Both Sides
o
Outer Side
Set a value for Gusset Thickness
.
Under Parameters, set values to locate the gusset profile: •
6.
Select where to apply gusset Thickness:
Select a profile location: o
Profile Locates at Start Point
.
o
Profile Locates at Mid Point
.
o
Profile Locates at End Point
.
•
If necessary, select Offset and set an Offset Value.
•
Flip Offset Direction
Click OK
SolidWorks 2004 Reference Guide
. Change the offset direction.
.
16-9
Chapter 16 Weldments
Weldments - Fillet Weld Beads You can add full length, intermittent, or staggered fillet weld beads between any intersecting weldment entities such as structural members, plate weldments, or gussets. To add fillet weld beads:
1.
Click Fillet Bead
2.
To add multiple fillet beads, in the PropertyManager, click Keep Visible
3.
Under Arrow Side: a.
on the Weldments toolbar, or click Insert, Weldments, Fillet Bead. .
Select a Bead type. .
Annotation: 4 - Bead size. Radius of the fillet bead 3 - Bead length. Length of each bead segment. Only with Intermittent or Staggered. 6 - Bead pitch. Distance between the start of each bead. Only with Intermittent or Staggered.
Full length
Intermittent
Staggered. Creates fillet bead on both the Arrow Side and the Other Side. b.
Set a value for Bead size
.
c.
For Intermittent or Staggered types, set a Bead length and a Bead pitch.
d.
Clear Tangent propagation if necessary. Although you must select planar faces for the face sets, fillet weld beads can follow non-planar, tangent contours when you select Tangent propagation.
e.
Select a face as Face Set1
Gusset face
16-10
.
Structural member face
f.
Click in Face Set2
, then select a second, intersecting face.
Structural member face
Plate weldment face
The system assigns Virtual edges based on your selections for Face Set1 and Face Set2 . A fillet weld bead preview appears along the edges between the intersecting faces. 4.
Click Other Side. If you selected Staggered as the Bead type, the Other Side is already displayed. With Staggered as the Bead Type, apply the fillet weld bead to the opposite side.
Staggered bead type a.
Select a Bead type.
Annotation: 4 - Bead size. Radius of the fillet bead 3 - Bead length. Length of each bead segment. Only with Intermittent or Staggered. 6 - Bead pitch. Distance between the start of each bead. Only with Intermittent or Staggered.
Full length
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Intermittent
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Chapter 16 Weldments
Staggered. Creates fillet bead on both the Arrow Side and the Other Side. b.
Set a value for the Fillet Size
c.
For Intermittent or Staggered types, set a Bead length and a Bead pitch.
d.
Select a second face as Face Set1
.
Gusset face
Structural member face
e.
Click in Face Set2
, and select the second, intersecting face for the Arrow Side.
Structural member face
Plate weldment face
The system assigns the Virtual edges based on your selections for Face Set1
and Face Set2
A fillet weld bead preview appears along the edges between the intersecting entities. 5.
Click OK
.
Fillet weld bead between structural member and gusset
16-12
Fillet weld bead between structural member and plate weldment
.
Weldments - End Caps End caps close off open structural members. You can add end caps only to profiles with linear edges. To add end caps:
1.
Click End Cap
on the Weldments toolbar, or click Insert, Weldments, End Cap.
2.
To add multiple end caps, in the PropertyManager, click Keep Visible
3.
Under Parameters: •
Select a profile face for Face
•
Set a value for Thickness
.
. .
You can apply end caps to different open structural members. The opening depends on the structural member and the corner treatment you applied.
Select Face
End cap preview 4.
Under Offset: a.
Click Use thickness ratio to specify the offset distance of the end cap as a ratio of the thickness of the structural member that is being capped.
b.
Set a value for Thickness ratio
(maximum is 1).
- or a.
Clear Use thickness ratio.
b.
Set a value for Offset distance
c.
Click Chamfer corners if you want to add a chamfer to the corners.
d.
Set a value for Chamfer Distance
SolidWorks 2004 Reference Guide
.
.
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Chapter 16 Weldments
5.
Click OK
.
Repeat steps 3 through 5 to cap any remaining open profiles.
Creating Sub-Weldments You create sub-weldments to segment complex weldment models into more manageable entities. After you create sub-weldments, you can create the cut lists used in drawings. Any changes made to a sub-weldment model are reflected in the weldment model from which you created the sub-weldment. Sub-weldments can include any entity listed in the Solid Bodies
folder, including structural members, end caps,
gussets, weld fillet beads, and structural members trimmed with the Trim/Extend
tool.
To create a sub-weldment:
1.
In the FeatureManager design tree of the weldment model, expand the Solid Bodies
2.
Select the entities to include in the sub-weldment, using Shift or Ctrl to group-select.
folder.
The selected entities highlight in the graphics area. 3.
Right-click and select Create sub-weldment. A sub-weldment folder
4.
containing the selected entities appears under the Solid Bodies
Right-click the sub-weldment
folder.
folder and select Save to File.
The sub-weldment model opens in a new SolidWorks window, and the Save As dialog box appears. 5.
Accept or edit the name for File name, and click Save.
Weldment Drawings Drawings of weldments support:
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•
Views of entire weldment parts
•
Views of single bodies of weldment parts (Relative Views)
•
Weldment cut lists
•
Balloons
•
AutoBalloons
•
Alternating crosshatch for section views
Example of Weldment Cut List
Balloons in Weldment Drawings All configurations reference the same cut list for creating balloons. Balloon numbers remain associative to the cut list, even if they are created in another view. A balloon attached to a body in a drawing view of the entire weldment and a balloon attached to the same body in a drawing view showing only the body have the same item number. If you insert a balloon into a drawing view of a weldment and the drawing does not contain a cut list, you are prompted whether you want to create a cut list. If you delete a cut list, all balloons related to the cut list change their Item Number to 1.
Weldment Cut Lists To insert a weldment cut list in a drawing, first create cut list items in the weldment part document. Cut lists are tables. Example To create cut list items:
1.
In a weldment part document, under Solid Bodies, select bodies or sub-weldments to be included in a cut list item. You can group similar bodies, and sub-weldments, into one cut list item.
2.
Right-click and select Create cut list item. The bodies become absorbed features of the cut list item. The cut list item displays an instance number, plus the number of its weldment items in parentheses. Only top level items (bodies and sub-weldments) are listed in the cut list.
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Chapter 16 Weldments
To delete cut list items:
Select the cut list item and press Delete. The cut list item is deleted and the bodies remain under Solid Bodies. To insert a weldment cut list into a drawing:
1. 2.
In a drawing, click Weldment Cut List Cut List. Select a drawing view.
on the Annotation toolbar, or click Insert, Tables, Weldment
3. 4.
Specify properties in the Weldment Cut List PropertyManager, then click OK . If you did not select Attach to anchor in the PropertyManager, click in the graphics area to place the cut list
Configurations Weldments have two default configurations: Default
DESCRIPTION
•
LENGTH
You can add properties to the cut list items. To add custom properties to cut list items:
1.
In the part document, right-click a Cut-List-Item and select Properties.
2.
In the Cut-List-Item Custom Properties dialog box:
3.
•
Type a property name in Name.
•
Type text or a value in Value.
•
Click Add.
Repeat step 2 as necessary, the click OK.
Weldment Cut List PropertyManager Specify properties for weldment cut lists. Table Template Click Browse for template insertion. Table Anchor Set the Anchored corner to:
16-16
to choose a standard or custom template. This option is available only during table
Top Left Top Right Bottom Left Bottom Right Attach to anchor. Attaches the specified corner to the table anchor. Configurations Cut lists are usually based on the Welded State configuration. Keep Missing Item If cut list items have been deleted from the weldment since the cut list was created, you can keep the items listed in the table. If missing items are kept, select Strikethrough to display text for the missing item with strikethrough formatting. Item Numbers Start at. The cut list starts with the number displayed. Do not change item number. Click for item numbers to remain with their rows when columns are sorted or reordered. Table Format Click to access the Table Format PropertyManager.
Weldment Cut List Column PropertyManager Specify the columns to be included in a weldment cut list and their position in the table. To add a new column to the table, right-click in a table column and select Insert, Column Right or Column Left. You cannot add columns from within the PropertyManager. To access the Column PropertyManager, click at the head of a column when the pointer changes to
.
Column Properties For the selected column, choose one of the following column types, listed with its header title. You can edit the header in the Title box below. •
Item number. ITEM NO. Data in the Item Number custom property for the cut list items populates the column.
•
Quantity. QTY. Data in the Quantity custom property for the cut list items populates the column.
•
Cut list item name. The name of the cut list item (Cut-List-Item1, for example) in the part document populates the column.
•
User defined. Edit
•
Cut list item property. Custom properties for cut list items in the part document. Select a property from the list below and edit text for the column header in Title. Properties such as DESCRIPTION and LENGTH are available automatically for bodies created through the Feature Palette. You can add other custom properties for cut list items.
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Chapter 16 Weldments
Properties. List of document's custom properties, available when you specify Cut list item property under Column Properties. Title. Edit the text of the column header. Column position. Click Move Column Left
or Move Column Right
to move the selected column.
Cell Properties Click to access the Table Cell PropertyManager. Table Properties Click to access the Weldment Cut List PropertyManager. Table Format Click to access the Table Format PropertyManager.
Custom Properties in Weldments In a weldment part, the custom properties for the weldments feature and for the cut list represent a different list from the custom properties that are stored at the document level. The list of optional custom property names is located: lang\
Profile sketch: Assign to the profile sketch any commonly used properties that are unique to the profile, and that you want inherited by the cut list item corresponding to a structural member feature. Description is such an example.
•
Weldment feature. Properties assigned to the weldment feature are propagated to all cut list items. This capability enables you to assign a property with a default value, which you can later edit for each cut list item. For example, you can add the Property Cost with a value in the appropriate monetary denomination.
•
Cut-List-Items . Cut list items inherit custom properties from the profile sketch and from the weldment feature. You can assign new properties or you can edit existing properties. For example, you can add the property Weight, and link that property to the model's mass properties. Creating the link between the two enables the SolidWorks application to calculate the weight of the first solid body in the cut list item. The system also computes and adds the property LENGTH for bodies generated by structural member features. The LENGTH property is not editable. Since the weight of only the first item is calculated from the cut list, the cut list should only include identical items.
16-18
Custom Property Values Values that you assign as custom properties can be •
Constant. For example, the material assigned when creating the structural member profile.
•
Derived. o
Linked to dimension values.
o
Linked to mass properties.
Custom properties are required to generate a cut list with associative balloons for a multibody part. To add custom properties:
1.
Under Solid Bodies
, right-click a Cut-List-Item, and select Properties.
- or To assign custom properties at the highest propagation level, right-click the Weldment 2.
feature.
In the dialog box: a.
To assign a new name, type a value for Name, -or To assign an existing name, select one from the Name list.
b.
Select an item in Type.
c.
Type a value that is compatible with Type for Value. - or Select an item in Linked to value to associate the Value.
3. Click OK. The custom property is added.
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Chapter 16 Weldments
16-20
17 SolidWorks Options
Overview of SolidWorks Options Customize functionality to suit your needs. Click Tools, Options to display system options and document property settings. Options Dialog Box Structure The SolidWorks Options dialog box structure emphasizes the difference between system options and document properties. The Options dialog box has two tabs: •
System Options. The system options are stored in the registry and are not part of the documents. Therefore, these changes affect all documents, current and future.
•
Document Properties. The document properties apply only to the current document, and the Document Properties tab is available only when a document is open. New documents get their document settings (such as Units, Image Quality, and so on) from the document properties of the template used to create the document. Use the Document Properties tab when you set up document templates.
The options listed on each tab are displayed in tree format on the left side of the dialog box. As you click an item in the tree, the options for the item appear on the right side of the dialog box. The title bar displays the title of the tab and the title of the options page. To access the Options dialog box:
You can access the Options dialog box in any of the following ways: •
Click Tools, Options. The Options dialog box appears with the System Options tab active.
•
Right-click in the FeatureManager design tree area and select Document Properties. (There must be no items selected in the FeatureManager design tree or graphics area in order to select Document Properties.) The Options dialog box appears with the Document Properties tab active.
•
Click Grid/Snap on the Sketch toolbar. The Options dialog box appears with the Grid/Snap page of the Document Properties tab active.
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Chapter 17 SolidWorks Options
System Options General System Options Lets you change general system options such as enabling the performance email option, the Confirmation Corner, and so on. To set general system options:
1.
Click Tools, Options, System Options, General.
2.
Select from the options described below.
3.
Click OK. •
Open last used document(s) at startup. Select Always or Never. Select Always if you want the documents that you used most recently to open automatically when you start the SolidWorks software.
•
Input dimension value. Specifies that the Modify dialog box is automatically displayed for the input of a new dimension value. Otherwise, you must double-click the dimension to change the value.
•
Single command per pick. Specifies that sketch and dimension tools clear after each use. (Double-clicking a tool causes it to remain selected for additional use.)
•
Show dimension names. Displays the dimension’s name as well as its value.
•
Show errors every rebuild. Displays an error message each time you rebuild the model, if errors are present.
•
Maximize document on open. Opens each document to its largest size within the SolidWorks window.
•
Use shaded face highlighting. Displays selected faces in a solid color (green by default). To specify a different highlight color, click Tools, Options, System Options, Colors, then select a different color for Selected Face, Shaded. Some third-party applications may require that you clear this option.
•
Show thumbnail graphics in Windows Explorer. Displays a thumbnail graphic instead of an icon in Windows Explorer for each SolidWorks part or assembly document. The graphic is based on the view orientation of the model when the document was last saved. A palette of 16 colors is used; if the model uses a color that is not available, a similar color is substituted. The thumbnail graphics are also used in the Open and Save As dialog boxes. If you do not see thumbnail graphics in the Open or Save As dialog boxes, you may have to open, then save your documents. When you re-open these dialog boxes, you will see the thumbnail graphics.
•
Use system separator for dimensions. Specifies that the default system decimal separator is used when displaying decimal numbers. o o
•
To set the system default, use the Windows Control Panel. To set a decimal separator different from the system default, clear the option, and type a symbol that you want to use (usually a period or a comma).
Use English language menus. If you specified the use of another language when installing the SolidWorks software, and the regional options in the Windows Control Panel are set to that language, select this option to change menus to English. You must exit and re-start SolidWorks for this change to take place.
17-2
•
Use English language feature and file names. Displays feature names in the FeatureManager design tree and automatically created file names in English. Existing feature and file names in a foreign language do not update when you select this option. This option is available when: o o
Use English language menus is cleared. You are running the SolidWorks software on a foreign language operating system and you installed SolidWorks for that foreign language.
•
Enable performance email. Turns on and off the sending of email to SolidWorks Corporation regarding the performance and usage of the software.
•
Enable Confirmation Corner. Displays the Confirmation Corner in the upper right corner of the graphics area.
•
Auto-show PropertyManager. Displays the PropertyManager automatically. For example, if you edit a sketch and select a sketch feature to edit, the PropertyManager for the selected sketch feature appears automatically.
•
Save eDrawings data in SolidWorks document. Saves the SolidWorks document with eDrawings data so you can open the SolidWorks document in the eDrawings Viewer. If you select Save eDrawings data in SolidWorks document, you can override this option when you save your document. To override this option, click File, Save As, and clear Save eDrawing data.
•
Notify if SNL could not be obtained for eDrawings Save. Select if: You use SolidWorks Office and have a SolidNetWork License (SNL). If you save an eDrawings file, but there are no SolidWorks Office licenses available in SNL, you cannot save the eDrawings file as review-enabled. You can still save the file; however, it will not be review-enabled. It is helpful to have Notify if SNL could not be obtained for eDrawings Save selected so you know if the eDrawings file will be review-enabled. Your company may have several SolidWorks and SolidWorks Office licenses. If you use SolidWorks (not SolidWorks Office), and you save an eDrawings file, SNL searches for an available SolidWorks Office license so that you can save the file as review-enabled. Clear if: You use SolidWorks (not SolidWorks Office) and have a SolidNetWork License (SNL). If you use eDrawings without a SolidWorks Office license, eDrawings files are not saved as review-enabled. The notification message appears each time you save the eDrawings file unless Notify if SNL could not be obtained for eDrawings Save is cleared.
•
Custom property used as component description. Set or type a name to define a custom description label. For example, the Open dialog box has a Description label that displays the model description. Instead of displaying the Description label, you can display a label that you specify. If you change the Custom property used as component description in a document that has already been saved, you must manually add the new description to the Summary Information dialog box.
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Chapter 17 SolidWorks Options
Drawings Options You can set options for all drawings. To set options for drawings:
1.
Click Tools, Options, System Options, Drawings.
2.
Choose from the following options, then click OK.
Automatic placement of inserted dimensions from model. When selected, specifies that inserted dimensions are automatically placed at an appropriate distance from the geometry in the view. Display drawing view borders. When selected (the default), displays borders around individual drawing views. Automatically scale new drawing views. New drawing views are scaled to fit the drawing sheet, regardless of the paper size selected. Show contents while dragging drawing view. When selected, the model is displayed as you drag a view. When cleared, only the view boundary is shown while dragging. (Similar to Show window contents while dragging in Microsoft Windows.) Smooth dynamic motion of drawing view. When selected (the default), dynamic operations to drawings such as panning and zooming display smoothly. In most cases, keep the default. For some combinations of drawing size (small drawings in particular), graphics card, and system performance, operations such as panning and zooming may cause slower display performance. In such cases only, clear the Smooth dynamic motion of drawing view check box. Dynamic drawing view activation. When selected, the view closest to the pointer is activated automatically. To stop the dynamic activation temporarily, you can lock a view or the sheet. Right-click the view or sheet, and select Lock View Focus or Lock Sheet Focus. Right-click again, and select Unlock View Focus (or double-click another view) or Unlock Sheet Focus (or double-click any view) to return to dynamic mode. When cleared, double-click a drawing view to activate it, or right-click the view and select Activate View. To activate the sheet, double-click a blank area of the sheet or right-click the sheet and select Activate Sheet. Display new detail circles as circles. When selected, new profiles for detail views appear as circles. When cleared, the sketched profiles appear. Select hidden entities. When selected, you can select hidden (removed) tangent edges and edges that you have hidden manually. When you pass the pointer over hidden edges, the edges appear in phantom line font. Eliminate duplicate model dimensions on insert. When selected (the default), duplicate dimensions are not inserted into drawings when model dimensions are inserted. This option setting becomes the default setting for Eliminate duplicate model dimensions in the Insert Model Items dialog box. Allow auto-update when opening drawings. When selected, drawing views update automatically as the drawing document opens. Detail item snapping when dragging corner. When you click a corner and drag a detail item (for example, a note or dimension), the corner you clicked can infer to the corners of stationary detail items, and vice versa. Detail item snapping when dragging center. When you click the inside of a detail item (a note or dimension) and drag it, the center can infer to the center of stationary detail items, and vice versa. Print out-of-sync watermark. When selected, a watermark, SolidWorks Detached - Out-of-Sync Print, is printed on detached drawing printouts if the drawing is not synchronized with the model. Show Reference Geometry names in drawing. If selected, when reference geometry entities are imported into a drawing, their names appear. Automatically hide components on view creation. If selected, any components of an assembly not visible in a new drawing view are hidden and listed on the Hide/Show Components tab of the Drawing View Properties dialog box. The components are present, and all component information is loaded. The component names are transparent in the FeatureManager design tree. Display sketch arc centerpoints. When selected, sketch arc centerpoints are displayed in drawings.
