Unigraphics Nx4 Manual

Practical Applications of NX Student Guide January 2006 MT10050 — NX 4

Publication Number mt10050_g NX 4

Manual History

Manual Revision

Unigraphics Version

Publication Date

Version 15.0

February 1999

Version 16.0

January 2000

Version 17.0

December 2000

Version 18.0

September 2001

Unigraphics NX

September 2002

A

Unigraphics NX 2

September 2003

A

NX 3

November 2004

A

NX 4

January 2006

This edition obsoletes all previous editions. Proprietary & Restricted Rights Notice This software and related documentation are proprietary to UGS Corp. © 2006 UGS Corp. All Rights Reserved. All trademarks belong to their respective holders.

©2006 UGS Corporation All Rights Reserved. Produced in the United States of America. 2

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mt10050_g NX 4

Contents

Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11 Intended Audience . . . . Course Objectives . . . . . Prerequisites . . . . . . . . How to Use This Course Class Standards . . . . . . Part File Naming . . Seed Parts . . . . . . . . Colors . . . . . . . . . . . Definitions of Terms . . .

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11 11 11 12 14 14 15 15 16

Getting Started . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-1 Starting NX . . . . . . . . . . . . . . . . . . . . . . Gateway Application . . . . . . . . . . . . . . . . Cue/Status Line . . . . . . . . . . . . . . . . . . . Windows File Dialogs . . . . . . . . . . . . . . . Activity — Creating a New Part . . . . . Opening Multiple Parts . . . . . . . . . . . . . . Activity — Opening an Existing Part . Activity — Save Part As (Copying a Part) Activity — Closing Parts . . . . . . . . . . . . . Exiting NX . . . . . . . . . . . . . . . . . . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . .

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. 1-2 . 1-3 . 1-4 . 1-5 . 1-7 . 1-9 1-10 1-12 1-14 1-16 1-17

The NX User Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-1 Toolbars . . . . . . . . . . . . . . . . . . . . . . . . . Customizing Toolbars . . . . . . . . . . . . Roles . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Working with Toolbars . . . Activity — Working with Roles . . . . . Mouse Navigation . . . . . . . . . . . . . . . . . . Mouse Pop-up Menu . . . . . . . . . . . . . Graphics Window View Manipulation Selecting Objects . . . . . . . . . . . . . . . . Preview Selection and QuickPick . . . . Activity — Manipulating Views . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . ©UGS Corporation, All Rights Reserved

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. 2-2 . 2-3 . 2-6 . 2-7 2-11 2-14 2-15 2-17 2-19 2-21 2-23 2-25

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3

Contents

Coordinate Systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-1 Overview of Coordinate Systems . . . . Manipulating the WCS . . . . . . . . . . . Move WCS (Dynamics) . . . . . . . . . . . Origin Handle . . . . . . . . . . . . . . . Axis Handles . . . . . . . . . . . . . . . . Rotation Handles . . . . . . . . . . . . Activity — Manipulating the WCS Summary . . . . . . . . . . . . . . . . . . . . .

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. 3-2 . 3-4 . 3-5 . 3-6 . 3-8 . 3-9 3-10 3-18

Introduction to Solid Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-1 Primitives . . . . . . . . . . . . . . . . . . . Block . . . . . . . . . . . . . . . . . . . . . . Activity — Creating a Block . . Cylinder . . . . . . . . . . . . . . . . . . . . Defining Vectors . . . . . . . . . . . Activity — Creating a Cylinder Summary . . . . . . . . . . . . . . . . . . .

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. 4-2 . 4-3 . 4-5 . 4-7 . 4-8 . 4-9 4-11

Positional Form Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-1 Creating Form Features . . . . . . . . . . . . . . . . . . Hole . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Boss . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Positioning Terminology . . . . . . . . . . . . . . . Positioning Methods . . . . . . . . . . . . . . . . . . Activity — Positioning Holes and Bosses . . . Slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Pocket . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Pad . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Additional Positioning Methods . . . . . . . . . . Parameter Entry Options . . . . . . . . . . . . . . Activity — Creating Pockets and Slots . . . . . Groove . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Positioning a Groove . . . . . . . . . . Editing the Size and Location of Form Features . Edit Positioning . . . . . . . . . . . . . . . . . . . . . Error Messages . . . . . . . . . . . . . . . . . . . . . . Editing Features with the Part Navigator . . Activity — Editing Positional Form Features Additional Positioning Techniques . . . . . . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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. 5-2 . 5-5 . 5-7 . 5-8 . 5-9 5-12 5-21 5-23 5-24 5-25 5-28 5-29 5-34 5-35 5-37 5-38 5-41 5-42 5-43 5-48 5-50

Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-1 Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-2 Creating and Editing Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-3 4

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mt10050_g NX 4

Contents

Activity — Getting Familiar with Expressions . . . . . . . . . . . . . . . 6-8 Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-12 Shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-1 Shell Feature Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Creating a Shell Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Creating a Shell Feature . . . . . . . . . . . . . . . . Activity — Creating a Shell and Removing Multiple Faces Activity — Creating a Shell with an Alternate Thickness . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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. 7-2 . 7-3 . 7-5 . 7-8 7-10 7-12

Edge Operations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-1 Overview . . . . . . . . . . . . . . . . . . . . Edge Blend . . . . . . . . . . . . . . . . . . . Activity — Creating Edge Blends Chamfer . . . . . . . . . . . . . . . . . . . . . Activity — Creating Chamfers . . Summary . . . . . . . . . . . . . . . . . . . .

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. 8-2 . 8-3 . 8-6 8-10 8-13 8-16

Model Construction Query . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-1 Visually Inspect the Part . . . . . . . . . . Layers . . . . . . . . . . . . . . . . . . . . . . . Layer Categories . . . . . . . . . . . . . Moving Objects Between Layers . Part Navigator . . . . . . . . . . . . . . . . . Information . . . . . . . . . . . . . . . . . . . Distance . . . . . . . . . . . . . . . . . . . . . . Mass Properties . . . . . . . . . . . . . . . . Activity — Model Construction Query Summary . . . . . . . . . . . . . . . . . . . . .

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. 9-2 . 9-3 . 9-6 . 9-7 . 9-8 . 9-9 9-11 9-12 9-13 9-24

Introduction to Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-1 Definitions and Descriptions . . . . . . . . . . . . . . . . . . . Introduction to Load Options . . . . . . . . . . . . . . . . . . Load Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . Load States . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Load Failure . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Setting Load Options . . . . . . . . . . . . . The Assembly Navigator . . . . . . . . . . . . . . . . . . . . . . Node Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Working with the Assembly Navigator Selecting Components in the Assembly Navigator Selecting Components in the Graphics Window . . Designing in Context . . . . . . . . . . . . . . . . . . . . . . Assembly Navigator Pop-Up Menu Options . . . . . ©UGS Corporation, All Rights Reserved

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. 10-2 . 10-4 . 10-5 . 10-6 . 10-7 . 10-8 10-10 10-11 10-13 10-15 10-16 10-17 10-21

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Contents

Activity — Working with the Assembly Navigator (continued) . . 10-23 Saving the Work Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-26 Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-27 Adding Components & Mating Conditions . . . . . . . . . . . . . . . . . . . 11-1 General Assembly Concepts . . . . . . . . . . . . . . . Assemblies Application . . . . . . . . . . . . . . . . . . . Assemblies Pull-down Menu . . . . . . . . . . . . Assemblies Toolbar . . . . . . . . . . . . . . . . . . . Adding Components to an Assembly . . . . . . Activity — Creating an Assembly . . . . . . . . Mating Conditions . . . . . . . . . . . . . . . . . . . . . . Mate Constraint . . . . . . . . . . . . . . . . . . . . . Align Constraint . . . . . . . . . . . . . . . . . . . . . Angle Constraint . . . . . . . . . . . . . . . . . . . . . Parallel Constraint . . . . . . . . . . . . . . . . . . . Perpendicular Constraint . . . . . . . . . . . . . . Center Constraint . . . . . . . . . . . . . . . . . . . . Distance Constraint . . . . . . . . . . . . . . . . . . Tangent Constraint . . . . . . . . . . . . . . . . . . . The Mating Conditions Dialog . . . . . . . . . . . Tree Listing . . . . . . . . . . . . . . . . . . . . . . . . Repositioning Components . . . . . . . . . . . . . . . . Activity — Mating the Nut Cracker Components Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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. 11-2 . 11-4 . 11-5 . 11-6 . 11-7 11-10 11-12 11-13 11-14 11-15 11-16 11-17 11-18 11-20 11-21 11-22 11-27 11-30 11-34 11-47

Datum Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-1 Datum Feature Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . Datum Planes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Creating Relative Datum Planes . . . . . . . . . . . . . . . . . . . Common Datum Plane Types . . . . . . . . . . . . . . . . . . . . . . Activity — Creating Relative Datum Planes . . . . . . . . . . . Selecting and Using Datum Planes . . . . . . . . . . . . . . . . . Activity — Cylindrical Faces and Datum Planes . . . . . . . . Activity — Creating a Feature on a Relative Datum Plane Activity — Creating a Hole Corner to Corner . . . . . . . . . . Datum Axis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Datum Axis Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Editing Datum Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Constraining Locations using Datums . . . . . . Datum CSYS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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. 12-2 . 12-3 . 12-4 . 12-6 12-16 12-21 12-23 12-28 12-33 12-37 12-38 12-43 12-44 12-51 12-52

Sketching . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-1 Sketching Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-2 6

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Contents

Sketches and the Part Navigator . . . . . . . . . . . . Sketch Visibility . . . . . . . . . . . . . . . . . . . . . . . . Creating a New Sketch . . . . . . . . . . . . . . . . . . . . . . The Active Sketch . . . . . . . . . . . . . . . . . . . . . . . Sketch Creation Steps . . . . . . . . . . . . . . . . . . . . Activity — Sketch Creation . . . . . . . . . . . . . . . . Sketch Curves . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Using the Sketch Profile Tool . . . . . . Creating Fillets . . . . . . . . . . . . . . . . . . . . . . . . . Trimming and Extending Curves . . . . . . . . . . . . Activity — Creating Fillets . . . . . . . . . . . . . . . . Activity — Using Quick Trim and Quick Extend Sketch Points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Dimensional Constraints . . . . . . . . . . . . . . . . . . . . Activity — Adding Dimensional Constraints . . . Editing Dimensions . . . . . . . . . . . . . . . . . . . . . . Activity — Editing Sketch Dimensions . . . . . . . . Geometric Constraints . . . . . . . . . . . . . . . . . . . . . . Show/Remove Constraints . . . . . . . . . . . . . . . . . Constraint Conditions . . . . . . . . . . . . . . . . . . . . Activity — Adding Constraints . . . . . . . . . . . . . Activity — Constraining a Profile . . . . . . . . . . . Activity — Sketching and Constraining a Gasket Convert To/From Reference . . . . . . . . . . . . . . . . Activity — Constraint Conditions . . . . . . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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Swept Features and Boolean Operations . . . . . . . . . . . . . . . . . . . . 14-1 Types of Swept Features . . . . . . . . . . . . . . . . . . . . . . . . . Extrude . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Starting the Draglink . . . . . . . . . . . . . . . . Boolean Operations . . . . . . . . . . . . . . . . . . . . . . . . . . Start and End Limit Options . . . . . . . . . . . . . . . . . . . Extrude with Offset . . . . . . . . . . . . . . . . . . . . . . . . . . Extrude with Draft . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Extruding with Offsets . . . . . . . . . . . . . . . Selection Intent . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Extruding Using Selection Intent . . . . . . . Sweep Along Guide . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Sweeping Along an Open Guide String . . . Activity — Sweeping Along a Closed Guide String . . . Revolve . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Creating Revolved Features . . . . . . . . . . . Activity — Adding a Revolved Feature to the Draglink Activity — Extruding to a Face . . . . . . . . . . . . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ©UGS Corporation, All Rights Reserved

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. 14-2 . 14-3 . 14-7 . 14-9 14-13 14-14 14-16 14-17 14-22 14-25 14-27 14-29 14-33 14-36 14-38 14-42 14-45 14-48

Practical Applications of NX

7

Contents

Editing the Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-1 Accessing the Options to Edit Features . . . . . . . . . . . . . Part Navigator . . . . . . . . . . . . . . . . . . . . . . . . . . . . Deleting Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Update Failures . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Edit and Delete Features . . . . . . . . . . . . . . . Activity — Using the Update Tool . . . . . . . . . . . . . . . . . Activity — Reordering Features with the Part Navigator Delaying Model Updates . . . . . . . . . . . . . . . . . . . . . . . . Move Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Reattaching a Feature . . . . . . . . . . . . . . . . . . . . . . . . . Activity — Reattaching and Moving Features . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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. 15-2 . 15-3 . 15-7 . 15-8 15-11 15-15 15-18 15-21 15-22 15-23 15-27 15-32

Instance Arrays . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-1 Instance Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Rectangular Instance Array . . . . . . . . . . . . . . . . . . . . . Circular Instance Array . . . . . . . . . . . . . . . . . . . . . . . . Activity — Rectangular Instance Array . . . . . . . . . . . . Activity — Circular Instance Array . . . . . . . . . . . . . . . Activity (Optional) — Associativity of the Rotation Axis Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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The Master Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-1 The Assembly Modeler . . . . . . . . . . . . . . . . . . . . . Master Model Example . . . . . . . . . . . . . . . . . . Activity — Exploring a Master Model Assembly Activity — Creating a Non-Master Part . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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Introduction to Drafting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-1 Working with Drawings . . . . . . . . . . . . . . . . . . . . . Creating New Drawing Sheets . . . . . . . . . . . . . . Opening a Drawing . . . . . . . . . . . . . . . . . . . . . . Editing a Drawing . . . . . . . . . . . . . . . . . . . . . . . Deleting a Drawing . . . . . . . . . . . . . . . . . . . . . . Activity — Creating New Drawing Sheets . . . . . Activity — Opening and Editing Drawing Sheets Drawing Monochrome Display . . . . . . . . . . . . . . View Preferences . . . . . . . . . . . . . . . . . . . . . . . . . . Hidden Lines . . . . . . . . . . . . . . . . . . . . . . . . . . Smooth Edges . . . . . . . . . . . . . . . . . . . . . . . . . . Virtual Intersections . . . . . . . . . . . . . . . . . . . . . Adding a Base View . . . . . . . . . . . . . . . . . . . . . . . . View Creation Options Bar . . . . . . . . . . . . . . . . 8

Practical Applications of NX

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. 18-2 . 18-3 . 18-4 . 18-5 . 18-7 . 18-8 18-12 18-15 18-17 18-18 18-19 18-20 18-21 18-22

mt10050_g NX 4

Contents

Adding Projected Views . . . . . . . . . . . . . . . . . . Editing Existing Views . . . . . . . . . . . . . . . . . . . Removing Views From a Drawing . . . . . . . . . . . Activity — Adding Views to a Drawing . . . . . . . Utility Symbols . . . . . . . . . . . . . . . . . . . . . . . . . Creating a Linear Centerline . . . . . . . . . . . . Activity — Creating a Linear Centerline . . . Manually Creating a Cylindrical Centerline . Activity — Creating a Cylindrical Centerline Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . Annotation Preferences . . . . . . . . . . . . . . . . Dimension Preferences and Placement . . . . . Appended Text . . . . . . . . . . . . . . . . . . . . . . Tolerances . . . . . . . . . . . . . . . . . . . . . . . . . . Text Orientation and Text Arrow Placement Editing an Existing Dimension . . . . . . . . . . Activity — Creating Dimensions . . . . . . . . . Text Creation . . . . . . . . . . . . . . . . . . . . . . . . . . Creating Notes . . . . . . . . . . . . . . . . . . . . . . Activity — Creating Notes and Labels . . . . . The Annotation Editor . . . . . . . . . . . . . . . . . Editing Notes . . . . . . . . . . . . . . . . . . . . . . . Activity — Creating More Notes . . . . . . . . . Master Model Drawing Guidelines . . . . . . . . . . Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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18-24 18-26 18-27 18-28 18-33 18-36 18-37 18-40 18-41 18-45 18-47 18-48 18-50 18-52 18-53 18-54 18-56 18-61 18-62 18-65 18-67 18-71 18-72 18-75 18-76

Additional Projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-1 Project 1 . Project 2 . Project 3 . Project 4 . Project 5 . Project 6 . Project 7 . Project 8 . Project 9 . Project 10 Project 11 Project 12 Project 13 Project 14 Project 15 Project 16 Project 17 Project 18 Project 19

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A-2 A-3 A-4 A-6 A-8 A-10 A-12 A-14 A-16 A-18 A-19 A-21 A-23 A-25 A-27 A-28 A-30 A-32 A-34

Practical Applications of NX

9

Contents

Project 20 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-36 Project 21 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-38 Project 22 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-40 Expression Operators . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-1 Overview . . . . . . . . . . . . . . Operators . . . . . . . . . . . . . . Precedence and Associativity Legacy Unit Conversion . . . Built-in Functions . . . . . . . .

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B-1 B-2 B-3 B-4 B-5

Point Constructor Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-1 Overview . . . . . . . . . . . . . . . . Methods to Specify a Point . . . WCS and Absolute Coordinates Offset . . . . . . . . . . . . . . . .

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Customer Defaults . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . D-1 Overview . . . . . . . . . . . . . . . . . . . . . . . Customer Defaults . . . . . . . . . . . . . . . . Customer Defaults Levels . . . . . . . . Setting Customer Defaults . . . . . . . USER, GROUP, and SITE directories Managing Your Changes . . . . . . . . . Updating to a New Release of NX . .

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D-1 D-2 D-3 D-6 D-8 D-9 D-10

Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Index-1

10

Practical Applications of NX

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mt10050_g NX 4

Overview Intended Audience This course is suited for designers, engineers, manufacturing engineers, application programmers, NC programmers, CAD/CAM managers, and system managers who have a need for understanding and using NXsoftware.

Course Objectives After successfully completing this course, the student should be able to: •

Demonstrate knowledge of CAD/CAM theory.

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Open and examine models.

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Create and edit parametric solid models.

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Create and modify basic assembly structures.

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Create and modify simple drawings.

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Modify existing geometry.

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Apply the standards used in class.

Prerequisites There are no prerequisites for this class.

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Practical Applications of NX

11

How to Use This Course

How to Use This Course Activities The format of the activities is consistent throughout this course. Steps are labeled and specify what will be accomplished at any given point in the activity. Below each major step are bulleted steps which describe the individual actions that must be taken. As your knowledge of NX increases, the action boxes will seem redundant as the step text becomes all that is needed to accomplish a given task. Step 1:

Open the design_topic_1 part. Choose the Open icon.

(File→Open)

Double-click on the parts folder. Select the design_topic_1 part and choose OK.

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Practical Applications of NX

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mt10050_g NX 4

Overview

Mouse Buttons The mouse will be used throughout this course to make selections. Examples of different mouse devices are shown. The mouse buttons are referred to as the first, second, and third mouse buttons, starting from left to right. On mouses with mouse wheels, the wheel acts as mouse button 2 when it is pressed. On two-button mouses, the buttons represent 1 and 3. Both buttons pushed together equals mouse button 2.

The functional assignment of the mouse buttons can be reversed in most operating systems for users who prefer that setup. The following abbreviations are used for the mouse buttons in this course. •

MB1 — Mouse Button 1

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MB2 — Mouse Button 2

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MB3 — Mouse Button 3

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Practical Applications of NX

13

Class Standards

Class Standards The following standards will be used in this course. Standardization allows you to work with and predict the organization of parts created by others. All work should be performed in accordance with these standards.

Part File Naming To facilitate the identification of design models without having to open a part, standard naming conventions can be established for the various files associated with the part definition. An example of a file naming standard is shown below:

1 2 3 4

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Part Number Configuration Revision Extension

Currently up to 128 characters are valid for file names. A four character extension (.prt) is automatically added to define the file type. This means the maximum number of user defined characters for the file name is actually 124.

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Practical Applications of NX

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mt10050_g NX 4

Overview

Seed Parts Seed parts are an effective tool for establishing customer defaults or any settings that are part-dependent (saved with the part). This may include non-geometric data such as: •

Preferences

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Commonly used expressions

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Layer categories

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User-defined views and layouts

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Part attributes Once a seed part is established, it should be write-protected to avoid accidental modification.

Two seed parts are available for use in this course, seedpart_in for inch parts and seedpart_mm for metric parts. These parts incorporate the standards described above.

Colors The following colors are preset to indicate different object types: Object Solid Bodies Sheet Bodies Lines and Arc (non-sketch curves) Conics and Splines (non-sketch curves) Sketch Curves Reference Curves (in sketches) Datum Features Points and Coordinate Systems System Display Color

Default Color Light Gray (87) Light Dull Azure (92) Dark Hard Blue (212) Dark Hard Blue (212) Obscure Dull Green (144) Dark Faded Cyan (105) Light Weak Red (81) Dark Hard Blue (212) Orange Orange Red (114)

NX identifies colors using numbers with ID’s that range from 1 to 216.

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Practical Applications of NX

15

Definitions of Terms

Definitions of Terms Explicit Modeling Explicit modeling is modeling that is not parametric. Objects are created relative to model space, not each other. Changes to one or more objects do not necessarily affect other objects or the finished model. Examples of explicit modeling include creating a line between two existing points or creating an arc through three existing points. If one of the existing points were moved, the line/arc would not change. Parametric Modeling A parametric model is one in which the values (parameters) used for the definition of the model are stored with the model for future editing. Parameters may reference each other to establish relationships between the various features of the model. Examples include the diameter and depth of a hole or the length, width, and height of a rectangular pad. The designer’s intent may be that the hole is always as deep as the pad is high. Linking these parameters together may achieve the desired results. This is not easily accomplished with an explicit model. Constraint-based Modeling A constraint-based model is one in which the geometry of the model is driven or solved from a set of design rules applied to the geometry defining the model as constraints. These constraints might be dimensional constraints (such as sketch dimensions or positioning dimensions) or geometric constraints (such as parallelism or tangency). Examples include a line tangent to an arc where the designer intends for that tangent condition to be maintained even though the angle of the line may change or a perpendicular condition being maintained as angles are modified. Hybrid Modeling Hybrid modeling refers to the selectively combined use of the three types of modeling described above. Hybrid modelers allow designers to use parametric modeling where needed without requiring that the entire model be constrained before proceeding. Because of this, designers have more flexibility in modeling techniques. The NXhybrid modeler supports traditional explicit geometric modeling along with constraint-based sketching and parametric feature modeling. All tools are integrated so they can be used in combination.

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Practical Applications of NX

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mt10050_g NX 4

1

Lesson

1

Getting Started Purpose This lesson is a fundamental introduction to working with NX parts. Objectives Upon completion of this lesson, you will be able to: •

Start an NX session.

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Create a New Part.

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Open a Part.

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Copy a Part.

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Close a Part and Exit NX.

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Practical Applications of NX

1-1

Getting Started

1

Starting NX The first step in working in NX is to log on to a workstation and start an NX session. Because this procedure may vary among companies and platforms, consult your system administrator for a site specific procedure to follow. After starting NX, you will see the "No Part" interface. This interface only allows you to perform actions such as changing defaults and preferences, opening an existing part, or creating a new part.

The graphics shown in this text are taken from a workstation with a Windows operating system. The display of windows and dialogs on a UNIX workstation will differ slightly from those shown.

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Practical Applications of NX

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mt10050_g NX 4

Getting Started

1

Gateway Application NX functions are divided into "applications". Gateway is the prerequisite for all other interactive applications, and is the first application you enter when you start NX and open or create a part. Gateway allows the review of existing parts. To create or edit objects within a part, another application, such as Modeling, must be started. 1 — Work and displayed part names 2 — Cue line

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3 — Status line 4 — Resource bar

Practical Applications of NX

1-3

Getting Started

1

Cue/Status Line The Cue/Status line appears at the top of the main application window. The Cue line prompts you for user interaction. The Status line gives you feedback about system activity. To relocate the Cue and Status line below the graphics window, choose Tools→Customize, choose the Layout tab, and change the Cue/Status Position to Bottom. Menu Bar Pull-Down Menus The Menu Bar is a horizontal arrangement of options displayed near the top of the main NX window. These options correspond to different NX functional categories. Clicking the first mouse button (MB1) over a Menu Bar option displays a pull-down menu. Arrows to the right of items in a pull-down menu indicate that further cascading menus are available. By default, menus appear “folded” so that only the frequently used options are shown. The down arrow at the bottom of the menu can be selected to display the full menu.

To permanently display the entire menus, choose Tools→Customize, choose the Options tab, and turn on the Always Show Full Menus option.

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Practical Applications of NX

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mt10050_g NX 4

Getting Started

1

Windows File Dialogs The New Part File, Open Part File, and Save Part File As dialogs have some useful common features. The Look in: option menu shows the name of the current selected drive or folder.

Choosing the arrow on the right side of the box (or anywhere within the box) will list a hierarchy of the available folders and drives. Choosing anywhere away from the list of the available folders and drives will dismiss the listing without selecting another folder or drive.

The list in the window below the Look In: box shows the available folders and files. NX parts have a .prt extension. The Up One Level option works with the Look in: option menu to traverse back up through the folder hierarchy.

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Practical Applications of NX

1-5

Getting Started

1 The Create New Folder option allows new sub-folders to be created in the current folder. The View Menu option menu allows the appearance of the listing in the window to be modified. The default is a List. Selecting the Details button will display a more detailed listing of the files and folders including Name, Size, Type, last Modified date and time, and any Attributes that may apply to the file. Other options include Thumbnails, Tiles, and Icons.

The option at the top right of the dialog changes the cursor to and allows selection of any of the controls in the dialog for a short description of their function.

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Getting Started

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Activity — Creating a New Part In this activity, you will create a new part. Step 1:

Create a new part. Choose the New icon.

(File→New)

The New Part File dialog appears as shown.

Step 2:

Specify the units of measure for the new part. Verify the Millimeters option is selected for the Units.

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Getting Started

1

Step 3:

Key in a new part name. With Mouse Button 1 (MB1), click in the File name field. Key in ***_new_1, where *** represents your initials. This will be a standard practice for this class to ensure that each student has unique part names. File names are governed by the naming conventions established for the operating system on the computer. In addition, standards set up by a company or project will affect naming conventions. Contact your system administrator for specific information on the number and types of characters for a valid file name. Ensure the folder is set to your “home” folder. This will also be a standard practice for this class. Parts that you create should be saved in a folder to which you have permissions. Choose OK. The part is created and “loaded” into the current NX session. As the creator of a part, you will have read and write access. This means that you can modify the file and save the changes.

Step 4:

Save the part. Choose the Save icon.

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Practical Applications of NX

(File→Save)

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1

Opening Multiple Parts More than one part may be open (loaded) at any time. This means that you may work on several parts concurrently. There are two special designations for loaded parts: •

Displayed - The part is displayed in the graphics window.

•

Work - The part is accessible for creation and editing operations.

In most cases the displayed part and the work part are the same. There are times when working in an assembly when it is advantageous that the work part be other than the displayed part. Changing the Displayed Part Since multiple parts may be open at any given time, you will need to control which part is displayed in the graphics window. This can be accomplished with the Window menu bar option. The Window option works in two ways: •

A list of up to ten previously displayed parts is generated. This list contains the latest displayed part at the top (excluding the currently displayed part) and then each previous part in the order that they were displayed until a total of ten are listed. To change the displayed part to any of these parts, simply select its name from the list.

•

Choose Window→More to display the Change Window dialog. This dialog lists all parts being referenced in the current session, excluding the current displayed part. This listing will include all components in an assembly structure as well as any loaded parts not contained in a loaded assembly.

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Getting Started

1

Activity — Opening an Existing Part In this activity, you will load an existing part into the work session. Step 1:

Open the intro_1 part. Choose the Open icon.

(File→Open)

The Open Part File dialog appears. Check the current folder displayed in the Look in: field. If necessary, choose the parts folder.

Notice that there are no options to specify units (Inches and Millimeters) in the Open Part File dialog. The units of the parts were determined when they were created and cannot be changed within an active NX session. The units of a part can be converted using a program called ug_convert_part.exe outside of the active session.

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Getting Started

Select intro_1 in the file list box and choose OK to open the part (or double-click on the file name).

The Status Line displays information while the part is being retrieved as well as other information pertaining to the operation being performed. Once the part is open the following actions occur: •

Options for viewing the contents of the file are available on the menu bar.

•

The graphics window is now active, showing the model in the condition in which it was last saved.

•

The title bar of the graphics window displays the name of the current work part and a status of Read Only. This means that changes may not be saved in this file.

A loaded part is only a copy of what is stored on disk. Any new work that you do is not permanent until the part is saved on disk. Step 2:

Leave the part open. It will be used in the next activity.

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1

Getting Started

1

Activity — Save Part As (Copying a Part) In this activity, you will make a copy of an existing part by saving it with a different name. Continue using the intro_1 part. Step 1:

Create a copy of a part. Choose File→Save As.

In the Save Part File As dialog, use the Save in: option menu to navigate to the proper folder to save the part. (HINT: This should be one level up from the parts folder.) Click in the File name field. Key in ***_intro_1 as the new part name where *** represents your initials.

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Getting Started

1

Choose OK. The Status Line states that the part is being saved. When the save is complete, the message “Part file saved” displays. Work in NX may be resumed. You can save your work and exit NX all at once by choosing File→Close→Save All and Exit. However, do not close or exit at this time. Step 2:

Leave the part open. It will be used in the next activity.

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Getting Started

1

Activity — Closing Parts In this activity, you will close parts. Continue using the intro_1 part. Step 1:

Close a specific part. Choose File→Close→Selected Parts. The Close Part dialog appears showing a list of all open parts in the session.

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Getting Started

1

Select the ***_intro_1 part and choose MB2. Because the part was not changed since it was last saved, it is immediately closed. If the part had been changed, a warning message would have appeared to let you know that the part has been modified.

Closing the part does not save the part, it only clears the part from the local memory. Changes that have been made to the part will be lost if you continue. Step 2:

Change the displayed part. Choose Window→***_new_1 from the menu bar. The ***_new_1 part is now the displayed part.

Step 3:

Close all parts. Choose File→Close→All Parts. If there are any open parts in the session that have been modified and have not been saved, a warning message displays.

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Getting Started

1

Exiting NX You can end an NXsession, by choosing File→Exit. If any parts are still open and have been modified without saving, a warning message displays.

Do not exit NX at this time.

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Getting Started

1

Summary In this lesson you: •

Started an NX session.

•

Created, opened, and saved parts.

•

Copied a Part.

•

Closed a Part.

•

Exited NX.

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1

Lesson

2

The NX User Interface

2

Purpose This lesson is a fundamental introduction to the NX User Interface. Objectives Upon completion of this lesson, you will be able to: •

Customize toolbars.

•

Save and restore toolbars by applying a Role.

•

Select objects in the graphics window.

•

Manipulate the orientation of the work view.

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The NX User Interface

Toolbars The NX user interface supports the use of toolbars to allow quick access to functionality via logical groupings of common functionality displayed as icons. Each application has a set of toolbars which support functions within that application (e.g. Modeling, Drafting, Assemblies, etc.).

2

When you exit an NX session, the state of the toolbars can be saved so that they will displayed the same when you start a new session. This is controlled by the Save layout at exit option under the General tab in the Preferences→User Interface dialog. Toolbars may be in one of two states:

2-2

•

Docked toolbars (1) are anchored to the main NX window, either horizontally or vertically. Docked toolbars are always within the NX window.

•

Undocked toolbars (2) are free floating on the screen. These toolbars are shown within the NX window, but may be located outside the window depending on screen setup.

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The NX User Interface

Customizing Toolbars The display of the toolbars as well as the display of each element within a toolbar may be customized.

2

The display of a toolbar may be controlled in one of two ways: •

Choose Tools→Customize from the main menu bar to access the Customize dialog. On the Toolbars page, choose the check box next to the toolbar name to display or hide it. The toolbars with a check are currently displayed.

The Text Below Icon option can be used to display the names of the icons in a toolbar.

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The NX User Interface

•

2

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Use the Third Mouse Button (MB3) within the NX window but outside the graphics window, to display a menu of all toolbars. The toolbars listed with a check box are displayed. Choosing a toolbar name with the First Mouse Button (MB1) will turn it on or off. The Customize option may be selected to access the Customize dialog.

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The NX User Interface

To turn on and off the display of icons within a toolbar, select the Toolbar Options area of the toolbar and choose Add or Remove Buttons, and the toolbar name. This will display a cascading menu with all of the available icons for the toolbar. Placing a check in the box next to the command will immediately display the icon in the appropriate toolbar. Removing the check will hide the icon.

The Toolbar Options menu can be accessed in an undocked toolbar as shown below.

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The NX User Interface

Roles NX has many advanced capabilities, but while learning you may want to use a smaller set of tools. Roles let you control the appearance of the user interface in a number of ways. Some examples are:

2

•

What items are displayed on the menu bar

•

What icons are displayed on the toolbars

•

Whether or not icon names are displayed below the icons

Choosing a Role NX comes with a number of built-in roles. There are System Defaults roles:

There are also roles that are tailored to particular industry types and experience levels, under the Industry Specific option:

In addition, you can define your own roles. For more information about any role, hold your cursor over its icon. To activate a role:

2-6

to open the palette on the resource bar.

•

Use the Roles tab

•

Click the role you want or drag it into the graphics window.

•

In the warning dialog, choose OK to accept the new role or choose Cancel to stop the change from occurring.

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The NX User Interface

Activity — Working with Toolbars In this activity, you will move toolbars in the Gateway application. The toolbars illustrated in this activity are shown without text below the icons. You may see this text on your screen to help you identify the icons. This is controlled by choosing Tools→Customize and specifying the Text Below Icon option for each toolbar. Step 1:

Open the intro_1 part. Choose the Open icon.

(File→Open)

Select intro_1 in the file list box and choose OK to open the part (or double-click on the file name). Step 2:

Verify which toolbars are displayed in the Gateway Application. Click MB3 in the toolbar area (1) and choose Customize (2).

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2

The NX User Interface

The Customize dialog helps you identify and control which toolbars are displayed.

2

The Text Below Icon option can be turned on for a toolbar to display the names of the icons in the toolbar. Verify that the Standard, View, Utility, Analysis, Snap Point, and Selection toolbars are checked on. The toolbars are displayed in a docked state. Toolbars may be docked horizontally on the top or bottom and vertically on the left or right. Choose Close to dismiss the Customize dialog. Step 3:

Undock a toolbar. Place the cursor on the handle portion (1) of the Analysis toolbar and press and hold down MB1.

Drag the toolbar onto the graphics window. 2-8

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The NX User Interface

Release MB1. The name of the toolbar is displayed in its title bar while it is undocked.

Step 4:

2

Dock a toolbar. Place the cursor on the header portion (1) of the Analysis toolbar and press and hold down MB1.

Drag the toolbar such that the header portion falls within the main menu bar as shown.

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The NX User Interface

Step 5:

Move a docked toolbar. Place the cursor on the handle portion of the Analysis toolbar and press and hold down MB1.

2

Drag the Analysis toolbar up to the first row of toolbars below the menu bar. Release MB1.

If necessary, select the Analysis toolbar on the handle and drag it so that it is aligned to the right of the Standard toolbar.

Step 6:

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Leave the part open. It will be used in the next activity.

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The NX User Interface

Activity — Working with Roles In this activity, you will use Roles to save and apply standard toolbar configurations. In this course, the Essential with Full Menus role will be used. Step 1:

Continue using the intro_1 part.

Step 2:

Apply the Essentials with Full Menus role. Choose the Roles tab in the resource bar on the right side of the graphics window.

If the resource is bar is not visible, choose View→Show Resource Bar to turn it on. Change the display of the Role palette to Tiles. This will display smaller icons so that all of the roles can be seen at once.

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2

The NX User Interface

Choose the Essentials with full menus role. The Essentials with full menus role displays a limited number of icons and toolbars. However, all NX functions are still available from the menu bar.

2

Choose OK in the message window warning you that your toolbar customizations will be overwritten. Changes you made to toolbars in previous activities are overwritten. The toolbar settings that are defined in the selected role are used. Step 3:

Start the Modeling application. Choose Start→Modeling. Starting a different application will introduce a new set of toolbars. The toolbars that were established in the Gateway application may move and include different icons.

Step 4:

Customize a toolbar in the Modeling application. Locate the Utility toolbar in the NX window.

Select the Toolbar Options area of the Utility toolbar and choose Add or Remove Buttons→Utility. Turn the Work Layer and Layer Settings icons on.

This change to the toolbar will be maintained in your future NX sessions as long as the Save layout at exit option is turned on in Preferences→User Interface. However, the change would be lost if you were to apply one of the roles in the System Defaults. 2-12

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The NX User Interface

Step 5:

Create a new user role with the toolbar change. Choose the Roles tab in the resource bar on the right side of the graphics window. Place the cursor in an open area of the Roles palette and choose MB3→New User Role. Choose OK in the Role Properties dialog to accept the default name of MyRole_0. The new role will appear in a User folder in the Roles palette.

If you make additional toolbar changes and want to incorporate them into your saved user role, place the cursor over the role and choose MB3→Edit, turn off the Preserve Layout Information option, and choose OK. Step 6:

Close the part. Choose File→Close→All Parts. If a warning is displayed and you are asked if you are sure you want to close the part, choose Yes.

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2

The NX User Interface

Mouse Navigation The mouse may be used as well as the keyboard to make selections. A mouse wheel acts as MB2 when it is pressed. On two button mouses, the buttons represent MB1 and MB3. Both buttons pressed together act as MB2.

2

Below is a summary of the various actions that can be performed using the mouse buttons. Mouse Button First Mouse Button MB1

Action Selects or drags objects.

Second Mouse Button OK while in an operator. Press and hold down while (center or both buttons) in the graphics window to Rotate the view. Hold MB2 down Shift+MB2 to Pan and hold down Ctrl+MB2 to Zoom In/Out. Third Mouse Button (in graphic window) MB3

Displays pop-up menu with short cuts to various functions. Also displays action information for objects selected with MB1.

Rotating mouse wheel Zooms in and out in graphics window. Scrolls in dialog list boxes, dialog option menus, and the Information window. Cursor over icons or option in a dialog

Displays either the icon or option label.

Cursor over objects, Pre–highlights objects based upon the Selection features or components toolbar setting (e.g. Select Features) in graphics window A combination of mouse buttons can also be used to pan (MB2+MB3) and zoom In/Out (MB1+MB2).

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The NX User Interface

Mouse Pop-up Menu The mouse may be used to perform various actions depending upon placement and position in the steps of the process. When the cursor is in the graphics window and MB3 is pressed and released, the View Pop-Up menu is displayed. This pop-up menu provides a shortcut to functions that are frequently used in NX to manipulate the viewing of objects in the graphics window.

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2

The NX User Interface

Option

2

Description

Refresh

Refreshes the entire graphics window. Erases temporary display entities.

Fit

Fits the entire part to the view. Utilizes the fit percentage found on the Preferences→Visualization→Screen dialog.

Zoom

Changes the view scale via a user specified rectangle.

Rotate

Activates the Rotate mode to rotate the view with the cursor.

Pan

Activates Pan mode to pan the view with the cursor.

Rendering Style

Specifies the method of shading and hidden edges in which the model is displayed.

Orient View

Displays the current view in a canned view orientation. The original visualization settings and view modifications are retained. Active only in modeling view.

Set Rotate Point

Defines a point that the model is rotated about. The point may be defined on a curve, edge, face, or point in space.

Clear Rotate Point

Removes the Rotate Point which has previously been set.

Undo

Removes the effect of the last single operation performed.

When you press and hold MB3, a radial pop-up displays icons that surround the cursor location. These icons include display options that you can choose just as you would from a menu. As you learn the position of the icons, just moving the mouse in the appropriate direction will choose the option. 1 — Shaded 2 — Shaded with Edges 3 — Studio 4 — Fit 5 — Wireframe with Dim Edges 6 — Face Analysis

The View toolbar may also be used to perform many of the view manipulation functions found in the View Pop-Up Menu.

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The NX User Interface

Graphics Window View Manipulation As you develop your model, you will need to view the model in different orientations. The view may rotated by pressing and holding down MB2 and dragging. If the cursor is near the boundary of the graphics window, rotation about a horizontal, vertical, or normal axis is inferred and the cursor is displayed in a single axis rotation mode. If the cursor is in the middle of the graphics window, the axis of rotation is determined by the direction in which you drag the cursor.

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2

The NX User Interface

Other options to manipulate the view orientation are described below: Orient View – Modifies the orientation of a specified view to a predefined view. Changes only the alignment of the view, not the view name. This option can be invoked from the View toolbar or from the MB3 pop-up menu.

2

Home Key — Orients the present view to the Trimetric view. End Key — Orients the present view to the Isometric view. F8 Key — Orients the present view to a selected planar face or datum plane or the planar view (top, front, right, back, bottom, left) that is closest to the current view orientation.

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The NX User Interface

Selecting Objects The Selection toolbar may be used to assist in the selection of an object for creation, modification, or information. In NX, you may either select an object first and then choose a function to perform, or, choose a function first and then select the required object. The Selection Type Filter is used to control precisely which type of object can be selected. When a type is chosen from this list, no other object types can be selected. The contents of the list depends on whether you have already chosen an NX function and which function you are performing.

There are many additional options which can be added as icons to the Selection toolbar to further discriminate in the selection of objects. Some of these options are also available by choosing Edit→Selection from the menu bar. MB3 may be used to choose an available operator for an object. The cursor must be on top of the object and the object highlighted for the MB3 pop-up menu to appear. The items on the pop-up menu will vary depending on the type of object. The following pop-up menu is typically displayed for a feature.

Options will also vary depending on the application (Modeling, Drafting, Manufacturing, etc.).

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2

The NX User Interface

If you press and hold MB3 over an object, a radial pop-up appears. The options will vary depending on the type of object. The following radial pop-up menu is typically displayed for a feature.

2

Deselecting Objects If you select the wrong object, you can deselect it by holding down the <Shift> key and selecting it again with MB1. To deselect all objects in the graphics window, press the <Esc> key.

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The NX User Interface

Preview Selection and QuickPick Preview Selection Preview Selection allows highlighting of objects as the selection ball passes over them. By default, Preview Selection is enabled but may be turned off by choosing Preferences→Selection from the menu bar. The color of the highlighting is determined by the Preselection setting found under Preferences→Visualization→Color Settings. This also applies to highlighting objects that are being deselected using the <Shift> key and MB1. The state of the Preview Selection setting is not saved with the part but remains in effect for the NX session. Using QuickPick for Multiple Selection Candidates When selecting objects in the graphics window, more than one object will often be within the selection ball. QuickPick is a selection confirmation interface that provides a way to browse through multiple candidates to select a specific object. Moving the selection ball over an object will highlight it for preview. If there is more than one selectable object at the selection ball location and the cursor lingers for a short period of time, the cursor changes to a QuickPick indicator:

This cursor display indicates that there is more than one selectable object at that position. Using MB1 after the cursor changes will display the QuickPick dialog.

The amount of time the cursor must be stationary for the QuickPick indicator to appear can be adjusted by choosing Preferences→Selection and using the QuickPick Delay slider bar.

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The NX User Interface

All selectable objects beneath the cursor are listed in the dialog. Use MB2 to cycle through the items in the list and then choose MB1 when the desired object is highlighted. The icons in the dialog may be used to narrow down list to include only construction objects, features, body objects (faces, edges, etc.), components, or annotations.

2

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The NX User Interface

Activity — Manipulating Views In this activity, you will change the view display and orientation. Step 1:

Open the view_clevis_1 part.

Step 2:

Manipulate the view.

2

Choose Shaded with Edges. (MB3→Rendering Style→Shaded with Edges) Click and hold MB3 and choose the Wireframe with Dim Edges icon.

from the radial pop-up.

In the graphics window, but not on top of the part, click MB3. Choose Orient View→Right in the pop-up menu. Press the Home key on the keyboard. The view is oriented to the Trimetric view.

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The NX User Interface

Place and hold the cursor at the location shown below until the QuickPick indicator appears.

2

Choose MB1 to display the QuickPick dialog. Choose MB2 until the front face shown below is highlighted.

Choose MB1 to confirm the selection of the face. Press the F8 key. The view is oriented so that the selected face is parallel to the graphics window. Press the Home key. Step 3:

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Close the part.

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The NX User Interface

Summary In this lesson you: •

Modified the location and contents of toolbars.

•

Applied a Role to restore saved toolbar settings.

•

Manipulated the work view orientation.

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Practical Applications of NX

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2

Lesson

3

Coordinate Systems 3

Purpose This lesson is an introduction to the coordinate systems that are used in NX. Objectives Upon completion of this lesson, you will be able to: •

Define the Absolute Coordinate System (ABS).

•

Define the Work Coordinate System (WCS).

•

Move the WCS using dynamic drag handles.

•

Obtain geometric information relative to the WCS.

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3-1

Coordinate Systems

Overview of Coordinate Systems Before creating solid models, you should have a basic understanding of how NX represents the location and orientation of objects. Since you will be creating models in a three-dimensional environment, model space is defined as the infinite extension of a three-dimensional field represented in the views of your graphics window.

3

All NX coordinate systems are right-hand, Cartesian coordinate systems, made up of a set of X, Y, and Z axes, 90° apart from each other. A three-axis symbol is used to identify a coordinate system. The intersection of the axes is called the origin of the coordinate system. The origin has the coordinate values of X=0, Y=0, and Z=0. The figure below illustrates that, starting at the origin, each axis has a positive direction and a negative direction.

There are several types of coordinate systems that are utilized in NX. This lesson will discuss the following types:

3-2

•

Absolute Coordinate System (ABS)

•

Work Coordinate System (WCS)

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Coordinate Systems

Absolute Coordinate System The Absolute Coordinate System (ABS) is not mobile. It defines a fixed point and orientation in model space. The Absolute Coordinate System is necessary to relate location or orientation between different objects, solid models, parts, and even MCAD/CAE systems. An object positioned at absolute X = 1, Y =1, and Z =1 in one part is the exact same absolute position in any other part. Work Coordinate System

3

Since the ABS is not mobile, the Work Coordinate System (WCS) is used to facilitate geometry construction in different orientations. The WCS can be located and oriented manually anywhere in model space. The WCS is not a selectable entity.

Most modeling operations in NX do not require manual manipulation of the WCS because features are added to a model relative to existing geometry. In those cases, the WCS is handled automatically. However, certain functions are dependent on the location and orientation WCS at the time they are performed. The location and/or orientation of the WCS will need to be considered when using the following functions: •

Creating a Primitive Feature (specifically a Block)

•

Defining a plane when creating a Sketch

•

Creating a Fixed Datum Plane or Fixed Datum Axis

•

Creating a Rectangular Instance Array

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3-3

Coordinate Systems

Manipulating the WCS You can access WCS options from the Utility toolbar or by choosing Format→WCS on the menu bar while a part is displayed. In general, there are four different options available to manipulate the WCS; Origin, Dynamics (Move), Rotate, and Orient. The Dynamics and Orient options will be the focus in this lesson.

