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Pro/ENGINEER Tutorials

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Pro/ENGINEER Tutorial Neutral Plane Drafts Advanced Drawing Tips and Tricks Top 20 Ways to Make Pro/E Easier to Use BMX Changing View display in Drawings Component Display Options Cross Sections Design Animation Drip/Stress loops: Cabling and Piping Pro/ECAD http://www.ptc-mss.com/Tutorial/proe_tutorial.htm (1 of 2) [28.11.2002 12:59:30]

Photorender - 1, 2 Pro/ENGINEER 2001 Details Pro/ENGINEER 2001 Update Pro/ENGINEER 2001 Drawing Cheat-Sheet Pro/ENGINEER Model Player Pro/PLASTIC-ADVISOR Pro/Process for Assemblies Pro/Program Relational Patterns

Pro/ENGINEER Tutorials

Explode States Instrumenting Your Design Innovation Days - Tips & Tricks Import Data Doctor Layers Linear Holes Mapkeys Mapkey Hotkeys Mass Properties Mechanism Design Option - 1 , 2, Mechanism Connections: Cam Modelcheck ModelCHECK Guide Mold Design

Resolve Mode Setup Units Simple Extruded Protrusion Simplified Rep.'s Simulating Gears in Pro/ENGINEER Shared Data in Pro/ENGINEER Sheetmetal - Cheat Sheet Sheetmetal: Tips/Tricks Sheetmetal: Basic Creation Sheetmetal: Packaging Shrinkwrap Sketcher Cheat Sheet - 2000i2 Sketcher Cheat Sheet - 2001 Surfacing Transform

Feedback - Search - Escalation Procedures - Pro/COLLABORATE Tutorials | Tips & Tech. | Tech. Support | Misc. Support | FAQ | PTC USER Area User Groups | PTC Products | Documentation | Training | News & Events | Customer Care Zone Last modified: October 27, 2002

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Homepage

Advanced Drawing Help Guide

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Index

Advanced Drawing News in 2000i² and 2001 • Drawing Templates •Hole Charts • True type fonts •Views • Usability Improvements • Standard support

Drawing Views • Valid View Type Menu Combinations • Drawing Views • Draft views • Different types of CrossSectional Views • Troubleshooting Incomplete or Incorrect CrossSection Views • Modifying Cosmetic Thread Display

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Index • Tips & Tricks

Working with Detail Items • Dimensions • Notes • Using True Type Fonts

Tolerances • Dimensional Tolerances • Creating Geometric Tolerances • Modifying Geometric Tolerances

Symbols • Creating a Generic Symbol

Frames, Tables and Boms • Creating a New Sized Format from an Existing Format • Using Parameters in Formats

Large Assembly Drawings • Config Options • Assembly Manipulation

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Index Techniques • Increasing Performance when Working with Large Assembly Drawings • Tips & Tricks

Additional Ideas? Write the Author

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Introduction to Pro/ENGINEER

News in 2000i²

Drawing Templates You can create drawing templates that help you create drawings automatically with the new drawing templates. Use them to define the layout of views, set view display, place notes, define tables, create snap lines, and show dimensions. You can create customized drawing templates for different types of drawings. For example, you could create a template for a machined part versus a cast part. The machine part template could define the views that are typically placed, set the view display of each view (that is, show hidden lines), place company standard machining notes, and automatically create snap lines for placing dimensions. Drawing templates are used when creating a drawing and automatically create the views, set the desired view display, create snap lines, and show model dimensions based on the template. The drawing templates improve efficiency and productivity by allowing you to create portions of drawings automatically. Procedure 1. Click File > New. The New dialog box opens. 2. Click Drawing, and then type the name of the template you are creating or accept the default. 3. Clear the Use default template checkbox, and then click OK. The New Drawing dialog box opens. 4. Click Empty or Empty with format, and then specify the orientation of the template by clicking Portrait, Landscape, or Variable. 5. Specify the size of the template, and then click OK. 6. In the Applications menu, click Template to enter Drawing template mode, and then click Views > Add Template. The Template View Instructions dialog box opens. 7. Type the View Name or accept the default, and then specify the View Orientation. 8. In the Model "Saved View Name text box, orient the view. 9. Specify view options and view values in the View Options and View Values areas. 10. Click Place View and select the location of the General view. Note: After you place the view, you now have the options to move the symbol, edit the view http://www.ptc-mss.com/Tutorial/Advdraw_site/News_2000i2/News_2000i2.html (1 of 7) [28.11.2002 13:00:06]

Introduction to Pro/ENGINEER

symbol, or to replace the view symbol. 11. To place additional views, click New, type the new view name, and orient the new view. Specify the view options and view values of the new view. 12. When you are done placing all of the desired views, click OK. Save the template.

Hole Charts You can now automatically create hole charts that relate to drawings. In addition, you can create tables for axes and datum points. This new functionality automatically creates a table for drillable hole features in a specified view. Hole charts includes: ●

Location in x and y coordinates (z for datum points)

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Hole diameter

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Sorting (x, y, Size)

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Ability to add additional columns for user-defined parameters

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ISO or ASME style hole labels (numbers versus alphanumeric)

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Ability to paginate tables

You can automatically create hole charts for a specified view increasing your productivity and efficiency within the drawing environment. Tip: Be aware that cuts are not added to the hole table. In case you have cuts in your part you can create a hole table with axis. You can also edit the hole table.