17-4
Display sketch entity points. When selected, the endpoints of sketch entities are displayed as filled circles in drawing sheets and drawing sheet formats, but not in drawing views. Save tessellated data for drawings with shaded and draft quality views. If cleared, file size is reduced by not saving tessellated data in drawing documents with shaded and draft quality views. If needed, the data is read from the model file. In view-only mode and in eDrawings, nothing appears in the drawing view. For drawings with high quality and other display types, tessellated data is not used, so file size cannot be reduced. Print out-of-date drawing views with crosshatch. Specifies what happens when you Print (or Print Preview) a drawing that contains out-of-date views, with Automatic view update cleared. (If Automatic view update is selected, the views update automatically, and the crosshatch is removed whenever you print the drawing.) •
Prompt (default). Notifies you if the drawing contains out-of-date views, and asks how to proceed. When the dialog box appears, click Yes to print the drawing with crosshatch on the out-of-date views, or click No to print the drawing without crosshatch.
•
Always. The printed drawing always includes crosshatch on out-of-date views.
•
Never. The printed drawing never includes crosshatch on out-of-date views.
Detail view scaling. Specifies the scaling for detail views. The scale is relative to the scale of the drawing view from which the detail view is generated. Custom property used as Revision. Specify a document custom property to be regarded as the revision data when checking a document into PDMWorks (a SolidWorks Office Professional product).
Display Style Options You can set options for the default display of edges in all drawing documents. NOTE: The specified display types apply to new drawing views, except for new views created from existing views. If you create a new view from an existing view (a projected view, for example), the new view uses the display settings of the source view. To set the default display of edges in drawing documents:
1.
Click Tools, Options, System Options, Default Display Type.
2.
Choose from the following options, then click OK.
Default display for new drawing views Specifies the way parts or assemblies appear in drawings: •
Wireframe - All edges appear.
•
Hidden lines visible - Displays visible edges as specified in Line Font Options; displays hidden edges in gray.
•
Hidden lines removed - Displays only edges that are visible at the chosen angle; obscured lines are removed.
•
Shaded with edges - Parts appear in shaded mode with edges that would appear in Hidden lines removed mode displayed. You can specify a color for the edges, and set whether to use the specified color or a color slightly darker than the model color in the System Colors Options.
•
Shaded - Parts appear in shaded mode.
Display quality for new views •
High quality - model resolved.
•
Draft quality - model lightweight, used for faster performance with large assemblies.
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Chapter 17 SolidWorks Options
Default display of tangent edges in new drawing views If you selected Hidden lines visible or Hidden lines removed, select one of the following modes for viewing tangent edges (the transition edges between rounded or filleted faces): •
Visible - A solid line.
•
Use font - A line using the default font for tangent edges defined in Tools, Options, Document Properties, Line Font. (You must have a drawing document active to access this option.)
•
Removed - Not displayed.
Area Hatch/Fill Options You can set the hatch or fill options for any area hatch that you apply to a face or to a closed loop of a sketch entity in a drawing. To set area hatch options for all documents:
1.
Click Tools, Options, System Options, Area Hatch/Fill.
2.
Select from the options described below. The pattern is displayed in the preview window.
3.
Click OK.
Type of hatch or fill. Choose None, Solid, or Hatch. The subsequent options are available only for Hatch. The default color of the solid fill is black. You can change the color of the fill by selecting the area hatch in the graphics area and clicking Line Color on the Line Format toolbar. Pattern. Select a crosshatch pattern from the Pattern list. Scale. Type a scale value. Angle. Type an angle in degrees.
System Colors Lets you set the system defaults for colors used in drawings, assemblies, sketches, grid lines, background colors, and so on. You can also change the color scheme of the FeatureManager design tree or change the skin displayed in the PropertyManager. To set system colors:
1.
Click Tools, Options, System Options, Colors.
2.
Select from the options described below.
3.
Click OK.
System colors Displays a list of colors used for sketches, highlighting, and so on. Select an item in System colors, then click Edit to change the color. •
PropertyManager Color. Sets the background color for the PropertyManager.
•
PropertyManager Skin. Sets the background skin (image) for the PropertyManager. Skins take precedence over a color scheme in the PropertyManager. If you want the same color from the PropertyManager Color box to appear in the PropertyManager, set PropertyManager Skin to None.
17-6
•
Reset All To Defaults. Resets all system colors back to the system default values.
•
Save As Scheme. Saves the set of colors you defined for the SolidWorks display. After you save a color scheme, you can select it from the Current Color Scheme list.
Additional Options •
Current Color Scheme. Displays the color scheme applied to the SolidWorks software. If you define a color scheme by saving your color choices with Save As Scheme, the color scheme appears in this list. Click Delete to delete a color scheme. After you click Delete, the path is gone. Click Cancel to undo the deletion, if necessary.
•
Use gradient background. Displays a gradient background for SolidWorks documents. Set System colors to Top Gradient Color or Bottom Gradient Color, then specify a color.
•
Match graphics area and FeatureManager backgrounds. Applies the same background color to the graphics area and FeatureManager design tree.
•
Use specified color for Shaded With Edges mode. Applies the specified color to model edges when the model is in Shaded With Edges mode. Set System colors to Edges in Shaded With Edges Mode, then specify a color. If you clear this option, the edges are slightly darker than the model color.
•
Use specified colors when editing parts in assemblies. Applies the specified color to the faces, features, and bodies of a part while it is being edited in an assembly. Set System colors to Assembly, Edit Part, then specify a color.
•
Go To Document Colors (parts and assemblies only). Opens the Document Properties - Colors dialog box to set document-specific colors.
Sketch Options Lets you set the default system options for sketching. To set the default sketching options:
1.
Click Tools, Options, System Options, Sketch.
2.
Select from the following options, then click OK. •
Use fully defined sketches. Requires sketches to be fully defined before they are used to create features.
•
Display arc centerpoints in part/assembly sketches. Displays arc centerpoints in sketches.
•
Display entity points in part/assembly sketches. Displays endpoints of sketch entities as filled circles. The color of the circle indicates the status of the sketch entity: Black = Fully defined Blue = Under defined Red = Over defined Green = Selected Over defined and dangling points are always displayed, regardless of this option.
•
Infer from model. Displays inferencing lines that relate to the lines and vertices of the underlying model when you are sketching on the face of an extruded part.
•
Prompt to close sketch. Displays a dialog box with the question, Close Sketch With Model Edges? if you create a sketch with an open profile, then click Extruded Boss/Base to create a boss feature. Use the model edges to close the sketch profile and select the direction in which to close the sketch.
•
Create sketch on new part. Opens a new part with an active sketch on the Front Plane.
•
Override Dims on Drag/Move. Overrides dimensions when you drag sketch entities or move the sketch entity in the Move or Copy PropertyManager. The dimension updates after the drag is complete. This option is also available in Tools, Sketch Settings, Override Dims on Drag/Move.
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Chapter 17 SolidWorks Options
•
Automatic relations. Automatically creates geometric relations as you add sketch elements. This option is also available in Tools, Sketch Settings, Automatic Relations.
•
Display plane when shaded. Displays the sketch plane when you edit a sketch in Shaded With Edges or Shaded mode. If the display is slow due to the shaded plane, it may be because of the Transparency options. With some graphics cards, the display speed improves if you use low transparency. To set a low transparency, click Tools, Options, System Options, Performance and clear High quality for normal view mode and High quality for dynamic view mode.
•
Display virtual sharps. Creates a sketch point at the virtual intersection point of two sketch entities. Dimensions and relations to the virtual intersection point are retained even if the actual intersection no longer exists, such as when a corner is removed by a sketched fillet or a sketched chamfer. (To set the display options for virtual sharps, click Tools, Options, Document Properties, Virtual Sharps.)
•
Over defining dimensions: o
o
Prompt to set driven state. Displays a dialog box with the question, Make Dimension Driven? when you add an over defining dimension to a sketch. Set driven by default. Sets the dimension to be driven by default when you add an over defining dimension to a sketch. Use Prompt to set driven state alone or with Set driven by default. Depending on your selections, one of four actions occur when you add an over defining dimension to a sketch: •
A dialog box appears that defaults to driven.
•
A dialog box appears that defaults to driving.
•
The dimension is driven.
•
The dimension is driving.
Display and Selection Options Lets you set system default options for the display and selection of edges, planes, and so on. To set display and selection options:
1.
Click Tools, Options, System Options, Display/Selection.
2.
Select from the options described below.
3.
Click OK.
Hidden edges displayed as Solid or Dashed. Select either solid lines or dashed lines to specify how hidden edges are displayed in Hidden Lines Visible mode in part and assembly documents. Selection of hidden edges
17-8
•
Allow selection in wireframe and HLV modes. Allows you to select hidden edges or vertices in Wireframe and Hidden Lines Visible modes.
•
Allow selection in HLR and shaded modes. Allows you to select hidden edges or vertices in Hidden Lines Removed, Shaded With Edges, and Shaded modes.
Part/Assembly tangent edge display Controls how tangent edges are displayed when the model is in Hidden Lines Removed or Hidden Lines Visible mode. •
As visible. Tangent edges displayed.
•
As phantom. Tangent edges display using the Phantom style line font (
•
Removed. Tangent edges are not displayed.
).
Edge display in shaded with edges mode Specifies how edges are displayed when the model is in Shaded With Edges mode. •
HLR. Any edges that would appear in Hidden Lines Removed mode are displayed in Shaded With Edges mode also.
•
Wireframe. All edges are shown in Shaded With Edges mode (like Wireframe).
Assembly transparency for in context edit Controls the transparency options when you edit assembly components. •
Opaque assembly. All components become opaque gray, except for the component you are editing, which becomes opaque pink.
•
Maintain assembly transparency. All components remain in their current state, except for the one you are editing, which becomes opaque pink.
•
Force assembly transparency. All components become transparent except the one you are editing, which becomes opaque pink. Use the slider to adjust the transparency level for Force assembly transparency. Move the slider to the right to make components more transparent.
Highlight all edges of features selected in graphics view. Specifies that all edges on the selected feature are highlighted when you click it. Dynamic highlight from graphics view. Specifies whether model faces, edges, and vertices are highlighted when you move the pointer over a sketch, model, or drawing. Show open edges of surfaces in different color. Makes it easier to differentiate between the open edges of a surface and any tangent edges or silhouette edges. To specify the edge color, click Tools, Options, System Options, Colors. Select Surfaces, Open Edges in System colors. Anti-alias edges. Smooths out jagged edges in Shaded With Edges, Wireframe, Hidden Lines Removed, and Hidden Lines Visible modes. To specify the anti-alias edge color, click Tools, Options, System Options, Colors. Select Edges in Shaded With Edges Mode in System colors. You must also select Use specified color for Shaded With Edges mode to use the color you selected.
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Chapter 17 SolidWorks Options
Example of anti-alias edges.
Anti-alias option selected
Anti-alias option cleared
You can customize the color of the edges. If you do not specify a color, the edges are slightly lighter or darker than the model color. Display shaded planes. Displays transparent shaded planes with a wireframe edge that have different front and back colors. To specify the shaded plane colors, click Tools, Options, Document Properties, Plane Display. Under Faces, click Front Face Color or Back Face Color to change the colors. Use the slider to adjust the transparency level for the planes. Move the slider to the right to make the planes more transparent. Enable selection through transparency. When selected, you can select opaque objects behind transparent objects in the graphics area. When cleared, you can select the nearest object regardless of transparency. Press Shift when you select objects to temporarily override the option. Display reference triad. Displays a reference triad to help orient you when viewing models. The reference triad is for display purposes only; you cannot select it or use it as an inference point. To specify the triad colors, click Tools, Options, System Options, Colors. Select any of the three axes to change: X axis of Reference Triad, Y axis of Reference Triad, or Z axis of Reference Triad in System colors.
Performance Options Lets you set system options related to performance. Changes to these settings do not affect documents that are already open. They only affect documents that are opened after the setting has been changed. To set performance options:
1.
Click Tools, Options, System Options, Performance.
2.
Select from the options described below.
3.
Click OK.
Verification on rebuild Contols the level of error checking when you create or modify features. For most applications, the default setting (off) is adequate, and results in a faster rebuild of the model.
17-10
Transparency High-quality transparency is similar to looking through clear glass. Low-quality transparency (the default) is similar to viewing an object through a mesh or screen. •
High quality for normal view mode. While the part or assembly is not moving or rotating, the transparency is high quality. When moved or rotated with the pan or rotate tools, the application switches to low-quality transparency, enabling you to rotate the model faster. This is important if the part or assembly is complex.
•
High quality for dynamic view mode. High-quality transparency is retained while moving or rotating the model with the pan or rotate tools. Depending on your graphics card, this option may result in slower performance. If the display is slow when using transparent planes in Shaded With Edges or Shaded mode, it may be because of the Transparency you specified. With some graphics cards, the display speed improves if you do not use high-quality transparency.
Curvature generation Select one of the following options: •
Only on demand. Initial curvature display is slower, but uses less memory.
•
Always (for every shaded model). Curvature displays more quickly on the first display, but extra memory is always used (RAM and disk) for every part that you create or open.
Assemblies •
Automatically load components lightweight. Loads all the individual components in assemblies that you open as lightweight. Sub-assemblies are not lightweight, but the parts that they contain are lightweight. For more information, see Lightweight Parts.
•
Remove detail during zoom/pan/rotate. Removes small components and faces (both interior and exterior) from the graphics area when you zoom, pan, or rotate the model to improve system performance. When Remove detail during zoom/pan/rotate is enabled, the Optimize Zoom/Pan/Rotate option is available if you change the model. Click View, Display, or right-click in the graphics area and select View, Optimize Zoom/Pan/Rotate, to recalculate which components and faces should be hidden. Remove detail during zoom/pan/rotate is automatically disabled when you move or rotate a component, during mate animation, and during drag-and-drop animation. You can temporarily disable Remove detail during zoom/pan/rotate by holding down the Alt key.
•
Check out-of-date lightweight components. Lets you specify how you want the system to load lightweight components that are out-of-date. o o
o
•
Don’t check. Loads the assemblies without checking for out-of-date components. Indicate. Loads the assemblies and marks them with an icon if the assemblies contain an outof-date component, even if the assembly is not expanded. You can right-click an out-of-date toplevel assembly and select Set Lightweight to Resolved. Always Resolve. Resolves all out-of-date assemblies during load.
Resolve lightweight components. Some operations require certain model data that is not loaded in lightweight components. This option controls what happens when you request one of these operations in an assembly that has lightweight components. See also Loading Additional Model Data. o
o
Prompt. Resolves lightweight components each time one of these operations is requested. In the dialog box that appears, click Yes to resolve the components and continue, or click Cancel to cancel the operation. If you select Always resolve (before you click Yes or Cancel), the option is set to Always. Always. Automatically resolves lightweight components.
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Chapter 17 SolidWorks Options
•
Rebuild assembly on load. Lets you specify whether you want assemblies to be rebuilt, so components are updated when you open them. o
Prompt. Asks if rebuild is desired each time an assembly is opened. Click Yes or No in the dialog box that appears when you open the assembly. If you select Don’t ask me again (before you click Yes or No), the option is updated to reflect your choice (Yes changes the option to Always, No changes the option to Never).
o
Always. Always rebuilds assemblies when opening.
o
Never. Opens assemblies without rebuilding.
•
Automatically convert drawing views to draft quality when unloading components. Changes drawing views from high quality to draft quality when you set the model views to lightweight.
•
Mate animation speed. Enables animation of mates and controls the speed of the animation. When you add a mate, click Preview or OK in the PropertyManager to see an animation of the mate you just created. Move the slider to Off to disable mate animation.
Enable clipping for zoom limitation in Windows ME Lets you select a portion of the model and zoom in on only the selected portion. On the Windows ME operating system, there is a limit beyond which you cannot zoom in on a model. You can zoom in on small details very closely, but the display is slower. Update mass properties while saving document Updates the mass properties information when you save a document. This means that the next time you access the mass properties, the system does not need to recalculate them (if the document has not changed). The updating may slow performance, however. Use shaded preview Shows shaded previews to help you visualize features you create. You can rotate, pan, zoom, and set standard views while maintaining the shaded preview.
Use Software OpenGL Disables graphics adapter hardware acceleration and enables graphics rendering using only software. For many graphics cards, this results in slower performance. Select this option only if instructed to do so by technical support. If you select Use Software OpenGL, SolidWorks changes some of your options settings for optimum software performance. Click here to see the options that change. You can override any of these settings if desired. This option is automatically selected and unavailable for change if your graphics card does not support hardware acceleration, or does not support it for the current combination of resolution, number of colors, refresh rate, and so forth. Go To Image Quality Click Go To Image Quality to switch to the Document Properties - Image Quality dialog box to set image quality options.
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Performance Settings Use Software OpenGL selected •
Turn on: o
•
High quality for normal view mode
Turn off: o
High quality for dynamic view mode
o
Display shaded planes
o
Use gradient background
o
Display plane when shaded
o
Shadows
Use Software OpenGL cleared •
•
Turn on: o
High quality for normal view mode
o
High quality for dynamic view mode
o
Use gradient background
o
Display shaded planes
o
Shadows
Turn off Display plane when shaded
Assembly Options Lets you set the behavior for dragging components in an assembly. To customize Assemblies options:
1.
Click Tools, Options, System Options, Assemblies.
2.
Select Move components by dragging to allow components to move or rotate within their degrees of freedom when you drag them in the graphics area. When cleared, you can still move or rotate a component with the Move with Triad function or the Move Component
3.
and Rotate Component
tools.
Click OK.
Large Assembly Mode Options Lets you set options for Large Assembly Mode. Most of the options under Large Assembly Mode are duplicated on other pages of the Systems Options dialog box. The selections you make under Large Assembly Mode apply only when Large Assembly Mode is on. Set options for normal use (with Large Assembly Mode off), under Performance, Display/Selection, and so on. When Large Assembly Mode is on, you cannot access duplicated options except under System Options, Large Assembly Mode. To customize Large Assembly Mode options:
1.
Click Tools, Options, System Options, Large Assembly Mode.
2.
Change the settings then click OK.
General Options •
Large assembly threshold. This is the number of resolved components above which Large Assembly Mode activates or sends a message, depending on your settings. If you have already activated Large Assembly Mode, the threshold is ignored.
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Chapter 17 SolidWorks Options
•
Automatically activate Large Assembly Mode: o
Prompt. When you reach the threshold, a message gives you the option to activate Large Assembly Mode.
o
Never. Ignore the threshold.
o
Always. When you reach the threshold, Large Assembly Mode automatically activates.
NOTE: If you save an assembly with Large Assembly Mode active, SolidWorks ignores the Automatically activate Large Assembly Mode option the next time you open the assembly. The assembly opens with Large Assembly Mode active. •
Check out-of-date lightweight parts: o
o
o
Don't check. Load without checking for lightweight components. Select for the fastest performance. Indicate. Load the assemblies and mark them with an icon if the assemblies contain an out-ofdate part, even if the assembly is not expanded. You can right-click on an out-of-date top level assembly and select Set Out-of-date Lightweight to Resolved. Always resolve. All out-of-date components are resolved during loading.
•
Automatically load components lightweight. Loads your assembly with lightweight components.
•
Update mass properties while saving document. Recalculates the mass properties on save. Clear to improve performance.