3

Move WCS provides an interface to dynamically control the location and orientation of the WCS by keying in distance and angle values or by dragging origin, axis, and rotation handles in the graphics window. Orient WCS displays the CSYS Constructor dialog which includes various options to position the WCS.

The Absolute CSYS option will move the WCS back to the Absolute origin and orientation. This can also be accomplished by using the Set WCS to Absolute icon which can be added to the Utility toolbar.

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Coordinate Systems

Move WCS (Dynamics) To access the Move WCS option and display the WCS in a dynamic mode, double-click the WCS in the graphics window, turn on the Move WCS icon in the Utility toolbar, or choose Format→WCS→Dynamics from the menu bar. Drag handles are displayed and are used to move the WCS. These handles are represented by a cube, three coneheads, and three spheres.

3

When the cursor passes over the WCS, it will highlight with temporary rotation planes to indicate that it can be selected. If there is other geometry in the vicinity and the WCS cannot be easily selected, use the Utility toolbar or menu bar to access it. After you move the WCS, you can either choose MB2 or turn off the Move WCS icon to confirm the location and the WCS will return to a normal display. Undo is available while in dynamic WCS mode and can be used to restore the WCS to a previous location or orientation.

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3-5

Coordinate Systems

Origin Handle When you select the cube-shaped handle at the origin of the WCS, you can relocate the WCS to any point in the graphics window as dictated by the Snap Point toolbar (End Point, Arc Center, etc.). Help indicators will display on a highlighted object to help you predict where the WCS will be relocated.

3

Snap Point Toolbar The Snap Point toolbar becomes active when you need to specify a location. It is available when the WCS origin handle is selected to help specify the origin for the WCS.

Cursor Location is always available regardless of the other options that are enabled in the toolbar.

3-6

Practical Applications of NX

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Coordinate Systems

Point Constructor Dialog The Point Constructor dialog is a common tool that appears throughout NX to define a location. It is available as an icon in the Snap Point toolbar after selecting the WCS origin handle. With this dialog, you can define points using existing geometry, coordinate values, or offsets.

3

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Practical Applications of NX

3-7

Coordinate Systems

Axis Handles When you select a conehead axis handle, a dynamic input field appears in the graphics window next to the WCS to input a specific distance or snap increment. You can also drag the handle to move the coordinate system along the axis.

3

Double-clicking an axis handle will reverse the direction of the axis. The Snap value is the incremental distance the WCS will move as you drag the axis handle. The default Snap value is 0 (zero) but you may enter a different value. The Distance value will update as you drag the handle.

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Practical Applications of NX

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Coordinate Systems

Rotation Handles When you select a spherical rotation handle, a dynamic input field appears next to the WCS to enter a specific angle or snap increment. You can also drag the handle to rotate the coordinate system about the axis.

3

The Snap value is an incremental angle to rotate the WCS. The default Snap value is 45 so the WCS snaps in 45 degree increments as you drag the rotation handle. The Angle value will update as you drag the handle.

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Practical Applications of NX

3-9

Coordinate Systems

Activity — Manipulating the WCS In this activity, you will move the WCS to different positions and orientations to help you obtain information about the location of points and objects on the model. By default, the WCS coincides with the Absolute Coordinate System in a new part. Moving the WCS can help you obtain information about geometry relative to a coordinate system other than the Absolute Coordinate System. Moving the WCS is also sometimes required for certain modeling functions.

3

Step 1:

Open the wcs_1 part.

Step 2:

Change the Work Coordinate System origin. Choose the Move WCS icon (Format→WCS→Dynamics)

Make sure Control Point toolbar.

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Practical Applications of NX

in the Utility toolbar.

is enabled in the Snap Point

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Coordinate Systems

Select the midpoint of the lower edge.

3

The origin handle is highlighted by default. You simply select locations in the graphics window to move the WCS based on the Snap Point toolbar settings. The WCS maintains the same XC, YC, and ZC directions. Choose MB2 to return the WCS to a normal display. Step 3:

Rotate the Work Coordinate System. Choose the Move WCS icon.

(Format→WCS→Dynamics)

Select the Rotation Handle shown.

A dynamic input field appears allowing an Angle or Snap to be entered.

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3-11

Coordinate Systems

Key in 90 in the Angle text entry field and press Enter. The origin of the WCS is unchanged, the coordinate system is rotated about the XC axis 90°. The direction of rotation is based on the Right Hand Rule.

3 Choose MB2. Step 4:

Find the location of a point on the model relative to the WCS. Choose Information→Point. The Point Constructor is displayed to specify the point. Select the arc center shown by placing the cursor over the circular edge. When the center highlighted, select the edge.

The coordinates of the arc center relative to both the WCS and Absolute Coordinate System are displayed in an Information window. Information Units Millimeters Point XC = 0.000000000 X = YC = 25.000000000 Y = ZC = -14.000000000 Z =

32.500000000 14.000000000 16.000000000

Close the Information window. Step 5:

Reverse the direction of the YC Axis. Choose the Move WCS icon.

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Practical Applications of NX

(Format→WCS→Dynamics)

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Coordinate Systems

Double-click the YC Axis Handle. This reverses the direction of the YC Axis so that is pointing downward.

3

Choose MB2. Step 6:

Change the orientation of the WCS. The image below has been rotated for clarity. You may shade or rotate the view for better viewing of the part.

Choose the Move WCS icon.

(Format→WCS→Dynamics)

Move the WCS origin to the location shown below.

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Practical Applications of NX

3-13

Coordinate Systems

Select the XC Axis Handle.

3 Select the edge at the location shown below. A vector will appear from the end of the selected edge.

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Coordinate Systems

Select the YC Axis Handle.

3

Select the edge at the location shown below. A vector will appear from the end of the selected edge.

Choose MB2 when finished orienting the WCS. Step 7:

Find the location of an object relative to the WCS.

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3-15

Coordinate Systems

Choose Information→Object. Select the lower edge of the part shown.

3

Choose OK in the upper left corner of graphics window (or MB2) to accept the selected edge. Information about the edge will appear in the Information window. The coordinates of the start and end points are displayed relative to both the WCS and Absolute Coordinate System. Edge Geometry Angle Length

= =

Line

0.000000000 33.000000000

Vertex 1

XC = 16.000000000 YC = -0.000000000 ZC = -25.000000000

X = 49.000000000 Y = 145.069219382 Z = -33.669872981

Vertex 2

XC = 49.000000000 YC = -0.000000000 ZC = -25.000000000

X = 16.000000000 Y = 145.069219382 Z = -33.669872981

Close the Information window. Step 8:

Move the WCS back to the Absolute CSYS. Choose Format→WCS→Orient. Choose Absolute CSYS

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Practical Applications of NX

in the CSYS Constructor dialog.

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Coordinate Systems

Choose OK. The WCS moves back to the Absolute origin and orientation.

3

The Set WCS to Absolute icon can be added to the Utility toolbar. This can be used without having to use the CSYS Constructor. Step 9:

Close all parts without saving them. Choose File→Close→All Parts. Choose Yes to confirm the closing of modified parts.

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3-17

Coordinate Systems

Summary The Absolute Coordinate System is a stationary coordinate system that defines a fixed point in model space while the Work Coordinate System (WCS) is a mobile coordinate system that may be moved and reoriented as necessary to support other functions. In this lesson you: •

Identified the difference between the Absolute Coordinate System and the Work Coordinate System.

•

Relocated, rotated, and reoriented the WCS.

•

Reviewed the Point Constructor and CSYS Constructor dialogs.

•

Obtained geometric information relative to the WCS.

3

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Practical Applications of NX

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Lesson

4

Introduction to Solid Modeling Purpose This lesson is a fundamental introduction to the NX Modeling application through the creation of primitives.

4

Objectives Upon completion of this lesson, you will be able to: •

Create and Edit a Block.

•

Define a direction vector.

•

Create and edit a Cylinder.

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4-1

Introduction to Solid Modeling

Primitives A Primitive is a solid object that is analytic in nature. A Primitive may be thought of as "raw stock" to which material will be added or removed to achieve the finished part. There are multiple ways of defining each of the four Primitive types. Primitives may be used as the basic shape at the start of the solid modeling process. When a Primitive is created, its type and its size must be specified as well as its location and orientation in model space. The four types of Primitives are:

4

•

Block

•

Cylinder

•

Cone

•

Sphere If a Primitive is used in a part, it should be used as the initial solid feature. Although NX allows the use of multiple Primitives in one solid body, the practice is not recommended because of the advantages and associativity of other solid modeling functionality. Primitives are positioned explicitly. Their origins are set by a specified point in model space. However, they can be moved manually by either using Transform or the Move Feature functions. The creation parameter values of a Primitive may be edited and made associative to each other.

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Practical Applications of NX

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Introduction to Solid Modeling

Block A Block may be created by specifying the size and location of the block in model space. The orientation will be implied from the orientation of the WCS. There are three different methods that may be used to create a Block, Origin Edge Lengths, Two Points Height, and Two Diagonal Points. The middle portion of the dialog and the Selection Steps change depending on the type of Block creation method you choose. This lesson discusses the first method, Origin, Edge Lengths.

4

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Practical Applications of NX

4-3

Introduction to Solid Modeling

Origin, Edge Lengths Method

•

Choose Insert→Design Feature→Block or choose the Block icon in the Form Feature dialog.

•

Choose the Origin, Edge Lengths type.

•

Define the length for each edge. The Length, Width, and Height are measured relative to the XC, YC, and ZC axes of the WCS, respectively. These must be positive values since they are stored as the parameters of the block.

4

•

Specify the origin of the corner of the block. The Snap Point toolbar is available to access the Point Constructor dialog or to specify a point relative to existing geometry. The edges of the block will be parallel to the XC, YC, and ZC axes. If an origin is not specified explicitly and OK is chosen, the corner of the block will be placed at the WCS origin.

•

Choose OK or Apply.

After the block has been created, its size may be changed by editing the values that were used for edge lengths during creation.

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Practical Applications of NX

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Introduction to Solid Modeling

Activity — Creating a Block In this activity, a Block will be created using the Origin, Edge Lengths method. Only numerical values will be used for the size of the block. Step 1:

Create a new inch part and name it ***_block_1 where *** represents your initials.

Step 2:

Start the Modeling application. (Start→Modeling)

Step 3:

Create a Block. Choose Insert→Design Feature→Block.

4 Verify the Origin, Edge Lengths

type is selected.

Key in the following parameters: Length (XC) = 8 (Tab)Length (YC) = 6 (Tab)Length (ZC) = 6/2 (an example of algebraic entry) Choose MB2.

Choose the Fit icon Step 4:

from the View toolbar. (MB3→Fit)

Change the size of the block. Place the cursor over the block and double-click on it. Select the p1=6.000 parameter to edit.

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4-5

Introduction to Solid Modeling

Change the parameter value to 4 and choose MB2 twice.

4 Step 5:

4-6

Choose File→Close→Save and Close.

Practical Applications of NX

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Introduction to Solid Modeling

Cylinder A cylinder may be created by specifying the orientation, size and location of the cylinder. There are two methods to create a cylinder. •

Diameter, Height

•

Height, Arc

Diameter, Height Method This method is used to create a cylinder by specifying the diameter and height values. The location and axis direction vector must also be specified. After choosing this method: •

Define the cylinder axis vector using the Vector Constructor.

•

Key in the Diameter and Height.

•

Define the cylinder origin using the Point Constructor.

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4-7

4

Introduction to Solid Modeling

Defining Vectors The Cylinder and Cone features require a direction vector to be specified to define the orientation of the axis. The Vector Constructor dialog is used to specify this direction.

4

The XC, YC, and ZC Axis options are sufficient for the purpose of this course. In the example below, the direction vector is the ZC Axis. The cylinder is shown created at an origin away from the WCS with a specified height in the direction of the vector.

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Practical Applications of NX

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Introduction to Solid Modeling

Activity — Creating a Cylinder In this activity, a cylinder will be created utilizing the direction vector menu. Step 1:

Open the seedpart_mm part.

Step 2:

Start the Modeling application. (Start→Modeling)

Step 3:

Create the Cylinder. Choose Insert→Design Feature→Cylinder. Choose Diameter, Height. Choose the YC Axis direction icon in the Vector Constructor dialog.

4

Key in the following values: Diameter Height

= =

75 200

Choose OK. (MB2) Locate the cylinder at XC=0, YC=0, ZC=0. Choose Reset in the Point Constructor menu if needed and choose OK. Choose Cancel. Choose Fit from the MB3 pop-up menu.

Step 4:

Edit the size of the cylinder. Place the cursor over the cylinder and double-click on it. Choose Feature Dialog.

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4-9

Introduction to Solid Modeling

Change the values as follows: Diameter Height

= =

15 150

Choose MB2 twice.

Step 5:

Choose File→Close→All Parts. Do not save the part.

4

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Practical Applications of NX

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Introduction to Solid Modeling

Summary This lesson was an introduction to the creation of solid models using primitive features. If a primitive feature is used, it should be the base feature and there should only be one in a part because they cannot be associatively positioned. In this lesson you: •

Created a block.

•

Changed the size of a primitive after creation.

•

Created and edited a cylinder.

•

Reviewed the Vector Constructor dialog.

4

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Practical Applications of NX

4-11

4

Lesson

5

Positional Form Features Purpose This lesson introduces Form Features that can be associatively positioned from other features. Objectives Upon completion of this lesson, you will be able to: •

Create Hole, Boss, Pocket, Pad, Slot, and Groove features.

•

Position features.

•

Edit the parameters and position of features.

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5

Practical Applications of NX

5-1

Positional Form Features

Creating Form Features Form features are used to add detail to a model. These features include holes, slots, bosses, pads, pockets and grooves. Form features are fully associative to the geometry and parameter values used to create them. These features can be accessed by choosing Insert→Design Feature or by adding them to the Form Feature toolbar.

5 Placement Face All form features require a placement face. For a groove, the placement face must be cylindrical or conical. For all other form features, the placement face must be planar. This planar placement face defines the X-Y plane of the coordinate system for the feature being created. Features are created normal to the placement face. A datum plane may be used as the planar placement face. In the following example, the datum plane is used as the Planar Placement face for the hole feature.

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Practical Applications of NX

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Positional Form Features

Horizontal and Vertical Reference The Horizontal Reference defines the X axis of the feature coordinate system. Any linear edge, planar face, datum axis, or datum plane that can be projected onto the planar placement face may be selected to define the horizontal direction. A Horizontal Reference is required to define the length direction of form features having a Length parameter (slot, rectangular pocket, and pad). It is also required to define horizontal or vertical positioning dimensions for features that do not initially require a Horizontal Reference (holes, bosses, and cylindrical pockets). 1 — Planar Placement Face 2 — Horizontal Reference 3 — X Length of Feature

5

If there are no selectable objects to define a horizontal direction, you can specify a Vertical Reference instead. The horizontal direction will be inferred as being perpendicular to it. Feature Coordinate System The WCS will move automatically to facilitate the creation of a feature based on the selected placement face and reference direction. The coordinate system being represented is called a Feature Coordinate System (FCS) and is stored with the feature definition. The WCS will return to the FCS orientation when you edit the position of the feature.

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5-3

Positional Form Features

Positioning Form Features Positioning dimensions are distance values measured along the placement face. They may be used to place the form feature at the proper location on the placement face. These dimensions should be considered as constraints, or rules, that the geometry must obey. 1 — Horizontal 2 — Vertical 3 — Parallel 4 — Perpendicular 5 — Parallel at a Distance

6 7 8 9

— — — —

Angular Point onto Point Point onto Line Line onto Line

5

Only the dimension types that apply to the feature being creating will be displayed. Positioning dimensions are not required, but it is recommended that they be added when features are created for ease of future editing.

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Practical Applications of NX

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Positional Form Features

Hole This option is used to create simple, counterbore, and countersink holes in an existing solid. The middle portion of the dialog contains fields to enter parameters and will vary depending on the type of hole that is chosen. The dialog below appears for the Simple hole type.

5

Hole Creation Procedure •

Choose the Hole icon (Insert→Design Feature→Hole).

•

Choose the Type (Simple, Counterbore, or Countersink).

•

Select the placement face. If a datum plane is selected choose the Reverse Side button as required.

•

Select the thru face if applicable.

•

Key in the required parameter values.

•

Choose OK or Apply.

•

Create positional dimensions as required. ©UGS Corporation, All Rights Reserved

Practical Applications of NX

5-5

Positional Form Features

Hole Types Simple

1 – Diameter 2 – Depth 3 – Tip Angle

Counterbore

1 – C-Bore Diameter 2 – C-Bore Depth 3 – Hole Depth

Countersink

1 – C-Sink Diameter 2 – C-Sink Angle 3 – Hole Depth

5

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Practical Applications of NX

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Positional Form Features

Boss The Boss feature is used to add a cylindrical shape with a specified height to a model, having either straight or tapered sides. 1 — Diameter 2 — Height 3 — Taper Angle

A positive or negative value may be entered depending on which way the wall is to incline. A zero value results in a vertical cylinder wall.

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Practical Applications of NX

5-7

5

Positional Form Features

Positioning Terminology •

Fully Specified — The feature is uniquely located by the positioning dimensions specified.

•

Underspecified — The feature position is not completely constrained.

•

Overspecified — The feature has had more positioning constraints applied to it than are necessary.

•

Target Solid — The solid body that a Boolean operation acts upon. In the context of a Form Feature it is the solid body that the Hole, Slot, Pocket or Groove will subtract from, or a Boss or Pad will unite with.

•

Target Edge — An edge on the Target Solid that is selected for positioning purposes.

•

Tool Solid — The solid representation of the feature being defined by the current operation. In the context of a Form Feature it is the representation of the Hole, Slot, Pocket, Pad, Boss, or Groove that will be subtracted from or united with the Target Solid.

•

Tool Edge — An edge on the Tool Solid that is selected for positioning purposes.

5

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Practical Applications of NX

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Positional Form Features

Positioning Methods

Horizontal Specifies the horizontal distance between two points, one on the target solid and the other on the tool solid. Horizontal is measured along the X-axis of the feature coordinate system (the Horizontal Reference). As edges are selected, the nearest valid point is selected (midpoints are not selectable). 1 — Horizontal Reference 2 — Target Edge (End Point) 3 — Tool Edge (Tangent Point)

5

Vertical Specifies the vertical distance between two points, one on the target solid and the other on the tool solid. Vertical is measured along the Y-axis of the feature coordinate system (perpendicular to the Horizontal Reference). As edges are selected, the nearest valid point is selected (midpoints are not selectable). 1 — Horizontal Reference 2 — Target Edge (End Point) 3 — Tool Edge (Arc Center)

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5-9

Positional Form Features

Perpendicular Specifies the shortest (normal) distance between a linear edge on the target solid (also datum planes or axis) and a point on the tool solid. The linear target edge is always selected first. 1 — Target Edge 2 — Tool Edge (Arc Center)

5 Point onto Line Specifies that the distance between an edge on the target solid (also datum planes or axis) and a point on the tool solid is zero. 1 — Target Edge (Datum Plane) 2 — Tool Edge (Arc Center)

Point onto Line is the same as the Perpendicular positioning dimension with the value automatically set to zero. You can change it to a non-zero value when you edit the feature.

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Practical Applications of NX

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Positional Form Features

Parallel Specifies the shortest distance between two points, one point on the target solid and the other point on the tool solid. As edges are selected, the nearest valid point is selected (midpoints are not selectable). 1 — Target Edge (Arc Center) 2 — Tool Edge (Arc Center)

5 Point onto Point Specifies the distance between a point on the target solid and a point on the tool solid is zero. This is commonly used to align arc centers (concentric) of cylindrical or conical features. This method fully constrains their location since rotation is not a degree of freedom for cylindrical or conical features. 1 — Target Edge (Arc Center) 2 — Tool Edge (Arc Center)

Point onto Point is the same as the Parallel positioning dimension with the value automatically set to zero. You can change it to a non-zero value when you edit the feature.

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Practical Applications of NX

5-11

Positional Form Features

Activity — Positioning Holes and Bosses In this activity, you will create and position hole and boss features.

Step 1:

Open the form_feature_1 part.

Step 2:

Start the Modeling application. (Start→Modeling)

Step 3:

Create a boss. Choose Insert→Design Feature→Boss.

5

Key in the following values: Diameter Height Taper Angle

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Practical Applications of NX

= = =

2 .125 0

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Positional Form Features

Select the top face of the block (1) as the placement face. Choose OK (MB2).

Notice Perpendicular is already selected. Select edge (2) and enter a value of 4. Select edge (3) and enter a value of 3. Choose OK. (MB2)

5

Step 4:

Create a simple thru hole. Choose the Hole icon.

(Insert→Design Feature→Hole)

Choose Simple for the hole Type. Key in a Diameter of 1.

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Practical Applications of NX

5-13

Positional Form Features

Select the top face of the boss (1) as the placement face and the bottom face of the block as the thru face. Choose Apply.

Choose Point onto Point. Select the top edge (2) of the boss. Choose Arc Center.

5

Step 5:

Create a counterbore thru hole. Choose Counterbore for the hole Type. Key in the following values: C-Bore Diameter C-Bore Depth Hole Diameter

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Practical Applications of NX

= = =

1 .5 .5

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Positional Form Features

Select the top face of the block as the placement face and the bottom face of the block as the thru face. Choose Apply.

Verify Perpendicular is selected. Select edge (1) and enter a value of 1.5. Select edge (2) and enter a value of 1.5. Choose OK (MB2).

5

Step 6:

Create another counterbore hole. Verify that Counterbore is still selected. Verify the following values: C-Bore Diameter = C-Bore Depth = Hole Diameter =

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1 .5 .5

Practical Applications of NX

5-15

Positional Form Features

Select the top face of the block as the placement face and the bottom face of the block as the thru face. Choose Apply.

Verify Perpendicular is selected. Select edge (1) and enter a value of 1.5. Select edge (2) and enter a value of 1.5. Choose OK (MB2).

5

Step 7:

Create a simple hole. Choose Simple Key in the following values: Diameter Depth Tip Angle

5-16

Practical Applications of NX

= = =

.25 1 0

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Positional Form Features

Select the top face of the block as the placement face in the approximate location shown (1). Choose Apply.

Choose Horizontal . Select a front edge (2) of the block as the Horizontal Reference, select the edge of the boss (3) as the target edge, and choose the Arc Center option.

5

Key in a value of 1.375 and press Enter.

Choose Vertical. Select the edge of the boss again as the target edge and choose the Arc Center option. Key in a value of 1.25. Choose OK.

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Practical Applications of NX

5-17

Positional Form Features

If the placement face was selected near the right or back of the block, the hole may initially be positioned on the wrong side of the target edge. The location where you select the placement face will determine the initial feature location. Always select the placement face approximately where you want the feature to be located. If the hole is on the wrong side of the target edge, you will have to change the positioning dimension to a negative value. Step 8:

Create another simple thru hole that is aligned with the edges of the front face of the block. Verify the Simple

hole type is selected.

Key in a Diameter of 1. Select the right face of the block (1) as the placement face and left face (2) as the thru face.

5

Choose OK.

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Practical Applications of NX

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Positional Form Features

Choose Point onto Line . Select the front edge (3) of the block.

. Choose Perpendicular Select the bottom right edge (4). Key in a value of 1.5 and choose OK.

5

Step 9:

Create another hole in the corner of the part. Choose the Hole icon.

Verify the Simple

(Insert→Design Feature→Hole)

hole type is selected.

Key in a Diameter of 7. Select the top face of the block as the placement face and bottom face as the thru face. Choose OK.

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Practical Applications of NX

5-19

Positional Form Features

Choose Point onto Point

.

Select the back right corner of the block (1).

5 The completed part should appear as shown.

Step 10: Close the part.

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Practical Applications of NX

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mt10050_g NX 4

Positional Form Features

Slot This option allows you to create a slot in a solid body as if cut by a milling machine tool. In each case, the shape of the cutting tool corresponds to the slot type and dimensions. The slot feature will be created so that the axis of the cutting tool is normal to the face or datum plane selected. Initially, the path of the slot will be parallel to the selected Horizontal Reference. There are several different slot types available. You will be prompted for the parameters that apply to the type of slot chosen. Rectangular Slot The Rectangular slot type uses a tool that has cylindrical end faces and will produce sharp edges along the bottom of the slot. 1 — Length 2 — Width 3 — Depth

5

The Width of the rectangular slot represents the diameter of the cylindrical cutting tool. The Depth of the slot is measured in a direction parallel to the tool axis from the placement face to the bottom of the slot. Depth values must be positive. The Length is measured parallel to the horizontal reference (X in the feature coordinate system). Length values must be positive.

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Practical Applications of NX

5-21

Positional Form Features

Other Slot Types The other available slot profiles are shown below. Ball-End U-Slot T-Slot Dove-Tail

Creating a Thru Slot The Thru Slot option can be applied to all slot types and extends the length of the slot along the placement face in the direction of the horizontal reference between two specified faces.

5

You will be prompted to select starting and ending thru faces instead of a length parameter. The two thru faces cannot be parallel to the placement face. The rectangular slot shown below was created with the Thru Slot option enabled. The selected starting and ending thru faces are shaded.

You should not dimension to the end arcs of the slot when positioning a Thru Slot. The length of a Thru Slot is determined by the selected thru faces. The only positioning dimension required is to locate an edge or centerline along the length of the slot (tool) to a target edge or datum. Parallel at a Distance can be used to constrain the feature and control the two remaining degrees of freedom.

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Practical Applications of NX

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Positional Form Features

Pocket The pocket feature is used to create a cavity in a solid body. There are three types of pockets: •

Cylindrical (not covered in this lesson)

•

Rectangular

•

General (not covered in this lesson)

Rectangular Pocket This option allows a rectangular pocket to be defined to a specified depth, with or without a floor and/or corner radius, having either straight or tapered walls. The following parameters may be specified: 1 2 3 4 5 6

— Length — Width — Depth — Corner Radius — Floor Radius — Taper Angle

5

The pocket is initially oriented so that the Length is parallel to the selected Horizontal Reference. Pocket features may be positioned from a tool edge or from the centerlines provided for this purpose.

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Practical Applications of NX

5-23

Positional Form Features

Pad This option allows a raised pad on a solid body. There are two types of pads: •

Rectangular

•

General (not covered in this lesson)

Rectangular Pad This option allows a rectangular pad to be defined to a specified height, with or without a corner radius and/or taper. The following parameters may be specified: 1 2 3 4 5

5

— Length — Width — Height — Corner Radius — Taper Angle

The pad is initially oriented so that the Length is parallel to the selected Horizontal Reference.

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Practical Applications of NX

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Positional Form Features

Additional Positioning Methods

Parallel at a Distance Specifies that a linear edge on the target solid (also a datum plane or datum axis) and a linear edge on the tool solid must be parallel and at a given distance. This is typically used for features with length (slot, pocket or pad). 1 — Target Edge 2 — Tool Edge (Centerline of Slot)

5 Using Parallel at a Distance will solve two of the three degrees of freedom necessary to fully specify a feature having a length (rotation and translation in one direction). Adding another Parallel at a Distance or Line onto Line dimension would overspecify the location of the feature. To fully specify the feature in the example an additional positioning dimension is required to solve the final degree of freedom (i.e. Horizontal, Vertical, Perpendicular).

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Positional Form Features

Line onto Line Specifies that the distance between a linear edge on the target solid (or a datum plane or datum axis) and a linear edge on the tool solid is zero and they are constrained parallel to each other. This is typically used for features with length (slot, pocket, or pad). 1 — Target Edge (Datum Plane) 2 — Tool Edge (Centerline of Slot)

5 Using Line onto Line will solve two of the three degrees of freedom necessary to fully specify a feature having a length (rotational and translation in one direction). Adding another Line onto Line or Parallel at a Distance dimension would overspecify the location of the feature. To fully specify the feature in the above example an additional positioning dimension is required to solve the final degree of freedom (i.e. Horizontal, Perpendicular, or Point onto Line). Line onto Line is the same as the Parallel at a Distance positioning dimension with the value automatically set to zero. This zero value can be changed to a non-zero value when editing the feature.

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Positional Form Features

Angular Specifies that a linear edge on the target solid (also a datum plane or datum axis) and a linear edge on the tool solid must be at a given angle to each other. The angle is measured in a counter-clockwise direction (with respect to the feature coordinate system), from the ends of the edges nearest to where they are selected. 1 — Target Edge 2 — Tool Edge (Edge of Pocket)

5

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Positional Form Features

Parameter Entry Options Parameter Entry Options let you easily define your model parametrically as you specify values during feature creation. They are accessed by choosing the “down-arrow” icon located next to many of the parameter entry fields throughout the Modeling application. Options are provided to let you specify a value based on a formula, a reference to an existing value, or a derived value from a measurement without having to copy and paste or reenter the values.

5

You can use these options to easily lookup functions and define relationships between features. You can use values that already exist in your model, making downstream changes easier and in agreement with your design intent. Referencing Existing Parameters Choosing the Reference option will display a Parameter Selection dialog and allow you to select an existing feature. Once a feature is selected, it’s parameters are listed in a dialog. Selecting one of the parameters and choosing OK will insert it into the entry field.

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Positional Form Features

Activity — Creating Pockets and Slots In this activity, you will locate a pocket and slot using the Line onto Line and Parallel at a Distance positioning methods.

Step 1:

Open the form_feature_2 part.

Step 2:

Start the Modeling application. (Start→Modeling)

Step 3:

Create and locate the rectangular pocket.

5

Choose Insert→Design Feature→Pocket. Choose Rectangular. Select the placement face (1) and horizontal reference (2) as indicated below.

The design intent is that the length of the pocket be the same as the Y Length of the block. ©UGS Corporation, All Rights Reserved

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Positional Form Features

Choose the Parameter Entry Option down-arrow button. next to the Length field and choose the Reference option.

Select the block feature from the graphics window. Choose the BLOCK(0) Size Y parameter from the Parameter Selection dialog and choose OK.

5

The parameter for the size of the block appears in the Length field for the pocket. This “p-number” may be different in your part.

Key in the remaining values: Width Depth Corner Radius Floor Radius Taper Angle

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Practical Applications of NX

= = = = =

1 .25 0 0 0

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Positional Form Features

Choose OK.

Choose Line onto Line tool (2) as indicated below.

and select the target (1) and the

Choose Point onto Line and select the target (3) and the tool (4) as indicated below.

5

Choose Insert→Design Feature→Slot. Verify the Thru Slot option is turned off and choose Rectangular.

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Positional Form Features

Select the placement face (1) and horizontal reference (2) as indicated below.

5 The design intent is that the depth of the slot be the same as the X Length of the block. Key in the following values: Length Width

= =

1 .55

Press the Tab key to highlight the Depth field (or double-click in the Depth field).

Choose the Parameter Entry Option down-arrow button next to the Depth field and choose the Reference option. Select the block feature from the graphics window. Choose the BLOCK(0) Size X parameter from the Parameter Selection dialog and choose OK. The parameter, or “p-number” for the X Length of the block will appear in the Depth field of the slot. Choose OK. 5-32

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Positional Form Features

Choose Parallel at a Distance and select the target (1) and the tool (2) as indicated below. Key in a value of 1 and choose OK.

Choose Perpendicular and select the target (3) and the tool (4) as indicated below. Key in a value of 1.25.

5

Choose OK. Step 4:

Close the part.

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5-33

Positional Form Features

Groove The groove feature requires a cylindrical or conical placement face. A groove can be thought of as a feature that would result from a part being cut in a lathe. After specifying the groove parameters, you will be shown a preview of the tool solid. The tool solid can be thought of as the path that the lathe would make as it cuts the solid. Positioning a Groove You only have to position a groove along the axis of the cylindrical or conical placement face. The Positioning dialog will not appear. Instead, you are only required to specify a horizontal dimension along the axis by selecting a target edge followed by a tool edge or centerline. Two grooves are shown in the following example. 1 — Target Edge 2 — Tool Edge (or centerline)

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Positional Form Features

Activity — Positioning a Groove In this activity, you will create a groove feature and position it along the axis of a cylindrical solid body.

Step 1:

Open the groove_1 part.

Step 2:

Start the Modeling application.

Step 3:

Create and locate the groove.

5

Choose Insert→Design Feature→Groove. Choose Rectangular. Select the outside cylindrical face as the placement face.

Key in the following values: Groove Diameter Width

= =

2.25 .25

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Positional Form Features

Select the front outside circular edge (1) as the target edge and the centerline of the groove (2) as the tool edge.

5

Key in a value of 1.5 to position the groove and choose OK (MB2).

Step 4:

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Close the part.

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Positional Form Features

Editing the Size and Location of Form Features As features are created the parametric data is captured in expressions. The parametric data consists of the actual feature size definition (i.e. diameter, height, length) as well as the positional data that is captured in the positioning dimensions. Edit Parameters The Edit Parameters and Edit with Rollback options allow you to redefine the parameter values of any parametric feature and update the model to reflect the new values. To edit the parameters of a feature: •

•

•

Select the feature to edit. –

With the cursor over the feature, choose MB3→Edit Parameters or MB3→Edit with Rollback.

–

Double-click on a feature. (The default action is Edit with Rollback.)

–

Double-click the feature or use the MB3 popup menu in the Part Navigator.

–

Choose Edit→Feature→Edit Parameters and select the feature.

–

Choose the Edit Feature Parameters icon

5

and select the feature.

Select the parameters to edit. –

Some parameters will appear in the graphics window.

–

Any of the valid parameters types may be chosen from the Edit Parameters dialog. This displays the original creation dialog where the parameters may be edited.

Choose OK until the editing dialogs are dismissed and the model updates.

Edit with Rollback This option allows you to edit the parameters of a feature but it also temporarily returns the model to its state when the feature was created. The features that occur after the edited feature in the model history are hidden from the display. This simplifies the display and makes it easier to select features to reference when using the Parameter Entry options.

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Positional Form Features

Edit Positioning This option allows a feature to be moved by editing its positioning dimensions. In addition, positioning dimensions may be added to features that are either underspecified or were not given any positioning dimensions at the time of creation. Once the feature has been selected, the following options are offered based upon the positioning status of the selected feature.

5

If the selected feature has no positioning dimension associated with it, the Add Dimension option is automatically selected. To edit the position of a feature: •

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Select the feature to edit. –

With the cursor over the feature in the graphics window, choose MB3→Edit Positioning.

–

With the cursor over the feature in the Part Navigator, choose MB3→Edit Positioning.

–

Choose Edit→Feature→Positioning and then select the feature to edit.

–

Choose the Edit Feature Positioning icon to edit.

and select the feature

•

Choose the type of edit (Add, Edit, or Delete).

•

Select an existing dimension or new dimension type.

•

Choose OK until the editing dialogs are dismissed and the model updates.

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Positional Form Features

Add Dimension This option may be used to add a positioning dimension to a feature. When adding positioning dimensions, any edge (1) resulting from the intersection of the feature being positioned (2) and a face on the target solid (3) may not be selected as the tool edge.

The intersection edge is a child object of the tool and target solid’s face and is defined by the boolean operation associated with the feature type being created. The boolean operation does not occur until after the position of the feature has been defined. Therefore, the intersection edge is not a valid selection to specify location. When adding positioning dimensions to a Thru Hole, no edges will be selectable as the target edge because both edges are intersection edges. The Identify Solid Face option is used to select the center of the cylindrical face (1).

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5

Positional Form Features

Valid target edges for positioning purposes must belong to features existing in the feature creation list of the model before the feature being positioned. In the example below the features are numbered in the order in which they were created. Feature (2) may not be positioned using any face or edge from feature (3). If an edge or face from feature (3) is selected as a target, a message is displayed stating that you cannot select an object from a later feature and a dialog will let you highlight those edges and faces which can be selected.

5 Edit Dimension Value Features may be moved by changing the values of the feature’s positioning dimensions. To use this option: •

Select the dimension to edit (if there is only one positioning dimension, it is selected automatically).

•

Key in the new value.

Continue editing as many dimension values as desired. Once all the desired dimension values have been edited, choose OK. Delete Dimension Use this option to delete a positioning dimension from a feature. The feature will then remain in its current location as its position is no longer associated to the model. If you are replacing a dimension, add the new dimension before deleting the old one. The Edit Positioning dialog is maintained when you add a dimension but is automatically dismissed when you delete a dimension.

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Positional Form Features

Error Messages If the model cannot be updated based on the new parameters or location of the feature, the Edit During Update dialog will be presented. This dialog provides several options for dealing with the failed update.

5

You can choose Show Current Model followed by the Show Failure Area option to help identify the problem visually.

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Positional Form Features

Editing Features with the Part Navigator The Part Navigator is a powerful tool that may be used to identify and edit features. Holding down MB3 on a feature node in the Part Navigator displays a feature specific pop-up menu. This menu provides an alternative method to edit the parameters and the position of a form feature. To access the Part Navigator, choose the icon on the resource bar on the right side of the NX window.

5

If the resource is bar is not visible, choose View→Show Resource Bar to turn it on.

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Positional Form Features

Activity — Editing Positional Form Features Step 1:

Open the edit_feature_3 part.

Step 2:

Start the Modeling application.

Step 3:

Edit size parameters. In the graphics window, select the hole feature indicated below.

5

With the cursor over the highlighted hole feature, click MB3 and choose Edit Parameters.

Choose Feature Dialog. Change the Diameter to .375 and choose OK twice. Notice that both holes changed. This is because a referenced parameter was established when the second hole was created. Step 4:

Edit the position. In the graphics window, select the same hole as before.

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Positional Form Features

With the cursor over the highlighted hole feature, click MB3 and choose Edit Positioning.

Choose Edit Dimension Value. In the graphics window, select the positioning dimension that equals 2.625 and change the value to 3.25. Choose OK three times to finish the update. Notice how both holes changed location. This is because a referenced parameter was established when the second hole was positioned.

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Positional Form Features

Step 5:

Change a hole type. In the graphics window, select the counterbore hole indicated below.

With the cursor over the highlighted hole feature, click MB3 and choose Edit Parameters. Choose Change Type. Choose Simple and choose OK. Choose OK to accept the Diameter value of .3125. Choose OK again to complete the edit of the hole. Step 6:

Change the positioning design intent. In the graphics window, select the same hole that you just edited. With the cursor over the highlighted hole feature, click MB3 and choose Edit Positioning. Choose Add Dimension. Choose Perpendicular.

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5-45

5

Positional Form Features

Select the front edge, as shown below, as the target edge.

Because the hole was created as a thru hole, you are limited in what you can select for a tool edge. In cases where you cannot select an appropriate tool edge or, if the resulting edge is not a true circle (like shown at one end), you can use the Identify Solid Face option.

5

Choose Identify Solid Face. Select the cylindrical face of the hole as shown below.

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Positional Form Features

Accept the dimension value by choosing OK. Notice the Status line indicates that the feature position is overspecified. There are two dimensions competing against each other. The design intent was changed to locate the hole from the front edge of the part so you will need to delete the old dimension causing the overspecified condition. Choose OK in the Positioning dialog. Choose Delete Dimension. Select the existing dimension causing the overspecified condition and choose OK.

5

Step 7:

Close the part.

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Positional Form Features

Additional Positioning Techniques Information→Feature Choosing Information→Feature will display a Feature Browser dialog where you can obtain detailed information about features in a model. Selecting a feature and choosing OK or Apply will display an Information window. Accessing the Information pull-down menu options will not cancel feature construction dialogs. This allows you to find necessary information needed while creating new features. You can also list information about a feature by highlighting it in the graphics window, choosing MB3→Properties, and then choosing the Information icon in the Properties dialog. Display Dimensions The Display Dimensions option in the Feature Browser temporarily displays the parameters of size and location in the graphics window for the feature. Refreshing the graphics window removes the temporary display of the parameters.

5

Display Dimensions can also be accessed using the Part Navigator.

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Positional Form Features

Positioning from Edges When you select an edge of the target solid to constrain a feature, a curve is extracted to match that edge. This curve is maintained internally and is linked to the target solid. If you modify the edge (for example, by adding a blend), the constraint is maintained to the original edge. Try to position features from edges before they are blended. This minimizes potential update errors when blends are modified or deleted. You can use the Make Current Feature option, within the Part Navigator, to add the feature before the blend feature in the Model History. When positioning from edges, select edges that are less likely to be affected by downstream features and editing operations. This will reduce the chances of future model update failures.

5

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Positional Form Features

Summary In this lesson you were introduced to Form Features. Form features are used to add detail to the model during creation. Form features are fully associative to the geometry and parameter values used to create them. The different form features are: Hole, Boss, Pocket, Pad, Slot, and Groove. This lesson you: •

Identified a Placement Face.

•

Identified a Horizontal Reference.

•

Identified Target and Tool Solids.

•

Created Hole, Boss, Pocket, Pad, Slot, and Groove features.

•

Applied positioning dimensions form features.

•

Edited parameters and positioning dimensions of form features.

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Lesson

6

Expressions Purpose This lesson is a fundamental introduction to Expressions. Objectives Upon completion of this lesson, you will be able to: •

Create Expressions.

•

Edit Expressions.

6

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6-1

Expressions

Overview Expressions are arithmetic or conditional formulas that define the characteristics of a part. Expressions define the dimensions and relationships of a model. Expressions are automatically created when: •

a feature is created.

•

a sketch is dimensioned.

•

a feature is positioned.

All expressions have a single, unique name and a string or formula that can contain a combination of variables, functions, numbers, operators, and symbols. Expression names are variables that you can insert in the formula strings of other expressions. This can be helpful in breaking up lengthy formulas as well as defining relationships that can be used in place of numbers. Expression formulas are evaluated for values. Here are some examples of expressions, their formulas and their resulting values:

6

Expression Name

Formula

Value

length

5*width

20

p39 (Extrude(6) End Limit)

p1+p2*(2+p8*sin(p3))

18.849555921

p26 (Simple Hole(9) Tip Angle)

118

118

Expression names are no longer case sensitive, with the following exceptions: • •

Expression names are case sensitive if their dimensionality is set to Constant. Expression names are case sensitive if they were created before NX 3.

When expression names are case sensitive, they must be referenced exactly when used in other expressions.

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Expressions

Creating and Editing Expressions To work with expressions, choose Tools→Expression. The Expressions Dialog with Less Options

1

Expression Name

Up to 132 letters, numbers, or underscore. Must begin with a letter. Case Sensitive.

2

Formula

Can contain a combination of numbers, functions, operators, and other expression names.

3

Dimensionality

Choose from Constant, Length, Area, Volume, Mass, and many others

4

Units

Units appropriate to the dimensionality will be available in a pull-down.

6

The system will handle unit conversions automatically if, for example, you specify inches in a metric part. Not active during editing or if dimensionality is constant. 5

More Options

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6-3

Expressions

The Expressions Dialog with More Options

6 1 Listed Expressions

Choose from User Defined, Named, Filter by Name, Filter by Value, Filter by Formula, Unused Expressions, Object Parameters, Measurements, and All

2 Expression list

List contains columns for Name (followed by usage in the part), Formula, Value, Units, and Comment

3 Accept Edit 4 Reject Edit 5 Less Options

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Expressions

Creating Expressions There are three methods to create expressions: •

System generated expressions (p#).

•

User defined expressions created during text input (Rad=5.00).

•

Predefined, user created expressions (Thk=0.60, Thk used as a text entry in a parameter field).

Procedure: •

Choose the Dimensionality and Units for the expression.

•

Key in the name of the expression in the Name field and press the <Enter> key.

•

Key in the formula for the expression in the Formula field and press the <Enter> key.

•

Choose Apply or OK to save the expression. After keying in the name of the expression the or = key can be used to advance the cursor to the Formula field.

6

Editing Expressions Procedure: •

Display the Expressions dialog with More Options.

•

Choose the expression to modify from the expression list. The expression will be displayed in the Name and Formula fields.

•

Modify the Name, Formula, or Units of the expression.

•

Press the <Enter> key or the Accept Edit icon.

•

Choose Apply or OK to save the expression. Editing the name of an expression will also edit the formula of any expression that references it.

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6-5

Expressions

Listing Expressions Associated with Features It is often necessary to determine which expressions control which features in a model. If the Listed Expressions option is set to All, all of the expressions in the part are listed. If an expression defines a feature, the feature name is listed with it (i.e. p8 (Simple Hole(5) Diameter). All of the expressions associated with a feature may also be listed in an Information window by choosing Information→Feature and selecting the feature or MB3→Information in the Part Navigator. List Referencers The List Referencers option provides a means of finding out if an expression is referenced in another expression and what feature(s) use the expression. To use this option, select the expression, and choose List Referencers from the MB3 pop-up menu.

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Expressions

Specifying Formulas while Creating Features The Expressions dialog may be accessed while creating a feature by choosing Formula from the parameter entry option menu. This will allow you to specify a complex formula for the expression that is generated for the feature parameter. Parameter entry options are available with many of the parameter entry fields throughout the Modeling application.

6

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Expressions

Activity — Getting Familiar with Expressions In this activity, you will create user-defined expressions. Step 1:

Open the expression_1 part.

Step 2:

Start the Modeling application.

Step 3:

Examine the Expressions of the Block. Choose Tools→Expression. Change the Listed Expressions option to All.

6

The dialog lists all of the expressions in the part. Notice the default expression names p0, p1, and p2 which define the block. Step 4:

Delete the Block. Choose the Delete icon (Edit→Delete)

from the Standard toolbar.

Select the block in the graphics window and choose OK 6-8

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Expressions

Step 5:

Create a new Block. Choose Insert→Design Feature→Block.

Choose Origin, Edge Lengths. Key in the following expressions: Length (XC) Width (YC) Height (ZC)

= = =

length=8 width=6 height=6/2

Choose OK. Step 6:

Examine the Expressions for the newly created Block. Choose Tools→Expression. Notice the expressions height, length, and width. These expressions are referenced in the formulas of the expressions defining the block.

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Expressions

Change the Listed Expressions option to Named.

This lists only the expressions in the part that you explicitly named. The formula for height is a constant numeric value 6/2. The desired design intent is that the height grows proportionally with the width. This relationship could not be established upon creation as the width expression was not in existence. Step 7:

Edit the expression. Select the height expression from the Expressions list. This will fill in the Name and Formula fields.

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Expressions

Key in a new formula for the expression width/2 and press Enter.

The formula for the expression height is now changed to width/2. Any time that the width changes, the height value will change accordingly. Step 8:

Change the width value. Select the width expression. Key in 4 for the formula and press Enter. Choose OK.