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Introduction to Pro/ENGINEER

Improved True Type Font Usability You can specify a font directory with the new config.pro option, pro_font_dir. All fonts in this directory automatically appear in the pull down lists inside dialog boxes. Previously, each font had to be specified using the aux_font detail setup option for it to appear in text font lists. pro_font_dir adds convenience and control when setting up additional fonts within Pro/ENGINEER.

Alignment of General Views You can now align general views to each other. Sometimes you may want to create several general views to annotate a model. You now have the ability to align these general views and have them move together the same way a projected view moves with its parent view.

Improvements to Broken Views Several major improvements were made to broken views. These include the ability to: ❍

Create projected broken views.

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Add and remove breaks from a broken view.

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Use standard break lines include S-curve and heartbeat.

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Introduction to Pro/ENGINEER

You now have the ability to create projected views of a broken view maintaining the same break points between the two views. You can now remove breaks from a broken view. Prior to Release 2000i2, the broken views would have been deleted and then re-created if a break had to be removed. In Release 2000i2, you can add and remove breaks. The S-curve and heartbeat standard break lines are now available when creating broken views. You can sketch your own break line or use one of these standard break lines to save time.

Usability Improvements ●

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New tool for navigating through sheets ❍ A new toolbar icon has been added to navigate through multi-sheet drawings. This new icon removes the need to enter the menus to change to a different drawing sheet reducing menu picks and mouse travel. Ability to modify multiple columns and rows sizes in a table at one time ❍ Multiple rows or columns can now be selected when modifying row/column size. Access to saved cross-hatching patterns for cosmetic features in drawing views ❍ Additional functionality for cross-hatched cosmetic features is now available in drawing mode when modifying cross-hatching. It is now possible to retrieve saved cross-hatch patterns from disk and to modify the cross-hatch line style. New parameter to show the scale of individual views ❍ A new parameter has been introduced that allows the scale of an individual view to be specified. The syntax is scale_of_view_x, where x is the view name. Move has been enabled for set datums attached to dimensions ❍ It is now possible to modify the location of a set datum attached to a dimension using the Move command. Set datums attached to cylindrical surfaces ❍ It is now possible to attach a set datum directly to a cylindrical surface. Improved Control over the Size of Basic Dimension Boxes ❍ Additional text can now be displayed inside or outside of the Basic dimension box by specifying the start and end points of the box.

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Introduction to Pro/ENGINEER ●

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Unordered datum references for geometric tolerances ❍ A new option has been provided for geometric tolerances. The option allows geometric tolerances to have unordered datum references. Limit dimension tolerances listed horizontally for parallel text ❍ When using parallel dimension text orientation, limit tolerances will be listed next to each other instead of stacked on top of each other. New filter for disallowing selection of hidden lines in no-hidden views ❍ A new filter has been created to prevent hidden lines from being selected in no-hidden views. Hidden lines will not be selected when this filter is enabled using the detail setup option select_hidden_edges_in_dwg. Enhanced diagnostics when view reference point is missing ❍ New messages will appear when the reference point for a view is missing. The new messages will indicate the view name with the missing reference point. Improved Symbol user interface for placing many symbols ❍ A new repeat button has been added to the symbol dialog box for quickly placing another symbol using the same definition. In addition, changes have been made to the symbol dialog box to allow a new symbol to be created based on an existing one. When an existing symbol is selected using Modify, all options are now available allowing a new one to be created and saved. Select many for axes ❍ Multiple selection has been enabled for selecting many axes at one time. Fractions no longer applied to metric dimensions ❍ Fractions will not be applied to metric dimensions when using dual dimensioning. Erasing of angular witness lines and arrow style modification ❍ Witness lines for angular dimensions can now be erased. This allows angular witness lines to be erased to improve clarity when placing many angular dimensions that share the same witness lines. In addition, the arrow style of angular dimensions can be modified. New option for setting default behavior for show/erase ❍ A new detail setup option has been introduced to specify the default behavior for show/erase. This new option, show_preview_default, allows the default behavior of Select to Keep or Select to Remove to be specified. Note that this option has also been made available in later builds of 2000i. Snap line support for view arrows and clipped dimensions

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Introduction to Pro/ENGINEER ❍

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View arrows and clipped dimensions can be placed on view snap lines. Cross-section view arrows, projection view arrows, and clipped dimensions are now supported by snap lines. This improves control over the placement of these items on drawing views.

Improved highlighting when unblanking members in a drawing view ❍ When unblanking blanked members using member display, you can select the view for highlighting the blanked members. This improves user efficiency by allowing only members in the desired view to be highlighted instead of all views on the sheet. Individual formatting of angular dimensions ❍ Individual angular dimensions can now be selected to set the format to degrees or Deg-MinSec. Automatic clipping of Diameter dims ❍ Diameter dimensions are now clipped automatically when the new detail setup option, clip_diam_dimensions, is set to yes. Diameter dimensions will be clipped when the reference geometry is located outside of the view border. Axes parallel to the screen can be selected as placement references ❍ Axes parallel to the screen can now be selected for placing geometric tolerances and notes. Improved UI for replacing tables in drawing formats ❍ All tables can now be removed in one action when replacing a drawing format. Improved interface for integrating drawings ❍ The user interface has been improved for integrating two different versions of a drawing. Multiple actions can now be applied to new classes of items to be integrated