•
Save auto recover info every. Specify how often to automatically save model information. Clearing this check box improves performance, but disables automatic save of your model.
Display Options To improve performance do the following:
•
Clear: o
o
o
•
Dynamic highlight from graphics view. Enables highlighting of entities in the graphics area as you move your cursor over the graphics area. Anti-alias HLR edges in shaded and fast HLR/HLV modes
o
Display shadows in shaded mode High quality transparency for normal view mode
o
High quality transparency for dynamic view mode
o
Use RealView graphics
o
•
Dynamic highlight from Feature Manager. Enables highlighting of entities in the graphics area as you move your cursor over the FeatureManager design tree.
Select: o
Remove detail during zoom/pan/rotate
o
Hide all planes, axes, sketches, curves, annotations, etc.
Select Only on demand in Curvature generation.
Drawings Options To improve performance do the following:
•
•
Clear: o
Show contents while dragging drawing view.
o
Smooth dynamic motion of drawing view.
o
Automatically load models for detached drawings.
Select: o
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Automatic hiding of components on view creation.
•
Select Hidden Lines Removed, Shaded, or Shaded with Edges in Default display style for new views.
•
Select Draft Quality in Default display quality for new views.
External References - Options Specifies how part, assembly, and drawing files with external references are opened and managed. To specify how SolidWorks manages references to external files:
1.
Click Tools, Options, System Options, External References.
2.
Change the settings then click OK.
External References •
Open referenced documents with read-only access. Specifies that all referenced documents will be opened for read-only access by default.
•
Don’t prompt to save read-only referenced documents (discard changes). Specifies that when a parent document is saved or closed, no attempt will be made to save its read-only, referenced documents.
•
Allow multiple contexts for parts when editing in an assembly. You can create external references to a single part from more than one assembly context. However, any individual feature or sketch within the assembly may only have one external reference.
•
Load referenced documents. Specifies whether to load the referenced documents when you open a part that is derived from another document (such as a base part, derived component part, part with a cavity feature, and so on.) o
o o
o
Prompt. Ask about loading externally referenced documents each time you open a document with external references. All. Opens all of the externally referenced documents. None. Does not open any of the externally referenced documents. External references may be shown as out of context until you open the externally referenced documents. Changed Only. Opens only the externally referenced documents that have changed since the last time you opened the original document.
•
Search file locations for external references. Specifies that SolidWorks should search the Referenced Documents list of folders in the File Locations Options dialog box. When cleared, the list is ignored.
•
Update out-of-date linked design tables to. Determines what happens to linked values and parameters if the model and the design table are out-of-sync. o
Prompt. The software prompts you when you open a document with a design table that is out-ofsync with the model.
o
Model. The design table updates with the model's values.
o
Excel. The model updates with the design table's values.
Assemblies •
Automatically generate names for referenced geometry. When this option is off, you can mate to parts for which you have read-only access because you are using the internal face IDs of the parts. Unless you will use component replacement, leave this option off, especially in a multi-user environment. When this option is on, you automatically create surface identifiers (for example: Face1, Face2) at the time you mate the part, therefore you need write access to the part, in most cases. Turn this option on if you intend to do component replacement using the same surface identifiers, remembering that you need write access to the parts you are using. (Rename the corresponding edges and/or faces on the replacement component to match the edge/face names on the original part.)
•
Update component names when documents are replaced. Clear this option only if you use the Component Properties dialog box to assign a component name in the FeatureManager design tree that is different from the filename of the component.
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Chapter 17 SolidWorks Options
Default Templates You can specify the folder and template file for automatically created parts, assemblies, and drawings. For example, when you import a file from another application or create a derived part, the default template is used for the new document. To specify a folder for document templates:
1.
Click Tools, Options.
2.
On the System Options tab, click Default Templates. The current path and folder for part, assembly, and drawing templates appears.
3.
To change the folder for one of the template types, click the browse button window.
next to the path display
In the New SolidWorks Document dialog box, select the new default template, then click OK. If you need to add a template that does not appear in this dialog box, add the template location with the File Locations option. 4.
5.
Select one of the following options: •
Always use these default document templates
•
Prompt user to select document template
Click OK.
File Locations Lets you specify and locate referenced documents. Folders are searched in the order in which they are listed in the Folders list. If one or more folders are selected in the Folders list, you can Delete existing folders and use Move Up or Move Down to change the folder search order. You can always Add new folders. To display file locations:
1.
Click Tools, Options, System Options, File Locations. The Show folders for box displays search paths for files of various types: •
Bend Tables
•
Library Feature Files
•
Revision Table Templates
•
Blocks
•
Macros
•
Sheet Formats
•
BOM Templates
•
Macro Feature Files
•
SolidWorks Journal File
•
Color Swatches
•
Material Databases
•
Textures
•
Custom Property File
•
Palette Assemblies
•
Web Folders
•
Dimension/Annotation Favorites
•
Palette Features
•
Weldment Profiles
•
Document Templates
•
Palette Forming Tools
•
Weldment Cut List Templates
•
Hole Callout Format File
•
Palette Parts
•
Weldment Property File
•
Hole Table Templates
•
Referenced Documents
When you select a file location for Macros, and then you run a macro, the software looks for a macro in the specified location. For instance, when you click Tools, Macro, Run, the Run Macro dialog box opens to the file location you specified. 2.
17-16
Click OK.
To add a folder for a file location:
1.
Click Tools, Options, System Options, File Locations.
2.
Select a folder type in Show folders for.
3.
Click Add to add a new directory path to the list.
4.
Browse in the Browse For Folder dialog box to locate the folder. If desired, click New Folder to create a new folder.
5.
Click OK.
To delete a folder from a file location:
1.
Click Tools, Options, System Options, File Locations.
2.
Select a folder type in Show folders for.
3.
Select the path in Folders and click Delete. After you click Delete, the path is gone. Click Cancel to undo the deletion, if necessary.
To change the folder search order in a file location list:
1.
Click Tools, Options, System Options, File Locations.
2.
Select a folder type in Show folders for.
3.
Select the path in Folders and click Move Up or Move Down as necessary. The paths for Referenced Documents are searched only if Search file locations for external references is selected in Tools, Options, System Options, External References. The paths for Palette Parts, Palette Forming Tools, Palette Features, Blocks, Custom Property Files, Macros, Macro Feature Files, and SolidWorks Journal Files are always searched, whether Search file locations for external references is selected or not.
FeatureManager Options Lets you set the default system options related to the FeatureManager design tree. To set the default FeatureManager design tree options:
1.
Click Tools, Options.
2.
On the System Options tab, click FeatureManager.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
FeatureManager Options •
Scroll selected item into view. Specifies that the FeatureManager design tree should automatically scroll to display the feature icon that is related to the selected items in the graphics area. If you have a very complex part or assembly, you may want to turn this option off. Then, when you want the FeatureManager design tree to scroll to a feature you can right-click the feature and select Go To Feature (in Tree).
•
Name feature on creation. When you create a new feature, the feature name in the FeatureManager design tree is automatically selected and ready for you to enter a name of your choice.
•
Arrow key navigation. Lets you use the arrow keys to traverse the FeatureManager design tree, and expand or collapse the design tree and its contents, as follows:
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Chapter 17 SolidWorks Options
•
o
Up arrow - Scrolls up the design tree
o
Down arrow - Scrolls down the design tree
o
Left arrow at top of design tree - Collapses the design tree
o
Right arrow at top of design tree - Expands the design tree
o
Left arrow on an item in the tree - Collapses the item to hide its contents
o
Right arrow on an item in the tree - Expands the item to display its contents, if any
Dynamic highlight. Specifies that the geometry in the graphics area (edges, faces, planes, axes, and so on) is highlighted when the pointer passes over the item in the FeatureManager design tree.
Spin Box Increments Lets you set the default incremental changes to the spin box values. To set the default spin box increment value:
1.
Click Tools, Options.
2.
On the System Options tab, click Spin Box Increments.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
Length increments Specifies the number of units added or subtracted when you click a spin box arrow to change a linear dimension value. You can set the values in English units or Metric units. Angle increments Specifies the number of degrees added or subtracted when you click a spin box arrow to change an angular dimension value.
View Rotation Options Lets you set the system defaults for view rotation. To set the default view rotation:
1.
Click Tools, Options.
2.
On the System Options tab, click View Rotation.
3.
Change the settings listed below and click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box.
Arrow keys Specifies the angle increment for view rotation when you use the arrow keys to rotate the model. Mouse speed Sets the speed of rotation when you use the mouse to rotate the model or assembly component. To get finer control and slower rotation, move the slider to the left. View animation speed Enables the animation-like display of changes in view orientation for part and assembly documents only. When you change from one view to another, the change occurs showing an animated sequence of frames between the old view and the new view. Move the slider to adjust the animation speed between Fast (default setting) and Slow. Move the slider to Off to turn off view animation.
17-18
View animation occurs when you change views, including the following: •
View orientation commands (For example, Front, Isometric, and so forth)
•
Zoom to Area, Zoom to Fit, Zoom to Selection
•
Shift+ arrows to rotate 90 degrees
•
Any command where the system changes the view orientation automatically, such as extruding the first sketch of a part NOTE: View animation might not always work for extremely large-sized or complex documents.
Backup Options Lets you choose how often you want to make backup copies of your files and where you want to store the backups. To set the default options for making backups:
1.
Click Tools, Options.
2.
On the System Options tab, select Backups.
3.
Choose from the following options: •
Save auto recover info every
o o
In a part or assembly document, a change is a rebuild or an action that requires a rebuild, such as the addition of a feature. To disable auto recover, clear the check box. Auto recover files are saved in <default drive>:\
•
Number of backup copies per document. Specify the number of backup copies you want to save of part, assembly, or drawing documents. Scroll to 0 (for none) or up to 10.
•
Save backup files in the same location as the original. Select this check box to save the backup file in the same location as the original file. Backup files use the naming convention: Backup of <document name>.sld*.
•
Save backup copies in directory. Name a directory where all backup copies are stored by default. Type the path or use click to browse to the directory to use. This option is disabled if Save backup files in the same location as the original is selected.
4.
Click OK to accept the changes. Click Reset All to return to the installed system defaults, or click Cancel to discard the changes and exit the dialog box. NOTE: You should examine backup directories occasionally to make sure your backup copies do not use too much space.
Document Properties Detailing Options Set options for detailing in the active document. You can also set the detailing options in Document Templates. To set detailing properties:
1.
Click Tools, Options, Document Properties, Detailing.
2.
Change the detailing options to meet your standard detailing style, and click OK.
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Chapter 17 SolidWorks Options
Dimensioning Standard Select a dimensioning standard from the list: ISO, ANSI, DIN, JIS, BSI, GOST, or GB. The standard affects some detailing styles, such as weld symbols, surface finish symbols, and dimension arrows. Dual dimensions display. When selected, dimensions are displayed in two kinds of units. Choose whether the second dimension is displayed On top or On the right. Fixed size weld symbols. When cleared (default), the size of the weld symbol is scaled according to the dimension font size, and the size of the weld symbol changes if the dimension font size changes. When selected, the size of the weld symbol is dependent on the selected dimensioning standard, and the size of the weld symbol remains constant regardless of changes to the dimension font size. This option is not available for the GOST dimensioning standard. Display datums per 1982. Select this checkbox to use the 1982 standard for the display of datums. This option is available only if you use the ANSI dimensioning standard. Trailing zeros. Select one of three settings: •
Smart. Trailing zeros are trimmed for whole metric values. (Conforms to ANSI and ISO standards.)
•
Show. Dimensions have trailing zeros up to the number of decimal places specified in Tools, Options, Document Properties, Units.
•
Remove. All trailing zeros are removed. Tolerances are not affected by this option.
Alternate section display. The section line does not display across the drawing view; the arrow lines stop at the boundaries of the section cut. Centerline extension. This value controls the centerline’s extension length beyond the section geometry when it is in a drawing view. The default value is set according to standards, but you can change it. Select the value in the edit box and enter a new value. When a centerline length is modified, the new length is used the next time the section is rebuilt. Auto insert on view creation The following items are inserted automatically into all appropriate entities in new drawing views. •
Center marks. Add to arcs and circles.
•
Centerlines. Add to model faces with parallel edges.
•
Balloons. Add to all visible components, without duplicates in multiple views.
•
Dimensions marked for drawing. Add dimensions to models, without duplicates in multiple views. The dimensions are indicated in the part sketches as Mark for drawing.
Extension lines Gap. Set a value for the distance between the model and dimension extension lines. Beyond dimension line. Set a value for the length of the extension line beyond the dimension line. Example
17-20
Datum features Display type. Select a default (Per Standard, Square, or Round (GB)) to appear in the Datum Feature PropertyManager. Next label. Type a letter to start the labels for datum feature symbols. Successive labels are in alphabetic order. Only uppercase letters are accepted. Surface finish symbols Display symbols per 2002. For ISO and related drafting standards, display surface finish symbols per 2002 standards. Center marks Size. Specifies the size of Center Marks, used with arcs and circles in drawings. Extended lines. Specifies whether the center mark lines are displayed. Centerline font. When selected, the lines in the center mark use the font specified for centerlines. Break lines Specify the following properties of break lines in a Broken View in a drawing. •
Gap. The distance between the break lines when they are inserted and after you break the view.
•
Extension. The length of the break lines beyond the model geometry.
Automatic update of BOM. When selected, if a Bill of Materials exists in a drawing, it automatically updates when relevant changes are made to the model. If you edit linked custom properties in a BOM and then rebuild the drawing, the properties are reset to the values in the Summary Info dialog box when this option is selected. Some manual edits are lost when the BOM is updated. Section Display Types Alternate Section Display Normal Section Display
Dimensions Options You can set options for dimensioning in the active document. To set dimensioning options:
1.
Click Tools, Options, Document Properties, Dimensions.
2.
Change the dimensioning options to meet your standards, and click OK.
Check Boxes Add parentheses by default. Reference dimensions in drawings are displayed within parentheses. Snap text to grid. The placement of dimension text snaps to the grid in a drawing or a sketch. Center between extension lines. Dimension text is centered between its extension lines. Include prefix inside basic tolerance box. For ANSI standard, any prefix added to a dimension with basic tolerance appears inside the tolerance box. Automatically jog ordinates. Ordinate dimensions are automatically jogged when inserted.
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Chapter 17 SolidWorks Options
Offset distances Specify values for the distances between baseline dimensions. •
•
From last dimension (B). The distance between dimension lines. This value is used for baseline dimensions and for Align Parallel/Concentric . SolidWorks automatically doubles the offset distance for dimensions displayed with tolerances. From model (A). The distance between the model and the first dimension for baseline dimensions. (Not used with Align Parallel/Concentric).
Arrows Style. Specify the default style of dimension arrows by selecting from the illustrated list. Outside, Inside, or Smart. Specify the placement of dimension arrows in relation to the extension lines. Smart arrows appear outside of extension lines if the space is too small to accommodate the dimension and the arrowheads. Display 2nd outside arrow (Radial). Check this option to specify that two outside arrows be displayed with radial dimensions. Arrows follow position of text (Radial). •
Arrow placement must be set to Smart.
•
When you drag radial dimensions inside or outside arcs or circles, the arrowheads move inside or outside with the dimensions.
Break dimension extension/leader lines Gap. Specify the gap in extension and leader lines when they are broken. Break around dimension arrows only. You can choose to have breaks occur only where the lines cross arrows. For ANSI standard, this option is selected by default. Bent leader length Specify the length of bent leaders. Text alignment Select Horizontal and Vertical default alignment for multiple lines of dimension text. Vertical alignment specifies where the leader is located relative to the text and applies only to certain standards, such as ANSI. Angle/linear-angled Display ANSI standard only. Select Use bent leaders to use bent leaders for: •
Dimensions of angles
•
Angular display of linear dimensions
Leaders Specify the alignment of dimension text with respect to the leaders. Precision Specify the dimension precision for the dimension value and tolerance values for Primary Units, Angular Units, and Alternate Units.
17-22
Tolerance Specify the type of tolerance, variation, font, and so on. See Dimension Tolerance Properties. You can set Tolerance display to None and then set the variations and font to defaults for the current document. When you modify the properties of a dimension, the default tolerance settings will be those set in these options.
Notes Options You can set note options for the active document. To set note options for the active document:
1.
Click Tools, Options, Document Properties, Notes.
2.
Choose from the following options, then click OK.
Text alignment Select Left, Right, or Center alignment for note text. Leader anchor Specify to which side of the note the leader should attach: Left, Right, or the side Closest to the attachment point. Leader style •
Leader style. Select Straight, Bent, or Underlined.
•
Leader length. Specify the distance between the leader bend and the text of the note for bent leaders.
Border •
Style - Select a style from the list. None results in text with leader, if a leader is specified, but no border enclosing the text.
•
Size - Select Tight Fit, expandable to tightly fit the text, or select a size to accommodate from one to five characters.
Balloons Options Set the default properties of balloons. To set default balloon properties:
1.
Click Tools, Options, Document Properties, Balloons.
2.
Specify the options described below, then click OK.
Single balloon Style. Select a style from the list. None results in text with leader, but no border enclosing the balloon. Size. Select a balloon size of Tight Fit, expandable to tightly fit any custom text you type in, or select a size to accommodate from one to five characters. Stacked balloons Style. Select a style from the list. None is not available for Stacked balloons. Size. Select a balloon size of Tight Fit, expandable to tightly fit any custom text you type in, or select a size to accommodate from one to five characters.
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Chapter 17 SolidWorks Options
Balloon text Upper. Select Item Number, Quantity, or Custom from the list for the upper section of a Circular Split Line balloon or for the whole balloon of all other styles. Lower. If the balloon style is Circular Split Line, the Lower box is available for you to select Item Number, Quantity, or Custom from the list. If you select Custom text, a window opens in the Balloon or Stacked Balloon PropertyManager for typing your text. Bent leaders Use bent leaders. Select for balloons to use bent leaders by default. Leader length. Enter a default value for the length of the leader nearest the balloon. AutoBalloon Layout Select a layout as the default for inserting autoballoons: Square Circular Top Bottom Left Right
Arrows Options You can set display options for arrows. The default options vary depending on the drafting standard specified in Tools, Options, Document Properties, Detailing. To set the options for displaying arrows:
1.
Click Tools, Options, Document Properties, Arrows.
2.
Specify the options described below, then click OK.
Size Specify the Height and Width of arrowheads, and the Length of the complete arrows, for leaders on dimensions, notes, and other annotations. Section/View Size Specify the Height and Width of arrowheads, and the Length of arrows, for section view lines and on view arrows (in auxiliary views, for example).
17-24
Attachments Specify the arrowhead styles to be used depending on where the leader is attached.
Virtual Sharp Display Options You can set display options for virtual sharps. To set the display options for virtual sharps:
1.
Click Tools, Options, Document Properties, Virtual Sharps.
2.
Select a style for the display of virtual sharps, and click OK.
Annotations Display Options You can specify the default display of annotations and select the types of annotations that you want to display by default. To set the default options for displaying annotations:
1.
Click Tools, Options, Document Properties, Annotations Display.
2.
Choose from the options described below, then click OK.
Display filter. To specify the annotation types to display by default, select Display all types, or clear Display all types and select individual types. Cosmetic threads
Shaded cosmetic threads
Datums
Geometric tolerances
Datum targets
Notes
Feature dimensions
Surface finish
Reference dimensions
Welds
Text scale (For part and assembly documents). When Always display text at the same size is cleared, you can specify a scale for the default size of annotation text.