6

The block will update with the new width and height. Step 9:

Close the part.

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Expressions

Summary Expressions are algebraic or arithmetic statements used to control the characteristics of a part. All expressions have a name, a formula, and a value and are used to define the dimensions and relationships of a model. In this lesson you: •

Created Expressions.

•

Edited Expressions.

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Lesson

7

Shell Purpose This lesson introduces the Shell feature operation. Objectives Upon completion of this lesson, you will be able to: •

Create a Shell feature.

•

Specify faces to be removed and apply an alternate thickness to a face.

7

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7-1

Shell

Shell Feature Overview The Shell feature operation provides additional definition to an existing solid by creating a cavity inside the solid or a shell around the solid based upon a specified thickness. This can be accessed in the Feature Operation toolbar or by choosing Insert→Offset/Scale→Shell. The entire solid body is hollowed during this operation but faces can be removed to create openings. In the following example, the top face was selected to be removed.

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Shell

Creating a Shell Feature When you choose the Shell option, the Shell dialog is displayed. The Remove Faces icon is initially active by default and you are prompted to select the faces to remove. You may also enter a Thickness value.

After the selecting faces to remove, the resulting solid previews in the graphics window. The Thickness can be adjusted by dragging the handle (1) to the desired value or keying in the value in the dynamic input field (2).

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7-3

7

Shell

Initially, the drag handle will point inward and a positive value for thickness will hollow the original solid. To reverse the direction, double click the drag handle (or use MB3). When the drag handle points outward, a positive thickness value will create a shell around the original solid. You may also specify a negative thickness value to create the shell in the opposite direction of the drag handle. When you achieve the desired Thickness value and direction , choose OK (or MB2) to create the feature. Selection Intent Face Options The Selection Intent toolbar is available to specify face selection rules while selecting faces. These rules can be applied to automatically select a collection of faces in a single step instead of selecting each one individually.

Alternate Thickness List

7

A unique thickness may be assigned to faces with the Alternate Thickness List option. This option allows you to select sets of faces and specify a different thickness value using a drag handle or entry field.

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Shell

Activity — Creating a Shell Feature In this activity, you will use the Shell feature to define a plastic molded part. Step 1:

Open the shell_hair_dryer part.

Step 2:

Start the Modeling application.

Step 3:

Inspect the Part.

7

Set the Rendering Style to Shaded with Edges and rotate the part to verify that a shell feature is required. Step 4:

Create the shell feature and remove the proper faces. from the Feature Operation Choose the Shell icon toolbar. (Insert→Offset/Scale→Shell)

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7-5

Shell

Key in a Thickness value of 2. Select the right (1), and back (2) planar faces to remove.

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Shell

Choose OK (MB2).

Step 5:

Rotate the part to verify the shell was created correctly.

Step 6:

Close the part.

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Shell

Activity — Creating a Shell and Removing Multiple Faces In this activity, you will create a Shell feature and select multiple faces to remove.

7

Step 1:

Open the shell_face_selection part.

Step 2:

Start the Modeling application.

Step 3:

Create a shell feature. Choose the Shell icon.

(Insert→Offset/Scale→Shell)

Key in a Thickness of .12. Select the following five faces to remove: front, back, left, right, and bottom.

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Shell

Choose OK. (MB2)

Step 4:

Edit the Shell feature. Orient the work view to Front. (MB3→Orient View→Front) Fit the view. (MB3→Fit) Choose Edit→Feature→Edit Parameters. Choose the Shell feature and OK.

7

Change the Thickness to –.12 and choose OK twice (or MB2 twice) to update the model. Notice the material is offset in the opposite direction. Step 5:

Close the part.

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7-9

Shell

Activity — Creating a Shell with an Alternate Thickness In this activity, you will create a Shell feature with an alternate thickness applied to a face. Step 1:

Open the shell_alternate_thickness part.

Step 2:

Start the Modeling application.

Step 3:

Create the shell feature. Choose the Shell icon.

(Insert→Offset/Scale→Shell)

Key in a Thickness of 4. Verify the Face option is set to Tangent Faces in the Selection Intent toolbar.

Select the top face to remove. This will automatically include the right and left faces because they are tangent.

7

Choose Alternate Thickness List. 7-10

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Shell

Select the bottom face.

Key in a Set1 T value of 8. Choose OK twice. (or MB2 twice)

7

Step 4:

Close the part.

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Practical Applications of NX

7-11

Shell

Summary The Shell feature creates a cavity inside, or a shell around an existing solid, based upon a specified thickness. In addition, selected faces may be assigned alternate thicknesses. In this lesson you: •

Created a Shell feature with a uniform thickness.

•

Created a Shell feature and selected multiple faces to remove.

•

Created a Shell feature and specified an alternate thickness for a face.

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Lesson

8

Edge Operations Purpose This lesson introduces Edge Blend and Chamfer operations. Objectives Upon completion of this lesson, you will be able to: •

Create Edge Blends.

•

Create Chamfers.

8

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Practical Applications of NX

8-1

Edge Operations

Overview Edge operations are available to provide additional definition to the edges of a model. These operations include Edge Blend and Chamfer. They are available in the Feature Operation toolbar or by choosing Insert→Detail Feature.

You may also create edge blends and chamfers by first selecting the edge(s) and choosing Blend or Chamfer from the MB3 pop-up menu.

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Edge Operations

Edge Blend This option creates cylindrical or conical faces in place of an edge on a solid body. Material is added or subtracted depending on the topology of the solid body and the faces intersecting the selected edges (1,2) are shortened.

Creating Edge Blends After choosing the Edge Blend option, a dialog is displayed and you are prompted to select a set of edges. You can key in the radius in the Set1 R field.

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Practical Applications of NX

8-3

Edge Operations

After the selecting edges, the result is previewed in the graphics window. The radius value can be adjusted by dragging one of the radius drag handles (1) or by keying in the value in the dynamic input field (2).

Choose OK, Apply, or MB2 twice to create the edge blend feature.

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Edge Operations

Multiple Edge Sets A single blend feature may consist of one or more sets of edges and each set may have a different radius value. After the first set of edges is selected and a radius is specified, choose the Complete set and start next set icon in the dialog (or MB2 once) to select another set of edges. The drag handles for the first edge set disappear and an anchor and label (Set1) are displayed. You may then select edges to include in the second edge set (Set2) and specify the radius using the new drag handles or dynamic input field.

You may continue to define another edge set or complete the blend operation by choosing OK (or MB2 twice). Selection Intent The Selection Intent toolbar is available while creating an edge blend to specify edge selection rules. These rules can be applied to automatically select a collection of edges in a single step instead of selecting each edge individually.

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Practical Applications of NX

8-5

8

Edge Operations

Activity — Creating Edge Blends In this activity, you will create Edge Blends.

Step 1:

Open the edge_blend_1 part.

Step 2:

Start the Modeling application.

Step 3:

Create the first Edge Blend. Select the edge (1), click MB3, and choose the Blend option from the pop-up menu.

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Edge Operations

Key in .75 for the radius and press Enter (or use the drag handles).

Choose OK (or MB2 twice) to create the blend. Step 4:

Create the second Edge Blend. Choose the Edge Blend icon. (Insert→Detail Feature→Edge Blend) In the Selection Intent toolbar, verify the Curve option is set to Tangent Curves.

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Practical Applications of NX

8-7

Edge Operations

Select the edge (1) shown below.

Notice the tangent edges are automatically selected based on the Add Tangent Chain selection rule. Key in a radius of .5 (or use the drag handles).

8

If you were to choose OK now, only the three tangent edges would be blended. Instead, you will blend the entire left side of the part so the additional edges must be selected manually.

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Edge Operations

Select the two additional edges on the left side of the part shown below.

Choose OK (or MB2 twice) to create the blend.

Step 5:

Close the part.

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Practical Applications of NX

8-9

Edge Operations

Chamfer This option bevels the edges of a solid body by defining the desired chamfer dimensions. Material is added or subtracted depending on the topology of the solid body and the faces intersecting the selected edges (1,2) are shortened.

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Edge Operations

Creating Chamfers The Chamfer dialog is displayed and you are prompted to select the edges to chamfer. You can specify an Input Option and offset values in the dialog.

After edges are selected, you can also use the drag handles or dynamic entry fields in the graphics window to specify the offsets. Choose OK (or MB2 ) to create the chamfer.

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Practical Applications of NX

8-11

Edge Operations

Chamfer Input Options

Symmetric Offsets

Asymmetric Offsets

Offset and Angle

The same offset value (1) is measured along both adjacent faces.

Different offsets (1, 2) are measured along the adjacent faces.

An Offset value (1) and an Angle (2) are required.

You can change the Input Option in the dialog or by highlighting the drag handle in the graphics window with the cursor and choosing MB3.

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Edge Operations

Activity — Creating Chamfers In this activity, you will apply chamfers to the edges of a model.

Step 1:

Open the chamfer_1 part.

Step 2:

Start the Modeling application.

Step 3:

Create a chamfer by specifying an offset and angle. Choose the Chamfer icon. (Insert→Detail Feature→Chamfer)

Choose Offset and Angle

in the Chamfer dialog.

Key in the following values: Offset Angle

= =

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1.75 30

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Practical Applications of NX

8-13

Edge Operations

Select the edge (1).

If your model does not look like the figure below, choose the Reverse Offsets icon

in the Chamfer dialog.

Choose Apply. Step 4:

Create a chamfer with asymmetric offsets. Choose the Asymmetric Offsets icon in the Chamfer dialog. Key in the following values:

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First Offset Second Offset

8-14

Practical Applications of NX

= =

.25 .5

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Edge Operations

Select the edge (2).

If your model does not look like the figure below, choose the Reverse Offsets icon.

Choose OK. Step 5:

Close the part.

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Practical Applications of NX

8-15

Edge Operations

Summary The Edge Blend and Chamfer operations are available to provide additional definition to the edges of a model. All of the blended edges or chamfered edges created in a single operation are considered to be one feature. In this lesson you: •

Blended a single edge.

•

Blended edges using a selection intent rule.

•

Chamfered edges using different input options.

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Lesson

9

Model Construction Query Purpose This lesson demonstrates different methods to query a part to determine creation method, design intent, and physical properties. Objectives Upon completion of this lesson, you will be able to: •

Retrieve layer information.

•

Access the Part Navigator.

•

Access feature and expression information.

•

Playback the model construction.

•

Suppress and Unsuppress features.

•

Identify where expressions are used.

•

Measure the distance between objects.

•

Assign a material and calculate mass properties.

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Practical Applications of NX

9-1

Model Construction Query

Visually Inspect the Part Visual inspection of the solid model may be accomplished by rotating the model to view the different features. At times this is very beneficial in order to clearly see what is displayed in the graphics window. The model may be rotated by using the middle mouse button or the Rotate icon in the View toolbar. Different rendering styles are available in the MB3 pop-up menu or View toolbar to display the part. You can choose from Shaded or Wireframe modes, with or without edges displayed.

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Model Construction Query

Layers Layers are used to organize a part. They work like invisible containers to house the different objects used to create an NX solid model. A layer is a system-defined attribute that all objects must have. There are 256 layers in NX, one of which is always the Work Layer. Any of the layers can be assigned to one of four classifications of status: •

Work

•

Selectable (on)

•

Visible Only

•

Invisible (off)

The Work Layer is the layer that objects are created on and is always visible and selectable while it remains the Work Layer. Layer 1 is the default Work Layer when a new part is created. When the Work Layer is changed, the previous Work Layer automatically becomes Selectable and could then be assigned a different status. The number of objects on one layer is not limited. You may choose which layers to create objects on and what the status will be. However, employing company standards for the use of layers is recommended.

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Practical Applications of NX

9-3

Model Construction Query

To assign a status to a layer or layers, choose the Layer Settings icon from the Utility toolbar or choose Format→Layer Settings from the menu bar.

Select a layer from the Layer/Status list area and choose one of the four options below the list (Selectable, Invisible, Make Work, or Visible Only). Double-clicking on a layer (other than the work layer) toggles it between Selectable and Invisible.

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Model Construction Query

Things to look for in the Layer Settings dialog: •

Object Count — Enabling Show Object Count using the checkbox will change the display in the Layer/Status listing window to a Layer/Status/Count listing window that shows the number of objects contained on each layer.

•

Category Names — Layers or groups of layers can be named using Categories. These names are listed in the Category listing window on the Layer Settings dialog as well as in the Layer/Status listing window next to assigned layers when Show Category Names is enabled.

•

Layer Listing — The filtering option menu at the bottom of the dialog allows the Layer/Status listing window to display All Layers, Layers with Objects, or All Selectable Layers.

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Practical Applications of NX

9-5

Model Construction Query

Layer Categories The following layer and category standards will be followed in this class. Model Geometry Object Geometry

Layer Assignment

Category Name

Solid Geometry

1–20

SOLIDS

Inter-part Modeling

15–20

LINKED_OBJECTS

Sketch Geometry

21–40

SKETCHES

Curve Geometry

41–60

CURVES

Reference Geometry

61–80

DATUMS

Sheet Bodies

81–100

SHEETS

Layer Assignment

Category Name

101–110

FORMATS

Layer Assignment

Category Name

Mechanism Tools

121–130

MECH

Finite Element Meshes and Engineering Tools

131–150

CAE

Manufacturing

151–180

MFG

Quality Tools

181–190

QA

Drafting Objects Object Geometry Drawing Borders Engineering Disciplines Object Geometry

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Model Construction Query

Moving Objects Between Layers While creating a model, it may be necessary to move an object to a different layer. This can be accomplished by choosing Format→Move to Layer. The objects which need to be moved are selected using the Class Selection menu and the Layer Move dialog appears.

The destination layer may be specified by keying it in the Destination Layer or Category field or by selecting it from the layer list. Choosing OK or Apply will move the object(s). If Apply is chosen, additional objects may be selected to move by choosing the Select New Objects button.

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Practical Applications of NX

9-7

Model Construction Query

Part Navigator The Part Navigator is useful to identify the features of the model. Selecting a feature in the Part Navigator window will highlight that feature in the graphics window and will also highlight its parent and/or child features in the Part Navigator. Conversely, selecting a feature in the graphics window will highlight that feature and its parents/children in the Part Navigator. To access the Part Navigator, choose the Part Navigator icon on the resource bar located vertically to the right of the graphics window.

If the resource is bar is not visible, choose View→Show Resource Bar to turn it on. Suppress and Unsuppress The display of features can be temporarily removed (suppressed) from the graphics window by selecting the check box next to the feature name. When a check is present, the feature is displayed in the graphics window. The Suppress and Unsuppress options are also in the MB3 pop-up menu of the Part Navigator, the Edit→Feature menu, and the Edit Feature toolbar. They can be used to help investigate how a model was created and how it would be affected if the feature was removed. Feature Playback The Playback option (Edit→Feature→Playback) can also be used to investigate a model. It temporarily hides features and allows you to step through the construction of the model, one feature at a time.

9

Playback does not suppress reference features or sketches. It does allow editing of features during the update.

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Model Construction Query

Information The Information pull-down menu offers a number of options to obtain information about the model. Information→Feature This provides another interface to identify Parent/Child relationships between the selected feature and the other features in the model. In addition, expressions that control the feature may be displayed in the graphics window by toggling on the Display Dimensions option. Choosing OK or Apply will display the Information window with the geometric data and associated expressions. Feature information may also be accessed by selecting the feature in the Part Navigator and choosing MB3→Information or, by selecting the feature in the graphics window and choosing MB3→Properties. Information→Object This is used to display information about selected objects in an Information window. Any type of geometric object may be selected including curves, edges, faces, and bodies. The Information window will display information such as name, layer, color, object type, and geometric properties (length, diameter, start and end coordinates, etc.). Information→Expression→List All This lists all expressions in the part in the Information window. From the Information window, the list can be printed or saved to a text file. Information→Expression→List All by Reference This is used to identify expressions that reference other expressions and the features that they define. The Edit→Find option within the Information window can be used to search for a specific expression.

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Practical Applications of NX

9-9

Model Construction Query

Referenced Expressions If an expression defines a feature directly, the feature name is listed with it in the Expressions dialog. However, an expression may also be included in the formula of other expressions. The referencing expressions and features may be identified by using the List References option in the Expressions dialog. To use this option: •

Choose Tools→Expression.

•

If necessary, change the Listed Expressions filter to list the expression to interrogate.

•

Select the expression and choose List References in the MB3 pop-up menu.

An Information window will list the features and other expressions that are referencing the selected expression.

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Model Construction Query

Distance This Distance option is used to obtain the minimum distance between any two objects such as points, curves, planes, bodies, edges, and/or faces. This can be accessed by choosing Analysis→Distance or the Distance icon in the Analysis toolbar. An icon option bar appears in the upper left corner of the graphics window with options to select the first point or object (1) and the second point or object (2).

After selecting the two objects, a temporary ruler and measurement result are displayed in the graphics window. The resulting units for the distance are determined by the setting in Analysis→Units.

Choosing the Information option will display the results in an Information window along with the closest points on each object and the delta distances relative to the absolute and work coordinate systems.

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9-11

9

Model Construction Query

Mass Properties Basic mass properties data can be calculated by choosing Analysis→Mass Properties and selecting the solid body. The units for the results are determined by the setting in Analysis→Units.

A density may be assigned to the solid body by choosing Edit→Feature→Solid Density or by choosing Tools→Material Properties and creating a new material or selecting a material from the existing library.

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Model Construction Query

Activity — Model Construction Query In this activity, you will identify feature relationships and design intent. Although detailed instructions are provided, it may be beneficial to attempt to navigate through the interface without using them. Step 1:

Open the inspect_arm_1 part.

Step 2:

Start the Modeling application.

Step 3:

Visually inspect the model. Choose the Shaded with Edges icon. (MB3→Rendering Style→Shaded with Edges) Rotate the model (MB2).

Choose the Trimetric icon to orient the view back to the trimetric orientation. (MB3→Orient View→Trimetric) Step 4:

Inspect the layers. Viewing the layers may help gain an understanding of the complexity of the model. If there is only one object on a “solids” layer and several objects on a “sketches” layer, the model is likely an extrusion.

9

Choose the Layer Settings icon. (Format→Layer Settings) Verify the Show Object Count option is turned on. Turn the Show Category Names option on. ©UGS Corporation, All Rights Reserved

Practical Applications of NX

9-13

Model Construction Query

Review the listing for category names and object count. Notice that there are objects on a SOLIDS layer, a SKETCHES layer, and a DATUMS layer.

Choose the Static Wireframe icon to better view interior features. (MB3→Rendering Style→Static Wireframe) Make layers 21 and 61 selectable so that the construction geometry may be seen. Choose OK in the Layer Settings dialog.

Choose the Fit icon.

Step 5:

(MB3→Fit)

Identify the features using the Part Navigator. Choose the Part Navigator icon from the resource bar on the right side of the graphics window. in the upper right corner of Choose the push pin icon the Part Navigator to permanently display it. If the graphics window is maximized, the display will be adjusted to fit the part within the viewing area.

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Model Construction Query

Choose Tools→Part Navigator and ensure the Timestamp Order option is turned on. This will list all features in the Model History tree of the Part Navigator.

Select Extrude(5) “large knuckle extrusion” in the Part Navigator Model History. The corresponding feature will be highlighted in the graphics window. The parent feature (Sketch(3) “S21”) and child (Simple Hole(7) “large thru hole”) will highlight in the Part Navigator. Select a few other features in the Part Navigator to identify them and their parent/child relationships. Step 6:

Review the model construction using Playback.

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Practical Applications of NX

9-15

Model Construction Query

Choose Edit→Feature→Playback. All of the solid features are suppressed except the reference features and the sketch. The Edit During Update dialog informs you that the Fixed Datum Plane(0) feature has been updated, this is the first feature in the model history.

9

Choose the Step option. The next feature, Fixed Datum Axis(1), is updated. You may have to move the slider to read the entire message displayed in the Edit During Update dialog.

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Model Construction Query

Choose the Step option again. The next feature (Fixed Datum Axis(2)) is updated. Continue to Step through the model until all features have been updated. Step 7:

Review the model construction using Suppress and Unsuppress. Starting at the top of the Part Navigator Model History list, select the check box in front of the first feature (Fixed Datum Plane(0)) to suppress it. Notice that many of the other features are also suppressed. This is because all of the features except for the two fixed datum axes are children of the suppressed datum plane.

Select Fixed_Datum_Plane(0) in the Part Navigator. Choose the Dependencies option at the bottom of the Part Navigator

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Practical Applications of NX

9-17

Model Construction Query

In the Dependencies area, expand SKETCH(3) ”S21”. Now you can see how the various features are dependent on the datum plane.

Choose the Dependencies option to close the area. Starting at the top of the Part Navigator Model History list, select the "empty" checkbox in front of the first feature with MB1 to unsuppress the feature. Continue down the list and unsuppress the remaining features, one at a time, by selecting each of the empty check boxes with MB1. Step 8:

Find the values that control the thickness of the web extrusion. In the Part Navigator, place the cursor on Extrude(4) “web extrusion”, press MB3, and choose Information. Scroll through the Information window to see the parameters and controlling expressions. The expression p4 is identified as the Both Side Distance. This expression controls the start and end distances from the section geometry for the extrusion. A value of .125 on both sides produces a web thickness of .25. Note that the parent of this feature is the sketch S21:Sketch(3). Close the Information window.

9

Step 9:

Identify the expression that controls the distance from the large hole center to the small hole center. Since the web feature was generated from the sketch geometry, the obvious place to look for the expression that controls the hole to hole distance is in the sketch.

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Model Construction Query

In the Part Navigator, place the cursor on Sketch(3) “S21”, press MB3, and choose Edit Parameters. Orient the view to the Front using the View toolbar.

The expression in question can clearly be identified as arm_length=8.500. Orient the view back to the Trimetric orientation. Choose Cancel in the Edit Sketch Dimensions dialog. Step 10: Close the Part Navigator. Select the push pin icon Part Navigator to hide it.

again and drag the cursor off the

Step 11: Determine how the large thru hole is positioned. You will select a feature directly from the graphics window rather than from a list which will take less time if you do not know the name of the feature. Choose Information→Feature. Select the Large Thru Hole feature in the graphics window and accept it if necessary. You can zoom, pan or rotate the part to get a better view of the feature. Turn the Display Dimensions option on in the Feature Browser dialog. The diameter and positioning dimension appear in the graphics window.

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Practical Applications of NX

9-19

9

Model Construction Query

Choose OK. (MB2) The Information window appears and shows that p18 is a parallel positioning dimension with a value of 0 (zero). The logical assumption can be made that the hole is located Point to Point relative to the Large Knuckle extrusion. Close the Information window. Step 12: Identify where an expression is referenced. Choose Tools→Expression. Change the Listed Expressions filter to Named. Select the small_dia expression. This expression is listed as defining (S21:Sketch(3) Diameter Dimension on Arc2) Choose MB3→List References. The Information window appears and also shows that another expression is referencing it (large_dia=2.5*small_dia). Close the Information window. Cancel the Expressions dialog. Step 13: Identify the arc in the sketch that is referencing the expression. Choose Information→Feature. Select S21:Sketch(3).

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Model Construction Query

Choose the Object Dependency Browser option. The child objects of the sketch are listed. Notice that Arc2 is present.

Select Arc - Arc2. The arc is highlighted in the graphics window. The feature and object associated with the expression have now been identified. Cancel the Object Dependency Browser dialog. Step 14: Measure a distance. Choose the Layer Settings icon. (Format→Layer Settings) Make layers 21 and 61 invisible and choose OK.

Choose the Distance icon (Analysis→Distance)

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9

in the Analysis toolbar.

Practical Applications of NX

9-21

Model Construction Query

For the first object, select one of the upper edges of the web.

For the second object, select one of the lower edges of the web.

The shortest distance between the edges is displayed. Step 15: Assign a material to the solid body. Choose Tools→Material Properties. Select the solid body in the graphics window.

Choose Library

in the Materials dialog.

Choose OK to accept the default search criteria. (MB2) Choose Steel and OK.

9

Choose OK in the Materials dialog. (MB2) Step 16: Determine the mass properties of the solid body in units of kilograms and meters. Choose Analysis→Units→kg -m 9-22

Practical Applications of NX

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Model Construction Query

Choose Analysis→Mass Properties. Select the solid body. Individual mass properties may be selected from the list in the graphics window or all of the properties may be listed in an Information window.

Choose the Information icon the graphics window.

in the upper left corner of

Step 17: Choose File→Close→All Parts.

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Practical Applications of NX

9-23

Model Construction Query

Summary In this lesson, you queried a model to determine the creation method and design intent. These skills are important to review parts created by other users. In this lesson you: •

Accessed the Part Navigator.

•

Examined layer settings.

•

Identified expressions.

•

Reviewed the model construction using Playback, Suppress, and Unsuppress.

•

Measured a distance.

•

Calculated mass properties.

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Lesson

10 Introduction to Assemblies Purpose This lesson introduces the Assembly application. Objectives Upon completion of this lesson, you will be able to: •

Set Load Options.

•

Work with the Assembly Navigator.

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Practical Applications of NX

10-1

Introduction to Assemblies

Definitions and Descriptions Assembly An assembly is a part which contains component objects. It is a collection of pointers to piece parts and/or subassemblies. In the figure below, the toy laser gun is an assembly consisting of many components.

Subassembly A subassembly is an assembly used as a component within a higher level assembly. The figure below shows the subassembly of the integrated circuit board for the toy laser gun. A subassembly has components of its own.

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Introduction to Assemblies

Component Objects A component object is the entity that contains the pointer that links the assembly back to the master component part. A component object can also be a subassembly made up of other component parts and/or component objects. An example of an assembly structure is shown below: 1 – Top level assembly. 2 – Subassembly. This is a component part and has been added to the top level assembly. 3 – Piece Parts. These are component parts and have been added to the top level assembly or subassemblies. 4 – A Component Object.

Component Parts A component part is a part which is pointed to by a component object within an assembly. The actual geometry is stored in the component part and is referenced, not copied, by the assembly. The term “piece part” is used to refer to master geometry as it exists outside of an assembly.

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10-3

Introduction to Assemblies

Introduction to Load Options When an assembly part is opened (loaded) using File→Open, the component parts that are referenced by the assembly must be found and loaded. The Load Options establish how and from where the component parts are loaded. The Load Options dialog can be accessed by choosing File→Options→Load Options or by choosing the Options button in the Open Part File dialog. 1 — Determines where to look for component parts. 2 — Determines which components will be loaded. 3 — Controls whether components are fully or partially loaded. 4 — Controls what to do if a component is not found.

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Introduction to Assemblies

Load Method The Load Method determines where to search for the component parts when an assembly is opened. There are three possible settings. •

As Saved — looks for each component part in the same directory it was in when the assembly was last saved.

•

From Directory — looks for each component in the same directory as the assembly part.

•

Search Directories — looks for each component in directories specified in a user-defined list.

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Practical Applications of NX

10-5

Introduction to Assemblies

Load States The Load Options also control whether component parts will be fully loaded, partially loaded, or unloaded when an assembly is opened. These are referred to as Load States. Fully Loaded A part is fully loaded if all of its data is loaded into system memory. All components can be fully loaded by changing the Load Components option to All Components and toggling off the Use Partial Loading option before opening the assembly. Partially Loaded When a part is partially loaded, only the data required to display the part is loaded into memory. Components will be partially loaded if the Use Partial Loading option is turned on when the assembly is opened. Partially loading components reduces the memory requirements and improves performance. This is beneficial when working with large assemblies. Unloaded A component part is unloaded if it is not loaded when the assembly is opened. Component parts may be refrained from loading by changing the Load Components option to No Components before opening the assembly. This will drastically reduce the amount of memory required and improve system performance but the component geometry will not be visible. Individual components or subassemblies may be opened at a later time when they are needed.

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Introduction to Assemblies

Load Failure The Abort Load on Failure option specifies what to do if a component part is not found, based on the current load method. •

When turned on, no parts are loaded unless all of the components are found. The first component that cannot be found will be listed in an error window.

•

When turned off, the assembly is loaded along with any of the components that are found. Those components that are not found will be listed in a warning window and left unloaded.

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Practical Applications of NX

10-7

Introduction to Assemblies

Activity — Setting Load Options In this activity, you will set load options to control how assembly components are opened. Step 1:

Set the Load Options to As Saved. Choose File→Options→Load Options. Verify the Load Method is set to As Saved. Verify Abort Load on Failure is turned on. Choose OK.

Step 2:

Open the test assembly. Choose the Open icon.

(File→Open)

Open the laser_test_assm_1 part. A warning appears informing you that a component could not be found. The system is trying to locate each component in the directory in which it resided when the assembly was last saved. The components may have been moved to a new directory or the original directory may no longer exist. The warning would also occur if you did not have read access to the original directory. Choose OK to dismiss the warning. Choose Options in the Open Part File dialog. Set the Load Method to From Directory. Choose OK. Open the laser_test_assm_1 part.

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If a warning appears informing you that the parts are read only, choose OK to dismiss the warning.

Step 3:

Review the list of components in the assembly. Choose Assemblies→Reports→List Components. Scroll through the Information window and confirm that all of the component parts are located in the same directory as the assembly part. Close the Information window.

Step 4:

Do not close any parts. You will use the assembly in the next activity.

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Introduction to Assemblies

The Assembly Navigator The Assembly Navigator provides a graphical display of the structure of the displayed assembly and provides a quick and easy method of manipulating components in the assembly. The Assembly Navigator may be accessed by choosing the Assembly Navigator icon from the resource bar on the right side of the graphics window.

You may re-size the Assembly Navigator window and use the scroll bars to see the entire tree structure and all of the columns.

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Node Display Each component of an assembly is displayed as a node in the assembly tree structure. If you select on a node with MB1, the system will highlight the component geometry in the graphics window. Each node consists of a check box, an icon, the part name, and additional columns. If the part is an assembly or subassembly, an expand/collapse box will also be present. Components may be selected for various operations by choosing the appropriate node in the Assembly Navigator with MB1. Icons Assembly (or subassembly) — If the icon is yellow, the assembly is within the work part. If the icon is gray with solid edges, the assembly is a non-work part. If the icon is gray with dashed edges, the assembly is closed.

Component Piece Part — If the icon is yellow, the component is within the work part. If the icon is gray with solid edges, the component is a non-work part. If the icon is gray with dashed edges, the component is closed. Expand/Collapse Box — Children of a node are only displayed when it is expanded. To expand or collapse the node, place the cursor over the box and click MB1. When a node is collapsed, the expand/collapse box is marked with a +. An expanded node is marked with a — . Check Boxes The check box provides a quick means of determining a part’s status. A check box also lets you load and show a part with a single action. No check — The part is closed. Clicking on this type of check box: •

Loads the component and its children partially or fully, depending on the load options. Unloaded parents may also be loaded at this time.

•

Any components that were blanked are now unblanked.

•

Afterwards, the check boxes of the part and its children will contain red check marks except for those which fail to load, are excluded from a reference set, or reside on invisible layers. ©UGS Corporation, All Rights Reserved

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Gray check — The part is blanked, and at least partially open. It also appears for unblanked parts which either have an excluded reference set or are on invisible layers. Clicking on this type of check box: •

Unblanks the component, along with any of its children that were blanked.

•

If any of its children were unloaded, they are now loaded.

•

Afterwards, the check boxes of the part and its children have large red checks, except for those whose loading failed, who have an excluded reference set, or are on invisible layers.

Red check — The part is unblanked, at least partially open, in a visible reference set, and on a visible layer. Clicking on this type of check box: •

Blanks the component and its unblanked children.

•

Afterwards, the component’s check box has a gray check and its children have gray checks (if blanked) or no checks (if unloaded).

You cannot close a part by clicking on its check box. To close a part, use the File→Close option or the Close option in the Assembly Navigator pop-up menu.

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Activity — Working with the Assembly Navigator In this activity, you will work with the Assembly Navigator. Continue working with the laser_test_assm_1 assembly. Step 1:

Review the nodes in the Assembly Navigator. Choose the Assembly Navigator icon from the resource bar on the right side of the graphics window.

If the resource is bar is not visible, choose View→Show Resource Bar to turn it on. Expand the laser_ic_board_13 node by clicking on the + sign.

Step 2:

Blank and Unblank a component node. Click MB1 on one of the laser_ic9_13 nodes. Notice the component highlights on the screen. Click the check box in front of the highlighted node. Notice the component is blanked. Click on the check box again to unblank the component.

Step 3:

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Blank and Unblank a subassembly node.

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Introduction to Assemblies

Click the check box in front of the subassembly laser_ic_board_13. Notice the subassembly and all of its components are blanked. Also notice the color of the check marks become gray. Click on the subassembly check box again to unblank the subassembly. Step 4:

Close a component. Choose File→Close→Selected Parts. Choose All Parts in Session at the top of the Close Parts dialog. Select laser_ic9_13 from the list and choose OK. In the Assembly Navigator, the laser_ic9_13 nodes no longer have check marks in their boxes and the components are not displayed in the graphics window. This means that the components are not loaded.

Step 5:

Open the components using the check box. In the Assembly Navigator, click on the check box in front of either laser_ic9_13 nodes. Both occurrences of the laser_ic9_13 component are now open and are once again displayed in the graphics window.

Step 6:

Do not close or save the part. You will use this assembly in the next activity.

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Selecting Components in the Assembly Navigator In many assembly functions, components may be selected from a list in a dialog or from the graphics window. You may also select components using the Assembly Navigator by choosing the appropriate node with MB1. You can select single or multiple components. To select multiple components in the Assembly Navigator, select the first component and then either: •

Use <Shift>MB1 (together) on another component to select all the components between those components

•

Or use MB1 on another component if you want only it and the first component

You can also use <Shift>MB1 on components in the graphics window or MB1 on components in the Assembly Navigator to deselect them. Identifying Components In the Assembly Navigator, if you click MB1 while the cursor is over a non-work part whose check box has a red check, that part is highlighted. The part remains highlighted until you select another part. (Hovering the cursor without clicking MB1 has no effect.) Check boxes of components that are not visible will have a thin gray check or no check. If you hover the cursor over a part that is not visible (e.g., blanked, on another layer, or unloaded), a box defining the boundaries of the component appears in the graphics window. The box disappears when you move the cursor to another part. This only occurs when the Preselect Invisible Nodes property is turned on. The Preselect Invisible Nodes property is accessed by clicking MB3 in the Assembly Navigator away from the component nodes and choosing Properties from the pop-up menu. Because of configuration differences, you may have to hold MB1 down for a few seconds before the box displays. In some cases, the box may not be drawn until you release MB1. Also, the box will not be drawn if you double-click MB1.

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Selecting Components in the Graphics Window The QuickPick dialog may be used to control the selection of components or objects within a component.

Once a component has been highlighted in the graphics window, the MB3 pop-up menu may be used to choose an available action for that component. The cursor must be on top of the component for the component-specific pop-up menu to appear.

The options available in the component pop-up menu will vary depending on whether the Assemblies and Modeling applications are on.

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Designing in Context Designing in Context is the ability to directly edit component geometry as it is displayed in the assembly. Geometry from other components can be selected to aid in the modeling.

The Displayed Part NX allows multiple parts to be open at the same time. This can occur either implicitly, as a result of being referenced by a loaded assembly, or explicitly, when you use File→Open. The part that is currently displayed in the graphics window, whether it be an assembly or component, is called the Displayed Part. There are several ways to change the displayed part: •

Select the component from the graphics window and use the MB3 pop-up menu.

•

Choose the Make Displayed Part icon

•

Choose Window→More (Change Window dialog).

•

Choose Window and selecting a part from the Loaded Part List, which contains up to the last ten loaded parts.

•

Use the Assembly Navigator pop-up menu.

•

Choose Assemblies→Context Control→Set Displayed Part.

in the Assemblies toolbar.

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Window Choosing Window→More will display the Change Window dialog which lists all partially and fully loaded parts other than the current displayed part.

When this dialog is active, a part may be selected by: •

Choosing it from the list of loaded parts. You may enter a portion of the part name in the Search Text field to help find the part in the list. The Options button can be used to specify how to perform the search.

•

Selecting geometry in the graphics window (if the current displayed part is an assembly).

•

Selecting the node in the Assembly Navigator.

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The Work Part The part in which geometry is created and edited is defined as the Work Part. The Work Part may be the displayed part or any component part which is contained in the displayed assembly part. When a part is opened, it will initially be both the displayed and the work part. The displayed part and the work part do not need to be the same. In the case where the displayed part is not the work part, the work part will be displayed in color and the other component parts will be de-emphasized. There are several ways to change the work part: •

Double-click on the component in the graphics window.

•

Select the component from the graphics window and use the MB3 pop-up menu.

•

Choose the Make Work Part icon

•

Use the Assembly Navigator pop-up menu.

•

Choose Assemblies→Context Control→Set Work Part.

in the Assemblies toolbar.

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If a component has already been selected, choosing the Make Work Part icon will immediately make it the work part. If no component has been selected, the Set Work Part dialog is displayed. This dialog allows you to select a component from a list or enter a name.

Choosing the Displayed Part option changes the work part back to the displayed assembly. This makes the displayed part and the work part the same.

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Assembly Navigator Pop-Up Menu Options If you position the cursor over a node in the Assembly Navigator that represents a component and click MB3, a pop-up menu appears.

The options available in the Assembly Navigator pop-up menu will vary depending on the status of the component and whether the Assemblies and Modeling applications are invoked. Pack and Unpack Pack removes multiple occurrences from the Assembly Navigator display and replaces them with a single node. (Multiple occurrences are components with the same parent, and whose prototype is the same part.) Unpack reverses this process and shows all occurrences.

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Make Work Part Selects the part in which to create new geometry or edit existing geometry, giving you the ability to design in context. Double clicking on a node in the Assembly Navigator will also make that component the Work Part. In addition the reference set is changed to Entire Part. When the component is no longer the work part, the reference set is returned to its original condition. Make Displayed Part Switches the display between currently loaded parts. The displayed part becomes the top node in the Assembly Navigator. Display Parent Switches the displayed part from a component or an assembly to one of its parent assemblies. The Maintain option in the Assembly Preferences dialog (Preferences→Assemblies) determines the work part when a parent becomes the displayed part. If Maintain is turned on, the component will remain the work part. If Maintain is turned off, the parent becomes the displayed part and work part.

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Activity — Working with the Assembly Navigator (continued) In this activity, you will use the Assembly Navigator to navigate through the assembly structure. Continue working with the laser_test_assm_1 assembly. Step 1:

Review the nodes in the Assembly Navigator. If the Assembly Navigator is not visible, choose the Assembly Navigator icon from the resource bar on the right side of the graphics window. Notice that there are several nodes of the same component. Packing the nodes will make the assembly structure easier to view.

Step 2:

Pack like nodes in the Assembly Navigator. In the Assembly Navigator, locate the laser_c1_13 nodes. On any of the laser_c1_13 nodes, click MB3 and choose Pack. Pack the laser_diode_13 nodes. In the Assembly Navigator, place the cursor in an open area below or to the left of the component nodes, click MB3 and choose Pack All. (Tools→Assembly Navigator→Pack All)

Step 3:

Make one of the laser_c1_13 components the work part. In the Assembly Navigator, select laser_c1_13x4 with MB3 and choose Unpack.

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Choose OK to the Read Only message. All of the components in the graphics window change to the same color except for one of the laser_c1_13 components, which remains in its original color. This color convention denotes laser_c1_13 as the work part. The component may now be edited and the design continued in the context of the assembly. Step 4:

Make laser_t1_13 the displayed part. You may not want to work on a component in the context of the assembly. If this is the case, you would make the component the displayed part. Select the component laser_t1_13 from the graphics window as shown below.

Place your cursor over the highlighted component, press MB3 and choose Make Displayed Part.

The pop-up menu may contain additional options if the Assemblies application is turned on. The assembly is no longer displayed.

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Step 5:

Display the top level assembly. In the Assembly Navigator, click MB3 on the laser_t1_13 node and choose Display Parent→laser_test_assm_1. The Maintain option in the Assembly Preferences dialog (Preferences→Assemblies) determines the work part when a parent becomes the displayed part. If Maintain is turned on, the component will remain the work part. If Maintain is turned off, the parent becomes the displayed part and work part.

Step 6:

Close all parts and do not save.

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Saving the Work Part After editing, the work part must be saved to keep the modifications. This can be performed with the File→Save or the File→Save Work Part Only option. File→Save •

If the work part is a piece part (lowest level component), only that part will be saved.

•

If the work part is an assembly or subassembly, all modified component parts below it are also saved. Higher level assemblies will not be saved even if they were modified.

File→Save Work Part Only The Save Work Part Only option will only save the work part, even if the work part is an assembly or subassembly. File→Save All saves all loaded parts in the session that have been modified regardless of the work part designation. Open parts for which you do not have write privileges will not be saved.

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Summary An assembly is a part which contains component objects. It is a collection of pointers to piece parts and/or subassemblies. Assemblies provides the ability to design in context. In this lesson you: •

Set Load Options.

•

Worked with the Assembly Navigator.

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11

Lesson

11 Adding Components & Mating Conditions Purpose This lesson demonstrates adding components to an assembly and the associativity that may be designed between components with mating conditions. Objectives Upon completion of this lesson, you will be able to: •

Add components to an assembly.

•

Define mating conditions.

•

Reposition components.

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11

General Assembly Concepts There are two basic ways to define an assembly structure. •

Top-Down Modeling

•

Bottom-Up Modeling (Demonstrated in this course)

Top-Down Modeling As the name suggests, an assembly is created at the top level hierarchy and parts are filed down the hierarchy, creating subassemblies and components. Bottom-Up Modeling A Bottom-Up assembly modeling approach starts by creating the lowest level piece parts that will make up the assembly. Existing component parts and subassemblies are added to assemblies as the process moves up the assembly level hierarchy. In the Bottom-Up approach, component parts are created separate from the assembly and later added to the assembly. This approach applies to purchased parts or existing parts. First, the pin is created in separate part outside of the assembly

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Then, the pin is added to the assembly as a component.

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All assemblies are automatically updated, when opened, to reflect changes made to the component parts. For example, if a hole feature is added to the solid in a component part, it will be seen in all occurrences of that component in the assembly when it is opened.

Combining Both Approaches It may be more practical for the methods to be combined. For example, purchased or existing hardware for the assembly may be added using the bottom-up method, new subassemblies and piece parts may be defined in a top down mode as the design progresses, and finally existing fasteners may be added in a bottom up mode from a standard parts library. Designing in Context The ability to make a component of an assembly the work part while leaving the assembly itself as the displayed part allows the assembly to be designed in context. All new geometry that is created is added to the work part. Edits can be made to the features and expressions residing within the work part. If a component exists several times in the assembly (i.e. a fastener), any change to the component while it is the work part will affect all the other occurrences as well.

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11

Assemblies Application The Assemblies application may be turned on and off by choosing Start→Assemblies. Toggling on the Assemblies application displays the Assemblies toolbar and expands the functions available in the Assemblies pull-down menu.

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11

Assemblies Pull-down Menu Turning on the Assemblies application will expand the Assemblies pull-down menu (1). Some assemblies functions are still available when the Assemblies application is turned off (2).

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11

Assemblies Toolbar Turning on the Assemblies application will also display the Assemblies toolbar.

If the Assemblies toolbar is not visible, choose Tools→Customize and turn it on in the Toolbars page. You can control which icons appear on this toolbar by choosing Add or Remove Buttons→Assemblies from the Toolbar Options as shown in a docked (1) and undocked (2) toolbar. This will list all of the available options in the toolbar and allow you to turn on those which you want to display.

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11 Adding Components to an Assembly A component part may be added to an assembly by choosing the Add Existing Component icon from the Assemblies toolbar or choosing Assemblies→Components→Add Existing from the menu bar. The Assemblies application must be turned on to access this option. The component part to add can be specified with the Select Part dialog.

There are several ways to identify a part when the Select Part dialog is active: •

Select Choose Part File to retrieve an unopened part.

•

Select a previously loaded part from the list.

•

Key in the name of a previously loaded part.

•

Select an existing component in the graphics window.

•

Select an existing component in the Assembly Navigator.

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11

After the part is identified, the Add Existing Part dialog appears. This dialog is used to specify how the existing part will be added as a component object to the assembly and what information will be stored with the component object.

Reference Set - Allows you to control the amount of data that is loaded from each component and viewed in the context of the assembly. •

Default reference sets are Empty and Entire Part.

•

Reference sets may be manually or automatically created. For a "BODY" reference set to be created automatically, the Model Reference Set Name option must be set to BODY in the customer defaults settings. (File→Utilities→Customer Defaults and then choose Assemblies→Site Standards)

Layer Options - Defines the layer to which the objects in the new component will be added in the current work part.

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•

Work - Places all objects from the component part on the current work layer.

•

Original - Places each object from the component part on the same layer in which it resides in the component part.

•

As Specified - Places all objects from the component on the layer specified in the Specified Layer entry field.

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11 Creating a New Parent Assembly This option lets you create a new parent assembly for your current work part. The new parent assembly is a completely new part, which becomes the new displayed part and work part in your session. When you choose this option, the New Part File dialog is displayed so that you can enter a name for the new parent. The former work part is added to the parent assembly as a component.

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11

Activity — Creating an Assembly In this activity, you will create an assembly and add a component. Step 1:

Open the seedpart_in part and save it as ***_clevis_assm.

Step 2:

Start the Modeling application.

Step 3:

Activate the Assemblies toolbar. Make sure the Assemblies application is turned on. (Start→Assemblies)

Step 4:

Add a component to the assembly.

Choose the Add Existing Component icon from the Assemblies toolbar. (Assemblies→Components→Add Existing) Choose Choose Part File. Select clevis_1 and choose OK. Choose OK to accept the defaults in the Add Existing Part dialog. Choose Reset to ensure that the coordinates are set to zero. Choose OK in the Point Constructor dialog.

Choose Cancel in the Select Part dialog. 11-10

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Step 5:

11

Verify the presence of the assembly and component parts. If the Assembly Navigator is not visible, choose the Assembly Navigator icon from the resource bar on the right side of the graphics window. The Assembly Navigator contains two nodes that represent the top level assembly and the component part.

Step 6:

Close all parts.

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Adding Components & Mating Conditions

11

Mating Conditions By applying mating conditions to components in an assembly, you establish parametric, positional relationships between objects in the components. These relationships are termed mating constraints. In the example shown, if you align the cylindrical face of a bolt to the cylindrical face of a hole in a block and then move the hole, the bolt will automatically move with it.

A mating condition is made up of one or more mating constraints. There are eight types of constraints.