Standard Support ●

Additional dimension display options

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Display stacked limit tolerances for Parallel Text

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Display metric as decimals with fraction display for dual dimensions (english/metric)

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Erase angular witness lines (and associated dimension arrows)

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User controlled sizing of Basic dimension text box

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Additional detailing attachment options

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Introduction to Pro/ENGINEER

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Allow Set Datum to be attached to cylindrical surface

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Allow Gtols and notes to be attached to axes parallel to screen

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Drawing Views

Drawing Views Valid View Type Menu Combinations

Drawing Views ●

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A general view is a view that is independent from other views in the drawing, and shown in the default orientation specified in the Pro/E environment A detailed view is a portion of a model shown in another view. Its orientation is the same as the view from which it is created, but its scale may be different so that you can better visualize the portion of the model that you are creating. The display of edges in a detailed view follows that of the view from which it is created (its parent view). A projection view is an orthographic projection of another view`s geometry along a horizontal or vertical direction. You can specify the projection type in the drawing setup file by basing it on third angle for ANSI (default) or first angle for DIN. An auxiliary view is a projection of the geometry of another view at right angles to a selected surface or along an axis. The selected surface in the parent view must be perpendicular to the plane of the screen. A revolved view is a planar area cross section from an existing view, revolved 90 degrees around the cutting plane projection, and offset along its length. It can be full, partial, exploded or unexploded. A graph view shows the sketch of a graph feature and its dimensions. The system updates any changes parametrically. An of flat ply view is a flat single-ply view of a composite model. It can exist in a regular drawing or in sequence drawings.

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Drawing Views ●

A copy & align view is an aligned partial view based on a specified view boundary and an alignment relative to the existing partial view.

Note: Detailed, projection, auxiliary, and revolved views have the same representation and explosion offsets, if any, as their parent views. You can simplify, restore, and modify the explosion distance of each view without affecting the parent view. However, detailed views always appear with the same explosion distances and geometry as their parent views.

Moving Views: If you move a view from which other views were projected (parent view), the projected views (children) also move to maintain view alignment. For example, if you move the top view horizontally, the front view also moves to maintain alignment because it was projected from the top view. Using the GET POINT menu, you can do exact drafting to place the view where you want it. For example, to exactly align one view with another general view, set the origin using Origin in the MODIFY VIEW menu and the GET POINT menu. This establishes a reference point for moving the view, so that you can easily place it anywhere on a drawing relative to another view.

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Drawing Views

If the configuration file option "allow_move_view_with_move" is set, DETAIL>Move moves the selected point on the view to the location that you specify by selecting a point. The GET POINT menu is not available.

Draft views Using the Draft View command in the TOOLS menu, you can set a drawing view to be the current draft view so the Pro/ENGINEER associates all new draft entities with that view. When you have associated draft entities with a drawing view, they move with the view when you move it, maintaining their location relative to that view. Also, when you scale the view or the drawing, the system scales all draft entities associated with a view by the same factor. The system uses the view scale of the current view when you create draft entities.

Different types of Cross-Sectional Views You can create a cross section in Part and Assembly modes and show it in a drawing or you can add it to a view in drawing mode while you are creating it. ●

A full cross section displays the whole view, whereas a local cross section shows a portion of the model within a closed boundary cross-sectioned, but not outside the closed boundary.

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A full & local cross section shows a full cross-sectional view with local cross sections.

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A half cross section shows a portion of the model on one side of a cutting plane, but not on the other side.

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A total cross section shows not only the cross-sectioned area, but the edges of the model that become visible when a cross section is made. An area cross section displays only the cross section without the geometry. An aligned cross section displays an area cross-sectional view that is unfolded around an axis, whereas a total aligned cross section shows an aligned cross section of a general, projection, auxiliary, or full view. An unfolded cross section shows a flattened area cross section of a general view, whereas a total unfolded cross section shows a total unfolded cross section of a general view.

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Drawing Views

Troubleshooting Incomplete or Incorrect Cross-Section Views When a cross-section view cannot be created in Drawing Mode, one of the following error messages may appear: ●

"Cross-section may be incomplete."

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"Cross-section could not be created."

During the creation of a cross-section view in Drawing Mode, Pro/ENGINEER performs an operation on the model analogous to a cut feature. Therefore, if the cross-section cutting plane intersects any "incorrect" geometry, the crosssection view may not be created successfully. In addition, if the cutting plane passes through a tangency point, unattached edge, or vertex either directly or by function of the model accuracy, the cross-section view will not be created. When a cross-section is made in Part or Assembly mode, it is simply a cosmetic which shows where the section lies in the model. Therefore, no error is given when a section is made through the previously mentioned entities. The following steps are recommended upon encountering an unsuccessful cross-sectional view in Drawing Mode.

Procedure 1. Be sure that the design intent of the model is clear by first verifying that no geometry checks exist within the model in areas where the cross-section intersects. This action is performed, by retrieving the model and selecting Info from the MAIN menu and Geom Check, if the selection is ungreyed. If available for selection, the information provided in the subsequent menus allows for precise resolutions to geometry issues, which could prevent a cross-section view from being created.