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Chapter 17 SolidWorks Options
Select from the following options: •
Always display text at the same size. When selected, all annotations and dimensions are displayed at the same size regardless of zoom. Note that drawings have this option disabled and always zoom the text height.
•
Display items only in the view in which they are created. When selected, any annotation is displayed only when the model is viewed in the same orientation as when the annotation was added. Rotating the part or selecting a different view orientation removes the annotation from the display.
•
Display annotations / Display assembly annotations. When selected, all annotation types that are selected in the Display filter are displayed. For assemblies, this includes not only the annotations that belong to the assembly, but also the annotations that are displayed in the individual part documents.
•
Use assembly’s setting for all components. When selected, the display of all annotations matches the setting for the assembly document, regardless of the setting in the individual part documents. Use this option along with the Display assembly annotations check box to display different combinations of annotations.
•
Hide dangling dimensions and annotations. If you delete features in parts and assemblies, this option automatically hides the dangling dimensions and annotations in the drawings. If you suppress features, SolidWorks automatically hides dangling reference dimensions in the drawing; this option automatically hides dangling annotations.
•
If you use JIS dimensioning standards, specify the JIS surface finish size (either 1, 2, or 3 Characters or Custom Scale). If you select Custom Scale, specify the scale value in the Scale box.
Annotations Font Options You can specify the default font for various types of annotations (Note, Dimension, Detail, Section, View Arrow, Surface Finish, Weld Symbol, Tables, and Balloon). The font for Detail applies to the label on the detail circle, but not to the label on the detail view. The font for Section applies to the label on the section line, but not to the label on the section view. The labels for detail and section views are Notes and use the font for Note. To specify the default font for a type of annotation:
1.
Click Tools, Options, Document Properties, Annotations Font.
2.
Select an Annotation type in the list. The Choose Font dialog box appears.
3.
Select a Font, Font Style, Height, and Effect, then click OK.
4.
Repeat steps 2 and 3 to specify default fonts for other annotation types as needed, then click OK.
Tables Options Set options for tables in the active drawing document. To set options for tables:
1.
Click Tools, Options, Document Properties, Tables.
2.
Choose from the following options, then click OK.
Hole Table
Origin indicator . Specify the appearance of the indicator of the origin from which the software calculates hole positions by selecting a standard. Standard. Select a specific standard or Per Standard (the standard set in Detailing Options). Tag angle/Offset from profile center. Specify the position from the hole profile center of the tag that the software generates to identify each hole.
17-26
•
Angle
•
Offset
. Angle from a vertical line through the center of the hole. . Distance from the hole profile.
Alpha/numeric control. Specify whether the hole tag is alphabetic or numeric. Scheme. •
Combine same tags. Merge cells with the same tags (A1, A2, and so on as A). All the holes labeled with the same tag are part of a pattern, so the hole sizes are the same. The Size cells are merged and locations are not listed.
•
Combine same size. Merge cells of same size holes.
Location precision. The precision at which the X and Y locations of the holes are displayed. Show hole centers. An asterisk identifies the center of each hole. Automatic update of hole table. The table data updates when the model changes. Revision Table Symbol shapes. Select from a circle, square, triangle, or hexagon for the revision symbol. Alpha/numeric control. Specify whether the revision is alphabetic or numeric. •
Start from where user left. If you change control from alphabetic to numeric or vice versa, previous revisions remain as they are.
•
Change all. If you change control from alphabetic to numeric or vice versa, previous revisions (except any you have edited) change to the new format.
Bill of Materials Table Zero quantity. Select whether to display zero quantities with a dash (-) or a zero (0), or to leave the cell blank. Missing component. •
Keep the row for missing component.
•
Display with strikethrough text. Display text in rows for missing components with strikethrough.
View Labels Options Set options for detail, section, and auxiliary view labels in the active drawing document. To set options for view labels:
1.
Click Tools, Options, Document Properties, View Labels.
2.
Choose from the following options, then click OK.
The options for each type of view are the same except for the text under Name, which is DETAIL, SECTION, or AUXILIARY. Detail View, Section View, and Auxiliary View Per standard. The options below follow the standard specified in Tools, Options, Document Properties, Detailing (ANSI, ISO, and so on) and are not available for editing. Name. Select a title to appear in the view label. Label. Select whether the label letter corresponding to the label on the parent view appears in the view label. Scale. Select whether the word SCALE appears next to the scale.
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Chapter 17 SolidWorks Options
Delimiter. Select the delimiter between the two scale numbers and whether the scale appears in parentheses. If you select #X, the number in (#) can be an integer or a real number. Display. Display the view label with name and label stacked on top of the scale (Stacked), or all data on the same line (In-line).
Grid and Snap Options You can display a sketch grid in an active sketch or drawing and set options for the grid display and snap functionality. The options for grid spacing and minor grid lines per major lines apply to the rulers in drawings as well as to sketching and drawing grid lines. To set grid and snap options for the active document:
1.
Click Grid/Snap
on the Sketch toolbar, or click Tools, Options, Document Properties, Grid/Snap.
2.
Select from the options described below.
3.
Click OK.
Grid •
Display grid. Turns the sketch grid on or off.
•
Dash. Toggles between solid and dashed grid lines.
•
Automatic scaling. Automatically adjusts the display of the grid when you zoom in and out.
•
Major grid spacing. Specifies the space between major grid lines.
•
Minor-lines per major. Specifies the number of minor grid lines between major grid lines.
Snap •
Snap only when grid is displayed. Turns on grid snap only when Display grid is selected.
•
Snap to points. Turns snap on. When snap is on, points that you sketch or drag snap to the nearest intersection of grid lines (or to intermediate points, if Snap points per minor is greater than 1).
•
Snap points per minor. Sets the number of snap points between minor grid lines.
•
Snap to angle. Specifies that sketched lines snap to a pre-defined angle. Specify the angle to which sketched lines should snap. The inferencing pointer displays the specified angle as you sketch.
Units Options Lets you specify units for the active part, assembly, or drawing document. If you use small units such as angstroms, nanometers, microns, mils, or microinches, it is helpful to create templates as the basis for documents that use the units. The templates could include settings such as:
17-28
•
grid spacing
•
dimension witness line gap and bent leader length
•
dimension offset distances
•
note bent leader length
•
balloon bent leader length
•
arrow size and section view arrow size
•
text scale and Always display text at the same size
•
material density
To set units for the active document:
1.
Click Tools, Options, Document Properties, Units.
2.
Select from the options described below.
3.
Click OK.
Unit system Displays a unit system: •
MKS (meter, kilogram, second)
•
CGS (centimeter, gram, second)
•
MMGS (millimeter, gram, second)
•
IPS (inch, pound, second)
•
Custom. Lets you set the Length units, Dual units, Angular units, Density units, and Force.
Length units Displays the length units. If you set Unit system to Custom, select the units and set the Decimal places. Otherwise, you can only set Decimal places. If you select microinches, mils, inches, or feet & inches, select Decimal or Fractions. If you select Fractions, the following options are available: •
Round to nearest fraction
•
Denominator (Only dimensions that are evenly divisible by this denominator are displayed as fractions.)
If you select feet & inches, you can select Convert from 2'4" to 2'-4" format. The format for feet & inches in the SolidWorks software is 2'-4". If you import a document in the 2'4" feet & inches format, you can convert the document to 2'-4". Once you have converted the document to 2'-4" format, you cannot convert back to the 2'4" format. Dual units Displays a second type of units just as you specify the Length units. To show dual units in the SolidWorks software, select Dual dimensions display in the Detailing options. Angular units Displays the angular units. If you select Degrees or Radians, set the Decimal places. Density units Displays the Mass and Per unit volume units. Force Displays the force units.
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Chapter 17 SolidWorks Options
Document Colors Lets you set model, feature, and view mode colors for the active part or assembly document. NOTE: Document Colors is not available when you have a drawing document active. To set model, feature, and view mode colors:
1.
Click Tools, Options.
2.
On the Document Properties tab, select Colors.
3.
In the Model\Feature colors box, select the feature type or view mode type for which you want to edit the color representation. If you are working with an assembly, the only color choices are Shading and Hidden. These are the display colors for Shaded mode and Hidden Lines Visible mode.
4.
Click Edit to change the color used to display the selected item. Select a color from the Color palette or click Define Custom Colors and define a new color.
5.
Click OK and view the selection in the preview box.
6.
In an assembly, if you selected a color to display in Hidden mode, the Advanced button is available. You can select additional display qualities such as Shininess, Transparency, and so on.
7.
Additionally, you have the following options:
8.
•
Reset All To SolidWorks Defaults. Click this button to restore the original default color settings.
•
Apply same color to wireframe, HLR and shaded. Select this check box to use the same color for these view modes. (This option is available only for parts.)
•
Ignore feature colors. Select this check box to specify that feature colors are not used. (This option is available only for parts.)
•
Curvature. Click this button to define the colors associated with the radii of curvature.
•
Go To System Colors. Click this button to switch to the System Options - Colors dialog box.
Click OK to accept your changes, or click Cancel to exit the dialog box without saving the changes.
Material Properties Options Lets you set crosshatch options and material density for the active part. These options are not available for drawing or assembly documents. To set material properties options:
1.
In a part document, click Tools, Options.
2.
On the Document Properties tab, click Material Properties.
3.
Type the material density in the Density box. NOTE: You can type the density value with any units. For example, if the units of the part are grams and millimeters, you can use a density value of pounds and inches. The software converts the value to the document’s units when you click OK.
4.
5.
In the Area Hatch/Fill box, select from the following: •
None
•
Solid
•
Hatch
If you select Hatch, do the following: •
Select a crosshatch pattern from the Pattern list.
•
If necessary, set the Scale and Angle of the crosshatch pattern.
A preview of the pattern is displayed in the preview box.
17-30
6.
Click OK. NOTE: You can also change the Density from the Measurement Options dialog box. Click Tools, Mass Properties, Options, to access this dialog box.
Line Font Options You can set the style and weight of lines for various kinds of edges in drawing documents only. NOTE: The line font options are available only if the active document is a drawing document. To set the style and weight of lines in drawings:
1.
Click Tools, Options, Document Properties, Line Font.
2.
Change the settings for one or more type of edge, and click OK.
Type of edge Select an edge type from the list: Visible Edges, Hidden Edges, Sketch Curves, and so on. Style Choose a style from the list: Solid, Dashed, Phantom, Chain, and so on. Thickness Choose a thickness from the list: Normal, Thin, Thick, and so on. Preview Displays the selected line font.
Image Quality Lets you select the display quality that is most efficient for you. To set the image quality options for the active document:
1.
Click Tools, Options, Document Properties, Image Quality.
2.
Select from the following options, then click OK.
Shaded and draft quality HLR/HLV resolution Controls the tessellation of curved surfaces for shaded rendering output. A higher resolution setting results in slower model rebuilding but more accurate curves. When Draft Quality HLR/HLV Shaded settings control Shaded With Edges Lines Visible
, and Wireframe
, Shaded
, Hidden Lines Removed
is turned on, the , Hidden
views.
•
Low (faster) High (slower). Controls the image quality resolution settings. Move the slider to adjust the settings, or type a value for Deviation.
•
Deviation. Reports the maximum chordal deviation in effect at the various tuning levels. The chordal deviation value is greater at the Low (faster) setting, and decreases as the resolution becomes more finely tuned at the High (slower) setting.
•
Optimize edge length (higher quality, but slower). Increases image quality if, after you move the slider to the highest setting, you still want higher image quality. This option causes slower system performance and increased file size.
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Chapter 17 SolidWorks Options
•
Apply to all referenced part documents (assemblies only). Applies the settings to all of the part documents referenced by the active document.
•
Save tessellation with part document (parts only). Saves disk space and decreases save time when the part has detailed surfaces where the tessellation data is larger than the size of the geometry on disk. When you clear this option, nothing is displayed when the part is opened in: o
View-Only mode
o
SolidWorks Viewer
o
eDrawings (if you open the part directly in eDrawings)
Additionally, re-opening the part could take longer because the display is regenerated. Wireframe and high quality HLR/HLV resolution Controls the image quality of model edges in drawings. When Draft Quality HLR/HLV the Wireframe settings control Hidden Lines Removed
, Hidden Lines Visible
is turned off, , and Wireframe
views. Low (faster) High (slower). Increases image quality. Move the slider to Low (faster) if you want to redraw the screen more quickly and the display quality is not of great importance; move the slider to High (slower) for high display quality, but a slower redraw. If you notice problems with your HLR image display, move the slider to the right. Go To Performance Click Go To Performance to switch to the System Options - Performance dialog box.
Plane Display You can set the following plane display options for part and assembly documents: •
Face color
•
Transparency
•
Intersection display and color
NOTE: You must enable the Display shaded planes option to display shaded planes. To set the plane display:
17-32
1.
Open a part or assembly document.
2.
Click Tools, Options. On the Document Properties tab, click Plane Display.
3.
Under Faces, set the following options: •
Front Face Color. Displays the Color dialog box that you use to set the front face color of planes.
Front face color
Back face color
•
Back Face Color. Displays the Color dialog box that you use to set the back face color of planes.
•
Transparency. Controls the plane transparency (0% displays a solid face color; 100% displays no face color).
0% transparency
75% transparency
100% transparency
NOTE: Edges take the same color as the front and back faces, are not transparent, and are always displayed. 4.
Under Intersections, set the following options: •
Show intersections. Select or clear the Show intersections check box to display or hide the intersection of planes
Plane intersection lines displayed • 5.
Plane intersection lines hidden
Line Color. Displays the Color dialog box that you use to set the plane intersection line color.
Click OK to accept the changes, or Cancel to discard the changes and exit the dialog box.