1 — Mate

4 — Parallel

7 — Distance

2 — Align

5 — Perpendicular 8 — Tangent

3 — Angle

6 — Center

FROM / TO When selecting objects to mate, the Cue line will be directing you to select FROM and TO objects. The FROM object is part of the component that is going to move to a new position. The TO object is part of the component that is remaining in its present location.

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11 Mate Constraint When applying the Mate constraint to components using planar faces and datum planes, the objects will be oriented so that their normals are parallel and point in opposite directions. The components will not necessarily have physical contact but will be coplanar. By definition, a face normal in a solid body points away from the solid.

When mating non–planar faces (i.e. cylindrical to cylindrical, spherical to spherical) the radii must be the same; for conical to conical faces, the taper must be the same.

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Adding Components & Mating Conditions

11 Align Constraint When you apply the Align constraint to components using planar objects (planar faces and datum planes), the objects will be oriented so that their normals are parallel and point in the same direction. The components will not necessarily have physical contact but will be coplanar.

When aligning non-planar faces, i.e. cylindrical to cylindrical, spherical to spherical, or conical to conical, the radii and/or taper do not have to be the same.

The Align constraint can also be used to position an edge or curve object of a component with a planar object (planar face or datum plane) of another component. A vector will be determined from the edge or curve object and the objects will be oriented so that the vector and the planar object lie on the same plane (same behavior as with mate constraint). Using the CSYS Filter The Align constraint allows existing coordinate systems to be used as FROM/TO selection objects. When using the CSYS option, select the FROM CSYS and then immediately select the TO CSYS. This constraint will remove all DOFs between the two components.

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11 Angle Constraint Use the Angle constraint when you need to control specific angles between objects of components. The example below illustrates an angle constraint that is being applied in conjunction with two other constraints. The two planar faces of the blocks must always be coplanar by virtue of the Mate constraint. The pivot for the Angle constraint is determined by the Align constraint that is applied to the two edges.

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Adding Components & Mating Conditions

11 Parallel Constraint Use the Parallel constraint when you need to establish parallelism between objects of components. Objects that have surface normals associated to them will be oriented parallel based on those normals. When applying the Parallel constraint to position a planar object of a component (planar face or datum plane) with an edge or curve object of another component; a vector will be determined from the edge or curve object. The vector and the planar object’s normal will then become parallel.

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11 Perpendicular Constraint Use the Perpendicular constraint when you need to establish perpendicularity between objects of components. Objects that have surface normals associated to them will be oriented perpendicular based on those normals. When applying the Perpendicular constraint to position a planar object of a component, (planar faces and datum planes), with an edge or curve object of another component; a vector will be determined from the edge or curve object, that vector and the planar object’s normal will then become perpendicular.

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11 Center Constraint Use the Center constraint to center 1 or 2 objects of a component to 1 or 2 objects of another component. Center Objects 1 to 1

Center Objects 1 to 2

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11

Center Objects 2 to 2

Procedure •

Choose the Center constraint.

•

Set the Object filter.

•

Specify the number of objects to use (Center Objects 1 to 1, 1 to 2, 2 to 1, or 2 to 2).

•

Select the objects as instructed in the Cue line.

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11 Distance Constraint Use the Distance constraint to define a distance between two geometric objects. The sign (+/-) of the dimension controls which side of the object the solution is on.

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11 Tangent Constraint Use the Tangent constraint to define a physical contact between two geometric objects. There can be multiple solutions to a tangent constraint. To specify which solution is desired, a help point will be computed from the pick position on the surface and used to find a unique solution to the tangent constraint. The following are some examples of tangent constraints: •

Point on Surface.

•

Line tangent to Surface.

•

Plane tangent to Sphere.

•

Plane tangent to Cylinder.

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11

The Mating Conditions Dialog Mating conditions are applied from the Mating Conditions dialog and can be accessed by choosing the Mate Component icon in the Assemblies toolbar or by choosing Assemblies→Components→Mate Component from the menu bar. 1 — Mating Conditions Tree Listing 2 — Mating Constraint Types 3 — Selection Steps 4 — Expression Value (for Angle and Distance constraints)

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11

Defining Mating Constraints •

Choose the type of constraint to apply.

•

Select the Filter type (optional).

•

Select an object FROM component to be mated (component you are moving).

•

Select an object on the component to mate TO (component that will remain stationary).

•

Choose Preview and then choose Apply (the dialog remains to let you add more constraints). or

•

Choose OK to accept the constraint and dismiss the dialog.

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11

Vary Constraints The Vary Constraints option can be used to reposition the active component in the Mating Conditions dialog. Existing mating constraints will limit the freedom of movement. This dialog is similar to the Reposition Component dialog. A different component can be selected and repositioned by choosing the Select Component icon.

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Adding Components & Mating Conditions

11

Degree of Freedom Indicators Temporary arrows are displayed to indicate the remaining degrees of freedom. The Show Degrees of Freedom/Remove Degrees of Freedom options in the Mating Condition pop-up menu may be used to turn on and off the display of these arrows. A Mate constraint applied to the faces shown below, constrains the small block in the direction normal to the faces. The small block is still free to translate and rotate in the plane that the two shaded faces have in common.

Preview The Preview option becomes active after all the objects have been correctly selected for a constraint. This option lets you preview the solution by actually moving the component based on the existing constraints. Additional constraints may still be applied. After previewing the constraint, choose Apply or OK to accept the constraint or continue creating another constraint. If the constraint is not correct, choose Unpreview and use the Selection Steps to define different FROM and TO faces.

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Adding Components & Mating Conditions

11

List Errors If there are no degree of freedom indicators visible and the Preview option is unavailable, you may have tried to define an invalid mating constraint. This will activate the List Errors option. Choosing it will present information about the error. The constraint must be deleted and recreated.

OK, Apply, and Cancel Buttons

11-26

•

OK — This should be selected only after all constraints have been applied. This will save the mating condition (and its constraints) and dismiss the Mating Conditions dialog.

•

Apply — This will apply the constraint and the dialog will remain open.

•

Cancel — This will dismiss the dialog without saving any of the constraints you added.

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11

Tree Listing The Mating Conditions Tree Listing list all of the assemblies mating conditions and constraints. Several options and viewing preferences may be controlled from the Listing Tree. 1 — Mating Condition expanded to display constraint 2 — Mating Constraint suppression toggle 3 — Mating Condition 4 — Mating Constraints 5 — Mating Constraint pop-up menu

Suppress/Unsuppress Mating Conditions or individual Mating Constraints may be suppressed or unsuppressed using the check box. •

A suppressed mating constraint is ignored during geometric edits.

•

If a mating constraint is being unsuppressed, the mating condition must be solved again.

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Adding Components & Mating Conditions

11

Mating Constraint Pop-up Menu The mating constraints pop-up menu is activated by placing the cursor on a mating constraint and pressing MB3. •

Alternate Solution – Produces any other solution that is applicable to the selected constraint.

•

Convert To – Allows the constraint to be changed to another applicable constraint, i.e. Mate to Distance.

•

Delete – Removes the selected mating constraint.

•

Rename – Allows the renaming of a mating constraint.

Mating Condition Pop-up Menu The mating condition pop-up menu is activated by placing the cursor on a mating condition and pressing MB3.

Highlight/Unhighlight – will highlight or unhighlight the current condition. •

From – Highlights the FROM object for all constraints of the selected condition.

•

To – Highlights the TO object for all constraints of the selected condition.

•

With/Without Direction – Controls the display of the object normal or direction vectors.

Show/Remove Degrees of Freedom – Controls the display of the remaining Degrees of Freedom (DOF). 11-28

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Suppress/Unsuppress – Controls the suppression status of the selected condition. Can also be performed by using the suppression toggle in front of the condition name. •

A suppressed mating condition is ignored during geometric edits.

•

No error messages will be displayed for suppressed mating conditions.

•

If you modify a component creating a failed constraint, that constraint must be deleted before the mating condition can be unsuppressed.

Delete – Removes the selected mating condition. Rename – Allows the renaming of a mating condition. Remember Constraints – Mating constraints may be saved for a selected mating condition within the assembly part. This allows “learned” or automatic mating when the same component is added to the assembly again.

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11

Adding Components & Mating Conditions

11 Repositioning Components The Reposition Component option may be used on a component that does not have any mating conditions, has suppressed mating conditions, or is only partially constrained. If the component is partially constrained, its mating constraints will be enforced within the reposition function. To reposition a component choose the Reposition Component icon from the Assemblies toolbar or choose Assemblies→Components→Reposition Components from the menu bar.

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11

Transform Options The Reposition Component dialog includes the following transform options: 1 — Point to Point 2 — Translate 3 — Rotate About a Point 4 — Rotate About a line

5 — Reposition 6 — Rotate Between Axes 7 — Rotating Between Points

Move Objects or Move Handles Only These radio buttons let you specify whether you want to move the component along with the drag handles or just the drag handles. The drag handles can be repositioned to a specific orientation and used to drag the component along a specific vector direction or about a specific axis.

Distance or Angle The Distance input field (or Angle field if a rotation is being defined) lets you define a distance (or angle) for movement. Snap Increment Snap Increment allows snapping to “whole-multiple” distances when using the direction or rotation drag handles. Vector Method Provides options to define a vector when moving a component using one of the direction drag handles. ©UGS Corporation, All Rights Reserved

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Adding Components & Mating Conditions

11

Snap Handles to WCS Provides a means for moving the handles to the origin and orientation of the current WCS. Motion Animation This slider lets you specify how finely the motion is animated (from Fine to Coarse) during the motion that you have defined. Collision Action Specifies what the system will do if a collision occurs.

•

None — no action is taken.

•

Highlight Collision — you can continue moving the components, and the areas that collided are highlighted.

•

Stop Before Collision — the motion stops just before a collision occurs. The distance between the components when the motion stops depends on the setting of the Motion Animation slider. The closer the slider is to Fine, the shorter the distance.

Collision Checking Mode Allows you to specify what types of objects will be checked for clearance while repositioning.

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11

Repositioning Components Using Drag Handles Components can be repositioned quickly and easily using drag handles. When the Reposition Component dialog is displayed, the graphics window displays a set of handles.

There are several ways to reposition a component with the drag handles. •

To move the origin of the component to a specific point, select the origin drag handle (filled square) with MB1 and then select a destination point. The destination points that can be selected are determined by the Snap Point toolbar.

•

To drag the component to an arbitrary cursor location, select the origin drag handle (filled square) with MB1 and drag to a new cursor location while holding down MB1.

•

To translate the component along an axis, select a translation drag handle (cone head) and drag the component while holding down MB1.

•

To rotate the component about an axis, select a rotation drag handle (filled circle) and drag the component while holding down MB1.

•

To orient the component to a saved coordinate system, select the origin drag handle (filled square) with MB1 and then select the saved coordinate system. The Move Handles Only option is used to first move the drag handles to a specific orientation before using them to move the component.

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Adding Components & Mating Conditions

11

Activity — Mating the Nut Cracker Components In this activity, you will assign mating constraints to components of an assembly. Most of the component parts have already been added to an assembly. In consideration of available class time, some of the parts have already had mating conditions applied to them. Apply associative relationships between components so that changes in size and shape to an individual component part will update the locations of adjacent components in the assembly. Step 1:

Open the nut_cracker_assm part and save as ***_nut_cracker_assm.

1 – Crank

4 – Ramrod

7 – Base

2 – Shaft

5 – Smasher Plate

8 – Mount

3 – Link

6 – Hinges

Step 2:

Start the Modeling application and turn on the Assembly application.

Step 3:

Assign mating conditions between the Mount and the Shaft. Choose the Reposition Component icon. (Assemblies→Components→Reposition Component) Select the Shaft component and click MB2.

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Select the square drag handle (origin) and while holding down MB1, drag the shaft to the location shown below, release MB1, and choose OK.

Choose the Mate Component icon. (Assemblies→Components→Mate Component)

Choose Center. Notice that the From Selection Step active.

is

The Cue line reads: “Select object FROM component to be mated.” Select the cylindrical face of the shaft component as shown below.

The Selection Step advances to the TO object and the Cue line reads: “ Select object on component to mate TO”.

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11

Adding Components & Mating Conditions

11

Select the cylindrical face of the Mount component as shown below and choose Preview.

Choose Apply. The constraint is applied and the selection step returns to From.

Choose Distance. Select the planar face of the Shaft component as shown below.

Select the face of the Mount component as shown below, key in a Distance Expression value of 1.5, and then choose Preview.

Choose Apply and then Cancel. Step 4:

Assign mating conditions between the Shaft and the Crank components.

Choose the Mate Component icon. (Assemblies→Components→Mate Component)

Choose Align. 11-36

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Adding Components & Mating Conditions

Select the planar face of the Crank component as shown below.

Select the planar end face of the Shaft component as shown below and choose Preview. The shaft is oriented to meet the constraint although it has not been applied yet.

Choose Apply. The previous constraint has now been applied.

Choose Center. Select the cylindrical face (1) of the Crank component as shown below.

Select the cylindrical face (2) of the Shaft component as shown above. Choose Preview to verify your constraint and then choose Unpreview. ©UGS Corporation, All Rights Reserved

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11

Adding Components & Mating Conditions

11 Choose Parallel. Select the internal planar face of the crank as shown below.

Select the planar face on the Shaft component as shown below and then choose Preview.

The shaft and crank are oriented to reflect the constraint. If the planar faces are flipped 180°, choose the Alternate Solution option and then choose OK. If the planar faces are oriented properly, choose OK until the Mating Conditions dialog is dismissed. Step 5:

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Add the nc_arm component to the assembly.

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11 Choose the Add Existing Component icon in the Assemblies toolbar. (Assemblies→Components→Add Existing) Choose Choose Part File. Select nc_arm and choose OK. The Component Preview window appears and displays the part. In the Add Existing Part dialog, verify the following settings: Reference Set = Body Positioning = Mate Layer Options = Original Choose OK. Choose Center. In the Component Preview window, select the cylindrical face as shown below.

In the main graphics window, select the cylindrical face of the shaft as shown below.

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Adding Components & Mating Conditions

11

In the Preview window, select the planar face of the Arm component for the FROM selection as shown below.

In the main graphics window, select the planar face of the Shaft component for the TO selection as shown below, enter a Distance Expression of -.25 and DO NOT press Enter.

Choose Parallel. Select the internal planar face of the Arm component as shown below.

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Adding Components & Mating Conditions

Select the planar face of the Shaft component as shown below and then choose Preview.

If the planar faces are flipped 180°, choose Alternate Solution and then choose Apply. If the planar faces are oriented properly, choose Apply. Cancel the Mating Conditions dialog. Step 6:

Reposition the crank component to see the effect of the mating conditions applied so far. Choose the Reposition Component icon. (Assemblies→Components→Reposition Component) Select the crank component and choose OK. Select the square drag handle (origin) and holding down MB1, drag the crank around in a circular motion and verify that the shaft and the arm rotate. Choose MB2 to cancel the repositioning.

Step 7:

Assign mating conditions between the Arm and Link components. Choose the Mate Component icon. (Assemblies→Components→Mate Component)

Choose Center.

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Adding Components & Mating Conditions

11

Select the cylindrical face of the link (1) shown below for the FROM selection. Select the cylindrical face of the arm (2) shown below for the TO selection.

Choose Apply to apply the constraints.

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Step 8:

11

Assign mating conditions between the link and the ramrod. Set the Center Objects filter to 2 to 2.

You will be selecting four faces. 1 2 3 4

— — — —

FROM TO Second FROM Second TO

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Adding Components & Mating Conditions

11

Select the faces below in the order indicated: 1 2 3 4

— — — —

FROM TO Second FROM Second TO

The orientation of your components may differ than the illustrations below.

Choose Apply. Set the Center Objects filter to 1 to 1.

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11

Select the faces below as indicated: 1 — FROM 2 — TO

Choose Apply.

Cancel the Mating Constraints dialog.

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Adding Components & Mating Conditions

11

Step 9:

Visually verify the mating constraints. Orient the view to the Trimetric view (MB3→Orient View→Trimetric).

Choose the Reposition Component icon. (Assemblies→Components→Reposition Component) Select the crank component and accept with MB2. Drag the crank around using the handles. Notice how the components move based on the constraints that have been assigned to them. Step 10: Save and close all parts.

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11

Summary Assemblies may be created using the Top-Down, Bottom-Up, or a combination of the two methods. By applying mating conditions to components, you were able to relate their locations and orientations in an assembly. The Reposition Component option may be used in preparation for mating components. In this lesson you: •

Added components to an assembly.

•

Defined mating conditions.

•

Repositioned components.

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11

Lesson

12 Datum Features

12

Purpose This lesson will define datum plane and datum axis features. Objectives Upon completion of this lesson, you will be able to: •

Create a Datum Plane.

•

Create a Datum Axis.

•

Use datum features to position other features.

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Datum Features

Datum Feature Overview Datum features are construction tools that assist in the creation of solid features and sketches in locations and orientations where planar placement faces do not exist or as associative linear objects. Datum Features may be created relative to an existing solid model or fixed in model space.

12

In the case where a hole must pierce a cylinder to a certain depth from the outside of the cylinder, a construction tool is necessary. This tool is needed because the hole feature requires a planar placement face for creation rather than the cylindrical face of the base solid.

Datum Features may be accessed from the General Datums and Points menu in the Feature Operation toolbar or by choosing Insert→Datum/Point.

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Datum Features

Datum Planes The datum plane option allows a planar reference feature to be created that has many uses. •

To define a sketch plane.

•

To serve as the planar placement face for the creation of form features (i.e. hole, slot, pad, boss, pocket).

•

As a target edge for positioning features.

•

As a horizontal or vertical reference.

•

For the mirror plane when using Mirror Body and Mirror Feature.

•

To define the start or end limits when creating extruded and revolved features.

•

To trim a body.

•

To define positioning constraints in assemblies.

•

To help define a relative Datum Axis.

Relative Datum Planes A relative datum plane is created in reference to other objects in your model. You can use curves, faces, edges, points, and other datums as reference objects for datum planes. There is a wide range of methods you can use to create relative datum planes. Fixed Datum Planes Fixed datum planes do not reference and are not constrained by other geometric objects. There are methods you can use to create fixed datum planes based on the WCS and Absolute coordinate systems and by using coefficients in an equation. You can also use any of the relative datum plane methods to create fixed datum planes by turning off the Associative option in the Datum Plane dialog.

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12

Datum Features

Creating Relative Datum Planes The Datum Plane dialog provides several methods to define a plane. Since Inferred Plane is the default, you can immediately begin selecting objects in the graphics window and the type will be inferred. As you select objects, a preview of the datum is displayed in the graphics window.

12

You can also select the objects first and then choose the Datum Plane option. The constraints will be inferred from the selected objects and a preview is displayed. While the datum plane is previewed, you can specify new constraints and objects or change the parameters using drag handles displayed in the graphics window.

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Datum Features

Cycle Solution This option allows you to cycle through alternate solutions when more than one type of datum plane can be created, based on the object selections and constraints.

Flip Direction The datum plane preview displays an arrow conehead in its center that points in the direction of the plane normal. You can change this direction by choosing this option or using MB3→ Reverse Direction on the conehead.

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12

Datum Features

Common Datum Plane Types The following are the common datum plane creation methods that will be covered in this lesson:

12

12-6

•

Offset Parallel and at a Distance

•

Centered Between Two Faces or Planes

•

Through the Axis of a Cylindrical Face

•

At an Angle to Face or Datum

•

Tangent to a Cylindrical Face

•

Through Three Points

•

Through a Point on a Curve

•

Through a Point and at a Specified Direction

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Datum Features

Offset Parallel and at a Distance (Insert→Datum/Point→Datum Plane)

•

Choose the Datum Plane icon.

•

Select a planar face. A preview of the datum plane displays, with an offset drag handle.

•

Do one of the following: –

Choose OK to accept a value of 0 (zero).

–

Key in an Offset value, press Enter, and choose OK.

–

Select the handle, drag the datum plane to the desired location and choose OK.

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Datum Features

Centered Between Two Faces or Planes (Bisector Plane)

12

12-8

(Insert→Datum/Point→Datum Plane)

•

Choose the Datum Plane icon.

•

Select a planar face. A preview of an offset datum plane displays.

•

Select a second planar face. A preview of the bisector plane is displayed.

•

Choose OK.

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Datum Features

Through the Axis of a Cylindrical Face •

Choose the Datum Plane icon.

•

Select the cylindrical axis symbol of the cylindrical face in the graphics window.

•

Choose OK.

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(Insert→Datum/Point→Datum Plane)

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12

Datum Features

At an Angle to a Face or Datum Plane and Through an Edge or Axis

12

12-10

(Insert→Datum/Point→Datum Plane)

•

Choose the Datum Plane icon.

•

Select the edge through which the datum plane is to pass. You may choose the axis of a cylinder instead of an edge.

•

Select the planar face or datum plane that the angle will reference.

•

Do one of the following: –

Key in a value for the angle (in degrees), press Enter, and choose OK.

–

Select the rotation drag handle and drag the datum plane to the desired angle and choose OK.

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Datum Features

Tangent to a Cylindrical Face and Through a Point (Insert→Datum/Point→Datum Plane)

•

Choose the Datum Plane icon.

•

Select the cylindrical face.

•

Turn on the Point on Curve option in the Snap Point toolbar.

•

Select an edge of the cylinder.

•

Drag the point to the desired location.

•

Choose Cycle Solution previewed.

•

Choose OK.

until the correct tangent datum plane is

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12

Datum Features

Tangent to a Cylindrical Face and At an Angle to a Face/Plane •

Establish a planar reference. This could be an existing face/plane or a new datum plane could be created as follows:

12

12-12

–

Choose the Datum Plane icon.

–

Select the cylindrical axis symbol.

–

Choose OK.

•

Choose the Datum Plane icon.

•

Select the cylindrical face (not on the axis).

•

Select the previously created datum plane.

•

until the correct tangent datum plane is Choose Cycle Solution previewed (parallel, perpendicular, or at an angle).

•

Choose OK.

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Datum Features

Through Three Points •

Choose the Datum Plane icon.

•

Set the Snap Point toolbar as desired.

•

Select three points. A preview of the datum plane is displayed.

•

Choose OK.

(Insert→Datum/Point→Datum Plane)

If it is difficult to select points using the Inferred Plane mode, you can choose the Curves and Points option in the Datum Plane dialog to prevent the selection of other inferred object types.

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12

Datum Features

Through a Point on a Curve

12

(Insert→Datum/Point→Datum Plane)

•

Choose the Datum Plane icon.

•

Choose the Plane on Curve type.

•

Select a point on a curve or edge. A preview of the datum plane is displayed, with the point on curve marked with a handle.

You can alter the datum plane by dragging the handle of the point to change its position along the curve or keying in a Location value.

•

until the desired datum plane (tangent, Choose Cycle Solution normal, binormal) is previewed.

•

If, in addition to the curve, you select another face or linear edge, the direction of the datum plane is defined based on this second object as follows:

•

12-14

–

for a planar face, the datum plane is made parallel to the object.

–

for a linear edge, the datum plane is made normal to the object.

–

for a non-planar face, the datum plane is made parallel to the tangent plane at the closest point on the surface.

Choose OK or Apply to create the datum plane.

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Datum Features

Through a Point and at a Specified Direction (Insert→Datum/Point→Datum Plane)

•

Choose the Datum Plane icon.

•

Choose the Point and Direction option.

•

Set the Snap Point toolbar as desired.

•

Select a point.

•

Use the Vector option menu to define a direction, or accept the default. A preview of the datum plane is displayed.

•

Choose OK or Apply to create the datum plane.

In the example below, a point was defined at the arc center of the hole and a direction was defined using the Vector Constructor dialog.

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Datum Features

Activity — Creating Relative Datum Planes In this activity, you will create relative datum planes that are associated to a solid model.

12

Step 1:

Open the datum_ref_1 part.

Step 2:

Start the Modeling application.

Step 3:

Create a Datum Plane Offset at a distance of 1 inch above the upper face of the block. Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane)

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Datum Features

Select the top face of the block (1) and confirm the selection if necessary.

12

A preview of the Datum Plane is displayed along with an Offset entry field. A direction vector points normal to the face and represents the positive offset direction.

Key in an Offset value of 1 and press Enter. Choose Apply (Ctrl-MB2).

Step 4:

Create a second datum plane through three points.

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12-17

Datum Features

The second datum plane will be created diagonally through the block. The Datum Plane dialog should still be displayed.

12

In the Snap Point toolbar, verify that Control Point turned on and Point on Curve

is

is turned off.

Select the first point (1) and confirm any of the edges. Any of the edges are acceptable because they share the end point. Carefully select each of the two midpoints (2 & 3).

Choose Apply. (Ctrl-MB2) The datum plane is created and positioned through the three selected points. The relationship of this datum plane through the points will remain if the block parameters are changed.

Step 5:

12-18

Create the third datum plane midway between the left and right faces.

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Datum Features

The Datum Plane dialog should still be displayed. Select the right planar face (1).

12

Select the left planar face (2).

Choose OK (MB2). The datum plane is created and located at the center of the part and is parallel to the faces selected.

Step 6:

Edit the block to verify the parametric relationship of the datum planes to the block. With the cursor over the block in the graphics window, press MB3 and choose Edit Parameters. Choose Feature Dialog.

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Datum Features

Key in the following parameters:

12

X Length

=

2

Y Length

=

2

Z Length

=

5

Choose OK. The revised values are displayed in the graphics window. The feature may still be modified without updating the model. Choose OK in the Edit Parameters dialog to complete the change.

Fit the view. (MB3→Fit) The constraints applied to the datum planes at the time of creation continue to control the positioning of the datum planes after the block is edited. Step 7:

12-20

Close the part.

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Datum Features

Selecting and Using Datum Planes To select a datum plane in the graphics window, the selection ball must be placed over one of its displayed boundaries. Form features created using datum planes as the planar placement face are created normal to the datum plane. These features are initially located in the center of the datum plane by default and will remain there if no positioning dimensions are specified. If positioning dimensions are specified, the feature will be moved to the constrained position. When a datum plane is selected for the planar placement face, a direction vector is displayed showing the side of the datum plane on which the feature will be created. An option is available to reverse the direction when creating the feature. Editing Datum Planes To edit the constraints or parameters of a datum plane, use any of the following methods: •

With the cursor over the datum plane boundary, choose MB3→Edit Parameters or MB3→Edit with Rollback.

•

Double-click on a datum plane boundary (The default action is Edit with Rollback).

•

Choose MB3→Edit Parameters in the Part Navigator.

•

Choose Edit→Feature→Edit Parameters and select the datum plane.

•

Choose the Edit Feature Parameters icon in the Edit Feature toolbar.

To edit the size of a datum plane, you can drag one of the handles along its boundaries. These handles appear when previewing the datum during creation and when editing its parameters.

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Datum Features

Deleting Datum Planes Use any of the following methods to delete a datum plane.

12

•

Choose Edit→Delete

•

With the cursor over the datum plane boundary, choose MB3→Delete.

•

Select the datum plane from the graphics window and either press the Delete key on your keyboard or choose the Delete icon.

•

Choose MB3→Delete in the Part Navigator.

Positioning Features to Datums When positioning a feature or sketch to a datum plane or axis, you cannot use positioning dimensions that constrain a point to a point, such as a Horizontal, Vertical, and Parallel dimensions. You can only use dimensions that constrain a point to a line, such as a Perpendicular dimension, or a line to a line, such as a Parallel at a Distance dimension. If a datum plane is selected, the system projects the datum plane until it intersects with the planar placement face of the target solid. The intersection between the datum plane and the target face forms a line, which is used to constrain the feature or sketch. The method used to position features should be dictated by the design intent. Construction of datum features can aid in the application of positioning dimensions by making design intent easier to achieve.

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Datum Features

Activity — Cylindrical Faces and Datum Planes In this activity, you will create relative datum planes associated to a cylindrical face. Step 1:

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Open the datum_ref_2 part.

A hole is required through the cylindrical face at the bottom of the part, centered in the feature. Relative reference features are required to accomplish this task. Step 2:

Start the Modeling application.

Step 3:

Create a Datum Plane through the feature axis, at an angle to the existing plane of 90 degrees. Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane)

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12-23

Datum Features

Move the cursor over the outside cylindrical face of the feature at the bottom of the part and select the cylindrical axis symbol.

12

Select the existing Datum Plane. Choose Apply to accept the default value of 90 and create the datum plane. (Ctrl-MB2) Step 4:

Create a datum plane tangent to the outside of the same cylindrical face to use as a placement face for the hole feature. The Datum Plane dialog should still be displayed. Select the cylindrical face of the feature at the bottom of the part. Select the original Datum Plane.

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Datum Features

Choose Cycle Solution until the new tangent datum plane is in the orientation shown below.

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Choose Apply to create the datum plane. (Ctrl-MB2) Step 5:

Create a center datum plane. Select the two faces shaded below.

Choose OK to create the datum. (MB2) Step 6:

Create a hole.

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12-25

Datum Features

Choose the Hole icon.

(Insert→Design Feature→Hole)

Choose Simple.

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Specify a Diameter of 10. Select the tangent datum plane as the placement face (1). Ensure that the tool solid for the hole is pointing into the part. Select the datum plane (2) at the center of the part as the thru face. Choose OK.

Use Point onto Line positioning to locate the hole centered on datum planes (3) and (4).

Step 7:

Move the datum planes to another layer. Choose Format→Move to Layer.

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Datum Features

Select all the datum planes. Choose OK.

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Key in 62 and choose OK. The newly created hole will remain centered in the part due to its relationship with the datum planes that are constrained to the solid body.

Step 8:

Close the part.

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12-27

Datum Features

Activity — Creating a Feature on a Relative Datum Plane In this activity, you will create a relative datum plane and use it as a placement plane for a hole feature.

12

Create a simple hole at an angle which can be controlled parametrically.

Step 1:

Open the datum_ref_1 part. If the part was opened recently, you can choose File→Recently Opened Parts and select the part from a short list rather than the Open Part File dialog. The Recently Opened Parts list may contain up to ten parts that have been opened in the current or previous sessions.

Step 2:

Start the Modeling application.

Step 3:

Create a datum plane through an edge and at an angle to a face. Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane)

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Datum Features

Select the right edge (1, not the mid point) and confirm the selection if necessary. Make sure Point on Curve is turned off in the Snap Point toolbar.

Select the top face (2), and confirm the selection if necessary.

Key in and Angle of 20 and press Enter. Choose OK (MB2) to create the datum plane. A datum plane is created at the specified angle from the top face and passes through the selected edge.

Step 4:

Create the hole normal to the datum plane. Choose the Hole icon.

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(Insert→Design Feature→Hole) Practical Applications of NX

12-29

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Datum Features

Choose Simple for the hole type. Key in .5 for the diameter.

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Select the boundary of the newly created datum plane for the placement face. Select the bottom face (1) of the block as the Thru Face.

Choose OK. (MB2) Features are initially located in the center of the datum plane. If no other positioning dimensions are specified, the hole will stay in this position. In this case, the hole will be positioned to the front and right edge of the model.

The Perpendicular icon positioning dimension.

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Practical Applications of NX

is already selected for the first

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Datum Features

Select the edge of the block shown (1), as the target edge.

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Key in .75 as the positional expression value. Select the edge of the block shown (1), as the target edge.

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Datum Features

Accept the value of 2.0 by choosing MB2. The hole is positioned to the newly constrained location.

12

Step 5:

Modify the angle parameter of the datum plane. Double-click on the datum plane. Change the angle from 20 degrees to 75 degrees. Choose OK. (MB2)

Try 80 and 90 degrees. Can you explain the results? Step 6:

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Close the part.

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Datum Features

Activity — Creating a Hole Corner to Corner In this activity, you will create a relative datum plane using the Point and Direction option. The intent is to create a hole feature that goes through one corner of a block and comes out the opposite corner and maintains associativity.

Step 1:

Open the seedpart_mm part and save it as ***_hole_corners, where *** represents your initials.

Step 2:

Start the Modeling application.

Step 3:

Create a block that is 200 x 100 x 100 on layer 1.

Step 4:

Change the work layer to layer 61.

Step 5:

Create a datum plane with the point and direction method. Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane) Choose Point and Direction. Select the end point (1) as shown to define a point on the datum plane.

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12-33

12

Datum Features

Set the Vector Method to Two Points.

12

Select the end points (1 & 2) shown below.

Choose OK (MB2). Step 6:

Create a simple hole perpendicular to the datum plane, through the block. Fit the view.

Choose the Hole icon.

(Insert→Design Feature→Hole)

Choose Simple for the hole type. Key in a diameter value of 25.

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Datum Features

Select the datum plane (1) as the placement face. If the hole is not going into the block, choose Reverse Side. Select the far side of the block as the thru face (2) and choose OK.

Choose Point onto Point . Select the end point (1) as shown.

Change the work layer to 1 and make layer 61 invisible.

Step 7:

Modify the size of the block. With the cursor on the block, click MB3 and choose Edit Parameters.

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12-35

12

Datum Features

Click on p2=100.000. Key in 400.

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Choose MB2 twice. Fit the view and note the associativity of the features. Step 8:

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Choose File→Close→Save and Close.

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Datum Features

Datum Axis This option allows a linear reference feature to be created and has several uses. •

Axis of rotation for revolved features.

•

Axis of rotation for circular arrays.

•

To help define a relative datum plane.

•

Directional reference.

•

Target for feature positioning dimensions.

Creating Datum Axes When you choose the Datum Axis option, the Datum Axis dialog is displayed. The default constraint type is Inferred so that you can immediately begin selecting objects in the graphics window to define the axis.

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12-37

12

Datum Features

Datum Axis Types Some common methods that will be covered in this lesson include:

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•

Through Two Points

•

Through an Edge

•

Through a Cylindrical, Conical or Revolved Face Axis

•

At the Intersection of Two Faces/Datum Planes

The important function of these Reference Features is that they are associative to existing geometry.

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Datum Features

Through Two Points To create a datum axis through two points, do the following: •

Choose the Datum Axis icon.

•

Set the Snap Point toolbar as desired.

•

Select two different point locations.

•

Choose OK.

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(Insert→Datum/Point→Datum Axis)

Practical Applications of NX

12-39

12

Datum Features

Through an Edge or Curve To create a datum axis through an edge or curve, do the following:

12

•

Choose the Datum Axis icon.

•

Select the edge or curve but not on a control point.

•

Choose OK.

(Insert→Datum/Point→Datum Axis)

The Point on Curve icon in the Snap Point toolbar must be off in order to create a datum axis through an edge or curve.

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Datum Features

Through a Cylindrical Face Axis To create a datum axis through a cylindrical face, do the following: •

Choose the Datum Axis icon.

•

Select the cylindrical face or axis symbol.

•

Choose OK.

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(Insert→Datum/Point→Datum Axis)

Practical Applications of NX

12-41

12

Datum Features

Through the Intersection of Two Faces/Datum Planes To create a datum axis through the intersection of two faces or datum planes:

12

•

Choose the Datum Axis icon.

•

Select the faces or datum planes.

•

Choose OK.

(Insert→Datum/Point→Datum Axis)

There is no option to create a datum plane at the intersection of two faces/planes at a specified angle. You would first have to create a datum axis at the intersection to serve as the pivot position. Then, create a datum plane through the axis using any other constraint that applies.

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Datum Features

Editing Datum Axes To edit datum axes parameters, use any of the following methods: •

With the cursor over the selection, click MB3 and choose Edit Parameters or Edit with Rollback.

•

Double-click a datum axis in the graphics window. (Edit with Rollback is the default action.)

•

Choose Edit→Feature→Parameters.

•

Choose MB3→Edit Parameters in the Part Navigator.

•

Choose the Edit Feature Parameters icon.

Deleting Datum Axes •

Use Edit→Delete

•

With the cursor over the datum axis, click MB3 and choose Delete.

•

Choose the Delete icon.

•

Choose MB3→Delete in the Part Navigator.

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12-43

12

Datum Features

Activity — Constraining Locations using Datums In this activity, you will create a relative datum axis and datum plane to constrain the pivot location of a hole feature.

12

A 0.5 inch diameter hole is to be located in a block. The origin of the hole will be on the top face and located from the right face. The hole is to remain centered in the block along the YC axis. The angle of the hole shall be editable in a plane parallel to the front face.

Step 1:

Open the datum_ref_1 part. If the part was opened recently, you can choose File→Recently Opened Parts and select the part from a short list rather than the Open Part File dialog.

Step 2:

Start the Modeling application.

Step 3:

Create the Reference Features. Change the work layer to 61.

Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane)

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Datum Features

Select the right face (1) on the block as shown.

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Key in -2 for the Offset value and press Enter. Choose MB2 to create the datum plane.

Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane) Select the back face (2) of the block as shown and confirm. Select the front face (3) of the block as shown and confirm.

Choose MB2 to create the datum plane. A center datum plane is created.

Choose the Datum Axis icon. (Insert→Datum/Point→Datum Axis)

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12-45

Datum Features

Select the datum plane (1) as shown. Select the top face (2) as shown.

12

Choose MB2 to create the datum axis. A datum axis is created at the intersection of the top of the block and the associative datum plane.

Choose the Datum Plane icon. (Insert→Datum/Point→Datum Plane) Select the right face (1) of the block as shown.

Select the Datum Axis. Key in an Angle value of –45 and press Enter.

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Datum Features

Choose Apply to create the datum plane.

12

Select the newly created datum plane. Key in 1 for the Offset value and press Enter. Choose OK (MB2) to create the datum. Fit the view.

Step 4:

Create a Simple Thru Hole. Choose the Hole icon.

(Insert→Design Feature→Hole)

Choose Simple. Key in .5 for the Diameter.

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Practical Applications of NX

12-47

Datum Features

Select the edge of the offset datum plane (1) as shown. Select the bottom face of the block (2) as the Thru Face, confirm and choose MB2.

12

Choose Point onto Line. Select the datum axis as the target edge. A positioning dimension appears in the graphics window with a value of 0. Choose Point onto Line. Select the center datum plane (1) as shown and choose MB2.

The hole will always remain on the datum axis and stay centered in the block.

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Datum Features

Step 5:

Modify the angle parameter of the datum plane. Double-click on the angled datum plane (1).

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Change the angle from –45 degrees to –20 degrees. Choose OK. The angle of the hole changes, but the point of entry remains the same. Step 6:

Change the Location of the Datum Axis. Double-click on the offset datum plane as shown.

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12-49

Datum Features

Change the Offset from -2 to -3 and choose OK.

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Step 7:

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Close the part.

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Datum Features

Datum CSYS A Datum CSYS (Insert→Datum/Point→Datum CSYS) provides a set of associative objects consisting of three planes, three axes, a coordinate system, and an origin point. The Datum CSYS appears as a single feature in the Part Navigator but its objects can be selected individually to support the creation of other features, constraining sketches, and positioning of components in an assembly.

The dialog provides options to create a Datum CSYS at the absolute coordinate system, relative to another existing Datum CSYS, or relative to existing geometry.

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Datum Features

Summary Datums are reference features that are used as construction tools to assist in the creation of solid features and sketches in locations and orientations where planar placement faces do not exist.

12

In this lesson you:

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•

Created associative datum planes and datum axes.

•

Used datum features to create and position form features.

•

Edited datum planes to see how associative features are affected.

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Lesson

13 Sketching 13

Purpose This lesson introduces the method of creating a sketch and free hand sketching of curves. Objectives Upon completion of this lesson, you will be able to: •

Create a sketch.

•

Create sketch curves.

•

Apply dimensional constraints to sketches.

•

Apply geometric constraints to sketches.

•

Identify constraints.

•

Convert a sketch curve to reference.

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13-1

Sketching

Sketching Overview What is a sketch? A sketch is a collection of two-dimensional geometry within a part. Each sketch is a named collection of 2D curves and points residing on a plane that you specify. You can use sketches to address a wide variety of design needs. For example, you might create.

13

•

Detailed part features by sweeping, extruding, or revolving a sketch into a solid or a sheet body.

•

Large-scale 2D concept layouts.

•

Construction geometry, such as a path of motion, or a clearance arc, that is not meant to define a part feature. This lesson will focus on the use of sketches to define detailed part features.

Sketcher tools let you fully capture your design intent through geometric and dimensional relationships that we refer to collectively as constraints. Use constraints to create parameter-driven designs that you can update easily and predictably. Sketcher evaluates constraints as you work to ensure that they are complete and do not conflict. Sketcher offers you the flexibility to create as many, or as few, constraints as your design requires. Geometric relations may be established between the curves within a profile as well as with curves in other profiles and model geometry such as edges or datums.

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Sketching

Why sketch? Sketches provide a high level of control over features and automate the propagation of changes. You can quickly apply constraints to capture a well-known design intent. Once a sketch is placed on a face or datum plane, it will automatically move when the position of the placement face/datum is changed. Since sketches do not require constraints, this approach is the quickest way to build features and still have a sufficient level of associativity. The inherent ability to solve a sketch in real time means that, as rules are applied, the sketch objects change and move to reflect the effect that the assigned rule has on the geometry. This gives you the ability to quickly change profiles of features created using sketches. Using Sketches for Detail Part Features When there is a commonly used shape that varies in size, a sketch can easily accommodate the iterations of the design by editing a single constraint.

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Practical Applications of NX

13-3

13

Sketching

Sketches should be used as base features of a model if the shape lends itself to extruded or revolved geometry.

13

Sketches may be used in a number of different ways. Consider them for guide paths for swept features, or as section curves for free form features.

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Sketching

An important aspect of modeling that will help you decide how to use a sketch is defining the design intent of the model. The design intent consists of two items: •

Design Considerations — The geometric requirements on the actual part, including engineering and design rules that determine the detail configuration of the part.

•

Potential Areas for Change — Known design changes or iterations, and their effects on the part configuration.

As a general rule, the more design considerations and potential areas for change, the more likely there are benefits from sketching.

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Practical Applications of NX

13-5

13

Sketching

Sketches and the Part Navigator Sketches can be created by choosing the Sketch Section icon in certain feature creation dialogs such as Extrude and Revolve, choosing the Sketch icon directly in the Form Feature toolbar, or by choosing Insert→Sketch. If you create a sketch from within a feature creation dialog, the sketch of the section remains internal to the feature. It does not display in the graphics window or in the Part Navigator. You can edit the sketch by accessing the associated feature. If the same sketch is required to create additional features, you can choose the Make Sketch External option from the MB3 popup menu in the Part Navigator and it will appear in the graphics window.

13

If a sketch is not created from within a feature creation dialog, it will appear as a separate feature in the Part Navigator.

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Sketching

Sketch Visibility Organizing the data in a part is an important aspect of modeling. The sketcher helps in this endeavor by automating the visibility of sketches are activated and deactivated. •

•

If a standalone sketch is created by choosing the Sketch icon in the Form Feature toolbar (or Insert→Sketch), the current work layer is assigned to the sketch as it is created. When you subsequently activate the sketch, the work layer is set to the layer assigned to the sketch so that you do not accidently construct objects in the active sketch across multiple layers. If the sketch is created internal to a feature, it automatically becomes visible when you edit the feature and choose the Sketch Section icon in the feature dialog.

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Practical Applications of NX

13-7

13

Sketching

Creating a New Sketch Defining a Sketch Plane When creating a sketch, you first need to define the plane on which to place the sketch curves. But, you must consider the state of the model. Since the goal is to develop a parametric model, all of the features need to be associative. Is the sketch going to define the base feature? Is the sketch going to be attached to an existing reference feature or face of an existing body?

13

An icon option bar shown below appears in the upper left corner of the graphics window and contains options to define the sketch plane.

1 – Sketch in Place

4 – YC–ZC Plane

7 – Datum CSYS

2 – Sketch Plane

5 – XC–ZC Plane

8 – OK

3 – XC–YC Plane

6 – Datum Plane

9 – Cancel

Defining the Sketch as the Base Feature If the sketch is going to define the base feature and there is no existing geometry or reference features in the part, you may define the plane by choosing one of the following options: • • • •

XC-YC Plane YC-ZC Plane ZC-XC Plane Datum CSYS

Initially, the XC-YC plane will be highlighted in the graphics window. You can accept this plane or choose one of the other options.

To accept the plane, choose OK

(MB2).

After the plane is accepted, the view in the graphics window is automatically oriented so that it is parallel to the sketch plane. If you do not want the view to be oriented in this manner, you can turn off the Change View Orientation setting in Preferences→Sketch.

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Sketching

Associate Sketch to Existing Face or Reference Feature You can also define the sketch plane on an existing planar face, Datum Plane, or Datum CSYS. A relative Datum Plane or Datum CSYS may also be created on the fly. To create the sketch on an existing face, Datum Plane, or Datum CSYS plane. •

Select the face, Datum Plane, or Datum CSYS plane.

•

Define the horizontal or vertical reference.

•

Choose OK.

13

To create a relative Datum Plane on the fly: •

from the icon option bar in the upper left Choose Datum Plane corner of the graphics window.

•

Select the required objects to define the Datum Plane.

•

Choose OK in the Datum Plane dialog.

•

Define the horizontal or vertical reference.

•

Choose OK. A similar procedure can be used to create a relative Datum CSYS on the fly.

If there is an existing Datum CSYS in the part and it is coincident with the WCS. The X-Y plane of the Datum CSYS will initially highlight as the default sketch plane. If you choose the XC-YC, YC-ZC, or ZC-XC option, you will be asked whether to use the corresponding Datum CSYS plane instead.

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Practical Applications of NX

13-9

Sketching

Defining the Reference Direction The reference direction is used to specify the horizontal direction on the sketch plane. When there is no linear object pointing in the desired horizontal direction, a vertical reference may be defined. Because vertical is 90 degrees (counterclockwise) from horizontal by definition, the horizontal direction is interpreted from it. In the example below, the shaded face (1) is specified as the placement face. An edge (2) is defined as the vertical reference. The resultant sketch orientation is shown to the right.

13

The direction of an axis may be changed as follows: •

To flip the direction of a sketch axis, double-click on it.

•

To specify a new direction, select the axis to redirect and then select a straight edge. The straight edge is projected to the sketch plane to define the new direction.

If a datum plane is selected to define the sketch plane, a Z axis will also be displayed. The normal of the sketch plane may be changed by double-clicking on the Z sketch axis.

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Sketching

Naming a Sketch Since a unique name is required for each sketch, a default name will initially be assigned with a numeric suffix. The format of the default name is "SKETCH_###" where ### is replaced by the next sequential three digit number beginning with 000 (SKETCH_000, SKETCH_001, etc.). A sketch name may be defined during or after the sketch has been created by clicking on the default sketch name, typing in the new name and pressing Enter.

13

The sketch can also be renamed by choosing Sketch→Sketch Properties. Sketches should be given descriptive names rather than accepting the default. This allows downstream users to understand the function of the sketch at a glance.