2. If the selection Geom Check is greyed out, create a cut feature in the model using the exact same placement references and geometry that were used to create the cross-section by selecting Feature, Create, Cut. When the cut feature fails, a "Failure Diagnostics" window will appear, along with an extensive amount of information concerning which feature and/or part the cut could not be made through. The cross-section should be redesigned to avoid the highlighted features, most effectively through offsetting from the intersecting edges or points until the cross- section view can be created successfully in Drawing Mode.

3. If the problem areas of the model for cross-section creation are still in question, a series of feature and/or part suppressions should be performed in the top-level model. If the drawing model is an assembly, select Component, Suppress from the main ASSEMBLY menu and suppress half of the assembly components. Change Window back to Drawing Mode and attempt to create the cross-sectional view. If the view creates http://www.ptc-mss.com/Tutorial/Advdraw_site/Drawing_views/Drawing_views.htm (4 of 12) [28.11.2002 13:00:31]

Drawing Views

successfully, the troublesome component is not active and will not interfere with the cross-section cut. If unsuccessful at creating the view, try suppressing the other half of the assembly and Component, Resume the previously suppressed components. Once the problem component is determined, continue diagnostic testing at the part level by selecting Feature, Suppress. After determining which feature is causing the cross-sectional failure, modify the cross-section so that it does not pass through any edges, vertices, or tangency points that could possibly cause the cross- section to incorrectly intersect this feature.

4. Continue to troubleshoot the failed cross-section by indexing, or slightly increasing, the offset position of the cross-section within the model. For planar cross-sections, select X-section, Modify, pick the name of the crosssection, and Dim Values. For offset cross-sections, select X-section, Modify, Redefine and either Section or Scheme. Minor offsets to the dimensions used to originally create and constrain the cross-section should be added. Again, the modified cross-section should continually be tested until the cross-sectional view in the drawing is created successfully.

Modifying Cosmetic Thread Display There are several ways to modify the display of cosmetic thread features while working in drawing mode. They can be erased using the Show/Erase dialog box or they can be blanked on layers. However these modifications will completely remove the display of the threads regardless of the display setting in the environment menu. Cosmetic thread features can also be modified in drawings to conform to ISO or ANSI standard based on the type of view, the location of the feature within the view, and the type of thread. The drawing setup file options "hlr_for_threads" and "thread_standard" are used to modify the display of cosmetic threads. When "hlr_for_threads" is set to "yes", the display of the threads conforms to the standard specified by the option "thread_standard".

Procedure 1. The exploded assembly shown in Figure 1a consists of a bolt part with an external thread and a nut part with an internal thread. Figure 1b shows side and front cross sectional views of the "bolt" part, "nut" part, and "bolt_&_nut" un-exploded assembly in Drawing mode when the drawing setup file option "hlr_for_threads" is set to "no" and "thread_standard" is set to "std_ansi".

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Drawing Views

Figure 1a (ANSI)

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Drawing Views

Figure 1b (ANSI)

2. After modifying the drawing setup file option "hlr_for_threads" to "yes" and changing "thread_standard" to "std_ansi_imp", the threads will display according to the ANSI standard as shown in Figure 2a. When the display of the views is set to No Hidden, none of the hidden lines for the thread feature will display. When "thread_standard" is set to "std_iso_imp", thread lines appear with a yellow, leader style as shown in Figure 2b. These lines continue to display even when the environment is changed to No Hidden. The ISO standard also dictates that on an end view of a visible thread feature, the thread roots should be represented by an arc of http://www.ptc-mss.com/Tutorial/Advdraw_site/Drawing_views/Drawing_views.htm (7 of 12) [28.11.2002 13:00:31]

Drawing Views

approximately three-quarters of the circumference. ANSI standard states that a full circle should represent this thread root. Both standards hold true for when the cosmetic thread is hidden in an end view as well, except that these thread roots display in hidden line style.

Figure 2a (ANSI)

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Drawing Views

Figure 2b (ISO)

3. In order for the line display of threads to be correct for assemblies, the drawing setup file option "thread_standard" should be set to either "std_ansi_imp_assy" or "std_iso_imp_assy" depending upon the appropriate standard. In order for the line display of the assembly to be correct, the following conditions must http://www.ptc-mss.com/Tutorial/Advdraw_site/Drawing_views/Drawing_views.htm (9 of 12) [28.11.2002 13:00:31]

Drawing Views

be true: The internal diameter of the nut must be equal to the diameter of the bolt's cosmetic thread. The diameter of the bolt must be equal to the diameter of the nut's cosmetic thread. Figure 3a displays the ANSI standard for thread lines and cross hatching. The standard dictates that externally threaded parts should always be shown covering internally threaded parts and should not be hidden behind them. Figure 3a shows how only one set of cross hatching displays at the thread overlap area and this cross-hatching belongs to the part with the external threads. Figure 3b displays the correct line display with regards to the ISO standard.

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Drawing Views

Figure 3a (ANSI)

Figure 3b (ISO)

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Drawing Views

Tips & Tricks When you create a detailed view of a part containing an axis that lies off the part (That is, model geometry does not enclose it), the axis does not appear in the detailed view.

When you move a broken view, for any subview (or portion of view) that you select to move, all subviews to its right and below it move the same distance. To move the entire broken view to a different location on the drawing, select the upper-left subview (1). This moves the entire view without altering the gaps between the subviews. Selecting any other subview moves all subviews below it and to the right of it the same distance. An aligned partial view that you create using the Copy & Align command has its own local cross sections. That is, when you create it, it does not have the local cross section of its parent view. You can add them and remove them later. The Origin and Perspective commands in the VIEW MODFY menu, and the Add Breakout and Del Breakout commands in the VIEW BNDRY are not available for aligned partial views.