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Chapter 17 SolidWorks Options
17-34
Index
Symbols $PRP 12-41 Numerics
1:1 scale output 13-10 2D IGES geometry 13-27 2D sketches in drawings 11-10 new 3-3 2D to 3D conversion 4-1 align sketches 4-6 create new sketch 4-10 extract sketches 4-5 extrude 4-7 import drawings 4-4 repair sketch 4-10 select chain 2-62 2D to 3D Toolbar 2-22 3 point arcs 3-59 3D curves in IGES 13-11, 13-29 3D models from 2D 4-1 3D sketches 3-68 3D frame points 3-51 coordinate systems 3-74 dimensions 3-75 Hole Wizard 6-77 line snap 3-69 lines 3-69, 3-70 sketch points 3-73 space handles 3-75 splines 3-49, 3-71 virtual sharps 3-75 A
absorbed feature 2-35 accelerator keys. See shortcut keys 2-18 ACIS files 13-17 edit imported features 13-4 export options 13-9 export units 13-9 export version 13-9 import 13-3, 13-7 import geometry 13-3 import options 13-7 import units 13-7 activate 11-5
SolidWorks 2004 Reference Guide
automatic view activation 17-4 configurations 10-1, 10-8 drawing sheets 11-4 drawing views 11-8 layers 11-58 add 15-28 corner trim 15-44 folders 2-50 forming tools to sheet metal parts 15-28 library features to parts 14-4 loft sections 6-104 palette features to assemblies 14-12 palette features to parts 14-10 relations in sketches 3-41 add-ins. See also translators eDrawings 13-24 PDF Files 13-33 SolidWorks MTS 13-39 advanced 9-68 color properties 7-9 component selection 9-68 mates 9-22, 9-23, 9-24 show/hide components 9-67 advanced smoothing 6-191 align 11-45 annotations 12-34 collinear/radial dimensions 12-24 concentric dimensions 12-23 dimensions 12-22 drawing views 11-49 grid 3-13 ordinate dimensions 12-17 parallel dimensions 12-23 sketches 4-6 with end faces 6-190 Align toolbar 2-22 align. See mating 9-13 aligned section views 11-42 alignment 11-45 aligned section views 11-42 auxiliary views 11-28 break view alignment 11-49 detail views 11-30 dimension text 17-21 drawing views 11-49
Index-1
mates 9-17 model views 11-19 projected views 11-26 relative to model views 11-22 section views 11-37 standard 3 views 11-17 alternate position views 11-43 ambient light 7-46 anchors 12-77 bill of materials 12-77 leaders 12-60, 12-64, 12-69, 17-23 tables 11-5, 12-77 angle mates 9-14, 9-19, 9-23 angular dimensions 3-37 between three points 3-37 between two lines 3-37 animate 13-24 drawings 13-24 mates 17-10 annotations 12-31 align 12-34 ANSI weld symbol 12-65 area hatch 12-66 assemblies 9-73 autoballoons 12-46 balloons 12-42, 17-23 blocks 12-69 center marks 12-48 centerlines 12-51 colors 11-56 cosmetic threads 12-54 datum feature symbols 12-58 datum targets 12-59 display filter 12-32, 17-25 dock points 12-35 dowel pin symbols 12-63 favorites 12-4 fonts 17-26 geometric tolerancing 12-60 hide/show 12-27 hole callouts 12-52 hyperlinks 2-42 insert into drawings 12-2, 12-3 layers 11-58 multi-jog leaders 12-35 multiple 12-33 notes 12-36, 17-23 options 12-31, 17-25, 17-26 parts 7-32 properties 12-32 stacked balloons 12-44 surface finish symbols 12-56 tables 12-76 underlined leader 12-38 weld symbols 12-64 Annotations toolbar 2-23 ANSI standard 17-19 1982 standard for datums 12-58 geometric tolerancing 12-60 tolerances 17-21 weld symbols 12-65 API - Application Programming Interface 2-91
Index-2
application protocols in STEP 13-37 arcs 3-60 3 point 3-59 3D arcs 3-68 centerpoint 3-59 dimensions 3-35, 3-38 in section lines 11-37 tangent 3-8, 3-59 area hatch 12-66 add to face or sketch 12-66 broken views 11-35 import 13-19 options 17-6 arrange icons 2-3 array of sketch entities 3-17, 3-25 arrows 12-12 aligned section views 11-42 auxiliary views 11-28 dimension display properties 12-10 dimension options 17-21 display options 17-24 flip in dimensions 12-6 mulit-jog leaders 12-35 projeced views 11-26 second arrow display 12-10 second outside arrow display 12-10 section views 11-37, 11-40 style 12-6, 12-12 assembiles envelops 9-66 features 9-55 mates 9-26 options 17-13 reorganize 9-38 assemblies 9-1 alignment condition 9-17 annotations 9-73 auto explode 9-69 bottom-up design 9-1 Collision Detection 9-74 colors 9-10 components 2-42, 9-4, 9-6, 9-9, 9-39, 9-62 configurations 10-4, 10-10, 10-12 create from split part 7-27 drawings 11-17, 11-40 Dynamic Clearance 9-76 envelopes 9-65, 9-66 exploded views 9-69, 9-70, 9-71 Feature Palette 14-7, 14-8 feature scope 9-56 FeatureManager design tree 9-2 features 9-49, 9-55 fix 9-11 float 9-11 hide 9-67 hole series 6-81 image quality 9-72 inferencing 9-6 interference detection 9-74 lightweight 9-61 loading component data 9-64 mates 9-8, 9-13, 9-17, 9-19, 9-25, 9-26, 9-28, 9-31
mirror components 9-51 molds 8-2 options 17-13 patterns 9-26, 9-49, 10-12 performance 9-61, 17-13 Physical Dynamics 9-75 Physical Simulation 9-33, 9-35 PropertyManager 9-10 reorder 9-53 reorganize 9-37, 9-38, 9-39, 9-61 roll back 9-53 save 9-6, 9-7, 9-46 send 2-20 show 9-67 sketches 3-11, 9-54 SmartMates 9-25 statistics 9-9 sub-assemblies 9-37, 9-39 suppress 9-28, 9-63, 9-64, 10-27 top-down design 9-1 transparency 9-48 weld beads 9-58 Assembly toolbar 2-24 at angle planes 5-2 attach dimensions 13-22 attachment point 12-24 dimension extension lines 3-38, 12-24 leaders 12-35, 12-36, 12-41, 12-60, 12-69, 17-24 auto explode 9-69 auto hatching 11-35, 11-38, 11-40 auto insert on view creation 12-6, 12-46, 12-48, 12-51, 17-19 auto reliefs 15-28, 15-29 autoballoons 12-46, 17-23 AutoCAD 2-91, 13-10 copying and pasting from 13-22 DXF/DWG files 13-19 font support 13-10 Mechanical annotation 13-19 moving from AutoCAD 2-91 proxy entities 13-19 XREFs 13-19 Autodesk Inventor files 13-17 autodimension 3-39 automatic 2-2 autoballoons 17-19 backups 2-2 center mark insertion 12-48, 17-19 centerline annotation insertion 12-51, 17-19 dimension insertion 17-19 drawing view update 11-45, 11-47 Fit tolerance 12-8, 12-29 inferencing 3-14 jog ordinates 12-17, 17-21 relations 3-40 save 17-19 solve 3-14 update of BOM 17-19 automatic mates. See SmartMates 9-25 autosize reference geometry 5-10 auto-start projected view 11-19 autotransitioning 3-8 auxiliary views 11-28, 11-51
SolidWorks 2004 Reference Guide
2D to 3D conversion 2-22 hide and show 11-51 label display 17-27 axes 5-12 broken views 11-35 hide 5-12 hole table datum origin 12-89 reference 5-12 show 5-12 B
background image 13-38 backups 2-2 automatic 2-2 options 17-19 balloons 12-42 auto insert 17-19 autoballoons 12-46 bill of materials 12-42, 12-81 options 17-23 stacked 12-44 base 6-44 center mark 12-50 extrude 6-45 flange 15-2 part 7-22 revolve 6-132, 6-151 scale 13-10 base point 12-69 baseline dimensions 12-17 bend allowance 15-22, 15-25 bend deduction 15-22, 15-25 bend deviation 15-39 bend table 15-24 bends 15-31 edit 15-23, 15-29, 15-31, 15-32 Excel file 15-23, 15-24 flat bends 15-13, 15-32 inserting 15-31 lofted 15-38 no bends 15-32 positions 15-13 reordering 15-31 round bends 15-13, 15-14 sharp bends 15-13 simplify 15-43 sketched bends 15-9 text file 15-23, 15-24 bent leader length 17-21 bilateral tolerance 12-28 bill of materials 12-81 anchor point 11-5, 12-77 balloons 12-42 child components 10-31 configurations 12-83 contents 12-84 custom properties 12-85 edit text 12-97 Excel-based 12-94, 12-99 insert 12-95 options 17-26 part numbers 12-98
Index-3
sort 12-85 stacked balloons 12-44 sub-assemblies 10-4, 10-31, 12-83 templates 12-78 bitmaps 11-5 in sheet formats 11-5 in sketches 3-67 black and white drawings 2-15 blanked surfaces on import 13-3 block settings 12-38 blocks 12-69 definitions 12-75 insert 12-69, 12-73 instances 12-74 bodies 6-149, 6-214, 7-10 bolt patterns 9-79, 9-89 bolts 9-77 BOM. See bill of materials 12-81 borders 12-38, 12-79, 17-23 boss 6-44 extrude 6-39 revolve 6-132, 6-151 thicken 6-195 bottom-up assembly design 9-1 bounding box 11-9 box selection 2-64 branch points 12-35 break alignment 11-49 break corner 15-35 break external references 9-43 break lines 11-35 break view 11-35 BREP 13-7, 13-11, 13-28, 13-34, 13-35 broken views 11-35 align with parent 11-46 break line gap 17-19 cut styles 11-37 broken-out section 11-34 C
CADKEY files 13-17 callouts 2-6, 3-43, 12-54 cam-follower mates 9-22 cap ends 6-46 capture mate references 9-17 capture type in TIFF 13-15 cascade window 2-3 casting parts (mold design) 8-2 CATIA graphics files 13-18 cavities 8-11 drafts 8-4 scaling factor 8-4 cells in tables 12-76, 12-80 center dimension text 12-13, 17-21 center marks 11-28, 12-48 centerlines 3-58 aligned section views 11-42 annotations 12-51 font for center marks 12-50, 17-19 lofts 6-101 section lines 11-37 section views 11-40
Index-4
centerpoint 3-59 arcs 3-59 rotate drawing views 11-49 centroid 5-14 CGR. See CATIA graphics files 13-18 chain 12-10 dimensions 12-10, 12-17 select 2-62 chamfer 6-7 dimensions 12-20, 12-21 feature 6-7 sketch 3-31 change assembly transparency 9-48 change URL 2-58 check 7-29 entity 7-31 face or edge 7-31 for out-of-date lightweight components 9-64 geometry 7-31 model geometry 7-30 planar surface 7-30 section views 11-41 sketch 3-16 sketch contours 3-16 child and parent relations 2-46, 11-9, 11-48 circles 3-55 detail views 11-30, 11-33 dimensions 3-36, 3-38 circular pattern 6-119, 12-48 circular sketch step and repeat 3-17 constrain spacing 3-19 fix radius 3-19 classification 12-8, 12-29 clearance 12-8, 12-29 click-click or click-drag 3-7 close 2-3 all documents 2-2, 2-3 sketches 3-21 closed corner 15-12 coincident mates 9-14, 9-20, 9-22 coincident relations 3-42 collapse 9-70 exploded views 9-70 FeatureManager design tree 2-46 collinear dimensions 12-24 Collision Detection 9-74 colors 17-6, 17-30 annotations 2-29, 11-56, 11-58, 12-6, 12-31 assembly instances 9-10 Color and Optics PropertyManager 2-37 component instances 9-72 curvature 7-39 display mode 11-56 document options 17-30 edit 7-7 faces or features 7-4, 7-8 layers 11-58 library features 14-5 material properties 7-5, 7-9 notes 11-56 parameter in design tables 10-33 parts in assemblies 9-72
print documents 2-15 sketch status 3-43 system options 17-6 tables 12-76 use assembly 9-72 combine parts 6-213 combine same sizes 12-88 combine same tags 12-88 combined features, MDT files 13-29 CommandManager 2-24 commands 2-83 comments 10-29 configurations 10-4 design tables 10-29 equations 7-16 summary info 7-33 component line font 11-55 component names 17-15 generate names for referenced geometry 17-15 update 17-15 components 9-4 assemblies 9-4, 9-10 Collision Detection 9-74 colors 9-72 configuration descriptions 2-45 configuration names 2-45 configurations 10-26 copy 9-51 derived 7-23 descriptions 2-44 drawings 11-17, 11-40, 11-55, 11-58 Dynamic Clearance 9-76 envelopes 9-65, 9-66 fix 9-11 float 9-11 hide 9-62, 9-67, 11-53 interference detection 9-74 layers 11-58 lightweight 9-61 loading additional data 9-64 mates 9-3, 9-13 mirror 9-51 molds 8-2 names 17-15 part numbers 10-28 patterns 9-49 Physical Dynamics 9-75 properties 9-9, 9-62, 9-67, 9-72 reorganize 9-37, 9-38, 9-39 replace 9-7 resolved 9-63, 9-64 select 9-66, 9-68 shared documents 2-42 show 9-62, 9-67 SmartMates 9-25 suppress 9-63, 9-64 visibility 9-62, 9-65 weld beads 9-58 composite curves 5-21 composite frames 12-62 compression scheme in TIFF 13-15 concentric 3-42
SolidWorks 2004 Reference Guide
dimensions 12-23 mates 9-14, 9-20 relations 3-42 ConfigurationManager 10-1 activate 10-1 split panel display 2-48 configurations activate 10-8 alternate position views 11-43 assemblies 10-10, 10-12 base parts 10-28 bill of materials 12-83 create manually 10-4 create with design tables 10-18 delete 10-13 derived 10-6 descriptions 2-45 dimensions 10-11, 12-26 edit 10-11 end conditions 10-10 equations 10-30 parts 10-8 previews 10-2 properties 10-4 sheet metal flat patterns 11-21 sketch dimensions 10-8 sketch planes 10-9 sketch relations 10-9 STEP files 13-37 weldment cut lists 16-15 confirm delete 2-35 confirmation corner 2-9, 17-2 conformance classes in STEP 13-37 conical 15-40 faces in sheet metal parts 15-15 holes for cosmetic threads 12-54 mates with conical features 9-26 connectors 6-9, 6-106 constrain all 3-19, 13-22 constraints. See relations 3-41 construction geometry. See also reference geometry 3-21 contents, bill of materials 12-84 contour map 6-201 contour selection 3-19 contour types for features 3-16, 3-17 conversion wizard 2-89 convert 2-89 2D to 3D 4-1 detached drawings 11-13 entities 3-22 lightweight drawings 11-16 older SolidWorks files 2-89 sketch lines to construction geometry 5-15 coordinate systems 5-13 3D sketches 3-74 scale parts 6-141 translate 5-13 copy 2-35 blocks 12-69 components 9-51 drag 2-7 drawing views 11-50
Index-5
entities from AutoCAD 13-22 features 7-4 options settings 2-90 planes 5-10 referenced files to server 2-58 references 9-46 sketch entities 3-8, 3-15 to clipboard 2-35 copy options wizard 2-90 corner 15-12 closed 15-12 treatment 15-42 trim 15-44 cosmetic threads 12-54 broken views 11-35 display 17-25 MDT files 13-29 pipe tap holes 6-88 tap holes 6-87 counterbore holes 6-84 countersink holes 6-85 create 3-3 configurations 10-4, 10-18 detached drawings 11-13 forming tools 15-25 new sketches 3-3, 3-4, 3-5, 4-10 openings on forming tools 15-27 palette items 14-8 sub weldments 16-14 crop views 11-33 crosshatch 11-10 area hatch 12-66 detail views 11-40 options 17-30 out-of-date drawing views 17-4 properties 12-68 section views 11-40 cursors. See pointers 3-6, 3-40 curvature 7-39 combs 3-52 display 7-41, 7-42 minimum 7-31 options 7-41 radius 7-40 sketch entities 3-52 curvature continuous 6-70 curve driven patterns 6-110 curved break line cut style 11-37 curves 5-15 composite 5-21 face curves 3-23 from file 5-17 helix 5-17 projected sketch onto face 5-18 projected sketch onto sketch 5-18 shape 6-144 sketches 3-22 spiral 5-17 split curves 3-32 split lines 5-20 through reference points 5-16 through XYZ points 5-16
Index-6
Curves toolbar 2-25 custom 11-7 drawing views 11-19 headers and footers 2-83 macro button 2-84 property values 11-7 scales 11-9, 11-21, 11-24, 11-27, 11-29, 11-31, 11-38 sheet formats 11-3, 11-6 table templates 12-79 template tabs 2-52 custom map SolidWorks to DXF 13-10 custom properties 7-33 bill of materials 12-85 design tables 10-32 drawings 11-4, 11-7, 12-41 in sheet formats 11-6 parts 7-33 weldments 16-18 custom standards 6-83 custom symbols. See blocks 12-69 customize commands 2-83 drawing sheet formats 11-5 headers and footers 2-83 keyboard 2-84 macro button 2-84 macros 2-93 menus 2-85 options 2-81, 2-86 SolidWorks 2-81 tolerance 13-7, 13-14 toolbars 2-86 cut 2-35 across sheet metal bends 15-34, 15-35 drawing views 11-50 extrude 6-50 normal cut 15-35 revolve 6-132 sketch entities 3-8 styles in broken views 11-37 thicken 6-195 to clipboard 2-35 tool 6-47 with surfaces 6-49 cut lists. See weldment cut lists 16-15 cylindrical faces in sheet metal parts 15-40 D
dangling 2-12 section views 11-41 sketch dimensions 7-4, 17-7 sketch geometry 3-43 dates, document properties 11-7, 12-41 datum feature symbols 12-58 datum origin 12-86, 12-89 datum targets 12-59 default 2-53 dimension properties 12-4 fonts 2-29 material properties 2-53 system colors 17-6 templates 2-53
view alignment 11-49 view rotation angle 11-49 defined in context relations 3-45 definition 12-69, 12-75 deform curve to curve deformation 6-9, 6-12 point deformation 6-19, 6-21 delete 2-35 area hatch 12-66 assembly components 9-6 background image 13-38 body 6-214 configurations 10-13 confirm 2-35 design tables 10-21 equations 7-15 faces 6-177 holes 6-179 layers 11-58 mates 9-28 patterns 6-128 relations 3-44 spline points 3-49 surfaces 6-177 tables 12-76 density 17-30 dependent 2-46 documents 9-42 drawing views 11-26, 11-28, 11-37 derived 3-11 configurations 10-6 drawing views 11-26 sketches 3-11 derived parts 7-21 base 7-22 components 7-23 edit 7-26 mirror 7-22 palette parts 14-10 design methods in assemblies 9-1 design tables base parts 10-28 colors 10-33 components 10-26, 10-27 configuration parameters 10-21, 10-23, 10-24 create 10-14, 10-18 custom properties 10-32 delete configurations 10-13 delete tables 10-21 dimensions 10-25, 10-32 edit 10-21, 10-36 Excel 10-14 expand sub-assemblies in BOMs 10-31 formatting 10-19 in drawings 10-35 lighting 10-31 MDT files 13-29 numerical configuration name 10-21 options 17-2 properties 10-5, 10-32 PropertyManager 10-17 saving 10-22
SolidWorks 2004 Reference Guide