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Practical Applications of NX

13-11

Sketching

The Active Sketch In any given part there may be numerous sketches of different features at different orientations. When using the sketcher, only one sketch may be worked on at a time. This sketch is called the active sketch. Curves created while a sketch is active become associated with the active sketch. When returning to a sketch to add to or modify a profile, the sketch must be activated. There are a few ways to activate a sketch:

13

•

Double-clicking on a sketch curve.

•

In the Part Navigator double-click on the sketch feature node.

•

Choose the Sketch icon and select the desired sketch from the Sketch Name pull-down.

There are also a few ways to deactivate an active sketch:

13-12

•

Choose the Finish Sketch icon.

•

Choose Sketch→Finish Sketch.

•

Activate a different sketch.

•

Choose Sketch→New and create a new sketch.

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Sketching

Sketch Creation Steps Sketch for a Base Feature •

Set the work layer for the sketch.

•

Choose the Sketch icon.

•

Define the sketch plane on a WCS plane (XC-YC, YC-ZC, or ZC-XC) or create a Datum CSYS at absolute coordinates.

•

Name the sketch.

•

Choose OK.

Sketch on an Existing Face or Reference Feature •

Set the work layer for the sketch.

•

Choose the Sketch icon.

•

Select the face, Datum Plane, or Datum CSYS plane. (You could also create a relative Datum Plane or Datum CSYS on the fly.)

•

Define the horizontal or vertical reference

•

Name the sketch.

•

Choose OK.

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Practical Applications of NX

13-13

13

Sketching

Activity — Sketch Creation In this activity, you will create a sketch on an existing face and another sketch on a datum plane that is created on the fly.

13

Step 1:

Open the seedpart_in part.

Step 2:

Start the Modeling application.

Step 3:

Create a sketch for a base feature. Make layer 21 the work layer.

Choose the Sketch icon.

(Insert→Sketch)

Choose the YC-ZC Plane. Click on the sketch name, key in base and press Enter.

Choose OK.

(MB2)

The sketch is created. In addition, a fixed datum plane is created on the specified sketch plane and two fixed datum axes are created along its major axes. The specified sketch plane defines a Feature Coordinate System (FCS) for the sketch such that the X axis is parallel to the horizontal direction and the Y axis is vertical. The WCS is automatically manipulated to the FCS orientation to facilitate the creation of sketch geometry. Step 4:

Exit the Sketcher. Choose the Finish Sketch icon.

Step 5:

Close the part and do not save.

Step 6:

Open the sketch_creation_1 part.

Step 7:

Start the Modeling application.

Step 8:

Create a sketch on an existing face.

(Sketch→Finish Sketch)

Make layer 21 the work layer. 13-14

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Sketching

Choose the Sketch icon. The Sketch Plane icon

(Insert→Sketch) is already selected.

Select the face (1) shown below. The 2D sketch plane indicator appears and the X-Axis is active (highlighted). Select the horizontal reference (2) at the location shown below.

Click on the sketch name, key in skt1 and press Enter.

Choose OK. Step 9:

(MB2)

Create a curve on the sketch plane. Choose the Circle icon.

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(Insert→Circle)

Practical Applications of NX

13-15

13

Sketching

Create a circle by selecting at location (1) and then location (2).

13

Choose the Finish Sketch icon.

(Task→Finish Sketch)

Step 10: Change the orientation of the face that defines the sketch plane. Choose Tools→Expression. Select the expression Change_Me and change the formula to 3.5. Choose OK. Rotate the part and notice how the circle remains associative to the face. Step 11: Create a sketch on a datum plane.

Orient the view to Trimetric.

(Home key)

Make layer 22 the work layer, layer 21 invisible, and layer 1 selectable.

Choose the Sketch icon.

(Insert→Sketch)

Choose Datum Plane. 13-16

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Select the two shaded faces shown below.

13

Choose OK in the Datum Plane dialog. A center datum plane is created.

The 2D sketch plane indicator appears and the X-Axis is active (highlighted).

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Select the edge for the horizontal reference at the location indicated below.

13

Click on the sketch name, key in skt2 and press Enter.

Choose OK.

(MB2)

YC ZC

XC

Choose the Finish Sketch icon. Step 12: Activate an existing sketch by selecting geometry. Make layer 21 selectable.

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Double-click on the sketch curve (1) shown below.

13

Fit the view. (MB3→Fit) Sketch SKT1 is activated and oriented in the graphics window.

Choose the Finish Sketch icon. Step 13: Activate an existing sketch by name. Choose the Sketch icon.

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Choose SKT2 from the sketch name option menu.

13

Sketch SKT2 is activated and oriented in the graphics window.

YC ZC

XC

Choose the Finish Sketch icon. Step 14: Close the part.

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Sketch Curves Sketch curves are created via the Sketch Curve toolbar. As curves are created geometric constraints are assigned to the curves relative to the Infer Constraints Settings. 1 2 3 4

– – – –

Profile Line Arc Circle

13

Infer Constraint Settings The Infer Constraints Settings dialog determines which constraints are automatically created during curve creation. It is accessed by choosing the Infer Constraint Settings icon from the Constraints toolbar or Tools→Constraints→Infer Constraint Settings.

As you create the curves a symbol will appear near the curve being created to represent the constraint that will be applied, if any. ©UGS Corporation, All Rights Reserved

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Sketching

Locking a Constraint When a constraint symbol appears during curve creation you may lock in that constraint by pressing MB2. For example, if you are creating a line and the parallel symbol appears, press MB2. As you move the cursor, the new line that is rubber banding is doing so parallel to the reference curve. Snap Angle The snap angle is a preference setting in the Sketch Preferences dialog that is applied when curves are being created. It is used to "snap" a line to horizontal or vertical. The default snap angle is set to 3° and is user definable between 0° and 20°. This angular tolerance is defined on either side of horizontal or vertical from the first specified location, effectively creating a 6° tolerance zone by default.

13

When creating lines outside of the sketcher, snap angle only applies when using inferred cursor location. Snap Point Toolbar The Snap Point toolbar can be displayed when creating most of the curve types in the sketcher so that you have more control over the selection of locations.

When the Snap Point toolbar is active, regardless of the point types turned on, cursor location is always available.

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Alignment Lines While Creating Curves In the process of creating a curve, if you are horizontally or vertically opposite a control point, the system will display an alignment line. The example below depicts an existing curve (1) with a new curve (2) being created as well as the alignment curves (3).

13

Profile Tool The Profile tool allows creation of a string of lines and arcs without having to specify a start for each curve after the first curve is created. The Profile tool is turned on by default when you first create a sketch and can be accessed by choosing the Profile icon on the Sketch Curve toolbar. The icon options in the upper left corner of the graphics window allow you to switch between creating lines (1) or arcs (2) and allow you to switch between Coordinate Mode (3) or Parameter Mode (4). Line creation and Coordinate Mode are the defaults.

Once you have created the first curve (line or arc), the default will revert back to Line. You can switch to arc creation by using press-drag-release with MB1.

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The "circle-X" symbol (1) controls the direction in which the arc will be created.

If the desired arc is in the wrong direction, release MB1, pass the cursor over the end of the line, and exit in a different quadrant of the symbol.

13

Arc originating from top quadrant

Arc originating from left quadrant

Arc originating from right quadrant

Arc originating from bottom quadrant

As you create curves with the profile tool, the string mode can be broken by clicking MB2.

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Creating Lines Line creation is accessed by choosing the Line icon on the Sketch Curve toolbar. Once in line creation, the icons in the upper left corner of the graphics window provide two options: Coordinate Mode (by cursor location or keying in an XC and YC coordinates) and Parameter Mode.

13 There are several ways to create a line: •

Locate the start, and then locate the end.

•

Locate the start, and then enter the length and angle parameters.

•

Locate the start, enter one parameter, and then locate the end.

•

Key in the parameters and then locate the start.

Once you indicate a start location, the system will switch to the Parameter Mode. But, you can still specify an end location without switching back to Coordinate Mode.

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Creating Arcs Arc creation is accessed by choosing the Arc icon on the Sketch Curve toolbar. Once in arc creation, the icons in the upper left corner of the graphics window give you two sets of options. The first is creation method, and the second is for the Coordinate/Parameter Mode.

13 There are two different arc creation methods: Arc by 3 Points — There are several ways to create the arc with this method: •

Locate the start, locate the end, and then locate a point on the arc.

•

Locate the start, enter a radius value and press Enter, locate the end point, and then move the cursor to preview and choose which of the four possible solutions to create.

•

The same as the previous, but enter the radius value after locating the end point, but before the point on arc.

Arc by Center and End Points — There are several ways to create an arc with this method: •

Locate the center, locate the start point, and locate the end point. (The start point location determines the radius.)

•

Locate the center, locate the start point, enter a radius value and press Enter, locate the end point.

•

Locate the center, enter radius and sweep angle values and press Enter, locate the start of the sweep, and specify the direction for the sweep.

Once you indicate a first location, the system will switch to Parameter Mode. But you can still specify locations with the cursor without switching back to Coordinate Mode.

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Creating Circles Circle creation is accessed by choosing the Circle icon on the Sketch Curve toolbar. Once in circle creation, the icons in the upper left corner of the graphics window provide two sets of options. The first is creation method, and the second is for the Coordinate/Parameter Mode.

13 There are two different circle creation options: Circle by Center and Diameter — There are a few ways to create a circle with this option: •

Locate the center, and then locate a point on the circumference of the circle.

•

Locate the center, enter a Diameter, and press Enter. The circle is created. You are then in multiple circle creation mode - just indicate another location for a circle center.

•

Locate the center, drag the radius until you get the size you want. Press Enter. The circle is created, and you are in multiple circle creation mode. Indicate another center.

Circle by 3 Points — There are two ways to create a circle with this option: •

Locate three points on the circumference of the circle.

•

Locate two points on the circumference of the circle, enter a radius value and press Enter, then choose which of the two options you want by cursor location.

Once you indicate a first location, the system will switch to the enter Parameters mode. But you can still give a location without changing back to XY.

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Activity — Using the Sketch Profile Tool In this activity, you will use the Profile tool to create sketch geometry.

13

Step 1:

Open seedpart_in and save it as ***_sketch_profile_1 where *** represents your initials.

Step 2:

Start the Modeling application.

Step 3:

Change the Work Layer to 21.

Step 4:

Create a sketch on the XC-YC plane. Choose the Sketch icon.

Choose OK Step 5:

(Insert→Sketch)

to accept the XC-YC Plane.

Add icons to the Sketch Constraints toolbar. Select the Toolbar Options area of the Sketch Constraints toolbar and choose Add or Remove Buttons→Sketch Constraints.

Make sure the Infer Constraint Settings and Create Inferred Constraints icons are toggled on. You may have to move the toolbar to see the icons after they are added. Step 6:

Set the Infer Constraints Settings. This is done so that only the constraints that you may want to apply will be available during curve creation.

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Choose the Infer Constraint Settings icon. (Tools→Constraints→Infer Constraint Settings) Turn on only the following constraints. Horizontal Vertical Tangent Parallel Perpendicular Coincident Dimensional Constraints

13

Choose OK. Step 7:

Create a Profile. In this step you will create the sketch curves shown below using the Profile tool.

Choose the Profile icon (Insert→Profile) and move the cursor into the graphics window. Select a start location with the cursor near the bottom left corner of the graphics window (approximately XC=-4, YC=-2)

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Move the cursor so that the rubber-banding line snaps to the horizontal orientation and the horizontal symbol displays (1) as shown below.

13

Notice the horizontal symbol indicating the constraint that is going to be applied to the line. Press MB2 to lock in the horizontal constraint. Now notice that as you move the cursor around, the rubber-banding line remains horizontal. Key in 3 for the Length and press Enter.

Notice that a dimensional constraint is created automatically. This is because a Length value was explicitly entered and the Dimensional Constraints option was turned on in the Infer Constraint Settings dialog.

Hold MB1 down and drag the cursor straight up from the end point of the last line and then release. You are now in Arc creation mode.

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Key in 1 for the Radius and press Enter. Key in 180 for the Sweep Angle and press Enter.

Click MB1 in the graphics window to apply.

13

Continue using the Profile tool to create the remaining curves in the sketch as shown below. You do not have to key in exact values but just create the approximate shape. Close the profile by selecting the end point of the first line.

Dimensions maybe added at a later time to constrain the remaining curves to specific sizes.

Choose the Finish Sketch icon. Step 8:

Save and close the part.

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Optional Challenge Practice sketching the following profiles:

13

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Creating Fillets Fillet creation is accessed by choosing the Fillet icon on the Sketch Curve toolbar. Once in fillet creation, icon options appear in the upper left corner of the graphics window. The Trim Inputs option (1) determines whether or not the original curves are trimmed. The Delete Third Curve option (2) determines whether the middle curve is deleted in a three-curve fillet. The Create Alternate Fillet option (3) will produce a complementary solution for the fillet (e.g. a 270 degree arc instead of the default 90 degree arc).

You can create fillets between lines, arcs or conics. You can also create a fillet between two parallel lines. There are several ways to create Fillets: •

Select two curves with a single selection (at their intersection), and then drag the size and quadrant.

•

Select two curves individually, and drag the size and quadrant.

•

Select one curve, enter a radius value, and select the second curve.

•

Select two curves individually, enter a radius value, and the indicate the desired quadrant.

•

Drag (with MB1) across the two curves you want to fillet. The size of the fillet is determined by where the curves are selected.

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Sketching

Trimming and Extending Curves

Quick Trim This option will allow you to trim any curve to the closest curve in the sketch and preview the results in preselection color.

13

You can trim multiple curves at one time, by using the "crayon" select method. Hold down MB1 and drag across the portion of curves you want to trim away.

You can select a specific curve to trim to, by using Ctrl-select to select the desired boundary curve. More than one bounding curve can be selected using this method. In the example below, both the arc on the left and the spline on the right were Ctrl-selected as boundary curves. With the cursor on the top line, (between the two boundary curves), the center section is previewed as the portion to be removed.

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When a curve is trimmed, appropriate constraints are automatically created. In the previous example, two Point on Curve constraints and one Collinear constraint are added. If one of the boundary curves is later trimmed to the line, the Point on Curve constraint would change to Coincident.

13

If you trim an arc to a line that is tangent, the tangency constraint is retained.

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Quick Extend This option will extend lines, arcs and conics to the closest curve in the sketch. The system will preview the results in the preselection color. The curve being extended must extend to an actual intersection with the boundary curve. You can extend multiple curves at one time, by using the "crayon" select method. Hold down MB1 and drag across the ends of curves you want to extend.

13

You can also select specific boundary curves by using the control-select method. As with Quick Trim, when you use Quick Extend, appropriate constraints are automatically created.

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Activity — Creating Fillets In this activity, you will create fillets in an existing sketch. Step 1:

Open the sketch_fillet_1 part.

13

Step 2:

Start the Modeling application.

Step 3:

Activate the sketch. Double-click on any of the sketch curves.

Step 4:

Set the Infer Constraints Settings.

Choose the Infer Constraint Settings icon. (Tools→Constraints→Infer Constraint Settings) Turn off the Dimensional Constraints setting. Choose OK. Step 5:

Create a 4 mm radius fillet using lines L16 and L20 with a single selection and trimming the lines.

Choose the Fillet icon.

(Insert→Fillet)

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Key in 4 in the Radius field on the graphics window, and press Enter.

Select both lines at the same time, by selecting at their intersection.

13

Drag the cursor around the screen and notice that you can select which quadrant you want. Select in the lower right quadrant to place the fillet in the desired quadrant.

Step 6:

Create a 4 mm fillet using lines L16 and L17 with a single selection and do not trim the lines. Turn off Trim Inputs. (background not highlighted)

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Select the two lines at their intersection.

13

Select in the upper right quadrant.

Step 7:

Create a 4 millimeter fillet between lines L17 and L18. Select by dragging across the two lines. The 4.0 Radius value should still be in the text field on the graphics window. With MB1 held down, drag across the two lines as below: (This is another method of selecting the curves to be filleted. The curves crossed with the "crayon" are the curves selected.)

Notice that the 4 millimeter radius was used.

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Step 8:

Create another fillet between lines L18 and L20 by using the "crayon", but this time do NOT use a radius value. Use Backspace to erase the 4 in the text field.

Drag (with MB1), as shown below:

13

It used the selection location of the curves to determine the radius.

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Step 9:

Create a fillet between lines L18 and L19, and drag the size and quadrant. Individually select the lines L18 and L19. Drag the cursor around the screen. Select a location to create an arc similar to the one shown below.

13

Choose the Finish Sketch icon. Step 10: Close the part.

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Activity — Using Quick Trim and Quick Extend In this activity, you will trim and extend existing sketch geometry. Step 1:

Open the sketch_quick_1 part.

Step 2:

Start the Modeling application.

Step 3:

Trim curves with Quick Trim.

13

Double-click on one of the sketch curves to activate the sketch.

Choose the Quick Trim icon.

(Edit→Quick Trim)

Select the line at the location of the arrow below.

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Hold MB1 down and drag the cursor across the two curves as shown below.

13

Ctrl-Select the curves (1) and (2) for boundaries. Select on curves (3) and (4) to trim the center portion.

Step 4:

Extending curves with Quick Extend. Choose the Quick Extend icon.

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Place the cursor on the arc at location (1) shown below.

13

The status line informs you that the curve cannot be extended. This is because there is no other curve that would intersect the arc. Place the cursor on the arc at location (2) shown below.

This time, an intersection is found and a preview is provided. Select the arc at location (2) to create the extension.

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Step 5:

Continue to experiment with Quick Trim and Quick Extend until the instructor is ready to continue.

Step 6:

Choose the Finish Sketch icon.

Step 7:

Close the part.

13

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Sketching

Sketch Points Sketch objects are defined by theoretical points. A line, for instance, is defined by two points. The sketcher attempts to mathematically solve for the location of the points by analyzing the constraints (rules) that are placed on objects. The points that the sketch solver analyzes are referred to as sketch points. By controlling the locations of these sketch points the curve itself may be controlled. There are various ways to control these points. The sketch points associated with different types of curves are illustrated in the graphic below.

13

Line

Arc

Circle

Spline

Fillet

Point

Ellipse

Degree-of-Freedom (DOF) Arrows Degree of freedom arrows are displayed at a sketch point when the solver is unable to fully determine where the sketch point is located on the sketch plane based on existing constraints and dimensions. They are only displayed during the creation of dimensions or constraints. The DOF arrows can point in both the horizontal and vertical directions. An arrow pointing to the right means that the sketch point is free to move left or right in the horizontal direction. An arrow pointing up means that the sketch point is free to move up or down in the vertical direction. These arrows provide visual feedback while you are constraining the sketch. Undefined in X and Y Directions

Undefined in Undefined in Y Direction X Direction

Defined in X and Y Directions (no display)

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DOF arrows are removed as rules are written that define the location of the sketch points. •

Arc - Arcs have sketch points at the center and at either end. These sketch points as well as the radius of the arc may be defined.

•

Circle - Circles may have the center point as well as a radius or diameter defined.

•

Ellipse - An ellipse may have the location of its center defined; also, the parameters for the size and orientation of the ellipse are stored for future editing.

•

Fillet - A Fillet is a special case of arc. By definition a fillet is tangent to the objects with which it is associated and this rule is applied as it is created. Fillets are also defined by the center and end points but the tangency will help determine the location of these points.

•

Line - Lines may have the sketch points at either end defined.

•

Point - Points may be defined relative to other objects or at specific locations in space.

•

Spline - Degree three splines may have their defining points located. Slopes of the spline at the defining points may also be defined. Splines that are of a degree other than three may be added to sketches; however, since their defining points are not located at their knot points, there is no way to locate their defining points using constraints.

If any of the sketch points that define a curve are unconstrained, the curve is displayed in the color specified by the Partially Constrained Curves setting in Preferences→Sketch→Colors. When all defining points are constrained, the curve will change to the color specified by the Fully Constrained Curves setting in Preferences→Sketch→Colors. Theses colors only apply during the creation of dimensions or constraints.

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Dimensional Constraints Design Intent The power in sketching is derived from the ability to capture design intent. You do this by creating rules, called constraints, that dictate how sketch objects will react to changes. As many or as few constraints as necessary may be applied to cause the sketch profile to update in the manner desired.

13

NX sketches are not required to be fully constrained. Creating Sketch Dimensions A dimension controls the size of a sketch object, such as the length of a line or radius of an arc, or the relationship between two objects, such as a distance or angle. Dimensions appear in the graphics window. Unlike drafting dimensions, changing the value of the sketch dimensions changes the shape and or size of dimensioned objects. This changes any features, such as extrude or revolve features, that the sketch curves control. Dimensions may be applied by using the dimension menu on the Sketch Constraints toolbar. 1 — The default Inferred Dimensions icon infers the dimension type based on the objects that are selected and the position of the cursor. 2 — The other dimension icons are useful when the system is unable to infer the desired dimension type. These different options are "filters" that when selected will only allow a specific dimension type to be created. Certain types of geometry may not be selectable if they do not coincide with the dimension type selected.

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As dimensions are being created, the dimension, its extension lines, and arrows are displayed as soon as the geometry has been selected. •

Drag the dimension until it is the correct type, for example horizontal or parallel.

•

Place the dimension by clicking MB1.

•

Click and drag the dimension to the desired location.

Sometimes, a dimension type may be inferred before all of the geometry has been selected. In this case, continue to select geometry until the correct dimension type is displayed, or select the icon for the dimension type you desire and select the geometry again. An expression is also created for each dimension. The name (1) and value (2) of the expression appear in a text box in the graphics window after the dimension has been placed. You may key in a new name or value. Press the Enter key to activate the change.

Sketch Dimension Dialog The Sketch Dimensions Dialog icon accesses the Dimensions dialog.

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Sketching

You can use the dialog to help create and edit dimensions. You can change the value of a dimension by either keying it in or using the slider bar.

13

There are also two option menus to change the appearance of the dimension. The Placement option menu is for defining how the text and arrows of the dimension will be displayed. Options are for automatic placement of text and arrows (1), manual text placement with arrows inside the extension lines (2), or manual text placement with the arrows outside the extension lines (3).

The Leader option menu is for defining whether the dimension’s leader is attached to the left (1) or right (2) of the dimension text.

Both of these option menus may be used before, during or after dimension creation. Text Height The Text Height controls the displayed height of the dimension text. Modifying this value will affect the display of all dimensions in the active sketch. The Text Height option can also be accessed by choosing Preferences→Sketch. The Fixed Text Height option in Sketch→Preferences controls the size of the dimension text when you zoom. If this option is turned on, the text will remain the same size relative to the screen as you zoom in and out. 13-50

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Dimension Types Inferred — The dimension type (except perimeter) is inferred based on the objects selected and the cursor location. Horizontal — Specifies a distance constraint between two points with respect to the X-axis of the sketch coordinate system. Points, points on sketch curves, edges, lines, and arcs are selectable.

Vertical — Specifies a distance constraint between two points with respect to the Y-axis of the sketch coordinate system. Points, points on sketch curves, edges, lines, and arcs are selectable.

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Parallel — Specifies a constraint for the shortest distance between two sketch points. All sketch objects are selectable using this method. The points selected will be inferred from the objects selected.

13

Perpendicular — Specifies a distance constraint measured perpendicular to a selected line and a point. If the desired point is an endpoint of a line, this endpoint must be selected as the second object.

Angular — Specifies an angular constraint between two linear objects.

Radius — Specifies a radial size constraint for an arc or circle.

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Diameter — Specifies a diameter size constraint for an arc or circle.

13 Perimeter — Constrains the collective lengths of lines and arcs to a desired value. After selecting the curves and choosing MB2, an expression is automatically generated with a “Perimeter_” prefix added to the name. (i.e. Perimeter_p7=6.456). There will be no graphical representation of this constraint in the graphics window.

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Activity — Adding Dimensional Constraints In this activity, you will capture the design intent for a part by adding rules that will control how the part is to change. These rules allow the part to be easily modified. The included angle of the adjustment slot should change from 45° to 75° by dimensional constraints.

13

Step 1:

Open angle_adj_1.

Step 2:

Start the Modeling application.

Step 3:

Add the required dimensions. Double-click on one of the sketch curves to activate the sketch. Choose Preferences→Sketch. Verify the Text Height is set to .10 and choose OK.

Choose the Inferred Dimensions icon. (Insert→Dimensions→Inferred) Select the lower angled line (1, not endpoint).

The system infers that you wish to create a horizontal, vertical, or parallel dimension depending on the placement of the cursor relative to the geometry. DO NOT PLACE THE DIMENSION!

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Select the upper angled line (2, not endpoint).

13

Select a cursor location to place the dimension. Select the horizontal line (1, not endpoint) across the bottom. Select the lower angled line (2, not endpoint).

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Select a cursor location to place the dimension.

13 Choose MB2 to exit dimension creation mode. Step 4:

Change the viewpoint. Choose MB3→Orient View to Model.

Choose the Finish Sketch icon.

There are times, such as geometry creation, when looking directly at the plane of the sketch is beneficial. At other times, it may help to change the view point to see the effects of changes on the geometry. Step 5:

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Editing Dimensions The editing of dimensions may be achieved as follows: •

To edit the value or the name, simply double-click on the dimension and edit the value or the name in the text box and press Enter.

•

To edit the position, place cursor over a dimension, press and hold down MB1, and simply drag the dimension’s location.

•

Additional editing that may be done with the Dimensions dialog as listed below: Name Value

— —

Position

—

Text placement — Leader side — Text height —

Key in a new name in the text entry field. Key in a new value in the text entry field or use the slider. Click and hold MB1 on the dimension and drag to new position. Select a different option from the option menu. Select a different option from the option menu. Key in a new text size in the text entry field.

The name and value of a dimension may also be edited by using the Expressions dialog. As dimensions are edited, the constraints are evaluated and the geometry is modified.

Delay Evaluation Delay Evaluation prevents geometry changes as one or more dimensions are modified. This is available as an icon on the Sketcher toolbar or by choosing Tools→Delay Sketch Evaluation.

Evaluate Sketch Evaluate Sketch controls sketch evaluation when Delay Evaluation is on. (Sketches are evaluated automatically when you exit from the Constraints dialog.) This is available as an icon on the Sketcher toolbar or by choosing Tools→Evaluate Sketch

Update Model Update Model forces the model to update without leaving the sketch function. (The model is updated automatically when you exit from the sketch environment.) This is available as an icon on the Sketcher toolbar or by choosing Tools→Update Model. ©UGS Corporation, All Rights Reserved

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Retain Dimensions When a sketch is deactivated the dimensions are normally hidden. Retain Dimensions is a toggle in the Sketch Preferences dialog to retain dimension display after the sketch is deactivated.

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Retain Dimensions applies only to the active sketch, thus to suit your needs you may have a mixture of sketches with and without retained dimensions. Use this setting when you need to display dimensions without an active sketch, for example to reference expression names between sketches, when creating features, or for plotting.

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Activity — Editing Sketch Dimensions In this activity, you will edit dimensional constraints and see that they do not sufficiently control the angle bracket from the previous activity. Step 1:

Open angle_adj_2.

Step 2:

Start the Modeling application.

Step 3:

Change the layer settings.

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Make layer 1 Selectable.

Fit the view.

(MB3→Fit)

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Step 4:

Edit a dimension. Place the cursor over a sketch curve and choose MB3→Edit. Choose MB3→Orient View to Model. Double-click on the 45° dimension. In the dynamic input field, key in 75 and press Enter.

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Step 5:

Edit another dimension. Double-click on the 15° dimension. In the dynamic input field, key in 25° and press Enter.

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Notice how the geometry updates. Basic geometric assumptions that we make when we look at this geometry are not specified to the system, i.e. the bottom line has no horizontal constraint applied. If the geometry had been created in the sketch rather than added to the sketch some of these geometric assumptions would have been added to the geometry as constraints during the creation process.

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Step 6:

Close the part. Choose Undo twice.

(MB3→Undo)

Choose the Finish Sketch icon. Close the part.

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Geometric Constraints A geometric constraint establishes a geometric characteristic of a sketch object (such as defining a line as being horizontal) or the type of relationship between two or more objects (such as requiring that two lines be parallel or perpendicular, or that several arcs have the same radius). Unlike dimensional constraints, geometric constraints have no editable numeric values; a constant angle constraint, for instance, simply dictates that the line stay at the angle it is at when the constraint is applied. To create geometric constraints, choose the Constraints icon, select the objects, and choose the desired constraint from the icon option bar that appears in the upper left corner of the graphics window. Only icons for constraints that apply to the selected geometry will be displayed.

You may also choose the constraint from an MB3 pop-up menu after selecting the geometry.

To assign multiple constraints at one time, press the Ctrl key while selecting the objects. The icon option bar for the constraints will then remain in the upper left corner of the graphics window after you choose the first constraint. You can use MB2 or the Esc key to cancel creation of constraints.

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Types of Geometric Constraints

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Coincident

Constrains two or more points as having the same location.

Collinear

Constrains two or more linear objects as lying on or passing through the same theoretical straight line.

Concentric

Constrains two or more arcs as having the same center.

Constant Angle

Constrains a line so as to remain in its current orientation without input of an angular value.

Constant Length

Constrains a line so as to remain at its current length without input of a length value.

Equal Length

Constrains two or more lines as being the same length.

Equal Radius

Constrains two or more arcs as having the same radius value.

Fixed

Constrains unchangeable characteristics for geometry, depending on the type of geometry selected. You can apply a Fixed constraint to an individual sketch point or to an entire object.

Horizontal

Constrains a line as being parallel to the FCS X-axis.

Midpoint

Constrains the location of a point to be equidistant from both ends of the curve. Select the curve anywhere other than at its end points.

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Parallel

Constrains two or more linear objects as being parallel to each other.

Perpendicular

Constrains two linear objects as being perpendicular to each other.

Point on Curve

Constrains the location of a point as lying on the path or projection of a curve.

Point on String

Constrains the location of a point as lying on an extracted string.

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Scale, Non–Uniform

When applied, a spline will scale in the horizontal direction while keeping the original dimensions in the vertical direction during modification.

Scale, Uniform

A spline will scale proportionally in both the horizontal and vertical when the horizontal length changes.

Slope of Curve

Constrains a spline, selected at a defining point, and another object as being tangent to each other at the selected point.

Tangent

Constrains two objects as being tangent to each other.

Vertical

Constrains a line as being parallel to the FCS Y-axis.

Displaying Constraint Symbols Constraint symbols are displayed when a sketch is active. Symbols for Coincident, Point on Curve, Midpoint, Tangent, and Concentric are always displayed. The Show All Constraints option will display the symbols for all the constraints in the active sketch. The various constraint symbols are shown below: Fixed

Constant Angle

Collinear

Concentric

Horizontal

Tangent

Vertical

Equal Radius

Parallel

Coincident

Perpendicular

Point on Curve

Equal Length

Midpoint of Curve

Constant Length

Point on String

Mirror

Scale, Uniform

Slope of Curve

Scale, Non-Uniform

If the sketch curves are relatively small (the view is zoomed out), the symbols may not be displayed. You may need to zoom in to see them.

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Show/Remove Constraints Show/Remove Constraints helps you manage constraints. The constraints may be listed by object(s) or all of the constraints of the active sketch may be listed at once. 1 — List all constraints or by object(s).

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2 — Filter for the type of constraint to list. 3 — Determines if the filtered constraint types will be included or excluded. 4 — Category of constraints to list. 5 — Actions to take on the listed constraints.

Constraint Interrogation While the Show/Remove dialog is displayed, you can determine what constraints are present by passing the selection ball over a sketch object. If the object has an associated constraint, the object will be pre-highlighted along with any other objects that share the constraint. The constraint symbol will appear next to the sketch objects. If an object which has no constraints associated with it, it will not highlight.

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Constraint Categories There are two major categories of constraints, Explicit and Inferred. Explicit constraints are constraints that you create by assignment using the constraints dialog or by virtue of the creation method. Inferred constraints are Coincident constraints that the system has inferred and created during the curve creation process. You have the option to list only Explicit constraints, only Inferred constraints, or both.

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Constraint Listing The constraints may also be listed in the Show/Remove Constraints dialog by selecting one of the three options at the top of the dialog window. Selected Object

Once an object is selected, the associated constraints, depending on the selected constraint category, are listed in the dialog. To view constraints associated with a different sketch object, simply select the new object.

Selected Objects

Allows the selection of multiple objects; the associated constraints, depending on the selected constraint category, are listed in the dialog. Objects may be deselected by holding the shift key down and selecting the object.

All in Active Sketch

List all the constraints of the active sketch, depending on the selected constraint category.

Listing Box Any time there are constraints listed in the list box they may be browsed by selecting the constraint to highlight it. When the constraint is highlighted in the list box, the sketch object(s) that is associated with it is also highlighted in the graphics window. The Step Up the List and Step Down the List buttons allow easy navigation through the various constraints. The Up and Down arrows on most keyboards will mimic this behavior.

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Information The Information button located on the Show/Remove Constraints dialog will list all of the constraints in the active sketch to the information window. This is useful should there be a need to make a hard copy of the constraints or save them as a text file. Removing Constraints Constraints may be deleted by these methods:

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•

Highlight them in the Show/Remove Constraints dialog List box and select Remove Highlighted Constraint(s), or just double click them in the list.

•

Turn on Select Constraints (on the Selection toolbar), select the constraint symbol on the graphics window, and then choose the Delete icon.

•

Turn on Select Constraints, select the constraint symbol on the graphics window, and then use MB3→Delete to delete selected constraint.

Undo Undo from the Edit pull-down menu, the Undo icon on the Standard toolbar, the MB3 pop-up menu, or the accelerator keys. Undo takes the user actions back one step at a time. After an Undo is performed, the Redo option is available in the Edit pulldown menu or Standard toolbar. Dragging Geometry Under constrained geometry can be dragged only when not in a constraint creation mode. Simply hold down and drag MB1 while on the selected curve(s) or point(s). Selection When in the Sketcher Task Environment, the selection toolbar changes. It has two icons that are only available in the Sketcher. Select Sketch Objects allows selection of curves and dimensions in the sketch. Select Constraints allows selection of constraint symbols in the graphics window.

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Constraint Conditions When either the Dimensions or Constraints option is chosen, the Status line lists the constraint condition for the active sketch. A sketch may be fully constrained, under constrained, or over constrained. When the sketch is under constrained the Status line will indicate the number of constraints needed. Sketch needs 4 constraints Sketch is fully constrained Sketch contains over constrained geometry

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A sketch is evaluated each time a constraint is placed upon the sketch. Each time a sketch is evaluated, the system attempts to solve the set of constraints that describe how the geometric objects are positioned and their relationships with each other. Fully Constrained In order to completely capture the design intent of a particular profile, it may be beneficial to fully constrain the sketch. This occurs when the solver is able to completely define all sketch geometry. There is no requirement to fully constrain a sketch. The design intent has been captured sufficiently when the constraint set applied to the profile causes it to update in the intended manner. Under Constrained A sketch is under constrained when there is insufficient information to completely locate each sketch point. Degree-of-freedom arrows are displayed at each point that can not be solved to identify the direction in which that point remains free to move. Over Constrained A sketch is over constrained when too much constraint information is supplied to the solver. For example, if an Equal Length constraint is applied to two lines and then dimensions are added to each to constrain their length, the sketch would be over constrained. The geometry and dimensional constraints that are causing the over constrained condition are highlighted in a different color to help you identify and resolve the issue. This color is determined by the Overconstrained Curves and Dimensions setting in the Sketch Preferences. An unwanted constraint must be removed before the system will change the geometric configuration. The sketch remains in the last solved condition. ©UGS Corporation, All Rights Reserved

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Conflicting Constraints Dimensional constraints and geometry that are in conflict in the current configuration with the current constraint set are also highlighted in a different color. This indicates that the constraint set that has been supplied is not solvable with the geometry in its current configuration. Constraints may need to be added or removed in order for the sketcher to be able to solve the constraint set. The highlight color is determined by the Conflicting Curves and Dimensions setting in the Sketch Preferences.

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Activity — Adding Constraints In this activity you will add constraints to the angle adjustment bracket to cause the expected update to occur when a dimension is modified. Step 1:

Open angle_adj_3.

Step 2:

Start the Modeling application.

Step 3:

Add the required constraints. Place the cursor over a sketch curve and choose MB3→Edit. Choose MB3→Orient View to Model.

Fit the view.

(MB3→Fit)

Choose the Constraints icon.

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Select the line (1) at the bottom of the sketch.

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in the upper left corner of the graphics Choose Horizontal window. (MB3→Horizontal) This constraint will keep the line from rotating around when dimensions are modified. There are six places where the curvature transitions need to maintain tangency.

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Select the six tangent curve pairs near the six points shown below, two adjacent curves at a time, and apply aTangent constraint to each pair. Be careful to select on the correct half of the arc.

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Lastly, the two arcs at the top of the slot should remain concentric.

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Select the two upper arcs (1) and apply a Concentric constraint.

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The slot should now be constrained such that the angle may be adjusted while the configuration remains as intended.

Choose MB2 to turn the Constraints option off. Step 4:

Edit the dimensions. Double-click on the 45° dimension and change it to 75°. The sketch geometry changes in the expected manner.

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Step 5:

Apply the change to the solid geometry. Choose the Update Model icon.

(Tools→Update Model)

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Choose the Finish Sketch icon. Step 6:

Close the part.

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Activity — Constraining a Profile Constrain the pipe vise sketch to satisfy the stated design intent. Apply constraints to the curves so that the following may be controlled:

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•

The outside envelope of the part.

•

The included angle of the angled lines.

•

The angled lines must remain centered in the part horizontally.

•

The width of the slot at the bottom of the angled lines is controlled by the radius at the bottom of the slot.

Step 1:

Open pipevise_1.

Step 2:

Start the Modeling application.

Step 3:

Activate the sketch. Double-click on a sketch curve.

Step 4:

View the system applied constraints.

Choose the Show/Remove Constraints icon. (Tools→Constraints→Show/Remove Constraints) Choose All In Active Sketch in the List Constraints For: area of the dialog. 13-76

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Verify the Show Constraints option is set to Explicit. The system created constraints are now displayed in the list box. The dialog should look similar to the graphic shown below.

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Choose the first constraint in the list. The object referred to in the list is highlighted in the graphics window. There should be one horizontal line highlighted. Use the UP and DOWN arrow buttons located to the right of the list box to browse through the constraint list. Cancel the Show/Remove Constraints dialog. Step 5:

View the degree of freedom arrows. Turn on the Constraints icon.

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Notice that there are degree of freedom arrows at each of the sketch points. Even though most of the objects in the sketch have constraints associated with them, the sketch points are free to move in all directions. This is because the system cannot locate any of the points relative to model space.

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Step 6:

Constrain the location of a point. Select the lower endpoint of the left vertical line. Select the vertical datum axis.

Choose the Point on Curve icon of the graphics window.

in the upper left corner

The geometry now changes to follow the constraint. The point at the bottom of the left vertical line is now constrained in the horizontal direction.

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Select the horizontal datum axis.

Choose the Point on Curve icon. The geometry now changes to follow the new constraint. The shared sketch point at the bottom of the left vertical line is now constrained in both the horizontal and vertical directions. The degree of freedom arrows go away and, due to the horizontal and vertical constraints on the lines that share the sketch point, one of the arrows on the opposite end of those lines has disappeared.

Choose MB2 to cancel the Constraints mode.

Fit the view. Step 7:

(MB3→Fit)

Move the datum planes and axes to layer 61. The datums have served their purpose of locating the sketch. You will now move them to ease selection of objects and clean up the screen display. Choose Edit→Object Display. Choose the Class Selection icon in the upper left corner of the graphics window. Choose Type.

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Choose Datums and choose OK. Choose Select All and OK. Key in 61 for the Layer in the dialog and press Enter. Step 8:

Continue adding constraints to satisfy the stated design intent.

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Turn on the Constraints icon.

(Insert→Constraints)

Hold the Ctrl key down and select the two horizontal lines (1) at the top of the profile.

Choose Collinear

and Equal Length.

Use the Esc key to deselect all the curves. (Edit→Selection→Deselect All). Select the right side of the arc at the bottom of the slot (1). Select the short right vertical line (2, but not on the end point).

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Choose Tangent. Create another Tangent constraint on the other side of the slot, selecting the left side of the arc and the left vertical line. Hold the Ctrl key down and select the bottom horizontal line and the lower endpoint of the line originating from the arc center.

Choose Point on Curve.

Choose Midpoint. Use the Esc key to deselect all the curves. (Edit→Selection→Deselect All). Select the line (1), shown below, between the midpoint and the arc center.

Choose Vertical.

Adding dimensional constraints to satisfy the controlling portions of the design intent will allow the profile to be changed by modifying the numerical values.

Choose the Inferred Dimensions icon. (Insert→Dimensions→Inferred) Select the bottom horizontal line. Drag the dimension to position it and select with MB1 to place it. ©UGS Corporation, All Rights Reserved

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Key in a value of 5 and press Enter. Notice the curves change color as they become constrained. Fit the view if necessary. Select the left vertical line and place the dimension for it. Change the value to 3.75. Select the top left horizontal line and place the dimension. Change its value to .5.

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Fit the view if necessary. Select the left angled line (1) and the top left horizontal line (2), avoiding the end points. Place the angular dimension and change its value to 45°.

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Select the right angled line and the top right horizontal line, avoiding the end points. Place this angular dimension and change its value to the ’p’ number assigned to the other angular dimension.

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Select the arc at the bottom of the slot. Place the radius dimension and change its value to .25. Select the line connecting the arc center and the midpoint and place this vertical dimension. Change its value to 1.5 and choose Enter. The Status line now informs you that the sketch is fully constrained. Remember that it is not necessarily required to fully constrain the profile if it is updating in the manner desired.

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Step 9:

Change the constraints on the sketch to alter the included angle in the notch. Click on the first angular dimensional constraint that was created and change it from a 45° to 30°.

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Notice that the depth of the notch is unchanged as a result of this edit. Should that have not been our intent, we would have to constrain the sketch in a different manner.

Choose the Finish Sketch icon. Step 10: Close the part.

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Activity — Sketching and Constraining a Gasket In this activity, you will create and constrain a gasket. To efficiently capture the design intent, constraints and dimensions will be added progressively. The center hole is the origin of the gasket. The three holes are located on a horizontal axis. The lines on the outer boundary of the profile are tangent to the arcs.

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Step 1:

Open the seedpart_in part and save it as ***_gasket_1 where *** represents your initials.

Step 2:

Start the Modeling application.

Step 3:

Create the sketch on a Datum CSYS. Change the Work Layer to 21 so that the part will be compliant with class standards.

Choose the Sketch icon.

(Insert→Sketch)

Click on the sketch name; key in s21_profile and press Enter.

Choose Datum CSYS.

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The X-Y plane of the Datum CSYS is highlighted as the default sketch plane.

Choose OK Step 4:

to accept the default plane.

Set the Infer Constraint Settings.

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Choose the Infer Constraint Settings icon. (Tools→Constraints→Infer Constraint Settings) Verify that the following constraints are turned on. Concentric Coincident Dimensional Constraints Choose OK. Step 5:

Create the circles in the center of the gasket. Choose the Circle icon.

Verify that Control Point toolbar.

(Insert→Circle)

is turned on in the Snap Point

Select the existing point at the origin of the Datum CSYS.

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Drag the cursor to preview circle as shown below. Key in a Diameter value of 2 and press Enter.

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The first circle is created. Key in a Diameter value of 3 for the second circle and press Enter. Select the existing point at the origin of the Datum CSYS.

Choose MB2. The two circles are fully constrained because of the dimensional and geometric constraints that were inferred as you created them. ©UGS Corporation, All Rights Reserved

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Step 6:

Create a circle representing the hole on the left side. Choose the Circle icon.

(Insert→Circle)

Click and drag to create a circle near on left side of the graphics window. Key in a Diameter value of 0.5 and press Enter.

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Choose the Constraints icon.

(Insert→Constraints)

Select the arc center of the circle and the horizontal datum axis.

Choose Point on Curve

.

Choose the Inferred Dimensions icon. (Insert→Dimensions→Inferred) Create a perpendicular dimension from the vertical datum axis to the arc center of the left circle. Change the value of the dimension to 2.625.

Step 7:

Create a circle for the outer boundary on the left side. Create another circle in the left side of the graphics window with a diameter of 1.

Choose the Constraints icon.

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Select the two circles on the left side and choose Concentric.

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Step 8:

Create circles representing the hole and outer boundary on the right side. Create two circles on the right side of the graphics window representing the hole and the outer boundary of the gasket. Do not explicitly enter the diameter values. You will constrain them to be equal to existing circles.

Choose the Constraints icon.

(Insert→Constraints)

Select the two new circles on the right and choose Concentric.

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Select the arc center of the circles on the right and the horizontal datum axis and choose Point on Curve. Select the smaller circle on the left and the smaller circle on the right and choose Equal Radius. Select the larger circle on the left and the larger circle on the

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right and choose Equal Radius.

Choose the Inferred Dimensions icon. (Insert→Dimensions→Inferred) Create a horizontal dimension from the arc center of the left circles to the arc center of the right circles. Change the value of the dimension to 5.25.

Step 9:

Set the Infer Constraint Settings before creating the lines. Choose the Infer Constraint Settings icon. (Tools→Constraints→Infer Constraint Settings) Disable all constraints except Point on Curve and Tangent. Choose OK.

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Choose the Line icon.

(Insert→Line)

In the Snap Point toolbar, disable all options except Point on Curve. Create the lines by selecting the circles representing the outer boundary of the gasket. Select the circles by placing the cursor near the expected tangency.

You should see Point on Curve and Tangent constraint symbols on each end of the lines as they are created. The Quick Trim option could be used to trim the circles. However, when extruding the sketch to create a solid body, it is possible to define the correct boundary of the gasket without trimming.

Step 11: Choose the Finish Sketch icon. Step 12: Choose File→Close→Save and Close.

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Convert To/From Reference At times it is useful to add a dimension to a sketch to see the effect of a change numerically. Adding a dimensional constraint, however, would cause the sketch to become over constrained. It also may be necessary to add sketch curves to aid in the construction and constraining of a profile without representing a portion of the swept feature.

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To support these needs, curve and dimensional constraints within a sketch may be converted to and from a Reference status. •

To convert objects, select them in the graphics window and choose Convert To/From Reference from the MB3 pop-up menu.

•

You may access a dialog by choosing the Convert To/From Reference icon from the Sketch Constraints toolbar (Tools→Constraints→Convert To/From Reference).

•

Reference curves are displayed in a phantom line font and are ignored during sweep operations.

•

Reference curves and dimensions are displayed in colors specified by the Reference Curves and Reference Dimensions settings in Preferences→Sketch→Colors.