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Working with Detail Items

Working with Detail Items Dimensions You can define snap lines on individual drawings to locate dimensions, notes, geometric tolerances, symbols, and surface finishes. The system positions the snap lines relative to the view outline, or a selected model edge or datum plane. After you have placed an item on a snap line, the item moves along if the grid line moves (for example, when the view outline expands). To control the display of snap lines, select Display Snap Line from the Environment dialog box. To turn on snapping, choose Snap to snap line. You also can put snap lines on drawing layers and blank them, but once you blank them, you cannot add new items to them. Existing items continue to snap. TIP: If you use snap lines, all items on them keep their distance relative to the view even if you switch the view to another sheet. ●

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When the sketching plane of an extruded or revolved section is neither parallel nor normal to the screen, the system still shows the linear dimensions of the section that are parallel to the screen. For clipped views, Pro/ENGINEER rotates the dimensions of a revolved section up to 180 degrees to bring them into the view outline. Pro/ENGINEER does not show dimensions (in a view) of features that you have suppressed using By View. If possible, it displays them in another view.

At least one of the entities being dimensioned must be within the spline and the view boundary.

When you create dimensions in drawing mode, the configuration file option "create_drawing_dims_only" determines whether the system saves them in the part or in the drawing as associative draft dimensions. When you set this option to "yes" (the default is "no"), it saves all new dimensions created in the drawing as associative regardless of the setting of the drawing setup file option. The length of dimensions created in drawing mode reflects the length of the entity as it appears in the view and is, therefore related to the drawing scale. http://www.ptc-mss.com/Tutorial/Advdraw_site/Detail_items/Detail_Items.htm (1 of 5) [28.11.2002 13:00:44]

Working with Detail Items

The dimension to be converted must be shown as linear. To modify a dimension type from linear to ordinate, you must first establish a reference baseline. If you just created a baseline, it remains set until you set another, or until you exit the MOD DIM TYPE menu. Only one baseline can be current (set) at one time. The following dimensions cannot be converted to ordinate: 1. A diameter dimension shown as linear 2. A centerline dimension.

Notes When you are entering notes from a text file, the file can reside in the current directory, or can be present anywhere within a search path that you have specified using the configuration file option "pro_note_dir". You can enter notes from a file that contains dimensions, parameters, special symbols and superscripted or subscripted text. However, you cannot enter information about characteristics such as text height, text width, text angle, and slant angle. You must use the commands in the MODIFY TEXT menu to change this information manually. When you use the keyboard to type note text manually, you can add blank lines, create superscripted and subscripted text, add symbols, and include parameter information. Balloon notes consist of text enclosed in a circle. To restrict the size of a balloon, use the drawing setup file options "max_balloon_radius" or "min_balloon_radius". To create superscripted text, type @+text@# and to create subscripted text, type @-text@#, where text is the note that is superscripted or subscripted.

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Working with Detail Items

To create a Text in a box, type @[Text@] where Text is the note that is in the box. You can place draft (add and dd) dimensions and reference(rd) dimensions parametrically in drawing notes and tables using &add or &dd. Draft(driven) dimensions and reference dimensions created in the drawing are updated when the model is regenerated. ●

Yes-No: When you set the drawing set up file option "yes_no_parameter_display" to "yes_no", parameters can have a "yes" or "no" value in drawing notes. When you set it to "true_false" (the default value), they can hane a "true" or "false" value.

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Dimensions: &d#, &rd or &ad#, where # is the dimension ID. Examples: &d12, &ad24, &rd2

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Instance Numbers: &p#, where p is the parameter ID. Example: &p3

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User defined parameters: &xxxx, where xxxx is a symbol defined in a relation.

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Datum names: &dtm_name, where name is the name of a datum plane.

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Drawing parameters: ¶meter:d, where parameter is the parameter name. You can modify the value by using the Value command in the MODIFY DRAW menu. Drawing labels: you can add the folowing drawing labels to a drawing: &todays_date: Adds the date as of the note´s creation in the form dd-mm-yy. You can edit it later as any other nonparametric note, using Text Line or Full Note. If you include this symbol in a format table, the system evaluates it wen it copies the format into the drawing.

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&model_name: Adds the model used in the drawing.

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&dwg_name: Adds the name of the drawing.

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&scale: Adds the scale of the drawing.

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Working with Detail Items ●

&type: Adds the drawing modeltype.

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&format: Adds the format size.

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¤t_sheet: Adds the sheet number for the sheet on which the note is located.

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&total_sheets: Adds the total numbers of sheets for the drawing.