split parts 10-32 suppress 10-27 user notes 10-33 detach segment on drag 3-22 detail circles 11-33 detail views 11-30 copy with parent view 11-50 detailed previews 6-215 hide with parent view 11-51 label display 17-27 modify 11-32 pin position 11-32 profile display 11-32, 17-4 scale 11-32, 17-4 detailing 12-1, 17-19 diagnostic tools 3-16, 3-45, 3-52, 9-28 diameters 3-36 circular dimensions 3-36 dimensions 12-6, 12-10 holes 6-86 holes for cosmetic threads 12-54 in revolve features 6-132 dimensions 3-33, 12-6 access 14-12 align 12-22, 12-23, 12-24 angular 3-37 arcs 3-35, 3-38 baseline 12-17, 17-21 chain 12-10, 12-14, 12-17 chamfer 12-20 circles 3-36, 3-38 configurations 10-11, 10-25, 12-26 copy 12-22 detached drawings 11-14 Dimension/Relations toolbar 2-26 dispaly 2-43 display 12-6 driven 12-10 dual 12-10, 17-19 equations 7-14 extension lines 3-38, 12-6, 12-24 favorites 12-4 foreshortened radius 12-10 hide/show 12-6, 12-27 hole callouts 12-52 horizontal 3-34, 3-35, 12-19 increment value 12-26 inserting into drawings 12-3 internal 14-12 layers 11-58 leaders 12-21 linear 3-34, 3-35, 12-10, 12-24 lines 12-6 link/unlink values 7-17 lock type 3-34, 12-19 mark for drawings 12-26, 17-19 midpoints 12-16 modify 3-33, 12-26 move 12-22 options 12-7, 17-2, 17-7, 17-19, 17-21, 17-25 ordinate 12-17, 12-19 overdefining 17-7
Index-7
override dimensions on drag 3-30, 17-7 parallel 12-19 parentheses 12-17 point-to-point 3-35 projected 11-10 properties 12-10 PropertyManager 12-8 radial 12-24 reference 12-16 selection 12-6 silhouette edges 12-16 sketches 3-33, 3-75, 10-8 standards 17-19 text 12-26, 12-32, 17-25 tolerance 12-28, 12-29 true 11-10 vertical 3-34, 3-35, 12-19 Dimensions/Relations toolbar 2-26 direction of lay 12-56 directional lights 7-47 display 7-42, 17-31 annotations 17-25 assembly annotations 9-73 auxiliary view arrows 11-28 axes in section views 11-40 background image 13-38 center points 17-4, 17-7 design tables in drawings 10-35 detail circle or profile 11-32 dimensions 12-6, 12-8, 12-21 drawing views 11-9, 11-45 entity points 17-4, 17-7 filter for annotations 7-32, 12-32, 17-25 Fit tolerances 12-29 image quality of assemblies 9-72 interfering bodies in HLR/HLG 9-72 modes 11-55, 11-56 OLE objects as icons 2-96 options 17-5, 17-19 quality 11-11 sketch status 17-7 surface cut in section views 11-42 symbols per 2002 12-56, 17-19 text at the same size 9-73 virtual sharps 17-7 display/delete relations 3-44 dissolve 9-39 library features 14-6 sub-assemblies 9-39 distance 3-33 mates 9-14, 9-21, 9-23 measure 7-18 offset 17-21 dock points 12-35 Document 2-82 document color options 17-30 document templates. See templates 2-52 documents 2-2 close all 2-3 colors 17-30 cycle between open 2-18, 2-53 in Windows Explorer 2-55
Index-8
names 12-41 open 2-53 print 2-13 properties 2-81, 11-7, 12-41 save 2-34 templates 2-52 windows 2-2 dome 6-30 dowel pin symbols 12-63 draft quality 2-68, 11-11, 11-16, 17-5 drafts 6-32 allow reduced angle 6-36 analysis 6-198 detailed previews 6-215 extrude 6-39, 6-50 mold design 8-4 neutral planes 6-32, 6-38 parting lines 6-35, 6-37 drag 2-7 and drop planes 5-2 blocks 12-69 break lines in broken views 11-35 components 9-4, 9-11, 9-12 detach sketch entity 3-22 detail view profiles 11-32 drawing views 11-50 edit assembly structure 9-37 feature handles to resize 6-208 FeatureManager design tree 2-56 files into assemblies 2-56 Internet Explorer 2-56 models into drawings 11-17 override dimensions 3-30 select 2-60 tables 12-76 drawing sheets 11-5 customizing sheet formats 11-5 delete 11-4 focus 11-8 formats 11-4, 11-5 multiple 11-4 reorder 11-8 setup 11-4 Drawing toolbar 2-26 drawing views activate 11-8 aligned section 11-42 alignment 11-49 alternate position 11-43 auxiliary 11-28 boundaries 11-9 broken 11-35 broken-out section 11-34 configuration 11-46 copy and paste 11-50 crop 11-33 derived 11-26 detail 11-30 empty 11-10, 11-25 exploded 11-26, 11-28, 11-30, 11-46 first and third angle projection 11-19 hide/show 11-51
isometric or projected dimensions 11-46 lock focus 11-8 model 11-19 perspective 11-19 predefined 11-24 projected 11-26 properties 11-46 relative to model 11-22 rotate 11-49, 11-50 scales 11-9 section 11-37, 11-41 select 11-1, 11-8 standard 11-17 standard 3 views 11-17 update 11-45, 11-47 drawings 11-1, 11-13 2D sketches 11-10 annotations 12-2 assemblies 11-8 component line font 11-55 construction geometry 3-21 design tables 10-35 detached 11-13 display modes 11-55 edge display 17-5 file size 11-13, 17-4 formats, sheets, and views 11-5 hide behind plane 11-53 hide edges 11-51 hide/show components 11-53 inferencing 3-14 insert model items 12-2 layers 11-58 lightweight 11-16 lines 11-55, 11-56, 17-31 move 11-48 names 11-3 new 11-3 OLE objects 11-45 options 11-2, 17-4 parts 4-4, 11-8 print 2-15, 2-16 reference geometry 12-2 save 11-1 scales 11-9 send 2-20, 11-12 sheet metal parts 15-41 show hidden edges 11-52 windows 11-8 driven dimensions 12-6, 12-10 duplicate entities in IGES 13-11 DXF/DWG files 13-19 attach dimensions 13-22 block import 12-69 constrain all 3-19, 13-22 copy/paste from AutoCAD 13-22 DWG preview 13-19 DXF 3D files 13-18 export 13-9, 13-10 export fonts 13-9, 13-10 export options 13-9, 13-10 export version 13-9, 13-10
SolidWorks 2004 Reference Guide
import 13-3 imported entities 13-22 insert 13-21 layer map export 13-10, 13-23 layers 11-58 line styles 13-10 mapping 13-23 View only 13-20 dynamic 7-3 drawing view activation 11-8, 17-4 feature editing 7-3 highlighting 2-59, 2-60 previews 2-68 transparency 2-79 Dynamic Clearance 9-76 E
edge display and selection 17-8 edge display in drawings 17-5 edge flange 15-3 edges 17-8 baseline dimensions 12-17 display options 17-8 hidden edge selection 17-8 highlighting 17-8 in drawings 11-51, 17-5 properties 7-8 edit 7-1 auto reliefs 15-29 bend parameters 15-29, 15-32 blocks 12-69 colors 7-7 configurations 10-11 crop views 11-33 definition 7-1 derived parts 7-26 design tables 10-21, 10-36 dimension access 14-12 equations 7-14, 7-15 exploded views 9-69, 9-71 features 7-1, 7-3 file locations 9-8 forming tools 14-9 imported features 13-4 joined parts 9-57 library features 14-5 macros 2-93 mates 9-8, 9-19 OLE objects 2-95 parts 7-20, 9-48 planes 3-12 seed features 6-129 sketches 3-2, 3-10, 3-12 tables 12-76 weld beads 9-58 eDrawings 13-11, 13-24, 13-25, 13-26 ellipses 3-57 email. See send mail 2-20 embed bitmaps in sheet formats 11-5 empty drawing views 11-10, 11-25 end conditions 6-39, 6-42, 10-10 entities 7-8
Index-9
IGES 13-28 offset 3-30 properties 7-8 envelopes 9-65 create 9-66 remove 9-66 select components 9-66 toggle visibility 9-65 equal length or radius 3-45 equations 7-14 comments and status 7-16 edit and delete 7-15 functions 7-16 in configurations 10-30 operators and constants 7-16 error reporting 2-12 errors in mates 9-31 Excel 17-2 bend table 15-24 bill of materials 12-99 design tables 10-14, 10-18 OLE objects 2-95 SolidWorks API 2-91 existing relations 3-41 exit sketch 3-11 explode blocks 12-69 Explode Sketch toolbar 2-27 exploded views 9-69 assemblies 9-69 collapse 9-70 edit 9-71 in drawings 11-8, 11-26, 11-28, 11-30, 11-46 lines 9-71 sketches 9-71 export documents 13-1, 13-2, 13-9 export options 13-9 ACIS files 13-9 DXF/DWG files 13-9, 13-10 eDrawings files 13-9, 13-11 IGES files 13-9, 13-11 multibody parts 13-16 Parasolid files 13-9, 13-13 STEP files 13-9, 13-13 STL files 13-9, 13-14 TIFF files 13-9, 13-15 VRML files 13-9 export sketch entities in IGES 13-11 extend entities 3-22 extend surface 6-157 extended lines 12-50, 17-19 extension lines 12-24 arcs and circles 3-38 display in dimensions 12-10, 12-13 flip 12-24 hide/show in dimensions 12-6 options 17-19, 17-21 external references 9-42 assemblies 9-42, 9-46 blocks 12-69, 12-75 break 9-43 file management 7-28 list 9-44
Index-10
lock 9-43 note properties 11-7 options 17-15 relations 3-45 rules 9-43 search file locations for 17-15 unlock 9-43 update path 9-43 external relations 3-45 extract sketches 4-5 extrude 6-44 2D to 3D conversion 4-7 boss/base 6-44, 6-45 cut 6-50 detailed previews 6-215 end conditions 6-42 surfaces 6-150 tabs on sheet metal parts 15-9 text 3-65 thin features 6-46 F
face curves 3-23 face fillets 6-70 help points 6-71 split lines 6-73 surfaces 6-156 faces 7-2 deletion 6-177 edit color 7-7 properties 7-8 replace 6-180, 6-181 fasteners 9-77 favorite dimensions and annotations 12-4 favorite hole types 6-80 add 6-81 delete 6-81 retrieve 6-81 update 6-81 feature control frames 12-62 Feature Palette window change dimensions 14-5 display 14-7 drag files into 2-56 edit items 14-9 forming tools 15-25 navigate 14-7 organize 14-7, 14-9 palette items 14-8 thumbnail graphics 14-9 feature statistics 7-28 feature-based mates 9-26 FeatureManager design tree add folders 2-50 assembly component icons 9-3 assembly conventions 9-2 blocks 12-69 color 17-6 component configuration descriptions 2-45 component configuration names 2-45 component descriptions 2-44 configuration descriptions 2-45
conventions 2-46 display by dependencies 9-2 display by features 9-2 displaying mates with components 9-2 drawings 11-8 external references 9-42 flyout 2-49 options 2-49 select drawing views 11-50 select from 2-50 sheet metal parts 15-17 split panel display 2-48 zoom to selection 11-8 features 6-1 accepting 2-9 assemblies 9-55, 9-56 boss/base 6-44, 6-132 chamfer 6-7 circular pattern 6-119 colors 7-7 combined 6-213, 13-29 contours 3-16 copy 2-7, 7-4 curve pattern 6-110 cut 6-47 deform 6-8, 6-9, 6-12, 6-19, 6-21 descriptions 2-43, 2-44 detailed preview 6-215 dome 6-30 draft analysis 6-198, 6-201 drafts 6-32, 6-35, 6-37, 6-38, 6-50 drag 2-7 edit 7-1, 7-2, 7-3 extrude 4-7, 6-39, 6-42, 6-44, 6-46, 6-50 fillets 6-57, 6-58, 6-60, 6-61, 6-62, 6-64, 6-67, 6-70, 6-71, 6-73
guide curves 6-97, 6-99, 6-101, 6-187, 6-189 hide and show bodies 6-175 holes 6-74 in-context 9-42 keep features 6-56 linear pattern 6-114 lofts 6-95, 6-96, 6-97, 6-99, 6-101, 6-104, 6-192 mirror 6-108, 6-125, 6-129 move 2-7, 6-208 out-of-context 9-42 parting lines 6-35, 6-37 patterns 6-108, 6-109, 6-123, 6-125, 6-126, 6-127 revolve 6-132 ribs 6-135, 6-138, 6-139 scale 6-141 scope 9-56 seed features 6-129 shape 6-142, 6-144 shells 6-145, 6-146 sketch driven pattern 6-121 suppress and unsuppress 7-21 sweeps 6-182, 6-183, 6-187, 6-189, 6-190, 6-193 table driven patterns 6-123 tangency 6-190, 6-191, 6-193 tapped hole 13-29 thicken 6-195
SolidWorks 2004 Reference Guide
thin 6-46, 6-94, 6-191 time-dependent 9-49 work 13-29 wrap 6-216 Features toolbar 2-27 file name extensions 2-52 favorites 12-4 sheet formats 11-6 table templates 12-78 file size 17-4 detached drawings 11-13 drawings 17-4 eDrawings 13-24 to send electronically 11-12 files 2-53 blocks 12-69, 12-75 external references 7-28 insert models into drawings 11-17 layers 11-58 locations 9-8, 17-16 names in notes 11-7 new 2-52 open 2-53 properties 7-33 save 2-34 sheet format files 11-6 fill 12-66, 17-6, 17-30 fill surface 6-164 fillets 6-57 constant radius 6-58 face blends 6-70, 6-71, 6-73 overflow type 6-59 radius 6-60 round corner 6-61 setback 6-62 sketch 3-31 surfaces 6-159 variable radius 6-64, 6-67 filter. See selection filter 2-63 find 2-50 in FeatureManager design tree 2-50 referenced documents 9-44 first angle projection 11-4, 11-19 first arc condition 12-10 Fit tolerances 12-8, 12-28, 12-29 fix component 9-11 fix relation 3-42 flag symbols 12-10 flange 15-2 base flange 15-2 edge flange 15-3, 15-4 miter flange 15-4, 15-6, 15-7 flatten 15-32 assembly hierarchy in IGES 13-9, 13-11 assembly hierarchy in Parasolid 13-9 sheet metal parts 15-32 flatten-bends 15-32, 15-44 flexible sub-assemblies 9-41 flip direction 11-40 dowel pin symbols 12-63 flat pattern view in drawings 11-21 section views in drawings 11-40
Index-11
flip side to cut 6-39 float components 9-11 folders 2-50 follow assembly order 12-42, 12-44, 12-83 Font toolbar 2-29 fonts AutoCAD support 13-10 component line font 11-55 detail circle label 11-31, 17-26 dimension text 12-8, 17-26 notes 12-38, 17-26 options 17-26 tables 12-79, 12-80 weld symbols 12-64, 12-65, 12-66, 17-26 foreshortened radius 12-10 form new sub-assemblies 9-37 forming tools 15-25 apply to sheet metal parts 15-28 create 15-25 edit 14-9 openings 15-27 positioning sketches 15-27 fractions 17-28 frame points 3-49 front 2-40 orientation 2-75, 3-4 plane 3-3 views 11-17 fully defined sketches 3-43 fundamentals of SolidWorks 2-1 G
gap 13-6, 17-21 break lines 11-35, 17-19 dimension lines 12-8, 17-21 GB standard 12-59, 17-19 gear mates 9-23 general 17-2 import options 13-7 system options 17-2 geometric characteristic symbol (GCS) 12-62 geometric relations 3-40 automatic 3-40 display/delete 3-44 sketch 3-41 geometric tolerancing 12-60 favorites 12-4 leaders, arrows, fonts 12-62 properties 12-62 geometry pattern 6-114, 6-121, 6-123, 6-127, 6-129 geometry-based mates 9-25 go to command 2-50 GOST standard 12-66, 17-19 gradient background 17-6 gravity 9-35 gray scale drawings 2-15 grid 17-28 align 3-13 options 17-28 snap 17-28 guide curves 6-97, 6-99, 6-101, 6-187, 6-189
Index-12
H
handles 2-6 hatch. See area hatch 12-66 HCG. See highly compressed graphics files 13-26 headers and footers 2-13, 2-83 helix 5-17 help 2-10 quick tips 2-91 SolidWorks 2-10 What's this? 2-10 help points 6-70 hems in sheet metal parts 15-10 hidden 11-55 edges in drawings 11-55 items 2-63 hidden lines removed 2-68, 2-69, 11-57, 17-5 hidden lines visible 2-68, 2-69, 11-57, 17-5 hide 9-62 assembly components 9-62, 9-67 axes 5-12 bodies 6-175 components in drawings 11-53 cosmetic threads 12-27 curvature combs 3-52 dimension extension lines 12-24 dimensions 12-27 drawing components behind plane 11-53 drawing views 11-51 edges in drawings 11-51 layers 11-58 planes 5-10 sketches in drawings 11-52 using envelopes 9-65 high quality 11-11 high trim curve accuracy in IGES 13-11 highlighting 2-59 highly compressed graphics files 13-26 HLR edges in shaded mode 11-55, 17-5 HLR. See hidden lines removed 2-69 hold lines in face fillets 6-71 hole callouts 12-8, 12-52 hole fit 12-8, 12-29 hole tables 12-86 add holes 12-88 datum origin 12-89 options 17-26 tags 12-86 hole wizard 6-77 callouts 12-52 custom standards 6-83, 6-84 favorites 6-81 parameters 6-80 placement 6-79 holes 6-77 3D sketches 6-77 add to table 12-86, 12-88 assemblies 6-81, 9-55 callouts 12-52 counterbore 6-84 countersink 6-85 delete. See surfaces 6-179 end conditions 6-76
fasteners 6-86 favorites 6-80, 6-81 features 6-74, 6-77 hole type 6-86 legacy 6-89 parameters 6-80, 6-86 pipe tap 6-88 placement 6-79 property 6-80 series 6-81 simple 6-74 standards 6-86 tap 6-87 wizard 6-77, 12-52 hollow feature. See shell 6-145 HOOPS files 13-27 horizontal 3-34 align drawing views 11-49 breaks 11-35 dimensions 3-34 ordinate dimensions 12-19 rotate views 11-49 hyperlinks 2-42 in notes 12-37 into drawings 11-17 I
icons 2-3 documents 2-2 FeatureManager 2-46 OLE objects 2-96 rebuild 2-50 IGES files 13-27 2D geometry 13-27 BREP export 13-11, 13-27 edit imported features 13-4 entity types 13-28 export 13-9 export options 13-9, 13-11 exported curves 13-29 exported surfaces 13-12 import 13-3 import hints 13-27 import options 13-7 import surfaces 13-3 import units 13-7 levels 13-29 open 2-53 image quality 9-72, 17-31 image type in TIFF 13-15 import 13-1 diagnosis 13-6 drawings into parts 4-4 files 13-1, 13-2, 13-3 formats 13-2 geometry 13-3 sheet metal parts 15-17 surfaces 13-3 import options 13-3, 13-7 ACIS files 13-7 general 13-7 IGES files 13-7
SolidWorks 2004 Reference Guide
STEP files 13-7 STL files 13-8 VDAFS files 13-7 VRML files 13-8 improve geometry. See simplify geometry 13-6 inches 17-28 in-context features 3-45, 9-42, 9-46, 9-47, 9-55 inferencing 3-14 annotations 12-34 lines 3-6, 3-14 pointers 3-6 to the assembly origin 9-6 inflection points 3-52 insert 12-2 blocks 12-69, 12-73 components into assemblies 9-4 configuration design tables 10-16 dimensions into drawings 12-2, 12-3 DXF/DWG files 13-21 imported geometry 13-3 model items into drawings 12-1, 12-2 SolidWorks data into other applications 2-97 spline points 3-49 inspection dimensions 12-10 instances 12-69 blocks 12-74 components in section views 11-40 holes in hole callouts 12-52 interference detection 9-74 internal dimensions 14-12 Internet open address 2-42 interrupt regeneration 7-32 intersection curves 3-24 invalid edges or faces 7-29 invalid solution found in sketches 3-43 invisible 12-38, 12-69 isometric views 2-75 iso-parametric. See face curves 3-23 item numbers 12-42 balloons 12-42 bill of materials 12-83, 12-85 weldment cut lists 16-16, 16-17 J
JIS standard 17-19 arrowhead style 12-8, 12-12 surface finish size 12-32, 12-57, 17-25 jog 15-36 lines 9-71 ordinate dimensions 12-17, 17-21 points 12-35 sheet metal parts 15-36 joined parts 9-56 create 9-56 edit 9-57 identify 9-58 JPEG files 13-29 jumps 11-17 auxiliary views to parent views 11-28 detail views to parent views 11-30 projected views to parent views 11-26 section views to parent views 11-37
Index-13
standard 3 views to parent views 11-17 stop current jump 2-41 justify text 12-8, 12-38 K
keep constrained corners in fillets 3-31 keep missing item 12-83, 16-16 keyboard 2-84 assign macros 2-93 customize 2-84 shortcuts 2-18 K-Factor 15-23 knit surfaces 6-161 L