•

Reference dimensional constraints are displayed with only the value portion of the expression. The values will be updated as the sketch is changed, but they do control the sketch geometry with which they are associated. Dimensions can be made reference as they are created by choosing Create Reference Dimension in the icon option bar.

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Activity — Constraint Conditions In this activity, you will constrain and edit a simple sketch to change the design intent. This configuration is not one that you would likely sketch, but its simplicity illustrates the concept of an over-constrained condition. Apply constraints to control the length and width of the sketch. The shape of the sketch should remain rectangular.

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Step 1:

Open seedpart_in.

Step 2:

Start the Modeling application.

Step 3:

Create a sketch on Layer 21. Change the work layer to 21.

Choose the Sketch icon.

(Insert→Sketch)

Choose Datum CSYS.

Choose Absolute CSYS. Choose OK. The X-Y plane of the Datum CSYS is highlighted as the default sketch plane.

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Step 4:

Set the Infer Constraints Settings. Choose the Infer Constraints Settings icon. (Tools→Constraints→Infer Constraint Settings) Verify that the following constraints are turned on. Horizontal Vertical Parallel Perpendicular Coincident

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Choose OK. Step 5:

Create a rectangle. Choose the Rectangle icon.

Verify that Control Point toolbar.

(Insert→Rectangle)

is turned on in the Snap Point

Select the existing point at the origin of the Datum CSYS.

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Drag the cursor to preview the rectangle and select a cursor location near the upper right corner of the graphics window.

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Step 6:

Interrogate the constraints that currently exist for this sketch. Choose the Show/Remove Constraints icon. (Tools→Constraints→Show/Remove Constraints) Choose All In Active Sketch. Set the Show Constraints to Explicit. Highlight the first constraint in the list and use the down arrow button to browse the constraints. Choose Cancel.

Step 7:

Apply dimensional constraints to control the length and width of the rectangle as per the design intent.

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Choose the Inferred Dimensions icon. (Insert→Dimensions→Inferred) Select the left vertical line and place the dimension. Change the value to 2.75. Select the bottom horizontal line and place the dimension. Change the value to 4.5.

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As dimensional constraints are being created, the degree-of-freedom arrows are eliminated and the curves change to the fully constrained color. The sketch is fully constrained with one vertical and one horizontal dimensional constraint, along with the geometric constraints inferred when the lines were constructed. Design Change — Modify the sketch so that it can be controlled by the angle and length of a diagonal line.

Step 8:

Create a diagonal line in the sketch and convert it to reference. Choose the Line icon.

(Insert→Line)

In the Snap Point toolbar, disable all options except Control Point. Select the lower left endpoint and the upper right endpoint of the rectangle to define the line. Step 9: 13-96

Convert the diagonal line to Reference status.

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Choose MB2 to exit the line creation mode. Select the diagonal line. Choose MB3→Convert To/From Reference. Step 10: Apply an angular dimensional constraint.

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Choose the Inferred Dimensions icon. (Insert→Dimensions→Inferred) Select the lower horizontal line (not the endpoint) and the diagonal line (not the endpoint). Indicate a location for the angular dimension and change the value to 35°. The Status line indicates that sketch is now over constrained. The sketch objects associated with the over constrained condition change to the color specified by the Overconstrained Curves and Dimensions setting in the Sketch Preferences. To correct the over constrained condition, one or more of the offending constraints must by removed. The new design intent is to control the sketch with angular and diagonal length dimensions.

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Step 11: Apply a parallel dimensional constraint. Select the diagonal line and place a parallel dimension. Change the value of the dimension to 6.5.

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Notice that the sketch configuration does not change when the value is modified. The system leaves the geometry in its last solved state until the over constrained condition is resolved. Step 12: Convert sketch dimensions to reference. Choose MB2 to exit the dimension creation mode. Select the horizontal and vertical dimensions. Choose MB3→Convert To/From Reference. The sketch is returned to a fully constrained condition. The reference dimensions reflect the value only. They do not control the geometry to which they are attached. The over constrained condition could also have been resolved by deleting the horizontal and vertical dimensions.

Choose the Finish Sketch icon. Step 13: Close the part.

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Sketching

Summary This lesson introduced the concept of sketch creation. Sketches may be used to define a base feature, guide paths, and additional associative features to the base feature. A sketch parametrically controls curves. It can also be defined on a sketch plane which is associative to a datum plane/face of a model. Both of these benefits allow you to capture and maintain design intent. Constraints are applied to sketch objects in order to capture the design intent. The level of constraint, partial or full, is determined by the design intent and what is necessary to capture it. In this lesson you: •

Created sketches on datum planes, solid faces, and a Datum CSYS.

•

Created freehand curves in a sketch.

•

Created and edited dimensional constraints.

•

Created inferred and explicit geometric constraints.

•

Converted sketch curves and dimensions to reference status.

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Lesson

14 Swept Features and Boolean Operations

Purpose This lesson introduces Swept Features and Boolean Operations.

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Objectives Upon completion of this lesson, you will be able to: •

Create an extruded feature.

•

Create an extruded feature with offsets.

•

Create a feature by sweeping a profile along a guide string.

•

Create a revolved feature.

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Swept Features and Boolean Operations

Types of Swept Features Swept features are created by extruding, revolving, or sweeping a section string. The section string may be composed of explicit curves, sketch curves, solid edges, solid faces, and sheet bodies. An Extruded feature is produced by sweeping the section string (1) in a linear direction for a specified distance.

14

A Revolved feature is produced by rotating a section string (1) around a specified axis (2).

A Sweep Along Guide feature is produced by sweeping a section string (1) along a guide string (2).

The features/bodies that are created will be associated with both the section string and the guide string.

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Extrude The Extrude option (Insert→Design Feature→Extrude) allows a feature to be created by sweeping planar, section string geometry in a linear direction for a specified distance. Extruding a Sketch A sketch can easily be extruded using an object/action approach by placing the cursor over it in the graphics window and choosing the Extrude option in the MB3 pop-up menu. The Start and End extrude distances can then be specified by using the drag handles or by keying in values in the dynamic input boxes. The Start drag handle is represented by a sphere (1) and the End drag handle is represented by a cone (2).

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Swept Features and Boolean Operations

The Extrude dialog is displayed and provides a single user interface to specify Limits, Offset, Draft, and Boolean operation for an extrusion.

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Selecting Sketches Using Selection Intent When you use Extrude, the Selection Intent toolbar is available to establish rules for selecting a section string. You may or may not want to use all of the curves in the sketch as the section string. To select all of the curves in a sketch in one step, set the Curve option in the Selection Intent toolbar to Any or Feature Curves. The other rules can be applied to select a single sketch curve or other collections of sketch curves.

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Extruding a partial sketch is a technique that is used when one sketch may define multiple features.

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Swept Features and Boolean Operations

Rules for Extruding Section String Objects The Body Type option which is found in the Extrude dialog and in Preferences→Modeling, controls whether a solid body or a sheet body is created when extruding section string geometry. When set to "Solid" the following rules will apply: •

Extruding a set of closed planar connected curves creates a solid body.

•

Extruding a set of closed planar connected curves with another closed set within the boundary of the first creates a solid with an interior hole.

•

Extruding a curve or set of planar connected curves which are not closed creates a sheet body unless offsets are used.

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Activity — Starting the Draglink In this activity, you will start to create a model for a draglink by extruding a sketch.

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Step 1:

Open the swept_draglink_1 part and save it as ***_draglink_1 where *** represents your initials.

Step 2:

Start the Modeling application.

Step 3:

Extrude the sketch. Place the cursor over one of the sketch curves and choose MB3→Extrude. The default direction for the extrude is normal to the sketch plane in the +ZC direction. Double-click the direction vector in the graphics window so that it is pointing in the –ZC direction. Key in 152.5 for the End value.

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Choose OK (MB2).

Step 4:

Save the part.

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Swept Features and Boolean Operations

Boolean Operations Boolean operations are used to create a single solid body out of two or more existing solid bodies. If a solid already exists in the part, a Boolean operation can be specified in the Extrude dialog to combine the new feature with the existing solid body instead of creating it as a separate solid body. 1 — Create 2 — Unite 3 — Subtract 4 — Intersect

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Boolean operations may also be created as separate features by choosing the Unite, Subtract, and Intersect options in the Feature Operation toolbar or by choosing Insert→Combine Bodies. When using these operations, you must select a Target solid and at least one Tool solid.

Creating the Boolean operations as separate features allows you to apply additional edits to them such as suppress and unsuppress. Defining Target and Tool Solids The Target solid is the solid body on which the operations are executed. The Tool solid is the solid body that operates upon the target solid. The target solid passes its attributes on to the Boolean operation result. Therefore, the resultant solid inherits the Layer, Material Density, etc. of the target solid.

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Swept Features and Boolean Operations

Unite This option produces one solid body by defining a target solid (1) and tool solid (2).

14 Subtract This option allows material to be removed from a target solid (1) by using another solid as the tool solid (2), leaving empty space where the tool solid existed.

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Intersect This option results in a solid occupying the volume common to the selected target solid (1) and tool solid (2).

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Boolean Errors If you attempt to unite a tool solid within a target solid and there is no change in topology, the following message appears.

If you attempt to unite, subtract, or intersect a tool solid with a target solid and the two solids do not touch, the following message appears.

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If you attempt to subtract a tool solid (1) from a target solid and the operation would produce a zero thickness (2), the following message appears.

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Start and End Limit Options Options are available to control the Start and End Limits of the extrusion by using existing geometry as well as keying in values. Value Symmetric Value

Until Next Until Selected Until Extended Through All

Key in a numeric value or a formula for the limit. If the extrusion is symmetric about the section string, this option can be used so that only one of the limit values has to be entered. Extend the extrusion to the next body along the direction path. Extend the extrusion to a selected face, datum plane, or body. Trim the extrusion to a selected face when the section curves extend beyond its edges. Extend the extrusion completely through all selectable bodies along the path.

These options are also available in an MB3 pop-up menu in the graphics window when you highlight the start or end limit drag handle.

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Swept Features and Boolean Operations

Extrude with Offset This option is used to apply offsets to an extrusion. When this option is turned on, the dialog expands to let you specify Start and End offset values. Drag handles (1) and a dynamic input boxes are displayed with the extrusion preview. The Start offset handle is represented by a sphere and the End offset handle is represented by a cone. Turn the Offset option off to remove the offset and handles from the preview.

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Offset Examples The values of the Start Offset and End Offset may be positive or negative. The positive direction is determined by the direction of the End Offset drag handle (cone). Start Offset Zero End Offset Positive

Start Offset Zero End Offset Negative

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Start Offset Negative End Offset Positive

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Extrude with Draft When this option is turned on, the dialog is expanded to let you specify a draft angle. A drag handle (1) and a dynamic input field are displayed with the extrusion preview. Turn the option off to remove the draft and drag handle from the preview.

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Rules for Extruding with Draft

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•

A positive taper angle creates an inward taper (A).

•

A negative angle creates an outward taper (B).

•

If the section string included interior holes, the holes would be tapered in the opposite direction to the outside objects.

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Activity — Extruding with Offsets In this activity, extruded features will be added to a part using offset values.

14 Step 1:

Open the swept_extrude_1 part.

Step 2:

Start the Modeling application.

Step 3:

Create a tube by extruding with an offset. Choose the Extrude icon. (Insert→Design Feature→Extrude) Select the inside, large circle as the section string.

Change the Boolean option to Unite. Confirm a value of 0 for the Start (Limit), key in 2.5 for the End (Limit) value, and press Enter.

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Turn the Offset option on. Key in –.25 for the End (Offset) value and press Enter. If the Offset drag handle is pointing away from the center of the part, use a negative value for the End offset. If the Offset drag handle is pointing toward the center of the part, use a positive value. Choose Apply (Ctrl-MB2). Fit the view. (MB3→Fit). The circle is extruded from its origin normal to its creation plane a distance of 2.5 units. The feature is .25 units thick measured inside the circle. The thickness was defined by the End offset value based on the direction of the offset drag handle.

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Step 4:

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Create a flange at the top of the cylinder.

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Verify the Curve option is set to Single Curve in the Selection Intent toolbar.. Select the top outer edge of the cylindrical extrusion.

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Change the Boolean option to Unite. Make sure the drag handle is pointing down. If it is pointing up, choose Reverse Direction

in the dialog.

Key in .25 for the End (Limit) value and press Enter. Turn the Offset option on. Key in .25 for the End (Offset) value and press Enter. If the Offset drag handle is pointing away from the center of the part, use a positive value for the End offset. If the Offset drag handle is pointing toward the center of the part, use a negative value.

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Choose Apply (Ctrl-MB2).

14 The selected edge is extruded from its origin, normal to its creation plane to a distance .25 units. The feature is defined as being .25 units thick measured outside the edge. The thickness was defined by the values entered in the End Offset fields relative to direction of the offset drag handle.

Step 5:

Subtract an extrusion from the flange. Select the inside circular edge shown to extrude.

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Change the Boolean option to Subtract. Make sure the direction vector is pointing down. If it is pointing up, double-click the vector in the graphics window or choose Reverse Direction

in the dialog.

Key in .075 for the End (Limit) value and press Enter. Turn the Offset option on. Key in .15 for the Start (Offset) value and .275 for the End (Offset) value and press Enter. If the Offset drag handle is pointing away from the center of the part, use positive values for the offsets. If the Offset drag handle is pointing toward the center of the part, use negative values. Choose OK.

Step 6:

Close the part.

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Swept Features and Boolean Operations

Selection Intent The Selection Intent toolbar is available to specify curve and edge selection rules for section strings when creating extruded features. These rules can be applied to automatically select a collection of curves or edges in a single step instead of selecting them individually. Curve Options When a feature requires the selection of a profile or individual curves and edges, the Curve options become available for collecting and section building. The pull-down menu displays the curve or edge selection rules that are applicable to the feature you are creating. The cursor changes to a Curve Collecting mode, indicating you can collect curves or edges. Choose the rule from the pull-down menu that best describes the action for the design intent of your feature.

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Any — Lets you use the original default intent method to extend a selection. The default method can vary based on the type of object you selected. For example, with Extrude the default could be All Curves of Feature if a curve is selected, and Single if the selected object is an edge. The Any method lets the controlling feature derive intent based on the type of object selected. Single Curve — Lets you single-select one or more curves or edges. No rule is applied to a collection of singly-selected curves, and it is basically a simple list of objects without intent. You can enhance a collection of singly-selected curves or edges by moving MB3 over one of the selected objects and then choosing another rule. Connected Curves — Lets you select a chain of curves or edges that share endpoints. No rule is applied if the chained curves are non-associative. The curve intent does not attempt to grow or shrink the chain if curves are added or no longer form a single chain after an edit to the model. 14-22

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Tangent Curves — Lets you select a tangent continuous chain of curves or edges. No rule is applied if the chained curves are non-associative. The curve intent does not attempt to grow or shrink the chain if curves are added or no longer form a single chain after an edit to the model. The system does not discard non-associative curves that are no longer tangent after an edit. Face Edges — Collects all edges of the face containing the edge you select. If you already selected an edge using another rule, you can select an adjoining face to define a collection with the Add All of Face rule. When you select an edge, the cursor-center location determines which face is selected. Sheet Edges — Collects all laminar edges of the sheet body you select. Feature Curves — Collects all output curves from curve features, such as sketches or any other curve features.

Stop at Intersection Select this option to specify that auto chaining stops not only at endpoints of the curve or edge but also on intersections with other curves or edges. When you select a chain, all other curves and edges visible in the selection view are checked for intersections with the current chain. At each of the intersection points (that is, where two or more objects meet at a point, either interior or at an end point) the system bounds the chain.

Follow Fillet You can use this option to automatically chain a section onto and off of a tangent arc. This option is available only when you are building a section, and only for Connected Curves and Tangent Curves chaining intents. If you select both Follow Fillet and Stop At Intersections, Follow Fillet overrides Stop At Intersections at branches where it applies

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Swept Features and Boolean Operations

More Selection Intent Options This option displays a dialog with other special conditions for the selected rule.

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Chain Between — Select this option to determine the number of objects you must select for chaining. When you clear this option, chaining is a single selection operation and you select a seed object and all objects that meet the current constraints (that is, the Chain or Chain Tangent options) are collected. When you select this option, chaining is a two selection operation and you must select the start and end of the chain before the chain is collected. This option is mutually exclusive of the Stop at Intersection option. If you select one, the other is cleared. Tangent Angle (Degrees) — Use this option to enter a real number for the highest possible value you want to specify as tangent degrees.

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Activity — Extruding Using Selection Intent In this activity, you will use Selection Intent options to extrude a sketch.

Step 1:

Open the swept_gasket_1 part. The part contains a sketch of a gasket profile. The circles defining the outer boundary of the profile were not trimmed.

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Step 2:

Start the Modeling application.

Step 3:

Extrude the sketch. Choose the Extrude icon. Feature→Extrude)

(Insert→Design

Turn the Enable Preview option off. Set the Curve option to Tangent Curves in the Selection Intent toolbar.

Turn on the Follow Fillet icon toolbar.

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in the Selection Intent

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Swept Features and Boolean Operations

Select one of the curves in the outer boundary of the gasket. The outer boundary of the gasket is highlighted.

Select the three interior circles that define the holes.

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Change the work view to the Trimetric orientation. (MB3→Orient View→Trimetric). Turn the Enable Preview option on. Key in the following values for the extrusion: Start (Limit)

=

0

End (Limit)

=

.125

Choose OK. (MB2)

Step 4:

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Close the part.

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Sweep Along Guide The Sweep along Guide option (Insert→Sweep→Sweep along Guide) allows a feature to be created by sweeping a section string along a guide string. Rules for Sweeping Section String Objects Along a Guide •

Solid or sheet bodies are created based on the current Modeling Preferences Body Type setting and the closure condition of the curves (i.e. open string or closed string). Open String

Closed String

14 •

An open section string swept along a guide path that forms an enclosed loop will automatically cap the end faces, providing the Modeling Preferences Body Type is set to Solid.

•

Open section strings will always be swept into a solid body when using the sweep with offset option.

•

Only one Section String and only one Guide String may be selected.

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Swept Features and Boolean Operations

Guide Strings Containing Sharp Corners When using Sweep along Guide where the guide string contains sharp corners, it is recommended that the section string be placed away from a sharp corner. The section string also needs to be located on an end point of one of the guide string objects. 1 — Guide String. 2 — Section String that is at sharp corner, a location that should be avoided. 3 — Section String that is located away from a sharp corner and located on an end point. 4 — Two separate line objects that provide the endpoint for the section string.

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Activity — Sweeping Along an Open Guide String In this activity you will continue to develop the draglink part by sweeping a section string along a guide.

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Step 1:

Make ***_draglink_1 the work part.

Step 2:

Start the Modeling application.

Step 3:

Create the swept feature. Make layer 22 the work layer and all other layers invisible. Make layer 23 selectable.

Choose the Sweep along Guide icon. (Insert→Sweep→Sweep along Guide) Set the Curve option to Feature Curves in the Selection Intent toolbar. ©UGS Corporation, All Rights Reserved

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Select one of the I-beam sketch curves as the section string (1). The I-beam is a sketch feature so all of the curves in the I-beam are selected except the reference line.

14 Choose OK. (MB2) Verify that the Curve option to Feature Curves in the Selection Intent toolbar. Select one of the curves from the sketch on layer 23 as the guide string (2).

Choose OK. (MB2) Verify that the First Offset and Second Offset are both set to 0 (zero). Choose OK. (MB2) 14-30

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Choose Create.

14 Cancel the Sweep along Guide dialog. Step 4:

Unite the new swept solid with the existing solid. Make layer 1 the work layer. Fit the view. (MB3→Fit)

Choose the Unite icon.

(Insert→Combine Bodies→Unite)

Select the first solid body created as the target body. Select the swept I-beam body as the tool body.

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Choose OK. (MB2)

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Step 5:

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Save the part.

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Activity — Sweeping Along a Closed Guide String In this activity, you will sweep an open section string along a closed guide string to create a solid body.

14 Step 1:

Open the swept_guide_1 part.

Step 2:

Start the Modeling application.

Step 3:

Create the swept feature.

Choose the Sweep along Guide icon. (Insert→Sweep→Sweep along Guide) Verify the Curve option is set to Feature Curves in the Selection Intent toolbar. Select the sketch of the open profile (1) as the section string.

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Select the sketch of the closed profile (2) as the guide string.

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Choose OK. (MB2) Choose OK to accept the direction. (MB2) Verify that the First Offset and Second Offset are set to 0 (zero). Choose OK. (MB2) The open section string was swept along the full length of the guide string and the system automatically caps the open ends to produce a solid body.

The Sweep along Guide function may be used to sweep any section string along a guide string.

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Step 4:

Optional Challenge — Undo the creation of the solid and create it again specifying a .25 single offset toward the outside of the curves. The part should resemble the figure shown below.

14 Step 5:

Close the part.

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Swept Features and Boolean Operations

Revolve The Revolve option (Insert→Design Feature→Revolve) allows you to create a feature by rotating a section string about an axis through specified angles. The Revolve feature requires a section (1), a location and direction for the rotation axis (2), and Start and End angles (3,4). The angles can be specified by using drag handles, keying in values in the dynamic input boxes, or in a dialog.

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You can also revolve a sketch by placing the cursor over it in the graphics window and choosing the Revolve option in the MB3 pop-up menu.

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The Revolve dialog is displayed and provides a single user interface to specify Angular Limits, Offset, and a Boolean operation.

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Rules for Revolving Section String Objects •

As with extruded sections, a solid or sheet body is created based on the closure condition of the curves and Body Type setting. The Body Type setting is found under Preferences→Modeling but can also be set in the Revolve dialog (after choosing the More Options icon).

•

When revolving an open section string a full 360°, the end faces will be automatically capped to produce a solid body if the Body Type option is set to Solid.

•

The Right Hand rule determines the direction of the sweep. You can reverse the direction by double-clicking on the axis vector in the graphics window or by choosing the Reverse Direction icon in the dialog.

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Swept Features and Boolean Operations

Activity — Creating Revolved Features In this activity, you will create revolved features. Step 1:

Open the swept_revolve_1 part. The part contains a sketch to be used as the section string and a datum axis to be used as the axis of revolution.

Step 2:

Start the Modeling application.

Step 3:

Revolve an open section string. Place the cursor over the sketch and choose MB3→Revolve.

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Key in the following values for the Angular Limits: Start

= 0

End

= 360

Choose MB2. Select the Datum Axis in the graphics window. Choose OK (MB2). A solid revolved body is created from the open section string. If you wanted to create a solid body with a sweep of less than 360°, the section string must be closed or offsets must be specified.

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Step 4:

Revolve an open section string with an offset. Now, you will use the same section string to create a new revolved body using an offset to form a shell. Choose Undo. (MB3→Undo or Ctrl-Z) Place the cursor over the sketch again and choose MB3→Revolve. Turn the Offset option on in the Revolve dialog. Key in the following values: Start (Limit)

=

0

End (Limit)

=

180

Start (Offset)

=

0

End (Offset)

=

.25

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Choose MB2. Select the Datum Axis in the graphics window. Choose OK. (MB2)

Notice that the revolution starts at the plane of the curves and revolves in a counterclockwise direction with respect to the positive axis of rotation (the Datum Axis). The Right Hand Rule for Positive Rotation applies. Step 5:

Revolve a solid face. Now, you will close one end of the solid by revolving the edges of an existing face.

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Choose the Revolve icon. (Insert→Design Feature→Revolve) Set the Curve option to Face Edges in the Selection Intent toolbar. Select the solid face (1) as shown.

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Key in the following values: Start Angle

=

0

End Angle

=

–90

Choose MB2. Select the short edge, as shown below, as the inferred rotation axis vector.

Choose OK. (MB2) Step 6: 14-40

Unite the new revolved solid body with the existing solid body.

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Choose the Unite icon.

(Insert→Combine Bodies→Unite)

Select the target (1) and tool solid (2) as shown below.

14 Choose OK. (MB2) Step 7:

Optional Challenge — This shell is one of two molded parts that must fit together. Add a lip to the outside edge of the part by extending the outside edges of the top planar face with an offset value and height value equal to half the shell thickness.

Step 8:

Close the part and do not save.

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Activity — Adding a Revolved Feature to the Draglink In this activity you will continue to develop the draglink part by adding a revolved feature. Step 1:

Make ***_draglink_1 the work part.

Step 2:

Start the Modeling application.

Step 3:

Revolve a section string (1) to create a feature (2).

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Make layer 24 selectable to view the section string (1) and make all other layers invisible. Layer 1 will remain the work layer.

Choose the Revolve icon. (Insert→Design Feature→Revolve) 14-42

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Verify the Curve option is set to either Any or Feature Curves in the Selection Intent toolbar. Select the sketch (1) shown below as the section string.

14 Choose MB2. Select the vertical line shown (2) to define the vector for the axis of revolution.

Key in the following values: Start Angle

=

0

End Angle

=

360

Choose OK. (MB2)

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Swept Features and Boolean Operations

Step 4:

Unite the new revolved solid body with the existing solid body. Choose the Unite icon.

(Insert→Combine Bodies→Unite)

Select the existing solid body as the target body. Select the new revolved solid body as the tool body. Choose OK. (MB2) Step 5:

Save the part.

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Activity — Extruding to a Face In this activity you will complete the development of the draglink part. Step 1:

Make sure ***_draglink_1 is the work part.

14 Step 2:

Extrude a section string to a face. Make layer 25 selectable and all other layers invisible. Layer 1 should still be the work layer. The section string geometry (1) is now visible.

Choose the Extrude icon. (Insert→Design Feature→Extrude) Verify the Curve option is set to Any or Feature Curves in the Selection Intent toolbar.

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Select the sketch (1) as the section string.

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Change the Boolean option to Subtract.

Choose Reverse Direction down into the existing solid.

so that the drag handle points

Verify the Start (Limit) value is set to 0. Change the End (Limit) option to Until Next.

The length of the extrusion is determined by the first face it intersects which is the bottom face of the part.

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Choose OK. (MB2)

14 Step 3:

Save and close the part.

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Swept Features and Boolean Operations

Summary Swept features are created by extruding, revolving, or sweeping a section string. The section string may be composed of sketch curves, explicit curves, solid edges, solid faces, and sheet bodies. Boolean operations are used to create a single solid body out of two or more existing solid bodies. In this lesson you:

14

14-48

•

Created extruded features.

•

Created an extruded feature with offsets.

•

Created a feature by sweeping a section string along a guide.

•

Created a revolved feature.

•

Applied boolean operations.

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Lesson

15 Editing the Model Purpose To modify solid body features by editing their defining criteria. Objectives In this lesson, you will: •

Edit feature parameters and positioning dimensions.

•

Delete features.

•

Reorder features in the Model History.

•

Reattach a feature to a different face.

•

Move features.

•

Rename a feature.

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Practical Applications of NX

15-1

Editing the Model

Accessing the Options to Edit Features There are several different ways to access options to edit features in NX.

15

15-2

•

Part Navigator — Many feature editing options are available in the Part Navigator. You may also use it to review the Model History and feature dependencies.

•

Feature MB3 Pop-up Menu — Some common feature editing options are available in the MB3 pop-up menu when you select a feature in the graphics window. The options available in this menu will depend on the type of feature and the method used to create it.

•

Edit Pull-Down Menu — Choosing Edit→Feature from the menu bar provides many options related to editing features. If you choose an editing options from this menu without first selecting a feature, a dialog will be displayed so that you can select features from a list.

•

Edit Feature Toolbar — Many of the options in the Edit→Feature pull-down menu are also available in the Edit Feature toolbar. This toolbar can be turned on and customized to display the icons of frequently used editing options.

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Editing the Model

Part Navigator The Part Navigator allows various actions to be performed on features. Holding down MB3 on a feature node in the Part Navigator displays a feature specific pop-up menu offering pertinent editing options. To access the Part Navigator, choose the icon on the resource bar on the right side of the NX window.

15

The options available in the pop-up menu will vary depending on the type of feature selected. Many of the options are not available if the Modeling application is not active.

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Editing the Model

Display Dimensions Choosing Display Dimensions causes the feature’s parameter values to be displayed (just as they are with Edit Parameters). The temporary display remains until a Refresh is performed. Show/Hide Allows the body or parents for the selected feature to be hidden or displayed. This function blanks/unblanks the object(s) and their display can be brought back by using the Show/Hide options or the options under Edit→Blank. The Hide Body option "blanks" the solid body that the feature is applied to. The Hide Parents option is more applicable to swept features. If the Hide Parents option is used on a swept feature, the system will hide (blank) the parent curves which generated the swept feature. If the swept feature is derived by a solid edge(s) then the Hide Parents option will hide (blank) the parent solid body. This option is not effective in showing or hiding "resulting curves," which are produced directly from a curve feature operation, such as with Offset Curve.

15

Make Current Feature Provides a quick and easy method for inserting features into a part. This option may be used to make an existing feature the current feature of the solid body, and then add more features at that point in the model history. If this option is used on a feature whose time stamp positions it in the middle of the model history, making it the current feature, all of the features after it become inactive. As new features are created they are inserted into the build hierarchy before the inactive features. Filter Lets you apply a system filter to the Part Navigator display tree based on the features currently selected. These filters let you simplify the display tree by hiding features by type or timestamp order. To turn off a filter, place the cursor in the Part Navigator away from a feature node, click MB3, and turn off the Apply Filter option in the pop-up menu. Edit Parameters Lets you edit the feature’s parameters (same as Edit→Feature→Parameters).

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Editing the Model

Edit with Rollback This option first rolls the model back to its state just prior to the feature being created, before reopening the feature’s creation dialog to edit parameters. This is shown in bold in the pop-up menu which indicates it is the default action when you double-click on a feature name in the Part Navigator. Edit Positioning Lets you edit the feature’s positioning dimensions (same as Edit→Feature→Edit Positioning) Suppress and Unsuppress Suppress temporarily removes the feature from the body and display. This can also be accomplished by clearing the checkbox associated with the feature node in the Part Navigator. The option changes to Unsuppress while a feature is suppressed. Unsuppress returns the suppressed feature back to the body and the display. Reorder Before/After

15

Allows the construction order of the features in the model to be altered by positioning the selected feature before or after other features in the build hierarchy. Choose the feature that the selected node is to be reordered relative to from the Reorder Before or Reorder After cascade menus. Nodes may also be dragged and dropped in the Part Navigator window to perform a feature reorder. Multiple features may be selected by holding the Ctrl key down during selection. Group Same as Format→Group Features. This option lets you group features into a special collection called a Feature Set. Members of a Feature Set can be controlled together during suppress, delete and move feature operations. Choosing Group causes the Sets of Features dialog to appear. The features included in the Feature Set can also be hidden so they do not show in the Part Navigator and can only be accessed under the Feature Set Name. If you delete a Feature Set, all of its member features are also deleted. To delete a Feature Set without deleting its members, first remove the members from the set. Replace This allows a feature’s definition to be replaced or "redefined" by another feature. For example, a surface that is used as a trim face could be replaced for a different surface without having to delete or redefine several other features. For more information on replace see the technical documentation. ©UGS Corporation, All Rights Reserved

Practical Applications of NX

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Editing the Model

Rename This option allows you to append a user-defined name to the feature. The user defined name will appear in addition to the system defined name in the Part Navigator (i.e. Simple Hole(6) “Alignment Hole”). Delete Deletes the selected feature (same as Edit→Delete). Object Dependency Browser The Object Dependency Browser allows the parent and child relationships of a feature to be interrogated. Information Provides information about the selected feature in the Information window. Properties

15

This option provides access to General and Attribute information for the feature selected. General properties include the feature name, which can be edited similarly to the Rename function. Attributes can be added to any feature to include information which could be called out in a specified column of the Part Navigator. For more information on feature attributes and Part Navigator columns see the technical documentation.

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Editing the Model

Deleting Features You can delete features by selecting the feature and choosing Delete from the MB3 pop-up menu. The feature can be selected in the graphics window or Part Navigator. If you choose the Delete icon from the Standard toolbar (or Edit→Delete), an icon options bar is displayed in upper left corner of the graphics window. Choosing the Features icon allows you to select features to delete

•

When a feature is deleted from a body, the space it occupied or voided is filled in exactly as it was before the feature was created.

•

If a feature is mistakenly deleted, Undo (Edit→Undo List or Ctrl-Z) may be used immediately after the deletion to restore the feature.

•

Any features whose placement, not position, is dependent on the deleted feature will also be deleted. For example, if a hole was created using a datum plane for its placement face, and the datum plane is deleted, the hole will also be deleted. A Notification dialog will be displayed to warn you that other features will be affected. Choosing the Information button will list the dependent features.

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15-7

15

Editing the Model

Update Failures When an edit is made to a feature, the model is updated (or rebuilt) to incorporate this change. Sometimes the edit may cause a failure in a feature that occurs later in the model history. The Edit During Update dialog will appear if an update failure occurs and allow you to resolve the problem. In the example below, an edit was made to a Shell feature that results in the removal of an edge that is later blended. After the edit is made, the blend fails during the model update and the Edit During Update dialog appears.

15

The options that allow you to advance forward through the model history (Step, Step To, and Continue) are disabled until the failure is resolved and the feature successfully updates. You may delete, suppress, or edit the current feature or step back and edit an earlier feature.

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Editing the Model

Additional Edit During Update Options Some of the options in the Edit During Update dialog apply specifically to update failures. Accept — used to acknowledge a single warning message about a failed feature (but not an error message) to allow the update to continue. The feature that fails is marked "out of date" in the Part Navigator.

The status of features may also be viewed by choosing Information→Feature. The features that are “out of date” are listed with a (!) in the Feature Browser.

Accept Remaining — acknowledges the update failures of the current feature as well as all subsequent features so that each warning message does not have to be accepted individually. Show Failure Area — temporarily displays failed geometry. This option is available only if an object involved in the failure, such as a tool body, is available for display. ©UGS Corporation, All Rights Reserved

Practical Applications of NX

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Editing the Model

Show Current Model — displays the part of the model that has been successfully rebuilt. For performance reasons, the display does not change during update when an update method other than Show Current Model is used. After the model update has finished, the display is updated. Post Recovery Update Status — specifies what should happen after an edit is made during an update failure. •

Continue — restarts the automatic update process from where it left off.

•

Pause — stops at the next feature after an edit is made and lets you choose other Edit during Update options, rather than automatically resuming the update.

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Editing the Model

Activity — Edit and Delete Features In this activity, you will edit the parameters of a feature, capture design intent by associating a positioning dimension to another feature, and delete a feature. Step 1:

Open the edit_feature_1 part.

Step 2:

Start the Modeling application.

Step 3:

Review the model. Choose the Part Navigator icon

15

from the resource bar.

Choose the push pin icon in the upper right corner to permanently display the Part Navigator. Select some of the features in the Part Navigator and view what highlights in the graphics window. Step 4:

Edit the width of the part. Double-click the Extrude(4) feature in the Part Navigator. (Edit→Feature→Edit with Rollback) The model “rolls back” to the state it was in when the Extrude feature was created. The Extrude dialog is also displayed. Change the End value to 2.75.

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15-11

Editing the Model

Choose OK. (MB2) After the update, the pad on the bottom is no longer centered. The design intent is that the pad should always remain in the center of the part. This situation will be remedied in the next step.

Step 5:

Edit a positioning dimension of the pad by selecting it in the graphics window.

15

In the graphics window, place the cursor over the rectangular pad shown in the above figure (Rectangular Pad(7)) and choose MB3→Edit Positioning.

Choose Edit Dimension Value. In the graphics window, select the p29=1.560 expression. To see the pad feature and expressions better, the view may need to be rotated. Since the pad should always stay in the center of the part, keying in a simple equation will capture this aspect of the design intent. Key in p11/2. The expression p11 is the End value of the Extrude feature and controls the width of the part. Choose MB2 three times. 15-12

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Editing the Model

Step 6:

Edit the width of the part. In the graphics window, place the cursor over the Extrude feature at the location as shown below. Place the cursor over the Extrude feature at the location as shown below and choose MB3→Edit Parameters.

If you have difficulty selecting the feature, wait until the QuickPick indicator appears, click MB1 and select Extrude(4) in the QuickPick dialog. Change the End value to 5.00 and choose OK. (MB2)

Fit the view.

(MB3→Fit)

The pad feature remains in the center of the block. Step 7:

Delete a feature.

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15-13

15

Editing the Model

Place the cursor over the T Slot feature and choose MB3→Delete.

A Notification dialog appears informing you that other features will be affected. Choose Information from the dialog to list the other features that will be deleted.

15

The three holes will be deleted because faces of the slot were used as their placement face or thru face. Close the Information window. Choose OK. The T Slot and the dependent hole features are removed.

Step 8:

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Close the part.

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Editing the Model

Activity — Using the Update Tool In this activity, you will make an edit to a feature which causes an update failure. You will resolve the problem using the Edit during Update dialog. Step 1:

Open the edit_feature_2 part.

15 Step 2:

Start the Modeling application.

Step 3:

Edit the width of the part. Double-click the Extrude(4) feature in the Part Navigator. (Edit→Feature→Edit with Rollback) Change the End value to 1.75.

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15-15

Editing the Model

Choose OK (MB2). The Edit during Update dialog appears.

15

The feature that has caused the failure to occur is shown in the graphics window. Choose Show Current Model. The model appears in the graphics window relative to the new 1.75 width value.

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Editing the Model

Choose Show Failure Area. The reason for the failure is now evident. The hole is positioned outside the solid body.

Choose Edit

in the Edit During Update dialog.

15

Choose Edit Position. Choose Edit Dimension Value. Select the p63=2.125 dimension from the graphics window. Key in p11-.5 and choose OK (MB2) four times. The hole is now located within the solid model and resolves the problem. The update completes successfully.

Step 4:

Close the part.

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15-17

Editing the Model

Activity — Reordering Features with the Part Navigator In this activity, you will reorder features to see how this impacts the design of the part. Step 1:

Open the edit_reorder_1 part.

Step 2:

Start the Modeling application.

Step 3:

Review the model.

15

Choose the Part Navigator icon

from the resource bar.

Choose the push pin icon in the upper right corner to permanently display the Part Navigator. Select some of the features in the Part Navigator and view what highlights in the graphics window. Step 4:

15-18

Reorder the Shell feature.

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Editing the Model

Place the cursor over Shell(3) feature in the Part Navigator, press and hold down MB1, drag the feature just below Unite(5). The hollow feature is reordered after the other extruded feature is united.

15 Press and hold down MB1 on Shell(5) and drag the feature just below Blend(6). Notice the sharp corners on the inside of the part.

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15-19

Editing the Model

Press and hold down MB1 on Shell(6) and drag the feature just below Blend(7). Now there is a radius on the inside edges.

15 Step 5:

Rename a Feature. Select the Blend(5) feature in the Part Navigator and choose MB3→Rename. Key in Throat Blend and press Enter. The new name is appended to the system-defined name in the Part Navigator. This can make the feature easier to identify when reordering or reviewing the model.

Step 6:

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Close the part.

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Editing the Model

Delaying Model Updates Delayed Update After Edit As more features are added to a model, the model will take longer to update. If you are making several minor edits to a complex model with many features, it may be beneficial to control when the model is updated. Instead of waiting for the model to update after each edit, you can delay the updates until after all edits are specified. To delay model updates, choose Tools→Update→Delayed after Edit. If this is an option that will be used often, you can add the Delayed Update after Edit icon to the Edit Feature toolbar. •

If Delayed Update after Edit is off, the part is updated after the completion of each edit operation. This is the default setting.

•

If Delayed Update after Edit is on, feature updates are delayed while edits are made. For example, the positioning dimension of a feature may be changed followed by an edit to the parameters of another feature without updating the model.

This option may not be used to delay a Delete, Suppress, or Unsuppress feature operation.

Update Model Once Delayed Update after Edit is enabled and edits are made, the Update Model option becomes available so that you can update the model when it is convenient. This option is accessed by choosing Tools→Update→Update Model. If this is an option that will be used often you can add the Update icon to the Edit Feature toolbar. The model will be updated automatically when the part is saved.

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15-21

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Editing the Model

Move Feature The Move Feature option (Edit→Feature→Move) allows you to move a feature that is not associatively positioned to a new location. •

This option excludes all swept features, relative datum features, and instance arrays as well as features whose location has been constrained using positioning dimensions.

•

Features whose position is determined by associative positioning dimensions must be moved by editing the positioning dimensions.

•

Move Feature can be used to move a primitive that is used as the base feature for the model.

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DXC, DYC, DZC

Moves the feature by specifying a rectangular coordinates, based upon the Work Coordinate System. (Delta XC, Delta YC, and Delta ZC)

To a Point

Moves the feature from a reference point to a destination point. The Point Constructor will become available during the operation to assist in the move.

Rotate Between Two Axes

Rotate the feature from a reference axis orientation to a destination axis orientation about a specified pivot point.

CSYS to CSYS

Repositions the feature from a Reference Coordinate System to a Destination Coordinate System. The coordinate systems are defined by using the CSYS Constructor.

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Editing the Model

Reattaching a Feature One of the options available for editing under Edit Parameters is Reattach. Reattach allows the feature references of the feature to be redefined. A feature reference may be an attachment face, a thru face, a target edge for positioning, etc. Objects that may have their references redefined include most form features (holes, pockets, grooves, pads, slots, and bosses), and linear instance sets of these features, trim faces of extruded and revolved features, and user-defined features (UDFs). In the example below, a pad feature and associated holes are reattached from the original placement face to a new face.

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15-23

Editing the Model

Using the Reattach Dialog The Reattach dialog only enables the options that pertain to the selected feature. For example, a feature must include a thru face for the Specify Thru Face option to be enabled and must include one or more positioning dimensions for the Redefine Positioning Dimensions option to be enabled. When an option is chosen, the existing references of the type in question are highlighted. For example, if a thru slot is selected and the Specify First Thru Face icon is chosen, the current thru face for the slot is highlighted. 1 — Current positioning dimensions 2 — Reference direction type 3 — Change reference direction 4 — Change the normal direction 5 — Specify location of feature

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Editing the Model

Reattach Options The following options are available to redefine feature references:

Specify Target Placement Face — allows a new attachment face for the feature being edited to be specified.

Specify Reference Direction — allows a new horizontal reference to be specified for the feature being edited.

Redefine Positioning Dimensions — allows new positioning dimensions to be specified for the feature being edited.

Specify First Thru Face — allows the first through/trim face of the feature being edited to be redefined.

15 Specify Second Thru face — allows the second through/trim face of the feature being edited to be redefined.

Specify Tool Placement Face — allows the tool face of a User Defined Feature (UDF) to be redefined. In addition, while using any of these redefine feature references options, the following options on the Reattach dialog are available: Filter — allows filtering of selectable object types including faces, datum planes, edges, and datum axes. The default is All Types. The list of filter options available is dependent on the specific Reattach option icon chosen. Positioning Dimensions — A list window displays the types of positioning dimensions currently on the selected feature. If MB1 is used to select a dimension in this list, its available references are highlighted in the graphics window. Double-clicking with MB1 on a dimension in the list allows it to be redefined. Direction Reference — allows the definition of a new Horizontal or Vertical feature reference. The default is always set for the existing reference type. Reverse Direction — allows the feature’s reference direction to be reversed. Reverse Side — allows the feature’s normal direction to be reversed when reattaching that feature to a datum plane. ©UGS Corporation, All Rights Reserved

Practical Applications of NX

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Editing the Model

Specify Origin — allows quick relocation of the reattached feature by moving it to a specified origin. This option is useful when reattaching features to datum planes. Since features are initially placed at the center of a plane, the update may fail since the plane’s center may not be near the feature’s actual position. This option may be used with all features. Delete Positioning Dimension — allows deletion of a selected positioning dimension. If a feature does not have any positioning dimensions, this option is grayed out.

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Editing the Model

Activity — Reattaching and Moving Features In this activity, you will reattach a feature to a new placement face. You will also move fixed datum features to change the orientation of an associated body.

15 Step 1:

Open the edit_reattach_1 part.

Step 2:

Start the Modeling application.

Step 3:

Reattach the pad feature. In the graphics window, place the cursor over the pad (Status line should read Rectangular Pad(6)) and choose MB3→Edit Parameters. Choose Reattach in the Edit Parameters dialog. The Reattach dialog displays icons for the selection steps and other options for reattaching the feature. The icon for Specify Target Placement Face is active. The current placement face for the Rectangular Pad feature is highlighted in the graphics window and the Cue line prompts you to select a new target face.

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Editing the Model

Select the right face of the solid (1). The second icon, Specify Reference Direction, is active. The current horizontal reference is highlighted in the graphics window and the Cue line prompts you to select a new Horizontal Reference. Select the lower edge of the face (2) as the horizontal reference.

15 The third icon, Redefine Positioning Dimensions, is active and the Cue line prompts you to select a Dimension to Redefine. Select the vertical positioning dimension from the graphics window (20.0). Select the lower front edge (1) of the solid as the target object. Select the bottom outside edge of the pad (2) feature as the tool edge.

Select the horizontal positioning dimension from the graphics window (30.0). 15-28

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Editing the Model

Select the right vertical edge (1) of the solid as the Target Object. Select the right outside edge (2) of the pad feature as the tool edge.

Choose MB2 twice to complete the reattachment of the feature.

The holes also move with the pad because they are child features of the pad. They were placed on a face of the pad and were positioned relative to the edges of the pad. The model was created by extruding a sketch. The XC-YC Plane option was chosen when the sketch was created so it is attached to a fixed datum plane and constrained to fixed datum axes. Now, you have been informed that the sketch should be in the YC-ZC plane so that part orientation is consistent with a standard product orientation used at your company. This can be accomplished by moving the fixed datum features. The sketch and all of the other dependent features will move with them.

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15-29

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Editing the Model

Step 4:

Move the fixed datum features. Make layer 21 selectable.

Choose Edit→Feature→Move. Select the three fixed datum features in the Move Feature dialog. (Click and drag MB1 over all three features or Ctrl-Select each feature.)

15

Choose OK. (MB2) Choose Rotate Between Two Axes. Choose Reset and OK to define the pivot point at 0,0,0.

Choose XC Axis

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Practical Applications of NX

as the reference axis.

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Editing the Model

Choose ZC Axis

as the reference axis.

The datum features and dependent features are rotated.

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Step 5:

Close the part.

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15-31

Editing the Model

Summary The editing options provide robust capabilities to change design, form, fit, and function. Because parametric values can be accessed and edited, investment of parametric design time is not wasted when the need for design changes occur. In this lesson you: •

Edited features to satisfy design intent.

•

Deleted features.

•

Used the Edit During Update dialog to resolve an update failure.

•

Reordered features using the Part Navigator.

•

Reattached a feature to a different placement face.