The configuration file option "todays_date_note_format" controls the initial format of the date displayed in the drawing. Year: %yy for 97 %yyyy for 1997 Month: %Mmmm for Jan %MMM for JAN %Month for January %MONTH for JANUARY %mm for 01 %m for 1 % m for <space>1 Date (if 2 digits are needed to represent the date, all three are the same. Therefore, "%dd%mm%yy" produces "01 01 97") %dd for 01 %d for 1 http://www.ptc-mss.com/Tutorial/Advdraw_site/Detail_items/Detail_Items.htm (4 of 5) [28.11.2002 13:00:44]

Working with Detail Items

% d for <space>1 The following formats are also valid: %dd-%Mmm-%yy (= 01-Jan-97) %mm/%dd/%yy (= 01/01/97) %Mmm %dd, %yyyy (= Jan 01, 1997) When you edit a note using Text Line and Full Note, the system preserves all of the attributes (font, height, width, or slant angle) applied to a portion of the text. However, the note appears much different from how it does on the drawing. The system breaks up a text string into portions wherever there is a new line of text or a parameter (such as dimensions), and encloses each portion of the text in braces ({}), giving it an integer label. Labels identify the initial order of the text, and any attributes for that portion. When editing text, or adding more lines, you can copy the attributes of a portion of text by using the same integer label.

Using True Type Fonts To access the true type fonts, you must first specify them in the drawing setup file, using the "aux_font" drawing setup file option: aux_font# font_name. True type fonts are more complicated than PTC fonts and therefore can take more time to repaint.

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Tolerances

Tolerances Dimensional Tolerances ● ● ● ●

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tol_display Set the tolerance display on and off tol_mode Set the default display for dimension tolerances Set Datums maintain_limit_to_nominal Maintains the nominal value of a dimension regardless of the changes that you make to the tolerance values. If you set it to "yes", the system does not modify the Nominal Value of a dimension with a Limits tolerance format when you set the format to Limits or change the value of the upper or lower tolerance. Before you can create dimensional tolerances you have to load the tolerance tables in the model. Set the tolerance standard to ISO/DIN and retrieve the tolerance tables you need.

TIP: Retrieve often used tolerance tables in the start part.

Creating Geometric Tolerances Geometric tolerances can be created in Part, Assembly, and Drawing modes. To create them in Part and Assembly modes, select Setup, Geom Tol, Specify Tol. To create them in Drawing mode, select Create, Geom Tol, Specify Tol. In either case, the Geometric Tolerance dialog box will appear as shown in Figure 1.

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Tolerances

Figure 1

Once the Geometric Tolerance dialog box appears, the procedures for creating a geometric tolerance are the same in Part, Assembly, and Drawing modes. The procedures are as follows:

1. Select the type of geometric tolerance to be placed. The possible types are graphically shown on the left hand side of the Geometric Tolerance dialog box, as shown Figure 1. In this example, the position tolerance type has been selected.

2. Select the model to be toleranced. The model may be selected from either the Model drop down list or by selecting Select Model... and picking the model from the screen. In Drawing mode, the list of available models will include all the models currently in the drawing as well as the drawing itself. For assemblies, the list of models will include the assembly as well as the components that make up the assembly. For parts, only the part can be selected as the model.

3. The next step is to assign datum references to the geometric tolerance. Select the Datum Refs tab from along the top of the Geometric Tolerance dialog box and choose the datums for the primary, secondary and tertiary references. For each reference, the material condition may also be set. In this example, the primary datum is being set as datum "A" with a maximum material condition (MMC) as shown in Figure 2. The secondary datum is being set as a compound datum "B-C" with an RFS(No Symbol) material condition as shown in Figure 3. For position and surface profile geometric tolerances, a Composite Tolerance can be set with or without a datum reference. Figure 4 shows the composite tolerance being set with a value of 0.005 and the primary datum (datum "A") being selected as the reference.

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Tolerances

In order for datum planes or axes to be selectable for use as datum references, they must have previously been set using the Set Datum option from the GEOM TOL menu.

Figure 2

Figure 3

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Tolerances

Figure 4

4. The next step is to set the tolerance value for the geometric tolerance. Select the Tol Value tab from along the top of the Geometric Tolerance dialog box and set the Overall Tolerance as desired. The Material Condition for the overall tolerance can also be specified. In this example, the tolerance is being set to 0.020 at MMC, as seen in Figure 5. For straightness, flatness, perpendicularity, and parallelism, a Per Unit Tolerance may be set. In this example, a Per Unit Tolerance is not applicable.

Figure 5

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Tolerances

5. The next step is to set the Symbols, Modifiers and a Projected Tolerance Zone. Select the Symbols tab from along the top of the Geometric Tolerance dialog box. The options Statistical Tolerance, Diameter Symbol, Free State, All Around Symbol, and Tangent Plane symbols may be selected depending on the type of geometric tolerance being placed. A Profile Boundary or a Projected Tolerance Zone may need to be established depending on the tolerance being set. Select any desired Symbols, Modifiers, Projected Tolerance Zone, or Profile Boundary. In this example, a Projected Tolerance Zone will be placed below the geometric tolerance with no specified Zone Height. If a specified Zone Height is desired, select the Zone Height option and enter the desired height in the input field.

Figure 6

6. The Reference Entity should then be set by first selecting from the Type drop down list in the Model Refs portion of the dialog box and selecting one of the available options. Once the desired Reference Entity type is selected (i.e.. Edge, Surface, etc.), the Select Entity... option will become depressed and the Reference Entity should be selected on the screen.

7. With the geometric tolerance now fully defined, place the geometric tolerance as desired by selecting the Placement Type from the drop down list. The possible placement options will vary depending on the type of geometric tolerance being placed. The list of possible options are, Dimension, Free Note, Leaders, Tangent Ldr, Normal Ldr, and Other Gtol. For this example, the geometric tolerance has been placed as a Free Note. The Place Gtol... option will become depressed after selecting the Placement type. Continue placing the geometric tolerance. If the geometric tolerance is placed, it does not mean that the definition of the geometric tolerance is complete. The geometric tolerance can be placed and actively changed until it is set. Figure 7 shows the geometric tolerance created in this example.