labels 11-4 detail views 11-30, 11-32 display options 17-19 next datum 11-4 next view 11-4 options 17-27 section lines 11-42 section views 11-37, 11-40 large assembly mode 9-61, 11-1 Layer Toolbar 2-29 layers 11-58 area hatch 12-68 drawings 11-56, 11-58 IGES files 13-29 import/export 11-58 insert model items 12-2 layer toolbar 2-29 line fonts 11-55 tables 12-76 layout sketches in assemblies 9-54 leaders 12-13, 12-21 balloons 12-42 blocks 12-69, 12-74 display with dimensions 12-10, 12-21 flip in dimensions 12-24 geometric tolerancing 12-60 multiple 12-41, 12-42, 12-60 notes 12-36, 12-69, 17-23 options 17-21 perpendicular 12-60 surface finish symbols 12-56 legacy holes 6-89 levels in IGES files 13-29 library features 14-2 add to parts 14-4 colors 14-5 comparison with palette features 14-1 create 14-3 dissolve 14-6 edit 14-5 limitations 14-1 mandatory references 14-2 lighting 7-45 advanced 7-50 ambient 7-46 basic 7-50 basic controls 7-45
Index-14
cone 7-50 directional lights 7-47 in design tables 10-31 point lights 7-48 position 7-51 spot lights 7-49 lightweight 9-61 components 9-61, 9-64, 10-27 drawings 11-13, 11-16 Limit Mates 9-13 limit mates 9-23 Line Format toolbar 2-29 linear dimensions 3-34, 3-36, 12-6 linear patterns 6-114, 12-48 linear sketch step and repeat 3-25 constrain angle 3-26 fixed spacing 3-26 linear springs 9-34 lines 3-53 2D 3-53 3D 3-69, 3-70 aligned section views 11-42 autotransitioning 3-8 circular center mark 12-50 colors 11-56, 11-58, 12-66 connection center mark 12-50 explode 9-71 extended center mark 12-50 fonts 11-55, 11-56, 17-31 inferencing 3-6, 3-14 jog 9-71 options 17-31 radial center mark 12-50 section lines 11-37 size in center marks 12-48 snap in 3D sketches 3-69 styles 11-55, 11-56, 11-58 thickness 11-56, 11-58 weights 2-14, 11-55 link 2-95 bitmaps to sheet formats 11-5 blocks to file 12-75 dimension favorites 12-4 dimension values 7-17 drawing views to parent views 11-8 errors 11-7, 12-41 notes to documents 12-37 notes to properties 11-7, 12-41 OLE objects 2-95 to thickness 6-39 list 9-42 external references 9-42 hide/show components 11-53 load 13-23 DXF/DWG mapping file 13-23 models in detached drawings 11-13, 11-14 selection criteria for components 9-68 lock 9-43 dimensions 3-34, 12-19, 12-22 external references 9-43 light to model 7-47, 7-48 sheet focus 11-8
view focus 11-8 lofted bends 15-38 lofts 6-90 add sections 6-104 centerlines 6-101 guide curves 6-97, 6-99, 6-101 maintain tangency 6-93 non-planar profiles 6-95, 6-99 planar profiles 6-97 simple 6-91 split lines 6-96 surfaces 6-153 synchronization 6-106 tangent 6-101, 6-103, 6-192 loop selection 2-65 loops 2-61 M
Macro toolbar 2-30 macros customize 2-93 customize buttons 2-84 debug 2-93 edit 2-93 folder 2-93 hot keys 2-93 menus 2-93 new 2-92 pause 2-92 record 2-92 run 2-93 stop recording 2-93 mail. See send mail 2-20 mandatory references 14-2 manual update of drawing views 11-45 manufacturing network 2-90 map file in DXF/DWG 13-10 mark for drawings 12-6, 12-26, 17-19 mark size 12-50 mass properties 7-38 match faces and edges 13-5 mategroups 9-18 material properties 7-5, 7-9 options 17-30 parts 7-5, 7-9 setting default 2-53 material shrinkage (scaling factor) 8-4 materials 2-69 RealView graphics 2-72 supported graphics cards 2-71 Materials Editor PropertyManager 2-38 mathematical relations 7-14 mating 9-13 alignment condition 9-17 angle 9-14, 9-19, 9-23 animation 17-10 assembly components 9-13 automatic 9-25 cam-follower 9-22 coincident 9-14, 9-20 concentric 9-14, 9-20 delete mates 9-28
SolidWorks 2004 Reference Guide
diagnostics 9-28 distance 9-14, 9-21, 9-23 entities 9-15 errors 9-31 feature-based 9-26 FeatureManager design tree 9-2 gear 9-23 geometry-based 9-25 limit 9-23 mate reference 9-17 mategroups 9-18 parallel 9-14, 9-21 pattern-based 9-26 perpendicular 9-14, 9-21 replace entities 9-8 SmartMates 9-25 standard types 9-14, 9-15 suppress mates 9-28 symmetry 9-24 tangent 9-14, 9-22 viewing 9-3 maximum 7-29 edge gap 7-29 radius of curvature 7-29 vertex gap 7-29 MDT. See Mechanical Desktop files 13-29 measure 7-18 measurement options 7-19, 7-38 Mechanical Desktop files 13-29 menus 2-8, 2-86 assign macros 2-93 customize 2-85, 2-86 shortcut 2-8, 2-18 merge tables 12-76 Metastream files. See Viewpoint 13-39 mid surface 6-162 middle mouse button functions 2-78 midpoints 2-63, 5-15 dimensioning to 12-16 relations 3-42 select 2-63, 5-15 minimum radius of splines 3-53 mirror 6-108 components 9-51 features 6-129 parts 7-22 patterns 6-125 sketch entities 3-27 miter flange 15-4, 15-6, 15-7 model views 11-21 models 2-2 geometry 7-29, 7-30 in detached drawings 11-14 modify 12-26 dimensions 3-33, 10-11, 12-26 mates 9-8, 9-19 perspective 2-73 section line properties 11-42 sketches 3-9, 3-15 mold tools 8-2 cavity 8-11 parting lines 8-4
Index-15
parting surfaces 8-7 ruled surfaces 8-9 scaling factors 8-4 shut off surfaces 8-9 tooling split 8-9 undercut detection 8-4 Mold Tools toolbar 2-30 motors 9-33 mouse 2-7 drag 2-7 middle button 2-78 speed 17-18 wheel 2-78 move 9-11 assembly components 9-11, 17-13 drag 2-7 drawing views 11-48 drawings on sheet 11-48 features 6-208 no solve 3-15 ordinate dimensions zero position 12-17 planes 5-10 sketch entities 3-8 sketches 3-27 move/copy 3-15 moving frames 3-49 MTS. See Viewpoint files 13-39 multibody 7-10 cavity 8-9, 8-11 cut 6-47, 6-49 extrude 6-45 feature scope 9-56 hide and show 6-175 modeling techniques 7-10, 7-11, 7-12, 7-13, 7-14 revolve 6-132, 6-151 split parts 7-23 sweeps 6-152, 6-185 versus assemblies 7-10 multi-jog leaders 12-35 multiple 12-33 annotations 12-33 drafts in a rib 6-138 drawing sheets 11-4 leaders 12-36, 12-41, 12-42, 12-56, 12-60 notes 12-36 radius fillets 6-60 multi-threaded retrieval 2-53, 2-55 N
named views. See model views 11-19 names 17-15 drawing sheets 11-4 favorites 12-4 planes 5-8 update 17-15 neutral plane draft 6-38 new assembly document 2-51, 9-39 detached drawings 11-13 drawing document 2-51, 11-3 part document 2-51, 9-47 sketches 3-2, 3-6, 4-10
Index-16
template tabs 2-52 windows 2-3 newlink WP0900 10-1 newlink WP1283 14-6 no solution found in sketches 3-43 no solve move 3-15 normal to curve planes 5-2 not solved status 3-43 notes 12-36 balloons 12-42 borders 17-23 colors 11-56 favorites 12-4 hyperlinks 12-37 in blocks 12-38 in sheet formats 11-5 link to properties 11-7, 12-41 options 17-23 nuts 9-81, 9-86 O
object linking and embedding. See OLE objects 2-95 objects. See OLE objects 11-5 offset 3-30 entities 3-30 planes 5-2 surfaces 6-154 OLE objects 2-95 display as icons 2-96 display contents 2-96 edit 2-95 in drawings 11-5, 11-45 insert existing files 2-95 insert SolidWorks data into other applications 2-97 linking versus embedding 2-95 properties 2-97 reset size 2-97 on surface planes 5-2, 5-5 online help 2-10 open 2-53 configurations of documents 10-3 documents 2-53 documents in other formats 13-3 drawings 11-1, 11-16 existing SolidWorks documents 2-53 files 2-53 parts within assemblies 2-54 sketches 3-6 open Internet address 2-42 optimize surfaces 6-164 options 2-81, 2-86 annotations 12-31, 17-25, 17-26 area hatch 17-6 arrows 17-24 assemblies 17-13 backups 17-19 balloons 17-23 colors, document 17-30 colors, system 17-6 crosshatch 17-30 detailing 12-1, 17-19 dimensions 12-7, 17-21
display style 17-5 drawings 11-2, 17-4 edge display 17-5, 17-8 export 13-9, 13-10, 13-11, 13-13, 13-14, 13-15 external references 17-15 FeatureManager 2-49 file locations 17-16 fonts 17-26 grid 17-28 image quality 17-31 import 13-7, 13-8 large assembly 17-13 line font 17-31 material properties 17-30 notes 17-23 performance 17-10 sketch 17-7 snap 17-28 spin box increments 17-18 system 17-2 tables 17-26 twist control 6-193 units 17-28 view labels 17-27 view rotation 17-18 virtual sharps 17-25 wizard 2-90 ordinate dimensions 12-17, 17-21 orientation 2-75 aligned section views 11-42 auxiliary views 11-28 relative to model views 11-22 section lines 11-42 section views 7-35, 11-37 view 2-75 origins 5-14 coordinate systems 5-13 datum for hole table 12-88, 12-89 inferencing in assemblies 9-6 rotate views 2-79 sketches 3-5 orthographic 11-17 model views 11-19 projected views 11-26 relative to model views 11-22 standard 3 views 11-17 views in drawings 11-19 out-of-context features 9-42 output coordinate systems 5-13, 13-9 over defined 3-43 sketch dimensions/relations 3-43 sketch geometry 3-43 sketches 3-43 overflow type 6-59 overlapping parts. See interference detection 9-74 overlay views. See alternate position views 11-43 override dimensions on drag 3-30 P
page setup drawing colors 2-15 headers and footers 2-83
SolidWorks 2004 Reference Guide
line thickness 11-56 margins 2-15 palette features 14-6 add to assemblies 14-12 add to palette 14-8 add to parts 14-10 comparison with library features 14-1 derived parts 14-10 forming tools 15-28 limitations 14-1 mandatory references 14-2 sheet metal parts 15-28 pan 2-79 paper 2-13 margins 2-15 size 11-4 parabolas 3-61 parallel 12-19 dimensions 12-19 mates 9-14, 9-21 relations 3-42 parallel plane at point 5-2 parallelograms 3-65 parameters 10-33 color 10-33 configurations 10-21, 10-23, 10-24 holes 6-80 Parasolid files 13-33 edit imported features 13-4 export 13-9 export options 13-9 export version 13-9 import 13-3 import surfaces 13-3 open 2-53 parent scale 11-9 parent/child relations 2-43, 2-46, 7-20 parentheses 12-6, 12-17, 12-29, 17-21 part configuration 10-4, 10-8 part numbers 10-28 balloons 12-42 bill of materials 12-83 components 10-28 partial ellipse 3-57 partial sections 11-41, 11-42 parting lines 6-35 drafts 6-35 face blend fillet 6-71 molds 8-4 split lines 5-20 step drafts 6-37 parting surfaces 8-7 parts 7-1 annotations 7-32 assemblies 9-4, 9-47, 9-48 base parts 7-22 check 7-30, 7-31 colors 7-4, 7-7 configurations 10-1, 10-8 curvature 7-39 derived 7-21, 7-22, 7-23, 7-26 dimensions 7-17
Index-17
drawings 11-17 edit 7-1, 7-3, 7-20, 9-48 equations 7-14, 7-15, 7-16 feature statistics 7-28 features 7-1, 7-21 files 7-28 geometry 7-29, 7-30 insert 7-22 join 6-213, 9-56 lighting 7-45 lightweight 9-61 mass properties and section properties 7-38 material properties 7-5, 7-9, 17-30 measure size and distance 7-18, 7-19 mirror parts 7-22 multibody 7-10 parent/child 7-14 references 17-15 section views 7-35, 7-37 sketches 3-3 split 7-23 summary information 7-33 suppress and unsuppress 7-20, 7-21, 10-27 parts list. See bill of materials 12-95 paste 2-35 patch 6-177 boundary 6-164 faces 6-177 patterns 6-108 area hatch 12-68, 17-6 center marks 12-48 circular 6-119, 12-48 components in assemblies 9-49 control and modify 6-126 crosshatch 12-68, 17-30 curve driven 6-110 delete 6-128 geometry 6-127 linear 6-114, 12-48 mates 9-26 mirror feature 6-129 of patterns 6-109 seed feature 6-129 sketch driven 6-121, 6-123 sketches 3-17, 3-25 SmartMates 9-26 table driven 6-123 vary sketches 6-128 pause macro 2-92 PDF Files 13-33 perform full entity check and repair errors 13-7 performance 17-10 data 17-2 large assemblies 9-61, 17-13 lightweight drawings 11-16 performance options 17-10 perpendicular 3-42 leaders 12-60 mates 9-14, 9-21 relations 3-42 perspective 2-72 modify 2-73
Index-18
views in drawings 11-19 views in models 2-72 phantom lines 11-43 Physical Dynamics 9-75 Physical Simulation 9-33, 9-35 gravity 9-35 linear springs 9-34 motors 9-33 overview 9-33 record 9-35 replay 9-35 toolbar 2-32 pictures 3-67, 13-38 pierce relations 3-42, 6-187 pin detail views 11-32 pins 9-77 pipe tap holes 6-88 planes 5-2 at angle 5-2 autosize 5-10 colors 5-8 copy 5-10 creating 5-2 drag and drop 5-2 hide 5-10 hiding components 11-53 line and point 5-2 move 5-10 neutral 6-34 normal to curve 5-2 offset 5-2 on surface 5-2, 5-5 parallel plane at point 5-2 rename 5-8 resize 5-10 show 5-10 show intersections 5-8 sketches 3-3, 3-4, 3-12, 3-13, 10-9 through lines/points 5-2 transparent shaded 5-8 play macro 2-93 point lights 7-48 pointers 11-8 inferencing 3-6 relations 3-40 points 3-55 2D sketch entities 3-55 3D sketch entities 3-73 spline points 3-49 point-to-point dimensions 3-35 polygons 3-63 pop up tooltips 2-10 portrait page orientation 2-13 positioning sketches for forming tools 15-27 precision 12-12 display properties 12-10 options 17-21 PropertyManager 12-8 predefined views 11-21, 11-24 press 12-8, 12-29 previous view 2-80 print 2-13
3D 13-16 background 2-13 break lines in broken views 11-35 documents 2-13 drawings 2-15, 17-4 eDrawings 13-24 headers and footers 2-83 line weights 2-14 margins 2-15 preview 2-18 references 9-46 selection 2-16 setup 2-13 printer settings 2-13 Pro/ENGINEER files 13-33 profiles 11-30 crop views 11-33 detail circles 11-33 detail views 11-30, 11-32 lofts 6-95, 6-97, 6-99 sketch 15-4 sweep sections 6-187, 6-189 projected curves 5-15 replace a sketch 5-19 sketch onto face 5-18 sketch onto sketch 5-18 projected dimensions in drawings 11-10 projected tolerance zone 12-62 projected views 11-26 projection 11-19 during view rotation 11-49 first and third angle 11-4, 11-19 split lines 5-20 propagate 12-48, 12-51 properties 7-2 annotations 9-73, 12-32 assemblies 9-9, 9-73 bill of materials 12-95 components 9-9, 9-67 configurations 10-4, 12-98 custom 7-33, 12-41 datum targets 12-60 design tables 10-5, 10-32 documents 11-7 drawing sheets 11-4 drawing views 11-46 files 7-33 layers 11-58 OLE objects 2-97 sub-assemblies 9-9 PropertyManager 2-4 auto-show 17-2 overview 2-4 skin 17-6 split panel display 2-48 proportional splines 3-47 PTZ. See projected tolerance zone 12-62 publish eDrawings 13-24 Q
quality 13-14 drawing view display 11-11, 11-16
SolidWorks 2004 Reference Guide
STL files 13-14 quick tips 2-91 R
radial center mark lines 12-50 radial dimensions 12-19, 12-22, 12-24 radians 17-28 radiate surface 6-175 radius 12-10 arc dimensions 3-35 circular sketch step and repeat 3-19 control points 6-67 dimension display 12-6, 12-10 fillets 3-31, 6-60 of curvature 7-31, 7-39, 7-40 range, print 2-15 rapid prototyping files 13-37 read-only 17-15 block settings 12-38, 12-69 dimensions 12-10 drawing view properties 11-46 external references 17-15 open 2-53 reload/replace 2-42 realign drawing views 11-49 RealView graphics 2-72 rebuild 2-36 interrupt 7-32 models 2-36 symbol 2-50 updating drawing views 11-47 record macro 2-92 rectangles 3-64 redo 2-36 redraw 2-36 reference axis 5-12 reference dimensions 12-16 baseline 12-17 ordinate 12-17 parentheses 12-17, 17-21 reference edges for auxiliary views 11-28 reference geometry 5-1 axes 5-12 composite curves 5-21 convert sketch entities 5-15 curves 5-15 helix 5-17 insert into drawings 12-2, 12-4 planes 5-2 points 5-22 spiral 5-17 Reference Geometry toolbar 2-31 reference plane normal to edge 3-13 reference points 5-22 reference points in sketch driven patterns 6-123 referenced documents 17-15 load 17-15 open read-only 17-15 save read-only 17-15 search for 9-44 referenced files 17-16 in assemblies 9-8
Index-19
locations 9-8 refresh screen. See redraw 2-36 regenerate. See rebuild 2-36, 7-32 relations 3-42 add relations 3-41 automatic 3-40 callouts 3-43 dangling 7-4 display/delete 3-41 equal length/radii 3-45 geometric 3-40 mathematical 7-14 parent/child 2-46 replace entity 3-41 sketch relations in configurations 10-9 relative to model views 11-22 reload 2-42 shared documents 2-42 sheet format 11-4 remove crop view 11-33 removed tangent edge 11-57, 17-5 rename 7-28 features 2-43 files 7-28, 9-37, 9-38 flat pattern configuration 11-21 menu items 2-85 planes 5-1 reorder 9-39 assembly components 9-39, 9-53 bends 15-31 reorderfeatures 2-43 repair imported document 13-6 repair sketch 4-10 replace 9-7 assembly components 9-7 background images 13-38 mated entities 9-8 shared documents 9-7 sketch entities 3-44 surfaces 6-180 reset size of OLE objects 2-97 resize 7-3 features 6-208, 7-1, 7-3 planes 5-10 view boundaries 11-9 resolve 9-63 ambiguity 7-27 assembly components 9-63, 9-64 lightweight components 9-64 lightweight drawings 11-16 restore 3-33 broken views 11-35 dimensions 3-33 retain folder structure 2-58 reverse surface 6-164 revert model to earlier state 2-47 revision tables 12-91 custom property 17-4 options 17-26 symbols 17-26 revolve 6-132 features 6-132
Index-20
surfaces 6-151 ribs 6-135 detailed previews 6-215 drafts 6-138 linear and natural types 6-136, 6-138 open sketch 6-139 right 2-40, 3-4 right-mouse menus. See shortcut menus 2-8 rigid sub-assemblies 9-41 rip 15-30 roll back 9-53 assemblies 9-53 rollback bar 2-47 rotate 2-79 assembly components 9-12, 17-13 blocks 12-74 center marks 12-48 drawing views 11-49, 11-50 sketches 3-27 surface finish symbols 12-56 views 2-79 roughness 12-56 round corner fillets 6-61 row numbers 12-96 ruled surfaces 8-9 rulers in drawings 11-8 run macro 2-93 S
sat files (ACIS) 13-17 satisfied sketch dimensions/relations 3-43 save 2-34 assemblies 7-10, 9-6, 9-7, 9-46 assembly as multibody part 7-10 automatic save 17-19 blocks 12-69 design tables 10-22 dimensions 3-33 documents 2-34 drawings 11-1, 11-13 DXF/DWG mapping file 13-23 files 2-34 IGES assemblies in single files 13-11 properties in sheet formats 11-7 save as 2-34, 2-82, 7-10, 9-6, 9-7 save as copy 9-6, 9-7 selection criteria for components 9-68 sheet formats 11-6 table driven patterns 6-125 templates 2-52 VRML assemblies in single files 13-9 scale 6-141 automatic 11-9, 17-4 blocks 12-69, 12-74 custom 11-9 detail views 11-32, 17-4 drawings 11-4, 11-9 parent 11-9 parts 6-141 predefined views 11-24 print drawings 2-15 section lines 11-42