•

Moved datum features

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Lesson

16 Instance Arrays Purpose This lesson is an introduction to Instance Arrays. Objectives Upon completion of this lesson, you will be able to: •

Create a Rectangular Array.

•

Create a Circular Array.

16

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16-1

Instance Arrays

Instance Feature You can use the Instance Feature option to duplicate existing features and eliminate repetitive tasks when creating models. This option can be accessed by choosing the Instance Feature icon from the Feature Operation toolbar or by choosing Insert→Associative Copy→Instance from the menu bar. An Instance is a shape linked feature, similar to a copy. The Instance not only duplicates the feature but preserves the parameters of the feature. Since all instances of a feature are associated, the parameters of the original feature may be edited and the changes are reflected in every instance of the feature. The instance itself is also a parametric feature so parameters such as the number of instances and spacing may be edited. The following Instance Types are available:

16

•

Rectangular Array

•

Circular Array

•

Mirror Body (Not covered in this lesson)

•

Mirror Feature (Not covered in this lesson)

•

Pattern Face (Not covered in this lesson)

There are three Methods available for creating Rectangular and Circular Instance arrays: •

General

•

Simple

•

Identical

In most cases, the General method is sufficient. However, system performance may be affected in complex models. Using the Simple method may increase performance and, in a worst case scenario, the Identical method may be required. Most Feature operations (such as Edge Blend, Chamfer, Shell, etc.) may not be instanced.

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Instance Arrays

Rectangular Instance Array This option is used to create a linear array of instances from selected feature(s). All rectangular arrays will be created in a plane parallel to the XC-YC plane. The position of the rectangular array will remain relative to the location of the feature that the array is based on. If the position of the original feature changes, the position of the array will also change. After selecting the feature(s) to be instanced, the following parameters must be specified: •

Number Along XC — The total number of instances in the XC direction, including the original feature.

•

XC Offset — The spacing between adjacent instances in the XC direction.

•

Number Along YC — The total number of instances in the YC direction, including the original feature.

•

YC Offset — The spacing between adjacent instances in the YC direction.

The offset values can be either positive or negative. The number of instances for both the XC and YC directions must be a whole number greater than zero. 1 — Hole selected for instance. Number Along XC = 3 XC Offset = .75 Number Along YC = 4 YC Offset = 1

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16-3

16

Instance Arrays

Circular Instance Array This option is used to create a circular array of instances from selected feature(s). After selecting the feature(s) to be instanced, the following parameters must be specified: •

Number — The total number of instances in the circular array, including the existing feature.

•

Angle — The angle between adjacent instances, measured about a reference point.

Once the feature and parameters are specified, a rotation axis must be defined. The circular instance array will be created in a plane normal to this rotation axis. There are two ways to define a rotation axis:

16

•

Datum Axis — An existing datum axis is selected. Associativity to the datum axis is maintained. If the datum axis is later moved, the instance array will move with it.

•

Point & Direction — The Vector Constructor dialog is used to specify a direction and the Point Constructor dialog is used to specify a reference point. The selected features will be rotated about the reference point in a plane normal to the vector direction. 1 — Hole selected for instance. 2 — Reference Point (Arc Center) 3 — Vector Direction (+ZC) Number = 8 Angle = 45

When using the Point & Direction option, positional associativity is not maintained. If geometry is used to define the reference point and vector direction and the geometry is later moved, the circular array will not move with it.

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Instance Arrays

Activity — Rectangular Instance Array In this activity, you will create a rectangular instance array of a hole feature. There will be a total of six holes in the instance array. Two holes in the XC direction and three holes in the YC direction.

Step 1:

Open the instance_array_1 part.

Step 2:

Start the Modeling application.

Step 3:

Orient the WCS so that the XC-YC plane is parallel to the plane of the array. Choose Format→WCS→Orient.

16 Choose X-Axis, Y-Axis. Select the X–Axis (1) and Y–Axis (2) as shown.

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16-5

Instance Arrays

The proper WCS orientation is shown below.

Choose OK. Step 4:

Create a rectangular array of the hole feature. Choose the Instance Feature icon. (Insert→Associative Copy→Instance)

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Choose Rectangular Array. Select Simple Hole(15). The feature may be selected from the graphics window or from the Instance dialog. Choose OK. Key in the following parameters: Method

=

General

Number Along XC

=

2

XC Offset

=

1.25

Number Along YC

=

3

YC Offset

=

.687

Choose OK. A preview of the instance array appears in the graphics window. Choosing Yes will create the instance as it is shown. Choosing No will return to the Enter Parameters dialog. 16-6

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Instance Arrays

Choose Yes.

Step 5:

Close the part.

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Instance Arrays

Activity — Circular Instance Array In this activity, you will create a circular instance array of multiple features. The finished part will have four legs that are identical and are to be equally spaced about center of the cylinder. The figure below illustrates the “Before and After” model.

16

Step 1:

Open the instance_array_2 part.

Step 2:

Start the Modeling application.

Step 3:

Create the Instance Feature.

Choose the Instance Feature icon. (Insert→Associative Copy→Instance) Choose Circular Array. Select the following five features from the Instance dialog: Extrude(5) Boss(6) Boss(7) Extrude(9) Simple Hole(12) Multiple features may be selected by pressing MB1, dragging over their names in the Instance dialog, and releasing MB1. Choose OK to confirm the selections. 16-8

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Key in the following parameters: Method =

General

Number =

3

Angle

120

=

Choose OK. The axis of rotation must be selected. Using a Datum Axis maintains positional associativity. Choose Datum Axis. Make layer 61 selectable. Select the Datum Axis (1).

16 A preview of the instance array appears in the graphics window. For better performance, only the first feature selected is previewed. Choose Yes if the temporary display looks correct. Step 4:

Add a chamfer to an instanced hole feature.

Choose the Chamfer icon. (Insert→Detail Feature→Chamfer) Key in the following parameters: Input Option

=

Symmetric Offsets

Offset

=

1.5

Chamfer All Instances

=

ON

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Instance Arrays

Select the circular edge of any one of the instanced holes. Confirm the selection if necessary and choose OK.

Step 5:

Edit the Instance array parameters. Place the cursor over any of the instanced features and choose MB3→Edit Parameters. All options available for editing the selected feature are displayed. The options may vary depending on which feature is selected.

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Choose Instance Array Dialog. Key in the following parameters: Method =

General

Number =

4

Angle

90

=

The Radius value is inferred by the distance from the arc center of the feature to the Datum Axis that was selected as the Rotation Axis for the Circular Array.

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Choose OK three times to complete the edit (or MB2). The part should now have four legs.

Step 6:

Close the part.

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Instance Arrays

Activity (Optional) — Associativity of the Rotation Axis In this activity, you will compare the positional associativity when the Point Direction and Datum Axis options are used to define the rotation axis of a circular instance array. Step 1:

Open the instance_array_3 part.

Step 2:

Start the Modeling application.

Step 3:

Investigate the model. Choose the Part Navigator icon

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from the resource bar.

Choose the push pin icon in the upper right corner to permanently display the Part Navigator.

Choose the Layer Settings icon (Format→Layer Settings) and make the display of ALL layers Selectable.

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The model contains two identical hole patterns. The center hole in each pattern is positioned associatively to the relative datum planes in the part. The hole pattern on the left was created by specifying a point in space and a vector as the rotation axis. The pattern on the right was created by selecting a datum axis as the rotation axis.

Step 4:

Edit the model. In the Part Navigator, double-click the Block(0) feature. Choose Feature Dialog. Key in the following parameters: X Length

=

5

Y Length

=

10

Z Length

=

1

16

Choose OK twice to update the model. (or MB2)

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Instance Arrays

The model updates to reflect the change. Notice that the hole pattern on the left does not move with the datum planes and center hole but maintains the same position in absolute space. This is because the hole pattern was created with a non-associative reference point and direction vector. The hole pattern on the right is associative to the datum axis that was used to define the rotation axis and updated accordingly.

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Step 5:

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Summary The Instance functionality duplicates existing features, eliminating repetitive efforts in the creation of models. In this lesson you: •

Created a Rectangular Instance Array.

•

Created a Circular Instance Array.

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Lesson

17 The Master Model Purpose This lesson introduces the Master Model concept. Objectives Upon completion of this lesson, you will be able to: •

Review an existing Master Model.

•

Edit a Master Model and update an associated non-master part.

•

Create a new Master Model.

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The Master Model

The Assembly Modeler An assembly is a part containing stored links to other part that are pieces of the assembly. The geometry that defines the piece parts of the assembly resides in the original part only, there is no duplication in the assembly part. A link in the assembly part is referred to as a component object. A component object stores information about the piece part such as its location, attributes, origin, orientation, permissions, degree of display, and its relationship to other parts. The Master Model Concept The Master Model Concept may be applied by simply creating an assembly consisting of one component part. It is valuable as a means of promoting concurrent engineering. The person responsible for the design of a part may not be the same person responsible for the downstream applications performed on the part such as drafting, manufacturing, analysis, etc. The Master Model Concept is also valuable in protecting the design intent of the part from inadvertent corruption by a downstream user. The downstream user will have write privileges to the assembly part, but only read privileges to the model. The solid model is referenced for the application work, but the downstream user will not have the ability to change it. Because the application information in the assembly or non-master part is referencing the original master model part, edits to the master model will be updated in the non-master part. Implementing the Master Model concept allows diverse yet dependent design processes to access the same master geometry during development. The entire part creation process becomes more efficient, allowing many disciplines to work at the same time and allowing master model edits to be automatically updated in non-master parts.

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The Master Model

The power of implementing a Master Model is that the independent design processes are dependent on the same master geometry during development.

Drafting

Assembly

Master Model

Analysis

N/C

Each application uses a separate assembly part. When the Master Model is revised, the other applications will automatically update with minimal or no associativity loss. The design intent of the various design applications can be maintained through protection of the Master Model.

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17-3

The Master Model

Master Model Example Manufacturing engineers have the need to design fixture devices, define machining operations, and designate cutter tools and save this data in their models. By creating a manufacturing "assembly" and adding a component to it, they can then generate their application specific geometry or data in a separate part which references the master geometry: •

This avoids duplication of model geometry

•

Different users can work in separate parts simultaneously abcd1234_mfg.prt Non-master part owned by manufacturing engineer. Contains manufacturing data and a component object which references the master model part.

abcd1234.prt Owned by designer. Contains master model geometry.

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The manufacturing engineer owns the assembly part but does not necessarily have write access to the master model which is owned by the designer.

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The Master Model

Activity — Exploring a Master Model Assembly In this activity, you will identify the advantages of using a master model. Step 1:

Open the mm_tapedisp_dwg part. Choose the Open icon.

(File→Open)

Choose Options. Verify the Load Method is set to From Directory in the Load Options dialog and choose OK. Choose the mm_tapedisp_dwg part and OK. Step 2:

Start the Drafting application. (Start→Drafting)

Step 3:

Inspect the drawing for dimensional values. Zoom in on section view A-A and note the slot width of .88 (1) and the corner radius of .13 (2). Both dimensions have been rounded from the model dimensions to two decimal places.

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Fit the view and note the drawing name, SH1, at the lower left corner. (MB3→Fit) Step 4:

Investigate the model. Start the Modeling application. (Start→Modeling)

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The Master Model

Choose Information→Feature and note that there are no features. Choose Tools→Expression and note that there are no expressions. Cancel the Expressions dialog. Choose Assemblies→Reports→List Components. The Information window appears showing the assembly structure for mm_tapedisp_dwg and indicates that there is one component named mm_tapedisp. This part contains the Master Model definition. Component Report Components of Part Name mm_tapedisp

C:\parts\mm_tapedisp_dwg.prt Ref Set Name SOLID

Component Name MM_TAPE_DISP

Close the Information window. Step 5:

Examine the display. Choose Information→Object. Place the cursor over the solid body. When the cursor changes to a QuickPick indicator, choose MB1. The QuickPick window lists each selectable object and the part in which it resides.

17

Choose Solid Body in MM_TAPE_DISP in the QuickPick list.

Choose OK.

(MB2)

The Information window appears with information regarding the solid, its owning part, and confirmation that it is a component. Information on object # 1 Owning part Comp member in part Layer

C:\parts\mm_tapedisp_dwg.prt C:\parts\mm_tapedisp.prt 1, inherited from component

Close the Information window. Step 6: 17-6

Open the Master Model part.

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The Master Model

Choose the Open icon.

(File→Open)

Choose the mm_tapedisp part and OK. Step 7:

Edit the expression for Roll_width. Choose Tools→Expression. Changed the Listed Expressions option to Named. Select the Roll_width expression.

Change the .875 Formula to .75 and choose OK.

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The opening for the tape roll changes in width to accommodate the modified dimension. Step 8:

Edit the blend on the inside of the spool cavity. Activate the Part Navigator

from the resource bar.

Double-click the Blend(21) feature. ©UGS Corporation, All Rights Reserved

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The Master Model

Key in a new value of .06 for the radius (Set1 R). Choose OK. (or MB2 twice) Step 9:

Change the Displayed Part to mm_tapedisp_dwg. Choose Window→mm_tapedisp_dwg to change the Displayed Part. Start the Drafting application. (Start→Drafting) Notice the drawing name now shows (OUT-OF-DATE) to remind you the views are not updated.

Step 10: Update the drawing. Choose the Update Views icon in the Drawing Layout toolbar. (Edit→View→Update Views) Choose All in the Update Views dialog and choose OK. Step 11: Zoom in on section A-A again to see the changes to the master model reflected on the drawing

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Step 12: Close all parts. (File→Close→All Parts)

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The Master Model

Activity — Creating a Non-Master Part In this activity, you will create a new non-master part which references an existing master model. Step 1:

Open the mm_master_1 part.

Step 2:

Start the Modeling application.

Step 3:

Verify the Assemblies application is turned on. (Choose Start→Assemblies if it is not already on).

Step 4:

Create the non-master part. Choose the Create New Parent icon. (Assemblies→Components→Create New Parent) Key in ***_master_1_dwg where *** represents your initials. Choose OK.

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Step 5:

Open the Assembly Navigator and verify the assembly structure.

Step 6:

Close all parts. (File→Close→All Parts)

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The Master Model

Summary This Master Model approach offers many benefits. Master model parts may be write-protected and owned by one user or group yet the data can be shared with other users or groups. Downstream users can access the latest data and incorporate updates as the part is being developed.

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Lesson

18 Introduction to Drafting Purpose This lesson will introduce the Drafting application. Objectives Upon completion of this lesson, you will be able to: •

Open, Create, and Delete drawings.

•

Add, Edit, and Remove Views on Drawings.

•

Modify Preferences.

•

Create Utility Symbols.

•

Create Dimensions.

•

Create Annotations.

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Introduction to Drafting

Working with Drawings You can use the Drafting application to quickly create drawings of 3D parts. Drawings are populated with views that do not need to be defined before the views are placed on the drawing. Some of the benefits of the Drafting application are: •

You can add views to the drawing just by indicating their location with the cursor.

•

When you add orthographic views, they will automatically be aligned with the parent view as you create them.

•

Every view is fully associated with the solid. If the solid is updated, the views will also be updated.

•

Drafting annotation is placed directly on the drawing.

•

Drafting annotation (dimensions, labels, and symbols with leaders) is fully associative to the geometry you select, and will update automatically if there are changes in the solid model.

•

Fully associative view boundaries are automatically calculated when the drawing is updated.

•

Section views are fully associative to the solid model.

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Introduction to Drafting

Creating New Drawing Sheets Upon entering the Drafting application, you will either see an existing drawing, or—if there are no drawing sheets in the part yet—you will be given the Insert Sheet dialog so that you can specify the parameters for a new drawing sheet. To create a new drawing sheet, define the drawing parameters: drawing sheet name, size, scale, units of measure and projection angle. Once the desired parameters have been set, choosing OK replaces the current display with a view of the new drawing of the specified size. There are a few different ways to create a new drawing sheet in a part that already contains drawing sheets. •

Choose the New Sheet icon in the Drawing Layout toolbar.

•

Choose Insert→Sheet from the menu bar.

•

Use MB3 over the drawing node in the Part Navigator and choose Insert Sheet from the pop-up menu.

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Introduction to Drafting

Opening a Drawing There are a few ways to open a drawing: •

In the Part Navigator, double click the sheet name or, use MB3 over the drawing sheet node and choose Open from the pop-up menu.

•

Choose the Open Sheet icon

•

Choose Format→Open Sheet and select the sheet name from a list.

and select the sheet name from a list.

To open a drawing, select from a list of previously created drawings. You can either select the desired drawing name from the list or enter a specific drawing name in the Drawing Sheet Name text field. If there are multiple drawings in the part, you can filter the list to include a specific series of drawings.

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Editing a Drawing In NX, the term "drawing" is used to define a collection of views. Think of each drawing as a separate page in the part. One part can contain many pages, in other words, many drawings. To edit a drawing, you can: •

Choose the Sheet icon

•

Choose Edit→Sheet.

•

Use MB3 in the Part Navigator to highlight the drawing sheet and choose Edit Sheet from the pop-up menu.

•

Select the dashed-line border of a drawing sheet with MB3 to access the pop-up menu and choose Edit Sheet.

in the Drafting Edit toolbar.

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Introduction to Drafting

The current state of the displayed drawing affects the options that are available. You should be aware of the following: •

The projection angle can only be changed if no projected views exist on the current drawing being modified.

•

You can edit the drawing to a larger or smaller size. You can even edit the drawing to a size small enough so that a portion of a view falls outside the boundary of the drawing. However, if you edit the drawing to a size so small that a member view falls entirely outside the boundary of the drawing, you will get an error message.

•

If you need to edit the drawing to a smaller size, but cannot due to the current position of the views, you will first have to move the views closer to the drawing’s origin at the lower left corner of the drawing.

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Deleting a Drawing There are a few different ways to delete a drawing sheet: •

Choose Edit→Delete Sheet. A Delete Sheet dialog lists of drawings eligible for deletion. The name of the current drawing sheet will not be in the list and cannot be deleted using the dialog.

•

Select the dashed-line border of the drawing sheet with MB3 then choose Delete from the pop-up menu. This will delete the current drawing sheet.

•

In the Part Navigator, select the drawing node with MB3 and choose Delete.

•

Choose the Delete Sheet icon from the Drawing Layout toolbar.

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Introduction to Drafting

Activity — Creating New Drawing Sheets In this activity, you will create new drawing sheets in an existing part that has no drawing sheets. Step 1:

Open the drafting_arm_1_dwg part. This is a non-master part. The master model part (drafting_arm_1) was added as a component.

Step 2:

Start the Drafting application and create a new drawing sheet. Start the Drafting application. (Start→Drafting) Because there are no existing drawing sheets in this part, the Insert Sheet dialog appears.

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Verify the following settings in the Insert Sheet dialog. •

Default drawing name is set to SH1.

•

Inches option is on.

•

Default drawing size is set to E - 34 X 44.

•

Scale is set to 1:1 (1 over 1).

•

Projection is set to 3rd Angle Projection.

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Introduction to Drafting

Choose OK. In the graphics window, the dashed lines define the border of the new E size drawing sheet. The name of the drawing sheet appears in the lower left hand corner.

Step 3:

Add another drawing sheet. Choose the New Sheet icon toolbar. (Insert→Sheet)

from the Drawing Layout

Verify that the default drawing name is set to SH2.

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Choose OK to accept the defaults. The name in the lower left corner of the graphics window shows that you have created a second drawing sheet. The Part Navigator will also list the existing drawing sheets in the part.

Step 4:

Close all parts.

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Introduction to Drafting

Activity — Opening and Editing Drawing Sheets In this activity, you will open and edit existing drawing sheets. Step 1:

Open the drafting_edit_1_dwg part. This is a non-master part. The master model part (drafting_edit_1) was added as a component. The drawing sheet 93A12345–3 is displayed.

Step 2:

Start the Drafting application. (Start→Drafting)

Step 3:

Change the current drawing size. In the graphics window, place the cursor over the dashed border of the drawing sheet and choose MB3→Edit Sheet. Choose the standard drawing size of A1 - 594 x 841.

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Choose Apply. The drawing changes to display the new size. Step 4:

Change the current drawing scale. The drawing scale establishes the default scale of all drawing views on the sheet. It is represented in a fractional format with two text fields arranged as a numerator and denominator. The drawing is currently displaying the views at 1/2 full size (1 in the top scale field and 2 in the bottom scale field).

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In this case you want every view on this drawing sheet to display the part full size. Leave the upper Scale field set to 1. Change the lower Scale field to 1, then choose OK. All the views that are present on the drawing assume the new scale. The positions of the drawing views do not change with the scale.

Step 5:

Open the SH1 drawing sheet. Open the Part Navigator

.

Double-click the Sheet “SH1” node in the Part Navigator (MB3→Open). Drawing sheet SH1 is displayed in the graphics window.

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Step 6:

Rename the current drawing. In the Part Navigator, place the cursor over the drawing sheet Sheet “SH1” and choose MB3→Rename.

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Introduction to Drafting

Key in Trimetric and press Enter. You can also rename the current drawing sheet by placing the cursor over the drawing border, choosing MB3→Properties, and keying in a new name. Step 7:

Close all parts.

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Drawing Monochrome Display Monochrome displays a drawing in a single color. You may specify the line and background colors. You can use the Monochrome Display option by: •

Choosing Preferences→Visualization and then choose the Color Settings tab.

Then turn the Monochrome Display option on in the Drawing Part Settings section. The four color selections become active.

The default colors for the foreground and background are black and gray but any color may be selected. The Show Widths option displays line widths.

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Introduction to Drafting

•

In the Part Navigator, place the cursor over the drawing sheet node and use MB3 to select Monochrome from the pop-up menu.

The Monochrome Display will take on the color selections already defined through the Visualization Preferences dialog.

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View Preferences The display of views is controlled by choosing the View Preferences icon or Preferences→View. You can then use the View Preferences dialog to define the display of hidden lines, silhouettes, smooth edges, as well as section view background lines, etc.

The Centerlines option automatically creates linear, cylindrical, and bolt circle centerlines for views where the axis of the cylindrical face is perpendicular or parallel to the plane of the drawing sheet.

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Introduction to Drafting

Hidden Lines If you turn the Hidden Line option off, Hidden Line is not performed and all hidden lines in the view will appear as solid lines. If you turn the Hidden Line option on, the color, font, and width of the hidden lines are determined by the settings in the Color/Font/Width menus.

The color option is not applicable in Monochrome mode. Widths are displayed only if Show Widths is turned on in the Preferences→Visualization dialog. Edges Hidden By Edges

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The Edges Hidden By Edges option controls the display of edges which are hidden by other overlapping edges. If this option is turned off, edges hidden by other edges are erased from the view.

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Smooth Edges Smooth edges are those whose adjacent faces have the same surface tangent at the edge where they meet.

If you turn the Smooth Edges option on, you can use the Color/Font/Width settings to specify their appearance. You can also use the End Gaps option to vary the edge intersection appearance.

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Introduction to Drafting

Virtual Intersections The Virtual Intersections option allows you to display imaginary intersection curves as required by the JIS standard (section 6.13) and the ISO 128-1982 standard (section 5.2.2). The Virtual Intersections option is used when you want to display the curves in a member view that show where blended faces theoretically intersect. The color, font, and width of virtual intersections can be controlled when the Virtual Intersections option is turned on.

The virtual intersection curves only display if the original surfaces joined or intersected before they were blended.

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Adding a Base View The first view to add to a drawing is the Base View. Other views will be projected from the base view. A drawing can have more than one base view. There are several ways to add a base view. •

In the graphics window, place the cursor over the dashed line that represents the drawing border and choose Add Base View from the MB3 pop-up menu. Add Base View is the default option (bold) in the pop-up menu. So, the base view can be added simply by double-clicking on the drawing border.

•

In the Part Navigator, select a drawing sheet node and choose Add Base View from the MB3 pop-up menu.

•

Choose the Add Base View icon in the Drawing Layout toolbar.

•

Choose Insert→View→Base View.

When using any of these methods, click in the graphics window to place the base view on the drawing.

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Introduction to Drafting

View Creation Options Bar After choosing Add Base View option, the View Creations Option Bar appears in the upper left corner of the graphics window.

1

Style — Provides the same set of parameters as the View Preferences option. However, when these options are set from this toolbar they are specific to the view that is being placed on the drawing.

2

View — Determines the orientation of the base view. A pull-down menu list the canned views and any custom views that have been created.

3

Scale — Provides a means to set the scale of the base view. A pull-down menu list several preset scales as well as the options to enter a custom scale or define the scale by an expression.

4

Orient View Tool — Provides a means to orient a view to a orientation that is not listed in the View pull-down menu.

5

Move View — This option only appears on the toolbar if there is already a view on the drawing. This option allows you to move existing views during the operation of adding a new view.

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Orient View Tool When the Orient View Tool is selected a preview screen is presented along with several options to orient the model as desired.

1 – Rotation Tool

4 – Associative Orientation

2 – View Plane Tool

5 – Reset

3 – Horizontal Direction

6 – Reverse Direction

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Introduction to Drafting

Adding Projected Views Immediately after placing a base view on the drawing, you may create a projected view from the base view by moving the cursor off the base view. A projected view may also be created from a view that has been previously placed on the drawing. This is accomplished by placing the cursor over a view’s border, when it highlights click MB3, from the pop-up menu choose Add Projected View. Projection Lines Once the cursor is moved off the base view the system displays projection lines. The view may be projected at any angle from the base view however, the system will snap at 45° increments. Preview As you move the cursor around on the drawing the new view may be previewed as a view border, wireframe, Hidden Wireframe, or shaded image. To select a preview option click MB3 and choose Preview Style.

1 — Projection lines 2 — Border preview of new projected view.

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View Creation Options Bar During the creation of a projected view the View Creation Options Bar is displayed in the upper left corner of the graphics screen with several different options. Displayed below the bar is the Offset dynamic input box.

1

Style — Provides the same set of parameters as the View Preferences option. If this option is not used the new view will inherit the style of its parent view.

2

Base View — Allow you to choose a different base view then originally selected.

3

Hinge Line — Used to define and associative projection. The projected view is 90° to the defined hinge line.

4

Vector Constructor — Pull-down becomes active if Hinge Line has been selected.

5

Reverse Direction — Changes the projection direction from the hinge line.

6

Move View — Allows you to move existing views during the operation of adding a new view.

7

Offset — Value is used to space the projected view from the parent view. The value is applied from the center of the views. The input box is made active by choosing MB3→Cursor Tracking while adding a projected view.

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To apply a value: Key in the value and press Enter. To Reset: Press Backspace and then Enter.

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Introduction to Drafting

Editing Existing Views Editing Style The style of an existing view may be changed by: •

Double-clicking on the view border or choosing MB3→Style on the view border.

•

Double-clicking or choosing MB3→Style on the drawing view node in the Part Navigator.

•

Choose Edit→Style.

Moving Views A view may be dragged around the drawing by placing the cursor over the hold MB1 border of the view, when the cursor changes to drag mode, down and move the view as required. As you move the view in proximity to another view, alignment lines will appear to aid in the positioning of the view. The alignment lines will appear relative to the top, bottom, left, right, or center of the view. If you select more than one view, they can all be moved simultaneously.

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Removing Views From a Drawing To remove views from a drawing, you can: •

Select the view border with MB3; choose Delete from the pop-up menu.

•

Use MB3 in the Part Navigator to highlight the view to be removed, and select Delete from the pop-up menu.

•

Choose the Delete icon

•

Choose Edit→Delete and select the view.

and select the view.

Once a view is removed from a drawing, all drafting objects or view modifications associated to that view are deleted.

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Activity — Adding Views to a Drawing In this activity, you will adding a base view and projected views to a drawing. Step 1:

Open the drafting_bearing_mount_dwg part. This is a non-master part. The master model part (drafting_bearing_mount) was added as a component.

Step 2:

Start the Drafting application.

Step 3:

Add a Base View. Place the cursor over the edge of the drawing border and double-click. The View Creations Option Bar appears and the top view is selected by default. You will use this view for the base view. Click MB3 and choose Preview Style→Wireframe.

Choose the Style icon

in the View Creations Option Bar.

Choose the General tab. Verify that Centerlines is checked and key in a scale of .5.

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Choose the Hidden Lines tab. 18-28

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Verify that Hidden Line is checked and the font is set to Invisible.

Choose OK. Locate the view in the upper left corner of the drawing by clicking MB1.

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Step 4:

Project a Front view. Move the cursor straight below the base view so that the alignment line is vertical. Locate the view in the bottom left corner of the drawing by clicking MB1.

Press MB2 to exit the Add Projected View function. Step 5:

Project a Right view off the Front view. Place the cursor over the Front view’s border; it becomes highlighted. Click MB3 and choose Add Projected View. Move the cursor to the right of the Front view so that the alignment line is horizontal.

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Locate the view in the bottom right corner of the drawing by clicking MB1.

Press MB2. Step 6:

Project an auxiliary view. Place the cursor over the Right view’s border. Click MB3 and choose Add Projected View. Move the cursor around the Right view from the 12:00 to the 9:00 position. Notice that at approximately the 10:00 position, a face in the Top and Front views highlight as well as the corresponding edge in the Right view. If you select a location with these faces highlighted you will create a true auxiliary view of that face.

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Select a location as shown below.

Press MB2 to exit. In some cases, you may have to explicitly define a hinge line for an auxiliary view. You can do this by choosing the Hinge Line option from the View Creation Options Bar and selecting an edge of the part. Step 7:

Close all parts.

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Utility Symbols The Utility Symbols option creates various centerlines, offset center points, target points, and intersection symbols. When you choose the Utility Symbol icon (or Insert→Symbol→Utility Symbol), the Utility Symbols dialog displays. This dialog allows you to specify settings that control the utility symbol as you create it. You can also use this dialog to modify existing symbols. The Utility Symbols dialog consists of four areas: 1 — Symbol Icons 2 — Point Position Options 3 — Symbol Display Parameters 4 — Preference Options

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Point Position Options You can determine a symbol’s placement by selecting an object (or objects) from which to create the utility symbol. When you select an object, the system evaluates the desired location relative to that object based upon the setting of the position option. 1 — Control Point 2 — Intersection Point 3 — Arc Center 4 — Cylindrical Face 5 — Screen Position

You can select up to 100 points to define a linear centerline, circular centerline or bolt circle. The Cylindrical Face option allows you to place cylindrical or symmetrical centerlines by choosing the desired cylindrical or conical face, even if it is hidden inside the solid. Multiple Centerlines This option, when turned on, allows you to create multiple linear or cylindrical centerline symbols without having to choose Apply after each object is selected. You can only apply multiple cylindrical centerlines when the point position option is set to Cylindrical Face. That’s because the system assumes the cylindrical objects are all oriented in the same manner and are of the same length.

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Using the Inherit Option You can set the symbol preferences by choosing the Inherit option. This allows you to select an existing symbol from which to inherit preferences. When the symbol is selected, the preferences matching those of the selected symbol will be set in the dialog and will be used to create a new symbol. Inherit can also be used to edit the display of an existing symbol. To do this, you would select the symbol you intend to edit, choose Inherit, then select the symbol whose preferences you wish to see reflected in the first. The new settings will be displayed in the dialog. Choose Apply to perform the edit. Using the Default Option The Default option resets the preferences to the customer default settings. You can use this option to set the preferences before creating a new symbol or to edit an existing symbol. To edit an existing symbol, select the symbol and choose Default. The default settings will be displayed in the dialog. Choose Apply to update the symbol. Associativity of Utility Symbols A utility symbol’s placement is controlled by a position on an object. The system will automatically size the symbol components to the objects selected to create it, based upon the local preference settings.

Deleting Utility Symbols You can delete a utility symbol by selecting the symbol from the graphics window and choose the Delete icon. (Edit→Delete) The symbols can be selected at any position. When you delete a utility symbol, any associated objects such as dimensions are also deleted unless the Retain Annotation option in Preferences→Drafting is turned on. Adding Automatic Centerlines Automatic center lines may be added to a view after its creation. The hole or pin axis must be either perpendicular or parallel to the plane of the drawing view To apply automatic center lines: •

Choose Insert→Symbol→Utility Symbol.

•

Choose Automatic Centerline.

•

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Creating a Linear Centerline A linear centerline is a straight line that passes through selected points or arcs, with a perpendicular line through each position. A linear centerline that passes through a single point or arc is called a simple centerline. To create a linear centerline, select the Linear Centerline icon, set the point position option if needed, select relative objects, and select Apply or OK. The following associativity rules apply to linear centerlines: •

If the linear centerline contains two associated points, repositioning or deleting one of those points results in an automatic resize and update of the linear centerline.

•

If the linear centerline contains three or more associated points and a point is removed from the centerline, that point is disassociated from the centerline.

•

If the linear centerline contains three or more associated points and all the associated points are moved, the centerline is automatically resized and updated. If all of the points are deleted, the centerline is also deleted, depending on the Retained Annotation status.

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Activity — Creating a Linear Centerline In this activity, you will create a linear centerline. Step 1:

Open the drafting_sym1_dwg part. This is a non-master part. The master model part (drafting_sym1) was added as a component.

Step 2:

Start the Drafting application. (Start→Drafting)

Step 3:

Verify that the work layer is 101. (Format→Layer Settings)

Step 4:

Create a simple centerline. Choose the Utility Symbol icon. (Insert→Symbol→Utility Symbol) Choose the Linear Centerline icon.

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Set the Point Position option to Arc Center.

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Select the single hole at the right end of the bar.

If you select the wrong point for the symbol position, choose the icon again to deselect the object and start over. Choose Apply to create the centerline (Ctrl-MB2).

Step 5:

Create a linear centerline through multiple points. A linear centerline is created if you select multiple collinear holes. Verify Multiple Centerlines is turned off. Select both of the outer circles of the counterbored holes.

The size of the symbol components is determined by the objects selected. The linear centerline would display with a different size if the inner circles had been selected.

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Choose Apply (Ctrl-MB2).

Any holes selected that are not collinear will not be added to the symbol.

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If a point is selected that is not collinear, the following error message will appear.

Step 6:

Close all parts.

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Manually Creating a Cylindrical Centerline You can create a cylindrical centerline that conforms to ANSI Y14.2 standards through points, arcs or cylindrical faces. The objects used to create cylindrical centerlines are defined by the Position Option. 1 — Control Point 2 — Intersection Point 3 — Arc Center 4 — Cylindrical Face 5 — Screen Position

The Cylindrical Face position option allows you to choose a cylindrical or conical face of a feature for placement. Point position options allow you to create a centerline associated to objects other than cylinders. The following associativity rules apply to cylindrical centerlines: •

A cylindrical centerline must be associated to two point positions.

•

A cylindrical centerline is updated when the data to which it is associated is moved or resized.

•

If one of the objects to which a cylindrical centerline is associated is deleted, the centerline will also be deleted.

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Activity — Creating a Cylindrical Centerline In this activity, you will create cylindrical centerlines using both the Arc Center and Cylindrical Face options. Step 1:

Open the drafting_sym4_dwg part. This is a non-master part. The master model part (drafting_sym4) was added as a component.

Step 2:

Start the Drafting application. (Start→Drafting)

Step 3:

Change the work layer to 101. (Format→Layer Settings)

Step 4:

Create a Cylindrical Centerline symbol. Choose the Utility Symbol icon. (Insert→Symbol→Utility Symbol) Select the Cylindrical Centerline icon.

Set the Point Position option to Arc Center.

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Select two arc center locations for each of the three centerline placements shown below:

1 — Select this pair of edges. 2 — Select this pair of edges. 3 — Select this pair of edges, confirming your selections if needed.

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The resulting cylindrical centerlines are shown.

When creating cylindrical centerlines, you may not always be able to use the Arc Center point position option. The larger hole depicted in the section view is partially hidden. Since you cannot see the left edge of the hole in this view, you would not be able to select it. In the orthographic view, you will find it impossible to select the right hand edge of a small hole without picking the center of the larger outside edge of the part instead. In this case, the Cylindrical Face option can be used to select a cylindrical or conical face of a feature for placement of a centerline symbol. Step 5:

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Create a centerline symbol using the Cylindrical Face option. Continue using the Cylindrical Centerline icon.

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Change the Point Position option to Cylindrical Face. Place your cursor over the cylindrical face as shown and select the face using MB1.

Indicate end points 1 and 2 of the cylindrical centerline, using cursor locations as shown. The indicated end points are projected to the axis of the cylindrical face, and two drafting points are created that are associated to the selected face.

When creating centerlines using the Cylindrical Face option, the local display parameter values that determine the symbol past part distances are disregarded.

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Close all parts.

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Dimensions The various dimensions types may be accessed two different ways. •

Choose Insert→Dimension and then choose the desired dimension type.

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•

Use the Dimensions toolbar. This toolbar offers a menu of the available dimension types.

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Annotation Preferences Dimensions may be displayed in many different ways. Some of the settings are for appearance, i.e. extension line and arrowhead. Other settings convey the value of the dimension, i.e. the number of decimal places used to define tolerance. In general most of the dimensions will share the same appearance. The Annotation Preferences dialog is used to capture those global settings. The Annotation Preferences dialog is activated by choosing Preferences→Annotation or by choosing the Annotations Preferences icon.

The following tabs apply to dimensions: •

Dimensions — Controls the display of extension lines and arrows, orientation of text, precision and tolerance, chamfer dimensions, and narrow dimensions.

•

Line/Arrow — Controls the style and size of leaders, arrows, and extension lines for both dimensions and other annotations. A preview area provides a rendition of the symbol with leaders and dimensions.

•

Lettering — Controls the alignment, justification, size, and font of text.

•

Units — Controls the desired unit of measure for dimensions and whether dimensions are created in single or dual dimension format.

•

Radial — Controls the settings that are unique to diameter and radius dimensions.

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Dimension Preferences and Placement Once a dimension type is selected, a Dimension icon option bar will appear in the upper left corner of the graphics window. This option bar accesses many of the same settings found in the Annotation Preferences dialog that apply to dimensions. However, when changes are made with this option bar, they only affect the dimensions being created in the current operation and do not change the global preference settings. The settings will return to the global condition when you exit dimension creation or choose Reset (5).

1 – Style 4 – Annotation 2 – Precision (decimal places) 5 – Reset 3 – Tolerance Type Annotation Placement Toolbar The Annotation Placement toolbar also appears when creating dimensions to help control the placement of the dimension.

1 2 3 4 5 6 7

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– Leader Type – Leader Placement – Opens the Create Leader dialog – Associate Origin with Helper Lines – Alignment Position – Opens the Origin Tool dialog – Annotation Plane

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The Snap Point Toolbar The Snap Point toolbar will be available when creating dimensions.

This toolbar acts as a filter for selecting points on parts. You can turn icons on (highlighted) or off in order to limit your selection to specific types of points. The Two Pick Intersection icon (at the right end of the toolbar) will let you select any two edges whose intersection you cannot get within the select ball. (When you turn it on, all of the other icons will be grayed out.) The Escape Key You can press the Escape key at any time to release all selected objects. It is often quicker than using Shift+Select. Placement Cues for Dimensions As you create dimensions it is now very simple to align the dimension with an existing dimension. To help you do this, the system will provide graphical cues whenever the origins of the dimensions line up. As you begin to locate the dimension, pass the cursor over the existing dimension that you want to align to. Whenever the placement image of the new dimension is aligned horizontally or vertically with the existing dimension (or other annotation), you will get a dashed help line.

18 If you want the new dimension associated with the existing dimension, make sure the Associate Origin with Helper Lines icon by default).

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Appended Text Text may be appended to a dimension while you are creating it. If you want only one line of appended text, you can select the object(s) to dimension and, prior to locating the dimension, choose one of the Appended Text options in the MB3 pop-up menu.

You may also use the right (after), left (before), up (above), or down (below) arrow key on the keyboard instead of the MB3 pop-up options. If the text is more complex, you will need to use the Annotation Editor dialog. You can access the Annotation Editor from the interactive toolbar at any time, or you can access it after selection of objects (and before locating the dimension) by using MB3. To add appended text to a previously created dimension that does not already have appended text, you can:

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•

Double-click on the dimension, and then use the Annotation Editor icon in the interactive toolbar.

•

Double-click on the dimension and then use the right (after), left (before), up (above), or down (below) arrow key on the keyboard to get the appended text location you desire. Key in the text and press Enter.

•

Double-click on the dimension, and then use MB3 to choose either Appended Text (for a single line of text), or Annotation Editor (for more complex text).

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To edit existing appended text, you can: •

Double-click on the appended text.

•

Double-click on the dimension and then use the right (after), left (before), up (above), or down (below) arrow key on the keyboard to get the appended text location you desire.

•

Select the dimension, and then use MB3 on the appended text. You get the following menu:

the Edit Appended Text option will access the Annotation Editor dialog.

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Tolerances There are several ways to add or edit tolerances. Prior to creating a dimension (after choosing a dimension icon), you can choose the Tolerance icon on the interactive toolbar, and set the desired tolerance type. The Tolerance Values icon is then added to the toolbar. Choose it and enter the desired values. While creating a dimension (after selecting the object to dimension), you can: •

Set the tolerance type by choosing either MB3→Tolerance Type or the Tolerance Type icon.

•

Set the desired tolerance values by choosing either MB3→Tolerance or the Tolerance Values icon.

Tolerance Type

Tolerance Values

To add a tolerance later, you can select the dimension and use the methods shown above. To edit a tolerance later, you can use one of the following three methods:

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•

Select the tolerance with MB3→Edit.

•

Double-click on the tolerance.

•

Double-click on the dimension to access the dimension bar (in the upper left corner of the graphics screen).

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Text Orientation and Text Arrow Placement To set the Text Arrow Placement or the Text Orientation while creating a dimension, use MB3 before locating the text. You get the following menu: Horizontal Aligned Text Over Dim. Line Perpendicular Text at Angle

Automatic Arrows Out Arrows In

To change Text Orientation or Text Arrow Placement of an existing dimension, double–click on the dimension, and then use MB3. You will get the same menu as shown above. Moving a Dimension To change the origin of an existing dimension, simply drag it with MB1, without any function active.

The cursor will change to

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when you are in the move mode.

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Editing an Existing Dimension There are two possible pop-up menus that can be displayed when working with an existing dimension. •

One pop-up menu appears when selecting a dimension (outside of dimension creation) with MB3.

•

The other pop–up menu appears when you double-click with MB1 on an existing dimension (while in or outside of the dimension function) and then click MB3.

18 When you access this pop–up menu, the dimension bar also appears in the upper left hand corner.

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If you again double-click (with MB1) on the selected dimension, you will access the Dimension Style dialog. Changing the Precision of a Dimension There are a few ways to change the precision of an existing dimension. After double-clicking on the dimension: •

Choose MB3→Nominal Precision.

•

Choose the precision from the icon option bar.

•

Press the number on the keyboard.

Inheriting Preferences from an Existing Dimension After a dimension has been created, to edit its preference setting to that of another existing dimension: •

Double-click (with MB1) on the dimension that is to change.

•

Click MB3 on the dimension and choose Inherit.

•

Select the dimension that has the desired preference settings.

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Deleting Dimensions You can use the dimension pop-up menu to delete a dimension or you can select the dimension(s) to delete, and use the Delete icon.

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Activity — Creating Dimensions In this activity, you will create several dimensions using various settings. Step 1:

Open the drafting_fitting_dwg part. This is a non-master part. The master model part (drafting_fitting) was added as a component.

Step 2:

Start the Drafting application.

Step 3:

Verify that the work layer is 101. (Format→Layer Settings)

Step 4:

Create a Horizontal dimension. Choose the Inferred Dimension icon toolbar. (Insert→Dimension→Inferred)

in the Dimension

Select near the end points of the solid edges.

18 If you select the wrong object, press the Escape key on the keyboard to deselect, and select again. Place the dimension by clicking MB1 at the desired location. If you need to change the style of an existing dimension, double-click it (to select it), then double-click it again to display the Dimension Style dialog.

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Step 5:

Create a Vertical dimension. The dimension you are about to create is based upon the selection of a linear centerline, not the arc centers. This allows the gap to be displayed between the centerline symbol and the dimension extension lines. Select the centerline symbol.

Choose Equal Bilateral Tolerance in the Dimension bar in the upper left corner of the graphics window.

Choose 1 decimal place for the Tolerance Precision in the Dimension bar.

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Choose Tolerance Values.

Key in .1 for the Tolerance and press Enter. Place the dimension.

Click MB2 to cancel vertical dimension creation. The Tolerance Type, Precision, and Value can also be changed using the MB3 pop-up menu after selecting the object(s) to dimension. Step 6:

Create a Cylindrical dimension for the diameter of the boss. This dimension requires that you append text in front of the diameter symbol.

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Choose the Cylindrical icon in the Dimensions toolbar. (Insert→Dimension→Cylindrical) 18-58

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Select the two edges of the boss (in any order).

Before placing the dimension, choose MB3→Appended Text→Before. In the dynamic input field, key in 2X and press the Enter key. You also need to adjust the placement before you establish the dimension. You can do this with the MB3 pop-up menu. Choose MB3→Placement→Arrows In.

Place the dimension as shown.

Step 7:

Align a dimension with an existing dimension.

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Select the two edges as shown below.

Choose Reset.

The appended text is no longer needed.

Pass the cursor over the

dimension.

Locate the dimension so that the alignment line indicates that it is aligned with the dimension above it.

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Click MB2 to exit the dimension function. Step 8:

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Text Creation The Annotation Editor is used to create notes, labels, and GD&T symbols. You can access the Annotation Editor interface by: •

Choosing the Annotation Editor icon toolbar.

•

Choosing Insert→Annotation.

from the Drafting Annotation

The Annotation icon option bar and the edit window will be displayed in the graphics window. However, the small edit window can be enlarged and moved.

1 — Annotation Bar 2 — Edit Window 3 — Annotation Placement Toolbar

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Creating Notes The Annotation bar is stationary. It will always remain in the upper left hand corner.

You can use it to: 1 — Access the full Annotation Editor dialog 2 — Change the Style for the annotation being created. 3 — Insert a special symbol. 4 — Insert a GD&T symbol. 5 — Insert a datum symbol. The above options are also available while locating an annotation, by using MB3 on the graphics window. The Edit Window, found in the upper left hand corner of the graphics window is also called the "Dynamic Mini-Text Box" because it lets you enter text and symbols for your notes and labels. The Edit window contains some default text (which is highlighted).

18 Because this is a window, you can drag any side or corner to change its size or drag the entire window to a different location. Also, you’ll see horizontal and vertical scroll bars appear whenever they are required.

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The Annotation Placement toolbar works the same as it does for dimensions.

Entering Text To enter text, begin typing over the highlighted text in the Edit window.