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Tolerances

Figure 7

8.After the geometric tolerance is placed, there are other options:

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Select New Gtol to create a new geometric tolerance. Select Cancel to quit the creation of the current geometric tolerance and exit the dialog box. Select OK to accept the current geometric tolerance and exit the dialog box.

Modifying Geometric Tolerances The modification of geometric tolerances can be performed in Part, Assembly, or Drawing modes by selecting Modify, Geom Tol. Once a geometric tolerance is chosen, the Geometric Tolerance dialog box will appear with options to change the geometric tolerance type, datum references, tolerance values, and symbols. None of the settings under Model Refs may be modified (which include the Model, Reference Entity, and Placement values). Also, note that if the Type of geometric tolerance is changed, datum reference information will be removed from the existing geometric tolerance or the settings under Datum Refs will become unavailable, depending on what information is proper for that particular type of geometric tolerance.

Procedure 1. Figure 1 displays a drawing view with a geometric tolerance. To change any of the values of this geometric tolerance, select Modify, GeomTol and choose the geometric tolerance.

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Tolerances

Figure 1

2.The dialog box appears and by default, the settings for Tol Value are available for modification. Values for Overall Tolerance and Material Condition can be changed, as displayed in Figure 2. Notice that any modifications made in the dialog box automatically update the model and/or drawing.

Figure 2

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Tolerances

3.Modify the datum references, material conditions, and compound/composite tolerance information by selecting Datum Refs from the Geometric Tolerance dialog box, as seen in Figure 3.

Figure 3

4.Make any changes necessary with respect to symbols, modifiers, and projected tolerance zone information by selecting Symbols, as shown in Figure 4.

Figure 4

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Tolerances

5.Once all of the desired changes are made, select OK from the Geometric Tolerance dialog box. The modifications made in the previous steps to the original geometric tolerance are displayed in Figure 5.

Figure 5

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Symbols

Symbols

Creating a Generic Symbol Procedure 1. To create a symbol, select Create from the DETAIL pull down menu, Symbol, Definition, Define, and enter the name of the new symbol. This will open up the SYM_EDIT sub window in which the symbol will be created. 2. Sketch the symbol as seen in Figure 1. The symbol can be sketched by selecting Detail, Sketch from the SYMBOL EDIT menu or by using Copy Drawing and selecting existing entities in the drawing window. The notes "\Note #\" and "\text\" were created using Detail, Create, Note from the SYMBOL EDIT menu. Because both notes are surrounded by backslashes "\", the text for these notes will be variable. Variable text allows for preset values to be defined as symbol attributes and selected when placing symbols on the drawing. Preset values may be used for each of these notes. If the text in a note is to remain constant, do not use any "\" before and after the text.

Figure 1 3. When all of the entities have been sketched, groups can be made so that several instances of one generic symbol can be made. Groups are useful because each instance of the symbol will be saved with the generic, rather than a separate symbol file for each instance. To create a group, select Groups, Create from the SYMBOL EDIT menu and enter in the name of a group: "triangle", for example. Select the entities seen in Figure 2 to be in the group, "triangle". If an entity is mistakenly omitted or one is chosen that does not belong to that group, Edit, Triangle, Add or Remove from the SYM GROUPS menu can be used to edit the group definition. Create another group called "text" and select the notes "\Note #\" and "\text\". Add the last group called "wings", which includes the two arcs on the top of the triangle.

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Symbols

Figure 2 4. Sub-groups need to be created in the top level group "triangle". To create a sub-group under "triangle", select Groups, Change Level, Triangle (this is the group under which the sub-group will be created), and This Level. Now, two groups called "point" and "bottom" need to be created. In the "point" group, the two slanted lines were selected, as seen in Figure 3. The horizontal line was included in the "bottom" group, which is omitted from Figure 3.

Figure 3

5. When placing an instance of the symbol, it is possible to exclusively include either the "point" or the "bottom" sub levels, without having both in the symbol at the same time. To select one of these groups, change the level to the "triangle" group using Groups, Change Level, Triangle, This Level. Then select Groups, Group Attr, Exclusive. Note that for this example, there were NOT any exclusive groups created.

6. Choose the attributes for the symbol by selecting Attributes from the SYMBOL EDIT menu. See Figure 4 for the Attributes dialog box. For this symbol, Free placement is being selected to allow the symbol to be placed anywhere on the drawing. The origin of the symbol is defined using the Pick Origin... button. Variable - Drawing Units is selected to allow for variable heights of the symbol when placing an instance utilizing the drawing units. The Var Text tab may be use to specify preset values for the variable texts from the notes. Select the OK button to http://www.ptc-mss.com/Tutorial/Advdraw_site/Symbols/Symbols_D.htm (2 of 5) [28.11.2002 13:01:23]

Symbols

finish the symbol definition.

Figure 4

7. As with the Attributes dialog box, there is a dialog box for defining an instance of a symbol to be placed on the drawing. Select Instance from the SYMBOL TYPE menu to define the instance. For the example in Figure 5, "SYM1" is retrieved, and a copy of the symbol is defined with "xyz" as the new name. The variable height has been changed to "3".