sketches 3-27 text of annotations 12-32, 17-25 scaling factor in mold design 8-4 scan equal 3-45 schematic 11-44 scope 9-56 assembly features 9-56 Collision Detection 9-74 multibody parts 9-56 Physical Dynamics 9-75 section views of assemblies 11-41 screen redraw 2-36 screws 9-77, 9-79 scroll. See pan 2-79 search 9-44 file locations for external references 9-44 results for assemblies 9-46 second arc condition 12-10 second arrow 12-10 second outside arrow 12-10 section display types 17-21 section lines 11-37 modify 11-40 stepped 11-37 straight 11-37 troubleshooting 11-41 section properties 7-38 section scope in drawings 11-40, 11-41 section views 11-37 aligned 11-42 assemblies 7-35, 11-40 auto hatching 11-38 broken-out 11-34 copy with parent view 11-50 create 2-73, 11-37 display only surface cut 11-42 drawings 11-37 hide with parent view 11-51 modify 11-40 partial 11-37 parts 7-35 planes 7-37 section line properties 11-42 Section View PropertyManager 2-74 selection 7-36 troubleshooting 11-41 VRML files 13-40 seed faces 6-161 seed features 6-110, 6-114, 6-119, 6-123, 6-129 select 2-60 area of drawing to print 2-15 chain 2-62 contours 3-19 drag select 2-60 from FeatureManager design tree 2-50 hidden entities 11-51, 17-4 in graphics area 2-60 loops 2-65 midpoints 2-63, 5-15 multiple items 2-60 other 2-63 select using envelope 9-66
SolidWorks 2004 Reference Guide
silhouettes 3-8 sketch entities 2-60 tables 12-76 tangency 2-65 through transparency 2-66, 17-8 views 11-8 selection 2-64 box 2-64 loop 2-65 partial loop 2-61 tangent 2-65 selection criteria for components 9-68 selection filter 2-63 hot keys 2-63 toolbar 2-63 send mail 2-20 assemblies 2-20 drawings 11-12 parts 7-32 service packs 2-91 set up drawing sheet 11-4 setback fillets 6-62 shaded 2-74 cosmetic threads 12-54, 17-25 preview 2-68, 17-10 sketch planes 3-12, 5-8 views 2-59, 2-74, 17-5 shaded with edges 2-75 shaft Fit 12-8, 12-29 shape 6-142, 6-144 feature adjustment controls 6-144 features 6-142 pressure and curve influence sliders 6-144 resolution slider 6-145 stretch and bend sliders 6-145 shared files 2-42 shared values 7-17 sheet formats 11-3 anchor points 11-5, 12-77 custom 11-5 lines 11-5 link notes to properties 11-7 new 11-3 new drawings 11-3 note text 11-5 save 11-6 sheet metal parts auto reliefs 15-28, 15-29 base flange 15-2 bends 15-9, 15-12, 15-13, 15-14, 15-22, 15-23, 15-24, 15-25, 15-29, 15-31, 15-32, 15-34
break corner 15-35 conical faces 15-15 cuts 15-34, 15-35 cylindrical faces 15-40 design methods 15-18, 15-19, 15-20, 15-21 drawings 11-21, 15-41 edge flange 15-3, 15-4 FeatureManager design tree 15-2, 15-17 flat pattern 15-32, 15-42 flat pattern configuration 11-21, 15-44 flatten 15-32
Index-21
fold 15-45 forming tools 15-25, 15-27, 15-28, 15-32, 15-42 hems 15-10 import 15-17 inserting bends 15-31 jog 15-36 lofted bends 15-38 mirror 15-33 miter flange 15-4, 15-6, 15-7 overview 15-1, 15-18, 15-19, 15-20, 15-21 rip 15-30 simplify bends 15-43 tabs 15-9 trim bends 15-8 unfold 15-32, 15-42, 15-45 walls 15-16 Sheet Metal toolbar 2-31 sheet properties 11-4 sheets. See drawing sheets 11-5 shells 6-145, 6-146, 6-147 shortcut 2-18 customize shortcut menus 2-86 keys 2-18 menus 2-8, 12-6 show 11-51 alignment 12-22 assembly components 9-62, 9-67 axes 5-12 bodies 6-175 component configuration descriptions 2-45 component configuration names 2-45 component descriptions 2-44 configuration descriptions 2-45 cosmetic threads 12-27, 12-54 curvature combs 3-52 dimension extension lines 12-24 dimensions 12-27 drawing views 11-51 edges in drawings 11-51 explode steps 9-71 feature descriptions 2-44 hidden edges in drawings 11-52, 17-4 hidden views 11-51 in design tables 10-26 planes 5-10 show annotation link errors 12-41 show STL info before saving file 13-14 sketches in drawings 11-52 using envelopes 9-65 shut-off surfaces 8-9 side views 11-17 silhouettes 3-8, 5-20, 12-16 simple hole 6-74 simplify 9-61 assemblies 9-61 bends 15-43 complex models 10-1 geometry 13-6 splines 3-49 simulation. See Physical Simulation 9-33 size features 6-208 sketch driven patterns 6-121
Index-22
sketch entities 3-57 arcs 3-59, 3-68 autodimension 3-39 centerlines 3-58 circles 3-55 copy 3-15, 3-27 ellipses 3-57 extend 3-22 lines 3-53, 3-69, 3-70 move 3-15, 3-27 parabolas 3-61 parallelograms 3-65 points 3-55, 3-73 polygons 3-63 rectangles 3-64, 3-65 rotate 3-15, 3-27 scale 3-15, 3-27 select 2-60 splines 3-46, 3-71 text 3-65 Sketch toolbar 2-32, 3-68 sketch tools 2-32 autodimension 3-39 chamfer 3-31, 3-58 circular step and repeat 3-17 construction geometry 3-21 convert entities 3-22 curvature combs 3-52 diagnostics 3-16, 3-45 extend 3-22 face curves 3-23 fillets 3-31, 3-58 intersection curves 3-24 linear step and repeat 3-25 mirror 3-27 modify 3-9 move/copy 3-15 offset entities 3-30 patterns 3-17, 3-25, 6-108 picture 3-67 select 2-60 split entities 3-32 trim entities 3-32 sketches 3-1 3D 3-68 align 4-6 assemblies 9-54 autodimension 3-39 broken views 11-35 close 3-11, 3-21 colors 3-43 complexity 3-5 copy 3-27 curves 3-22 cut 3-8 derived 3-11 dimensions 3-33, 10-8 edit 3-2, 3-10, 3-12 equations 3-33 exit 3-2, 3-11 extract 4-5 frame points 3-49
geometry 3-14, 3-21 grids 3-13 imported 13-22 in drawings 11-10, 11-28, 11-30, 11-37, 11-40, 11-42, 11-52, 11-56
inferencing 3-6, 3-14 modes 3-7, 3-8 move 3-9, 3-15 new 3-2, 3-6 no solve move 3-15 options 17-7 origins 3-5 parts 3-3 paste 3-8 patterns 3-17, 3-25, 6-123 planes 3-12, 3-13, 10-9 relations 3-40, 3-42, 3-43, 3-44, 10-9 repair 4-10 rotate 3-27 scale 3-27 select chain 2-62 splines 3-49 starting a sketch 3-3, 3-4, 3-5 status 3-43 status bar 3-5 skins 2-87, 17-6 slant extension lines 12-6, 12-24 SldTrans 1.0 (Pro/ENGINEER) 13-33 SldUG 1.0 (Unigraphics II) 13-39 Smart Fasteners 9-77 add nuts and washers 9-86 bolt patterns 9-89 bottom stack 9-78, 9-86 change type 9-85 configurations 9-89 defaults 9-78, 9-90 edit 9-85, 9-86, 9-87 flip 9-85 holes 9-77, 9-83 insert 9-78 overview 9-77 part numbers 9-88 patterns 9-83 PropertyManager 9-78 top stack 9-78, 9-86 unsupported hole types 9-83 update 9-90 SmartMates 9-25 feature-based 9-26 geometry-based 9-25 moving components 9-27 pattern-based 9-26 snap 17-28 3D sketches 3-69 blocks 12-69 dimension text 17-21 notes 12-36 software OpenGL 17-10 Solid Edge files 13-36 solid fill 12-66 SolidWorks 2-1 basic concepts 2-2
SolidWorks 2004 Reference Guide
fundamentals 2-1 service packs 2-91 subscription service 2-91 SolidWorks API 2-91 SolidWorks Office toolbar 2-33 SolidWorks web site 2-92 solve 3-14 equations 7-14 mategroups 9-18 move/copy 3-15 relations in imported drawings 3-19 sketch geometry 3-14 sort 12-76 space handles 3-75 spin box increments 3-33, 12-26, 17-18 spiral 5-17 splines 3-46 3D 3-71 curvature combs 3-52 fit spline 3-48 inflection points 3-52 insert points 3-49 minimum radius 3-53 moving frames 3-49 proportional 3-47 simplify 3-49 Spline Tools toolbar 2-33 split 2-48 bar 2-4 entities 3-32 hole series 9-87 panel display 2-43, 2-48 parts 7-23 tables 12-76 split lines 5-20 balloon style 12-42 drafts 6-35, 6-37 fillets 6-71, 6-73 lofts 6-96 projection 5-20 silhouette 5-20 surfaces 5-20 spot lights 7-49 springs 9-34 stacked balloons 12-44, 12-46, 17-23 standard 3 views 11-17, 11-19 standard mates 9-14, 9-15 Standard toolbar 2-33 Standard Views toolbar 2-40 standards 17-19 ANSI 1982 12-58 ANSI basic tolerances 17-21 holes 6-80, 6-86 surface finish symbols 12-56, 12-57, 17-19 welds 9-58 start command when creating new drawing 11-21 statistics, assembly 9-9 status bar 2-10, 3-5 STEP files 13-37 edit imported features 13-4 export 13-9, 13-13 import 13-3
Index-23
import options 13-37 import surfaces 13-3 import units 13-7 open 2-53 wireframe import 13-37 STL files (stereolithography) 13-37 export 13-9, 13-14 export options 13-9, 13-14 stop current jump 2-41 stop macro 2-93 stp files (STEP) 13-37 straight break line cut style 11-37 styles 11-56 cuts in broken views 11-35, 11-37 detail circles 11-32, 11-33 lines in drawings 11-55, 11-56 lines in layers 11-58 sub-assemblies 9-36 automatic change of editing focus 9-41 create 9-36 dissolve 9-39 editing limitations 9-41 flexible 9-41 forming a new 9-37 inserting a new 9-39 lightweight 9-61 manual change of editing focus 9-40 modify 9-36 rigid 9-41 summary 7-33 suppress 10-27 assembly components 9-63, 9-64 components or features in design tables 10-27 features 2-43, 7-2, 7-20, 7-21 mates 9-28 surface errors on import 13-3 surface finish symbols 12-4, 12-56, 17-25 surface flaws on import 6-164 surface representation in IGES 13-12 surfaces 6-148 bodies 6-149 colors 7-8, 17-8 cut 6-49, 6-195 delete 6-177, 6-179 draft analysis 6-198 drafts 6-32 extend 6-157 extruded 6-150 filled 6-164 fillets 6-64, 6-156, 6-159 hide and show bodies 6-175 import 13-3 knit 6-161 lofted 6-153 mid surface 6-162 molds 8-6, 8-7, 8-9 offset 6-154 optimize 6-164 parting 8-7 planar 6-149, 7-30 planes 5-2, 5-5 radiate 6-175
Index-24
replace 6-180 reverse 6-164 revolve 6-151 ruled 8-9 shut-off 8-9 swept 6-152 thicken 6-195 trim 6-170 untrim 6-172 Surfaces toolbar 2-40 sweeps 6-182 advanced smoothing 6-191 align with end faces 6-190 follow path 6-193, 6-194 follow path and guide curves 6-193 guide curves 6-187, 6-189 intermediate sections 6-189 keep normal constant 6-193 orientation 6-193, 6-194 overview 6-182 simple 6-183 smoothing 6-190 surfaces 6-152 tangency 6-191, 6-193 thin feature 6-183 symbols 12-10 flag 12-10 geometric tolerancing 12-62 in note text 12-10, 12-38 revision 12-91, 12-92, 17-26 symmetric relations 3-41 symmetric tolerance 12-8, 12-28 symmetry 3-58 about centerlines 3-58 mates 9-24 synchronize detached drawings 11-13 system color options 17-6 system options 2-81 T
table driven patterns 6-123, 6-125 table pattern coordinates 6-125 tables 12-76 anchors 12-77 bill of materials 12-81 columns 12-85, 12-90, 12-93, 16-17 custom templates 12-79 design tables 10-18 drag 12-76 edit 12-76 format 12-79, 12-80 hole tables 12-86 options 17-26 revision tables 12-91 templates 12-78, 12-79 weldment cut lists 16-15 tabs on sheet metal parts 15-9 tag name 12-38, 12-69 tags for hole tables 12-86, 12-89 tangent 3-42 arcs 3-59 lofts 6-101, 6-103, 6-192
mates 9-14, 9-22 selection 2-65 sketch relations 3-42 sweeps 6-190, 6-193 tangent edge display 11-57, 17-5 tangent to surface planes 5-5 tap holes 6-87 templates 2-52 bill of materials 12-78 create 2-52 default 2-53 file types 2-52 predefined views 11-24 schematic 11-44 tables 12-78, 12-79 tabs 2-52 view reference geometry 5-1 temporary axes 5-12 text 17-25 dimensions 12-22 extruded text on part 3-65 notes 12-36 size of annotations 12-32, 17-25 sketch 3-65 textures 2-39, 2-77 thicken surfaces 6-195 thickness 11-56, 11-58 thin features 6-45, 6-46, 6-94, 6-191 third angle projection 11-19 third party products. See add-ins 2-89 threads, cosmetic 12-54 through lines/points planes 5-2 thumbnail graphics 14-9 palette items 14-9 TIFF files 13-38 export 13-9, 13-15 export options 13-9, 13-15 import 13-38 tile graphics windows 2-3 time-dependent features 9-49 tip of the day 2-10 tolerances 12-28 chamfer dimensions 12-20 dimensions 12-28 Fit 12-8, 12-28, 12-29 geometric tolerancing 12-60 include prefix 17-21 options 17-21 simplify splines 3-49 toolbars 2D to 3D 2-22 Align 2-22 Annotations 2-23 arrange 2-21 Assembly 2-24 Curves 2-25 customize 2-86 Dimensions/Relations 2-26 dispaly or hide 2-21 Drawing 2-26 Explode Sketch 2-27 Features 2-27
SolidWorks 2004 Reference Guide
Font 2-29 Layer 2-29 Line Format 2-29 Macro 2-30 Mold Tools 2-30 Reference Geometry 2-31 Selection Filter 2-63 Sheet Metal 2-31 Simulation 2-32 Sketch 2-32 SolidWorks Office 2-33 Spline Tools 2-33 Standard 2-33 Standard Views 2-40 Surfaces 2-40 Tools 2-41 View 2-41 Web 2-41 Weldments 2-43 tooling split 8-9 tools 2-41 check 7-31 curvature 7-39 equations 7-14 mass properties and section properties 7-38 measure 7-18 Tools toolbar 2-41 tooltips 2-10 top 2-40 gradient color 17-6 orientation 2-75, 3-4 views 11-17 top-down assembly design 9-1 trailing zeros 17-19 transitional 12-8, 12-29 translate sketches 3-15 translators 13-2 ACIS 13-7, 13-9, 13-17 Autodesk Inventor 13-17 CADKEY 13-17 CATIA Graphics 13-18 DXF 3D 13-18 HCG 13-26 HOOPS 13-27 IGES 13-7, 13-11, 13-27, 13-28, 13-29 JPEG 13-29 Mechanical Desktop 13-29 Parasolid 13-13, 13-33 PDF Files 13-33 Pro/ENGINEER 13-33, 13-34, 13-35, 13-36 Solid Edge 13-36 STEP 13-7, 13-13, 13-37 STL 13-8, 13-14, 13-37 Unigraphics 13-39 VDAFS 13-7, 13-39 Viewpoint 13-39 VRML 13-8, 13-15, 13-40 ZGL 13-40 transparency 2-66, 2-79, 3-12, 5-8, 9-48, 9-62, 17-8, 17-10 triad 9-11, 9-12 move 9-11 rotate 9-12
Index-25
trigonometric functions in dimensions 3-33 trim 3-32 sheet metal bends 15-8 sketch segments 3-32 surfaces 6-170 trimmed surfaces in IGES 13-11 troubleshooting section views 11-41 True Position Tolerancing 12-62 true type dimensions 11-10 U
un-break broken views 11-35 under defined 2-46 sketch geometry 3-43 sketches 3-43 undercut detection 8-4 underlined leader 12-38 undo 2-36 Unigraphics II files 13-39 units 17-28 dimension properties 12-10 options 17-28 spin box increments 17-18 unlink values 7-17 unlock external references 9-43 unsuppress 7-21 components 10-27 features 7-2, 7-20, 7-21, 10-27 untrim surface 6-172 update 11-45 dependent drawing views 11-49 detached drawings 11-13 drawing views 11-45 paths in assemblies 9-43 section views 11-40 views in detached drawings 11-13 user notes in design tables 10-33 UV curves. See face curves 3-23 V
variable radius fillets 6-64 variable thickness shells 6-146 variables 12-52, 12-53 vary sketches in patterns 6-128 VBA 2-94 VDAFS files 13-39 edit imported features 13-4 export 13-9 import 13-3 import options 13-7 import surfaces 13-3 import units 13-7 open 2-53 vertical 3-34 align drawing views 11-49 breaks 11-35 dimensions 3-34 ordinate dimensions 12-19 rotate views 11-49 vertices 5-13 angular dimensions 3-37 baseline dimensions 12-17
Index-26
chamfers 6-7 coordinate system 5-13 end condition 6-76 reference points 5-22, 6-123 view 2-75 animation speed 17-18 axes 5-12 bodies 6-175 dependencies 9-2 features 9-2 mates 9-3 orientation 2-75 planes 5-10, 11-53 reference geometry 5-1 section 7-37, 11-37 temporary axes 5-12 view boundaries 11-9 detached drawings 11-13 resize 11-9 view label options 17-27 View only DXF/DWG 13-20 view only mode 2-53 view rotation options 17-18 View toolbar 2-41 view/hide toolbars 2-21 Viewpoint files 13-39 views 2-68 draft quality 2-68 hidden in gray 2-69 hidden lines removed 2-69 middle mouse button 2-78 new windows 2-3 orientation 2-75 pan 2-79 perspective 2-72 previous 2-80 quality 11-11 RealView graphics 2-72 rotate 2-79 shaded 2-74 shaded with edges 2-75 SolidWorks Viewer 2-78 textures 2-77 view-only mode 2-78 wireframe 2-78 zoom 2-80, 2-81 virtual sharps 3-58, 3-75, 17-25 visible 10-26 components in a design tables 10-26 cosmetic threads 12-54 edges in drawings 11-55 layers 11-58 tangent edge display 11-57, 17-5 Visio 11-44 Visual Basic for Applications 2-94 VRML files 13-40 edit imported features 13-4 export 13-9 export options 13-9 import 13-3 import surfaces 13-3 open 2-53
W
walls in sheet metal parts 15-16 washers 9-82, 9-86 watermarks 11-13, 11-16 web folders change URL 2-58 copy referenced files to server 2-58 opening files from 2-57 overview 2-57 saving files to 2-57 Web support 2-42 open address 2-42 stop jump 2-41 Web toolbar 2-41 weld beads 9-58 automatic weld symbols 9-60 create 9-58 edit 9-58 select faces 9-60 standards 9-58 types 9-58 weld symbols 12-64 ANSI 12-65 display 17-19 edit 12-64 favorites 12-4 fonts 17-26 GOST 12-66 insert 12-64 options 17-19 properties 12-64 weldment cut lists 16-15 anchor 12-77 configurations 16-15 custom properties 16-15 item numbers 16-16 templates 12-78 weldments 16-1 corner treatments 16-4 custom properties 16-18 cut lists 16-15 end caps 16-13 fillet weld beads 16-10 gussets 16-7 structural members 16-1 sub weldments 16-14 trim and extend 16-5 weldment drawings 16-14
SolidWorks 2004 Reference Guide
Weldments toolbar 2-43 What's this? 2-10 What's wrong? 2-12 windows 2-2 cascade 2-3 close all 2-2 drawings 11-8 new 2-3 tile 2-3 Windows Explorer 2-55 wireframe 2-78, 17-5 witness lines. See extension lines 12-24 wizards 2-90 conversion 2-89 copy options 2-90 holes 6-77 work features, MDT files 13-29 wrap 6-216 X
X display 12-20 x_b or x_t files (Parasolid) 13-33 xmt_bin or xmt_txt files (Parasolid) 13-33 XREFs 13-19 Z
zebra stripes 7-42, 7-44 zeros 17-19 color default 10-33 configuration parameter default 10-24 leading 17-19 trailing 17-19 ZGL files 13-40 zig zag break line cut style 11-37 zone 12-93 zoom 2-81 in/out 2-81 to area 2-80 to fit 2-80 to selection 2-81, 11-8
Index-27
Index-28
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