You can use CTRL-i, CTRL-b, and CTRL-u to for italics, bold, and underlined text as you compose the note. It also appears on the cursor as a placement image.

After you locate the text, it remains in the edit window for you to use again or edit for the next annotation. You can also create a note on a drawing by dragging a .txt file from an operating system window to the drawing.

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Creating Leaders on Notes and Labels

To create a leader, do the following: •

Key in the desired text.

•

Locate the cursor on the curve/edge/face where you want the arrowhead located (with the cursor displayed as shown below).

If you want the leader to point to empty space instead of an object use the same procedure. The only difference is that the cursor will not display in a “ leader” mode if an object is not selected.

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•

Press (and hold down) MB1 and drag the cursor away from the selection point. A temporary display of the leader will be shown on the screen.

•

Click MB1 at the location for the text.

If you want a second leader, repeat the second and third steps before defining a text location with MB1. You can quickly change a leader location by clicking MB3 over the leader, choosing Edit Associativity, and specifying the new location.

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Activity — Creating Notes and Labels In this activity, you will create notes and labels on a drawing. Step 1:

Open the drafting_fitting_dwg part. This is a non-master part. The master model part (drafting_fitting) was added as a component.

Step 2:

Start the Drafting application.

Step 3:

Verify your current work layer is set to 101. (Format→Layer Settings)

Step 4:

Create a note.

Choose the Annotation Editor icon.

(Insert→Annotation)

The Annotation Bar, Edit window, and Annotation Placement Toolbar will be displayed.

18 Press Backspace to remove the text from the Edit window. Key in your name into the Edit Window. It will be placed in the title block. There are no limits on the number of characters per line, or the total number of characters that can be entered.

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Step 5:

Place the note on the drawing. Zoom in on the Title block. Drag the note to the desired location on the drawing, and indicate the placement by clicking MB1.

Because you are currently using the system defaults for the Lettering preferences, the text alignment position is located at the mid-center of the note. Notice that the text remains behind the cursor in the graphics window. The text will continue to follow the cursor until the Edit window is closed. Step 6:

Create a label. In capital letters, key in the following text in the Edit window. OMIT PAINT FOR ELECTRICAL BONDING Click and hold down MB1 on the phantom circle in the front view and drag the text until you see a leader; release MB1. Click MB1 once again to place the label as shown below.

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Click MB2 to close the editor. Step 7:

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Do not close the part, it will be used in the next activity.

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The Annotation Editor The Annotation Editor creates notes or labels consisting of text and drafting symbols. You can include the following in a note or label: •

Drafting symbols

•

Fractions and two-line text

•

GD&T symbols

•

User-Defined symbols

•

Expression values

•

Part and Object Attributes

You can access the Annotation Editor dialog by choosing the Annotation Editor icon

from the Drafting Annotation icon option bar.

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The Annotation Editor dialog will be displayed.

18 1 — Toolbar 2 — Text Entry Window 3 — Preview Window (Show Preview icon must be selected) 4 — Symbol Display and Text Preference Options

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As you enter text and symbols, the text and control characters appear within the Text Entry Window. In this window you may use the formatting options available on the Toolbar to customize the appearance of your text. For example, you may want your name to appear as italic, underlined letters. As you type, the text will appear in the graphics window and in the annotation editor preview window (if turned on) as shown.

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Annotation Editor Tools

The Annotation Editor dialog contains several options for text formatting. Some of the more common options are described below.

1 — Clears the display in the text entry and preview area. 2 — Opens (or closes) the preview area. 3 — Text font. 4 — Text scale factor. 5 — Options to add text attributes (bold, italicized, underlined, superscript, subscript) 6 — Deletes text attributes.

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Introduction to Drafting

Editing Notes You can edit text in a previously created note or label by selecting it from the drawing and using the MB3 pop-up menu. You get the following menu:

You can also edit annotation objects by double-clicking (with MB1) on the note or label. You can also use MB1 to select multiple objects (but this will reduce the options available on the MB3 pop-up menu). Helper Lines Helper lines act as a guide that allows you to line up notes, labels, dimensions, symbols, and views to other drawing objects on the drawing. Helper lines appear as a dashed line. To use helper lines, move the cursor over the object to which you want to align as you are placing the new annotation. The note highlights and helper lines appear.

18

Press and release MB1 to place the annotation at the desired location.

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Introduction to Drafting

Activity — Creating More Notes In this activity, you will creating more notes on a drawing. Step 1:

Continue using drafting_fitting_dwg.

Step 2:

Create a note. Choose the Annotation Editor icon.

(Insert→Annotation)

In capital letters, key in the note shown below. NOTE: 1) DIMENSIONS AND TOLERANCING PER ASME Y14.5M-1994. 2) BREAK ALL SHARP EDGES. Place the text in the lower left corner of the drawing as shown below by clicking MB1 at that location.

Step 3:

Create another note using the Annotation Editor dialog. Choose the Annotation Editor icon from the icon option bar in the upper left corner of the graphics window.

18 Choose the Clear icon the editor.

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in the dialog to clear any text in

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Introduction to Drafting

Verify the Font is set to blockfont and the change the Character Scale Factor to 1.75.

In capital letters, enter the text for the drawing number 05-FIT-2475. Locate the drawing number in the title block as shown below.

Step 4:

Complete the title block. Choose Clear

on the Annotation Editor dialog.

Key in: 1/1 Place the text in the Scale area of the title block. Key in 2DAY. Pass the cursor over 1/1 so that a dashed alignment help line is shown. Place the text in the “Date” area of the title block.

18

Complete the Title Block by adding the sheet numbers.

Close the Editor and click MB2 to exit. Step 5:

Change the date on the drawing to today’s date. Click MB3 on the date 2DAY in the title block.

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Choose Edit Text from the pop-up menu. Highlight 2DAY in the Edit Window and type in today’s date (MM-DD-YY). Click MB2 to close the Edit Window. Step 6:

Reposition the date. Using MB1, drag the date so that the right end fits inside the box. Notice how it maintains alignment with the scale note. If required, drag the 1/1 note down so that the date does not lay on top of the word “DATE”.

Step 7:

Close all parts.

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Introduction to Drafting

Master Model Drawing Guidelines 1. Open the master model part. (File→Open) 2. Start the Assemblies application (Start→Assemblies) 3. Create a new parent part (Assemblies→Components→Create New Parent, xxxxx_dwg) As an alternative, you could create a ’drawing’ file using a seed part and then add the master model as a component (Assemblies→Components→Add Existing). 4. Start the Drafting application (Start→Drafting) 5. Adjust the sheet; name, units, size, projection angle (Edit→Sheet) 6. Add the drawing formats; title block, border, revision block, standard notes (Site dependent) 7. Set View Display Preferences; hidden line removal, section backgrounds, threads (Preferences→View) 8. Add the base view, typically top or front (Insert→View→Base View and choose the view to add) 9. Add more views; projected, detail, section, isometric, exploded (Insert→View) 10. Adjust the view display; size, orientation, etc. (Edit→Style or Edit→View) 11. Clean up individual views with view dependent edits; erase object, edit entire object, edit object segment (Edit→View→View Dependent Edit) 12. Add the Utility Symbols; centerlines, target symbols, intersection symbols (Insert→Symbol→Utility Symbol) 13. Add the dimensions (Insert→Dimension) 14. Add the notes, labels, and GD&T symbols (Insert→Annotation)

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Introduction to Drafting

Summary The Drafting Application provides for the creation of drawings. Views and dimensions that are placed on a drawing are associative to the solid model and update when changes are made to the model. The Annotation Editor interface makes it easy to create, edit and delete notes and labels. The annotation bar and edit window allows you to work with notes and labels without opening the Annotation Editor dialog. In this lesson you: •

Modified a drawing.

•

Added views to a drawing.

•

Created Utility Symbols.

•

Created Dimensions.

•

Added annotation to a drawing.

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Appendix

A Additional Projects

This appendix contains Additional Projects for you to work on.

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A-1

Additional Projects

Project 1

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Project 2

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A-3

Additional Projects

Project 3

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A-5

Additional Projects

Project 4

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A-7

Additional Projects

Project 5

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A-9

Additional Projects

Project 6

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Additional Projects

Project 7

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Additional Projects

Project 8

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Additional Projects

Project 9

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Additional Projects

Project 10

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Project 11

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Additional Projects

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Project 12

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Additional Projects

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Project 13

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Additional Projects

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Project 14

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Additional Projects

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Project 15

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Project 16

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Project 17

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Project 18

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Project 19

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Project 20

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Project 21

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Project 22

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A

Appendix

B Expression Operators Overview The following information lists the various operators that may be used in expressions.

B ©UGS Corporation, All Rights Reserved

Practical Applications of NX

B-1

Expression Operators

Operators There are several types of operators that you may use in the expression language. Arithmetic Operators

Example

+

Addition

p2=p5+p3

-

Subtraction and Negative Sign

p2=p5–p3

*

Multiplication

p2=p5*p3

/

Division

p2=p5/p3

%

Modulus

p2=p5%p3

^

Exponential

p2=p5^2

=

Assignment

p2=p5

Relational and Boolean Operators >

Greater Than

<

Less Than

>=

Greater Than or Equal

<=

Less Than or Equal

==

Equal

!=

Not Equal

!

Negate

& or &&

Logical AND

| or ||

Logical OR

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Expression Operators

Precedence and Associativity In the table below, operators in the same row have equal precedence while operators in the following rows have less precedence. Precedence and Associativity Operators ^

Associativity Right to Left

– (change sign) *

/

%

Left to Right

+ – >

<

==

>=

<=

!=

&& || =

Right to Left

When using operators with the same precedence in an equation without parameters, use left-to-right or the right-to-left rule from the table. For example: X = 90 – 10 + 30 = 110 (not 50) X = 90 – (10 + 30) = 50

B ©UGS Corporation, All Rights Reserved

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B-3

Expression Operators

Legacy Unit Conversion Although when dimensionality is specified and units are assigned the system handles conversions, legacy parts may have used functions for unit conversion. For legacy compatibility these functions are supported. Functions for Unit Conversion cm

cm(x) converts x from centimeters to the default units of the part

ft

ft(x) converts x from feet to the default units of the part

grd

grd(x) converts x from gradients to degrees

in

in(x) converts x from inches to the default units of the part

km

km(x) converts x from kilometers to the default units of the part

mc

mc(x) converts x from microns to the default units of the part

min

min(x) converts x from minutes to degrees.

ml

ml(x) converts x from mils to the default units of the part

mm

mm(x) converts x from millimeters to the default units of the part

mtr

mtr(x) converts x from meters to the default units of the part

sec

sec(x) converts x from seconds to degrees

yd

yd(x) converts x from yards to the default units of the part

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Expression Operators

Built-in Functions Built-in functions include math, string, and engineering functions. Scientific Notation You may optionally enter numbers in scientific notation. The value you enter must contain a positive or negative sign. For example, you can enter: 2e+5 which is the same as the value 200000 2e-5 which is the same as the value .00002 Built-in Functions abs

Returns the absolute value of a given number

arccos

Returns the inverse cosine of a given number in degrees

arcsin

Returns the inverse sine of a given number in degrees

arctan

Returns the inverse tangent of a given number in degrees from –90 to +90

arctan2

Returns the inverse tangent of a given delta x divided by a given delta y in degrees from –180 to +180

ASCII

Returns the ASCII code of the first character in a given string or zero if the string is empty

ceiling

Returns the smallest integer that is bigger than a given number

Char

Returns the ASCII character for a given integer in the range 1 to 255

charReplace

Returns a new string from a given source string, character to replace and the corresponding replacement characters.

compareString Case sensitive compare of two strings cos

Returns the cosine of a given number in degrees

dateTimeString Returns the system date and time in the format “Fri Nov 21 09:56:12 2005\n” floor

Returns the largest integer less than or equal to a given number

format

Returns a formatted string, using C-style formatting specification

getenv

Returns the string value of a given environment variable string

hypcos

Returns the hyperbolic cosine of a given number

hypsin

Returns the hyperbolic sine of a given number

hyptan

Returns the hyperbolic tangent of a given number

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B B-5

Expression Operators

Built-in Functions log

Returns the natural logarithm of a given number

log10

Returns the logarithm base 10 of a given number

MakeNumber

Returns the number or integer of a given numerical string

max

Returns the largest number from a given number and additional numbers

min

Returns the smallest number from a given number and additional numbers

mod

Returns the remainder (modulus) when a given numerator is divided by a given denominator (by integer division)

NormalizeAngle Normalizes a given angle (degrees) to be between 0 and 360 degrees pi()

Returns pi

Radians

Converts an angle in degrees into radians

replaceString

Replaces all occurrences of str1 with str2

round

Returns the integer nearest to a given number, returns the even integer if the given number ends in .5

sin

Returns the sine of a given number in degrees

sqrt

Returns the inverse square root of a given positive number

StringLower

Returns a lowercase string from a given string

StringUpper

Returns an uppercase string from a given string

StringValue

Returns a string containing a textual representation of a given value

subString

Returns a new string containing a subset of the elements from the original list

tan

Returns the sine of a given number

ug_ functions

see the documentation for descriptions of dozens more specialized math and engineering functions

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C

Appendix

C Point Constructor Options Overview This appendix describes the various Point Constructor methods that may be used. The Point Constructor dialog provides a standard way to specify points. It allows the creation of point objects as well as the determination of locations in three-dimensional space.

Points may be specified in one of two ways: either choose one of the provided, icons at the top of the dialog, or directly enter the X-Y-Z coordinates in the fields provided.

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Point Constructor Options

C

Methods to Specify a Point The top of the Point Constructor dialog displays icons representing various methods for specifying a point. As the cursor is passed over these icons, the icon block displays the name of the method. The icon methods are described below.

Inferred Point Depending on where you select when using this option, one of the following single selection options will be used: cursor location, existing point, end point, mid point or arc center. This option does not require a selection of the particular point type for each selection.

Cursor Location Use this option to construct points anywhere on the screen by positioning the cross hairs and indicating a location. The location defined lies on the WCS Work plane. To locate points quickly and precisely, use a grid (see Preferences→Work Plane →Show Grid). When Snap to Grid is on, points snap to the nearest grid position. The grid spacing may be set as desired. The spacing in the X-direction does not need to be the same as the spacing in the Y-direction. For example, if the smallest increment on the part is in eighths of an inch (.125), then the grid spacing would be set to .125. A point at exactly one inch in X and two inches in Y could be created by counting over eight grid points in X and up sixteen in Y and indicating a screen position.

Existing Point Use this option to specify a location by selecting an existing point. Remember that the point constructor allows locations in model space to be specified. In the instance where an existing point is being selected it is generally a case of using that point to aid in the construction of another object such as a the endpoint of a line, or the location of an object, such as placement of a drawing border.

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Point Constructor Options

C End Point Use this option to specify locations at the end points of existing lines (1), arcs (2), conics (3), and splines (4).

When selecting geometry, place the selection ball near the end point (1) you wish to select. The point is located at the end of the curve nearest to where it was selected (see below). Closed curves, such as complete circles, have only one endpoint because the two ends are at the same coordinate location.

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C-3

Point Constructor Options

C Control Point Use this option to locate points at the control points of geometric objects. The control points, which vary for each object type, include: Existing points, End points of conics, End points and Mid points of open arcs, Center points of circles or arcs, Mid points and End points of lines, and End points or Knot points of splines. Use the cursor to select objects. Since some objects have more than one control point, place the cross hairs near the control point desired. The system locates the control point nearest the position where the curve is selected. The illustration below shows the various locations of control points on existing lines (1), arcs (2), conics (3), and splines (4).

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Point Constructor Options

C Intersection Point Use this option to locate a position at the intersection of two curves or at the intersection of a curve and a surface or plane. If the curves intersect more than once, the system creates the point nearest to where the second curve was selected.

When two selected curves are not coplanar with the XC-YC plane the system creates the point on the first curve (1) selected. By projecting the second curve (2) parallel to the ZC axis an apparent intersection is calculated and the point (3) is defined on the first object selected (see below). Projections are always done along the ZC-axis.

ZC YC

XC

Positions may be indicated at the intersection of any two non-parallel curves. Implied intersections may be located even if the objects do not actually touch (see below).

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C-5

Point Constructor Options

C Arc/Ellipse/Sphere Center Use this option to specify a position at the center of an arc or ellipse by selecting the arc along its circumference.

In the example below, selecting with the circumference (1) of the large circle within the selection ball defines the center point (2) of the large circle.

Selecting near the center of the large circle (1) will not select the center of the large circle since the selection ball touches the circumference of the small circle.

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Point Constructor Options

C Angle on Arc/Ellipse Use this option to locate a position (1) at an angular location on an arc or an ellipse.

The angle value is entered in degrees. The angle is referenced from the positive XC axis and is measured counterclockwise in the WCS. The angular position on the arc or ellipse may also be defined on the unconstructed portion (2) of an arc or ellipse.

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C-7

Point Constructor Options

C Quadrant Point Use this option to locate positions at the quarter points of an arc or an ellipse.

Points may be located at the starting point of the arc or ellipse and then at quarter-distance intervals along the object. The point located (1) is the quadrant point nearest to the position selected (2). The quadrant position may also be defined on the unconstructed portion (3) of an arc.

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Point Constructor Options

C Point on Curve/Edge Use this option to locate positions on a curve or edge by specifying a U Parameter. After choosing this option and selecting a curve or edge, the Point Constructor dialog will display an entry field for a U Parameter.

The U Parameter can be a value between 0 and 1 where a value of 0 would be the start and a value of 1 would be the end of the curve or edge.

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C-9

Point Constructor Options

C Point on Surface Use this option to locate positions on a surface (face) by specifying a U Paremeter and a V Parameter. After choosing this option and selecting a face, the Point Constructor dialog will display entry fields for the U and V Parameters.

The U and V Parameters can have values between 0 and 1 to define the location on the face.

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Point Constructor Options

C

WCS and Absolute Coordinates Choose WCS or Absolute to specify the coordinate system to reference when entering values in the Base Point fields. The WCS (Work Coordinate System) is the default. The WCS may be moved to any location and placed in any orientation. The absolute coordinate system is a fixed coordinate system.

Reset The Reset button sets the values X, Y, and Z coordinates of the Base Point to 0 and sets the Offset method to None.

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C-11

Point Constructor Options

C

Offset This option allows you to specify a position in model space offset from a reference position. The offset may be specified in several different methods.

Once an offset method has been specified, it remains in effect until another one is chosen. The default is None (no offset). Rectangular Offset This option allows a position to be offset by keying in values that represent the X, Y, and Z directions relative to the coordinate system specified from a reference point (see below). The location of the offset point (1) relative to the reference point (2) is determined by the coordinate system (3) selected and the orientation of that coordinate system. The origin of the coordinate system has no effect on the offset.

Z Y X

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Point Constructor Options

C

Cylindrical Offset This option allows an offset point (1) to be specified by keying in cylindrical coordinates. The offset values for Radius (2), Angle (3), and Delta-ZC (4) are defined relative to the specified coordinate system and applied as illustrated below. The radius and the angle always lie in the X-Y plane of the coordinate system specified. A cylindrical offset may reference either the absolute coordinate system or the work coordinate system.

ZC YC XC

Spherical Offset This option allows specification of an offset position using spherical coordinates, two angles and a radius (see below). Angle 1 always lies in the X-Y plane, and Angle 2 defines the elevation of the offset point from the X-Y plane. The radius defines the distance between the base point and the offset point. A spherical offset may reference either the work coordinate system or the absolute coordinate system.

Z Y X

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C-13

Point Constructor Options

C

Vector Offset This option allows specification of an offset point (1) by indicating a direction and distance (2). A vector (3) is defined by selecting a line (4). The direction of that vector is determined by which end of the line is selected.

Z Y X

Offset Along Curve This option allows an offset point (1) to be defined along a curve by a specified arc length distance or a percentage of the total curve path length.

The direction of the offset is determined by the where the curve is selected relative to reference point. In the example below, the reference point (1) is in the middle of the curve. Selecting the curve at position (2) to produce direction (3) and selecting at position (4) to produces direction (5).

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Appendix

D Customer Defaults

D

Overview There are utilities and customization files which affect the default interface and behavior of NX. This appendix covers these topics which would normally be the responsibility of a system administrator.

©UGS Corporation, All Rights Reserved

Practical Applications of NX

D-1

Customer Defaults

Customer Defaults Customer defaults are accessed by choosing File→Utilities→Customer Defaults.

D

When NX is first started (out-of-the-box) the defaults are set to User and a variable points to a user file which may or may not exist. This is an extract from the log file for a user named “nxuser” after logging in and starting NX for the first time: Processing customer default values file C:/Documents and Settings/nxuser /Local Settings/Application Data/Unigraphics Solutions /NX4/nx4_user.dpv User customizations file C:/Documents and Settings/nxuser /Local Settings/Application Data/Unigraphics Solutions /NX4/nx4_user.dpv does not exist

The fact that the file does not exist is of no concern because the path is writable for the person logged in. NX will create the file nx4_user.dpv when and if the user makes a change to the defaults. If the administrator wishes to prevent the user from changing the defaults, i.e., set them as User (Read Only), there are various ways to accomplish it:

D-2

•

Create the file and customize it as you wish, and then make it read only.

•

Define the file in a path to which the user cannot write. The file and the path need not exist.

•

Lock one or more defaults at a higher level, i.e. group or site level.

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Customer Defaults

Customer Defaults Levels There are three levels of defaults that your system administrator can set. These are site, group, and user. Any of all of these levels may be read-write, although it is customary to set the site and group levels to read only.

At the Site and Group levels the dialog displays padlocks beside each default, enabling the administrator to lock out a particular default for lower levels. When a lock is active not only is the text de-emphasized but value change is prohibited. Even if the site (or a lower) DPV file is writable the value of a locked default can not be changed until the lock icon has been toggled off for the given default).

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Practical Applications of NX

D-3

D

Customer Defaults

For example, to lock out the ability to create promotions, the administrator clicks the lock beside promotions at the site or group level. The icon changes color and the text is de-emphasized.

D

At the user level, that default is de-emphasized an a padlock is displayed beside it.

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Customer Defaults

The system administrator can use the Default Lock Status to set the global locked status for all of the customer defaults on all defaults pages. This allows strategies like All are locked except..." or All are unlocked except... instead of requiring the assertion of 5000+ individual locks.

Locks at the group level change color and the text is de-emphasized. The user then sees all options for Site Standards de-emphasized and padlocked. No Site Standards may now may be changed at the user level.

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D-5

D

Customer Defaults

Setting Customer Defaults Customer defaults have as-shipped default settings that are hard-coded. When you change defaults at any level (assuming you have write permission and the levels are defined) a file is created to save the settings. By default the file is called nx4_user.dpv, nx4_group.dpv, or nx4_site.dpv.

D

Only the defaults that are changed from the hard–coded settings are saved, thus the DPV files can be very small in size. Customer defaults files are defined by environment settings. These are typically set in ugii_env.dat on Windows systems or .ugii_env on UNIX; however, the administrator may prevent a user from spoofing these settings by creating a file named ugii_env.master in the UGII directory where NX is installed to define these particular environment settings. When this file exists any attempt to redefine the environment variables will be ignored. When you change defaults the changes are NOT effective immediately. They will be in effect the next time NX is started.

D-6

Practical Applications of NX

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mt10050_g NX 4

Customer Defaults

There are two possible settings for the user level and one each for the group and site levels: Variable Defaults File Heading

Description

UGII_LOCAL_USER_DEFAULTS MISCELLANEOUS

This variable is a fully qualified file specification: it can be any file name in any location. The recommended file extension is .dpv The file need not exist. The file will be created when the initial customizations are saved. The directory path must exist and be writeable to create the file.

UGII_USER_DIR UGALLIANCE Variables

This directory pointed to must have the startup directory defined in structure outlined below. The file nx4_user.dpv will be created when the initial customizations are saved (if it does not already exist) in the startup folder. Define this ONLY if UGII_LOCAL _USER_DEFAULTS is NOT defined.

UGII_GROUP_DIR Not defined

The file nx4_group.dpv will be created when the initial customizations are saved (if it does not already exist) in the startup folder under the directory pointed to.

UGII_SITE_DIR UGALLIANCE Variables

The file nx4_site.dpv will be created when the initial customizations are saved (if it does not already exist) in the startup folder under the directory pointed to.

©UGS Corporation, All Rights Reserved

Practical Applications of NX

D-7

D

Customer Defaults

USER, GROUP, and SITE directories There is a standard structure for customer site installation of menu files and shared libraries. This directory structure defines three subdirectories. For the purpose of this discussion only the startup folder need exist; however, you might encounter the others if you have site customization.

D

D-8

startup

Contains site-specific menu files, defaults files, and shared libraries of menu actions to be loaded automatically at NX startup to customize Gateway.

application

Contains site-specific files defining menus and shared libraries of menu actions for customizing NX or third-party applications, such as NX Open programs. Loading of each shared library is deferred until you enter the application that names the library on the LIBRARIES statement in the menu file definition for the Application Button for the application. User Tool Definition files, GRIP programs, User Function programs that are referenced by menu file actions.

udo

Contains the shared libraries defining methods for site-specific User Defined Objects (another NX Open topic.)

Practical Applications of NX

©UGS Corporation, All Rights Reserved

mt10050_g NX 4

Customer Defaults

Managing Your Changes The DPV files contain only the defaults that are changed from the hard–coded settings. You may review your changes at any time: •

Set the Defaults Level to the level you want to examine, Site, Group, or User.

•

Choose Manage Current Settings on the Customer Defaults dialog.

Here is an example of standard classroom defaults at the group level:

Here is an example of defaults additionally set for Design Applications using NX.

©UGS Corporation, All Rights Reserved

Practical Applications of NX

D-9

D

Customer Defaults

Updating to a New Release of NX To update to a new release, you need only define the DPV files you want to use at whatever levels your organization uses.

D

When you receive the new software use Import Defaults to validate your previous settings against the new release. Importing Customer Defaults values file: file.> Total settings and locks imported:


10

Total settings rejected due to values not valid in this release:

0

Total settings rejected due to values being locked at the higher level: Total settings already set to the same value and lock status: Total settings not recognized in this release:

D-10

Practical Applications of NX

0

0

0

©UGS Corporation, All Rights Reserved

mt10050_g NX 4

Index

A Absolute Coordinate System Alignment Lines . . . . . . . . Analysis Distance . . . . . . . . . . . . . Mass Properties . . . . . . . Annotation preferences . . . . . . . . . . . Annotation Editor . . . . . . . Applications Gateway . . . . . . . . . . . . . Assemblies Selecting Components . . . Assemblies Application . . . Assembly . . . . . . . . . . . . . . Add Components . . . . . . Assembly Concepts . . . . . . Assembly Navigator . . . . . . Pop-Up Menu . . . . . . . . .

. . . . . . 3-3 . . . . . 13-22

DPV . . . . . . . Files . . . . . . . Setting Levels Cylinder . . . . .

. . . . . . 9-11 . . . . . . 9-12

D

. . . . . 18-47 . . . . . 18-67 . . . . . . . 1-3 . . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . .

10-15 11-4 10-2 11-7 11-2 10-10 10-21

B Block . . . . . . . . . . . . Boolean Operations . Errors . . . . . . . . . Boss . . . . . . . . . . . . Bottom-Up Modeling

. . . . .

. . . . .

. . . . .

. . . . .

. . . . .

. . . . .

. . . . .

. . . . .

. . . . .

. . . . .

. . 4-3 . 14-9 14-11 . . 5-7 . 11-2

Chamfer . . . . . . . . . . . . Change Displayed Part . Coordinate System . . . . . Absolute . . . . . . . . . . . WCS . . . . . . . . . . . . . . CSYS Constructor dialog Cue line . . . . . . . . . . . . . Customer Defaults Directory Structures . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

C 8-10 . 1-9 . 3-2 . 3-3 . 3-3 . 3-4 . 1-4

. . . . . . . . . D-8

©UGS Corporation, All Rights Reserved

... ... .. ...

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . . D-6 D-3, D-6 . . . . D-3 . . . . 4-7

Datum Axis . . . . . . . . . . . . . . . . . 12-37 Deleting . . . . . . . . . . . . . . . . . . 12-43 Editing . . . . . . . . . . . . . . . . . . . 12-43 Intersection of 2 Faces . . . . . . . 12-42 Through Cylindrical Face Axis . . 12-41 Through Edge or Curve . . . . . . 12-40 Through Two Points . . . . . . . . . 12-39 Datum CSYS . . . . . . . . . . . . . . . . 12-51 Datum Features . . . . . . . . . . . . . . . 12-2 Datum Plane . . . . . . . . . . . . . . . . . 12-3 Angle to Face Thru Edge . . . . . . 12-10 Center . . . . . . . . . . . . . . . . . . . . 12-8 Deleting . . . . . . . . . . . . . . . . . . 12-21 Offset at a Distance . . . . . . . . . . 12-7 Point and Direction . . . . . . . . . . 12-15 Relative . . . . . . . . . . . . . . . . . . . 12-3 Tangent to Cylindrical Face . . . . . . . . . . . . . 12-11–12-12 Through a Point on Curve . . . . . 12-14 Through Cylindrical Axis . . . . . . 12-9 Through Three Points . . . . . . . . 12-13 Delay Evaluation . . . . . . . . . . . . . 13-57 Delayed Update after Edit . . . . . . 15-21 Delete Feature . . . . . . . . . . . . . . . . 15-7 Density . . . . . . . . . . . . . . . . . . . . . 9-12 Design in Context . . . . . . . . . . . . 10-17 Dimensions creating . . . . . . . . . . . . . . . . . . 18-45 Displayed Part . . . . . . . . . . . . . . . 10-17 Distance between objects . . . . . . . . 9-11 DOF . . . . . . . . . . . . . . . . . . . . . . 13-46 Drafting Application . . . . . . . . . . . 18-2 Practical Applications of NX

Index-1

Index

Drawings adding a base view . . . adding projected views creating new sheets . . deleting . . . . . . . . . . . deleting views . . . . . . . editing . . . . . . . . . . . . editing views . . . . . . . opening . . . . . . . . . . . view preferences . . . . .

I . . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . .

18-21 18-24 18-3 18-7 18-27 18-5 18-26 18-4 18-17

Infer Constraint Settings Information . . . . . . . . . . Feature . . . . . . . . . . . Instance . . . . . . . . . . . . Circular . . . . . . . . . . . Rectangular . . . . . . . . Intersect . . . . . . . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . . . .

. . . . .

13-21 . 9-9 5-48 16-2 16-4 16-3 14-10

. 9-3 . 9-7 10-4 10-7 10-5 10-6

L E Edge Blend . . . . . . . . . . . . . . Edit Parameters . . . . . . . . . . . . . Positioning . . . . . . . . . . . . . with Rollback . . . . . . . . . . . Editing Features . . . . . . . . . . Evaluate Sketch . . . . . . . . . . Exit NX . . . . . . . . . . . . . . . . . Expressions Dialog with less options . . . Dialog with more options . . Editing . . . . . . . . . . . . . . . . functions . . . . . . . . . . . . . . List Referencers . . . . . . . . . List References . . . . . . . . . . operators . . . . . . . . . . . . . . precedence and associativity Extrude . . . . . . . . . . . . . . . . . Draft . . . . . . . . . . . . . . . . . Offset . . . . . . . . . . . . . . . . .

. . . . . 8-3 . . . . . .

. . . . . .

. . . . . .

. . . .

5-37 5-38 5-37 15-2 13-57 . 1-16

. . . . . . . . . . .

. . . . . . . . . . .

. . . . . . . . . . .

. . . . . . . . .

. . . . . . . .

6-3 6-4 6-5 B-5 6-6 9-9 B-2 B-3 14-3 14-16 14-14

F Feature Coordinate System . . . . . . . 5-3 Form Features . . . . . . . . . . . . . . . . . 5-2 G Gateway Application . . . . . . . . . . . . 1-3 H Hole . . . . . . . . . . . . . . . . . . . . . . . . 5-5 Index-2

Practical Applications of NX

Layers . . . . . . . . Moving Layers Load Options . . . Load Failure . . Load Method . Load States . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

Make Current Feature Mass Properties . . . . . Master Model . . . . . . Mating Conditions . . . Align . . . . . . . . . . . Angle . . . . . . . . . . . Center . . . . . . . . . . Distance . . . . . . . . . Mate . . . . . . . . . . . Parallel . . . . . . . . . Perpendicular . . . . . Tangent . . . . . . . . . Vary Constraint . . . Mouse Buttons . . . . . . Mouse Pop-Up Menu . Display Mode . . . . . Fit . . . . . . . . . . . . . Orient View . . . . . . Pan . . . . . . . . . . . . Refresh . . . . . . . . . Rotate . . . . . . . . . . Set Rotate Point . . . Undo . . . . . . . . . . . Zoom . . . . . . . . . . . Move Feature . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . . . . . . . . . .

. 15-4 . 9-12 . 17-2 11-12 11-14 11-15 11-18 11-20 11-13 11-16 11-17 11-21 11-23 . 2-14 . 2-15 . 2-16 . 2-16 . 2-16 . 2-16 . 2-16 . 2-16 . 2-16 . 2-16 . 2-16 15-22

M

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mt10050_g NX 4

Index

N Notes and Labels annotation editor . . . . . . . . . . . 18-67 O Opening Parts . . . . . . . . . . . . . . . . . 1-9 P Pad . . . . . . . . . . . . . . . . Parameter Entry Options Formula . . . . . . . . . . . Part Change Displayed . . . . Close . . . . . . . . . . . . . Create . . . . . . . . . . . . Open . . . . . . . . . . . . . Save As . . . . . . . . . . . Part Navigator . . . . . . . . Placement Face . . . . . . . Pocket . . . . . . . . . . . . . . Point Constructor dialog Positioning Edit Add Dimension . . Delete Dimension . Edit Dimension . . . . . Form Features . . . . . . Positioning Methods Angular . . . . . . . . . . . Horizontal . . . . . . . . . Line onto Line . . . . . . Parallel . . . . . . . . . . . Parallel at a Distance . Perpendicular . . . . . . . Point onto Line . . . . . . Point onto Point . . . . . Vertical . . . . . . . . . . . Preferences Annotation . . . . . . . . . view . . . . . . . . . . . . . . Preview Selection . . . . . .

. . . . . . . . 5-24 . . . . . . . . 5-28 . . . . . . . . . 6-6

Quick Trim . . . . . . . . . . . . . . . . . 13-34 QuickPick . . . . . . . . . . . . . . . . . . . 2-21 R Reattach a Feature . . . . . . . . . . Reference Direction . . . . . . . . . . Reference Features . . . . . . . . . . Datum CSYS . . . . . . . . . . . . . Referencing Existing Parameters Reposition Component . . . . . . . . Revolve . . . . . . . . . . . . . . . . . . .

. . . . . . .

15-23 . . 5-2 . 12-2 12-51 . 5-28 11-30 14-36

S . . . . . . . . .

. . . . . . . . 1-9 . . . . . . . 1-14 . . . . . . . . 1-7 . . . . . . . 1-10 . . . . . . . 1-12 5-42, 9-8, 15-3 . . . . . . . . 5-2 . . . . . . . 5-23 . . . . . . . . 3-7

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

5-39 5-40 5-40 . 5-3

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

5-27 . 5-9 5-26 5-11 5-25 5-10 5-10 5-11 . 5-9

. . . . . . . 18-47 . . . . . . . 18-17 . . . . . . . . 2-21

Q Quick Extend . . . . . . . . . . . . . . . . 13-36 ©UGS Corporation, All Rights Reserved

Selection Preview . . . . . . . . . . . . . . QuickPick . . . . . . . . . . . . . Selection Intent curve/edge rules . . . . . . . . Edges . . . . . . . . . . . . . . . . Faces . . . . . . . . . . . . . . . . Follow Fillet . . . . . . . . . . . selecting sketches . . . . . . . Stop at Intersection . . . . . Shell . . . . . . . . . . . . . . . . . . Show/Remove Constraints . . Sketch Constraining . . . . . . . . . . Constraints . . . . . . . . . . . Convert To/From Reference Creating . . . . . . . . . . . . . . Curve Creation . . . . . . . . . Arc . . . . . . . . . . . . . . Circle . . . . . . . . . . . . . Fillets . . . . . . . . . . . . Line . . . . . . . . . . . . . . Profile . . . . . . . . . . . . Dimensions . . . . . . . . . . . Editing . . . . . . . . . . . Types . . . . . . . . . . . . . Naming . . . . . . . . . . . . . . Overview . . . . . . . . . . . . . Reference Direction . . . . . Show/Remove Constraints Text Height . . . . . . . . . . . Sketch Points . . . . . . . . . . . .

. . . . . 2-21 . . . . . 2-21 . . . . . . . .

. . . . . . . .

. . . . . . . .

. . . . . . . .

14-22 . . 8-5 . . 7-4 14-23 . 14-4 14-23 . . 7-2 13-66

. . . . 13-48 . . . . 13-63 . . . . 13-92 13-8, 13-13 . . . . 13-21 . . . . 13-26 . . . . 13-27 . . . . 13-33 . . . . 13-24 . . . . 13-23 . . . . 13-48 . . . . 13-57 . . . . 13-51 . . . . 13-11 . . . . . 13-2 . . . . 13-10 . . . . 13-66 . . . . 13-50 . . . . 13-46

Practical Applications of NX

Index-3

Index

Slot . . . . . . . . . . . . . . positioning . . . . . . . Snap Angle . . . . . . . . Snap Point toolbar . . . Starting NX . . . . . . . . Status Line . . . . . . . . Subassembly . . . . . . . Subtract . . . . . . . . . . Sweep Along Guide . . Symbols utility symbols . . . . linear centerline

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. . . . . . . . .

. 5-21 . 5-22 13-22 . . 3-6 . . 1-2 . . 1-4 . 10-2 14-10 14-27

. . . . . . . . . 18-33 . . . . . . . . . 18-36

T Toolbars . . . . . . . . Assemblies . . . . . Customizing . . . . Selection . . . . . . Snap Point . . . . . Top-Down Modeling

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . . . . . 2-2 . . . . . 11-6 . . . . . . 2-3 2-19, 10-16 . . . . . . 3-6 . . . . . 11-2

Update Failures . . . . . . Update Model . . . . . . . Utility Symbols . . . . . . cylindrical centerline linear centerline . . . .

. . . . .

. . . . .

. . . . .

. . . . . . 15-8 13-57, 15-21 . . . . . 18-33 . . . . . 18-40 . . . . . 18-36

V Vectors . . . . . . . . . . . . . View Preferences . . . . . . Edges Hidden by Edges Hidden Lines . . . . . . . Smooth Edges . . . . . . . Virtual Intersections . .

... ... .. ... ... ...

. . . . . .

. . . . . .

. . . . . .

. . . . . .

. . 4-8 18-17 18-18 18-18 18-19 18-20

. . . .

. . . .

. . . .

. . . .

. . . .

. . 3-3 . . 3-5 . . 3-5 10-19

W WCS . . . . . Dynamics Move . . . Work Part .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

. . . .

U Unite . . . . . . . . . . . . . . . . . . . . . . 14-10

Index-4

Practical Applications of NX

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mt10050_g NX 4

UGS Education Services offers a blend of training solutions for all of our product lifecycle management products. Our Online Store “Learning Advantage” was developed to provide our customers with “just in time” training for the latest in application developments. Here are some of the Learning Advantages: • Customers have direct access • Self-paced course layout • Online Assessments • Just in time training for the latest release

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Types of products/parts/data that you work with Reason for training Please verify/add to this list of training for Unigraphics, I-deas, Imageware, Teamcenter Mfg., Teamcenter Eng. (I-Man), Teamcenter Enterprise (Metaphase), or Dimensional Mgmt./Visualization. Medium means Instructor-lead (IL), On-line (OL), or Self-paced (SP)

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Practical Applications of NX Course Agenda Monday

Morning • Introduction & Overview • Lesson 1. Getting Started • Lesson 2. The NX User Interface Afternoon • Lesson 3. • Lesson 4. • Lesson 5. • Lesson 6.

Tuesday

Coordinate Systems Introduction to Solid Modeling Positional Form Features Expressions

Morning • • • •

Lesson 7. Shell Lesson 8. Edge Operations Workbook Project Description & Section 1 Rear Differential Modeling Lesson 9. Model Construction Query

Afternoon • Lesson 10. Introduction to Assemblies • Lesson 11. Adding Components & Mating Conditions • Workbook Section 2 Rear Differential Assembly Wednesday

Morning • Lesson 12. Datum Features • Workbook Section 3 Rear Axle Modeling and Assembly • Workbook Section 4 Left Pinion Modeling and Assembly Afternoon • Lesson 13.

Thursday

Sketching

Morning • Lesson 14. Swept Features and Boolean Operations • Workbook Section 5 Power Pack Sketching • Workbook Section 6 Rear Drive Gear Modeling Afternoon • Workbook Section 7 Part and Assembly Editing • Lesson 15. Editing the Model • Lesson 16. Instance Arrays • Workbook Section 8 Rear Drive Gear Completion

Friday

Morning • Workbook Section 9 Assembly Completion • Lesson 17. The Master Model • Lesson 18. Introduction to Drafting Afternoon • Workbook Section 10

Rear Differential Drafting

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Accelerators The following Accelerators can be listed from within an NX session by choosing Information→Custom Menubar→Accelerators. Function File→New... File→Open... File→Save File→Save As... File→Plot... File→Execute→Grip... File→Execute→Debug Grip... File→Execute→NX Open... Edit→Undo Edit→Cut Edit→Copy Edit-Paste Edit→Delete... Edit→Selection→Top Selection Priority - Feature Edit→Selection→Top Selection Priority - Face Edit→Selection→Top Selection Priority - Body Edit→Selection→Top Selection Priority - Edge Edit→Selection→Top Selection Priority - Component Edit→Selection-Select All Edit→Blank→Blank... Edit→Blank→Reverse Blank All Edit→Blank→Unblank Selected... Edit→Blank→Unblank All of Part Edit→Transform... Edit→Object Display... View→Operation→Zoom... View→Operation→Rotate... View→Operation→Section... View→Layout→New... View→Layout→Open... View→Layout→Fit All Views View→Visualization→High Quality Image... View→Information Window View→Current Dialog View→Reset Orientation Insert→Sketch... Insert→Design Feature→Extrude... Insert→Design Feature→Revolve... Insert→Trim→Trimmed Sheet...

Accelerator Ctrl+N Ctrl+O Ctrl+S Ctrl+Shift+A Ctrl+P Ctrl+G Ctrl+Shift+G Ctrl+U Ctrl+Z Ctrl+X Ctrl+C Ctrl+V Ctrl+D or Delete F G B E C Ctrl+A Ctrl+B Ctrl+Shift+B Ctrl+Shift+K Ctrl+Shift+U Ctrl+T Ctrl+J Ctrl+Shift+Z Ctrl+R Ctrl+H Ctrl+Shift+N Ctrl+Shift+O Ctrl+Shift+F Ctrl+Shift+H F4 F3 Ctrl+F8 S X R T

Insert→Sweep→Variational Sweep... Format→Layer Settings... Format→Visible in View... Format→WCS→Display Tools→Expression... Tools→Journal→Play... Tools→Journal→Edit Tools→Macro→Start Record... Tools→Macro→Playback... Tools→Macro→Step... Information→Object... Analysis→Curve→Refresh Curvature Graphs Preferences→Object... Preferences→Selection... Start→Modeling... Start→All Applications→Shape Studio... Start→Drafting... Start→Manufacturing... Start→NX Sheet Metal... Start→Assemblies Start→Gateway... Help→On Context... Refresh Fit Zoom Rotate Orient View-Trimetric Orient View-Isometric Orient View-Top Orient View-Front Orient View-Right Orient View-Left Snap View

V Ctrl+L Ctrl+Shift+V W Ctrl+E Alt+F8 Alt+F11 Ctrl+Shift+R Ctrl+Shift+P Ctrl+Shift+S Ctrl+I Ctrl+Shift+C Ctrl+Shift+J Ctrl+Shift+T M or Ctrl+M Ctrl+Alt+S Ctrl+Shift+D Ctrl+Alt+M Ctrl+Alt+N A Ctrl+W F1 F5 Ctrl+F F6 F7 Home End Ctrl+Alt+T Ctrl+Alt+F Ctrl+Alt+R Ctrl+Alt+L F8

Evaluation – Delivery NX 4 PAU, Course #MT10050 Dates

thru

1. 2. 3. 4. 5. 6. 7. 8. 9. 10. 11. 12.

STRONGLY AGREE

7

AGREE

Instructor:

SOMEWHAT AGREE

If there were 2 instructors, please evaluate the 2nd instructor with “X’s”

SOMEWHAT DISAGREE

5

DISAGREE

Instructor:

STRONGLY DISAGREE

Please share your opinion in all of the following sections with a “check” in the appropriate box:

…clearly explained the course objectives …was knowledgeable about the subject …answered my questions appropriately … encouraged questions in class …was well spoken and a good communicator …was well prepared to deliver the course …made good use of the training time …conducted themselves professionally …used examples relevant to the course and audience …provided enough time to complete the exercises …used review and summary to emphasize important information …did all they could to help the class meet the course objectives

Comments on overall impression of instructor(s): Overall impression of instructor(s)

Poor

Excellent

Suggestions for improvement of course delivery:

What you liked best about the course delivery:

Class Logistics: 1.

The training facilities were comfortable, clean, and provided a good learning environment 2. The computer equipment was reliable 3. The software performed properly 4. The overhead projection unit was clear and working properly 5. The registration and confirmation process was efficient Hotels: (We try to leverage this information to better accommodate our customers) Best hotel I’ve stayed at

1.

Name of the hotel

2.

Was this hotel recommended during your registration process?

3.

Problem? (brief description)

YES

NO

SEE BACK

Evaluation - Courseware NX 4 PAU, Course #MT10050

The training material supported the course and lesson objectives The training material contained all topics needed to complete the projects The training material provided clear and descriptive directions The training material was easy to read and understand The course flowed in a logical and meaningful manner

6.

How appropriate was the length of the course relative to the material?

Too short

Too long

STRONGLY AGREE

AGREE

SOMEWHAT AGREE

SOMEWHAT DISAGREE

Material: 1. 2. 3. 4. 5.

DISAGREE

Please share your opinion for all of the following sections with a “check” in the appropriate box

STRONGLY DISAGREE

:

Just right

Comments on Course and Material:

Overall impression of course

Poor

Student: 1. 2. 3. 4. 5.

I met the prerequisites for the class (I had the skills I needed) My objectives were consistent with the course objectives I will be able to use the skills I have learned on my job My expectations for this course were met I am confident that with practice I will become proficient

Name (optional):

Location/room

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Thank you for your business. We hope to continue to provide your training and personal development for the future.

Excellent