Figure 5

8. The grouping of the symbol instance is controlled through a tree representation of the group levels and sub levels as seen in Figure 6. The window to the right allows for the preview of the symbol before it is actually placed. As shown in the dialog box, the sub level group "BOTTOM" (which contains the horizontally sketched line) is not selected in the tree, and consequently not seen in the preview of the instance.

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Symbols

Figure 6

9. The last step in defining the instance is to give values for the variable text. In Figure 7, the value of "1" was given for "Note #", and the value of "PTC" was given to the "text" variable text.

Figure 7

10. Once the Grouping and Var Text have been defined, the instance can be placed by selecting Place Inst... from the Placement tab (see Figure 5) and selecting a location on the drawing. 11. The symbol can be written to disk so that it can be used on other drawings by selecting Definition, and then Write from the DWG SYMBOL menu. 12. All of the 14 instances shown in Figure 8 can be created from the generic symbol by selecting various combinations of the groups.

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Symbols

Figure 8

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Frames, Tables and Boms

Frames, Tables and Boms Creating a New Sized Format from an Existing Format The following procedure describes the suggested technique for creating a format of different size from an existing format using IGES or DXF translation. The end result of this procedure will be a new format, which contains all of the tables and draft entities from the original format, scaled to fit the new format size.

Procedure 1. Retrieve an existing format into memory using Mode, Format, Search/Retr and select the name of the format to be copied from the SELECT_FILE menu. 2. If the format has Pro/E tables which contain parameters, the tables will need to be saved so they can be placed on the new format once the IGES or DXF file has been read in. To save a table to disk, use Table, Save/Retrieve, Store and select one of the tables on the format. When prompted to "Enter a name for the drawing table [QUIT]:", enter a name that will be easy to remember, such as "title_block". Repeat this process for all tables on the format. 3. Once all of the tables have been saved, delete them all from the current format. This is necessary to prevent table lines from being converted into draft entities during IGES and DXF transfer. To delete a table, use Table, Delete and select a table. When prompted "Do you really want to delete the table? [N]:", enter yes. 4. When all of the tables have been deleted from the format, the IGES or DXF file can be created. To do this, use Interface, Export and select either IGES or DXF, and enter the file name. Both IGES and DXF are equally effective. 5. Create a new format by selecting Mode, Format, Create enter in the new format name. Select a new format size from the DWG SIZE menu, and then select the units of the new format from the FORMAT UNITS menu. 6. Import the IGES or DXF file created in step 4 by using Interface, Import select either Iges or DXF, http://www.ptc-mss.com/Tutorial/Advdraw_site/Frames_Tables/Frames_D.htm (1 of 5) [28.11.2002 13:01:37]

Frames, Tables and Boms

and enter in the name of the file created in step 4. When prompted "Drawing is smaller/larger than format. Scale to fit format? [Y]:", enter yes. 7. Unless the format just created has the same proportions as the original format (A,C, and E sized formats have the same proportions; B and C sized formats have the same proportions) the file just imported will not "fit" the new format size correctly. The entities on the new format can be stretched using Detail, Tools, Stretch. When this is done, some entities may have to be redrawn or copied from existing entities on the format. 8. When all of the sketched entities have been finalized, the tables that were saved to the hard disk can be retrieved onto the new format using Table, Save/Retrieve, Retrieve. Enter in the name of one of the tables and place it on the format using options from the GET POINT menu. Repeat this process for all of the tables stored from the original format.

Using Parameters in Formats There are two types of parameters, which can be used on a format, user defined parameters and those supplied by Pro/E. Each parameter has certain unique characteristics which allow them to be used in different ways when placed on a format.

Procedure 1. Create a title block similar to the one shown in Figure 1 on a format. The table can be created using standard Table functionality.

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Frames, Tables and Boms

Figure 1

2. There are two different types of parameters that can be used in a format: Pro/E parameters and user defined parameters. Pro/E parameters include "&model_name", "&current_sheet", "&total_sheets" "&scale", and "&todays_date". See the section entitled "Including Parameter Information" on page D-219 of the Pro/E User Guide for a listing of the Pro/E supplied parameters. Pro/E parameters, with the exception of "&todays_date", can be placed on a format as text in a Table cell or as a note. When the format is added to a drawing, these parameters will update with the appropriate value. For example, "&dwg_name" will update with the name of the drawing file, "¤t_sheet" will update with the number of the current sheet of the drawing. Since the Pro/E parameters "&model_name", "&scale", and "&type" all need to reference a model in order to update with the correct information, it is good practice to add the model to a drawing before a format is added. 3. Add the Pro/E parameters similar to those shown in Figure 2 to the format table.

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Figure 2 4. Figure 3 illustrates how this table would look if the format were added to the drawing both before and after a view of the model. Figure 3-top is the table that was added before a view of the model, and Figure 3-bottom is the table that was added after a view of the model. Notice in Figure 3-top that the parameters "&model_name" and "&scale" have not updated. They evaluate to MODEL NAME and DRAWING SCALE, respectively. In Figure 3-bottom, these two parameters have updated. This is because there was a model to reference to find the appropriate information. If a model is added after the format is added, then add the format again by using Sheets, Format, Add/Replace.

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Frames, Tables and Boms

Figure 3 (top, bottom)

5. Although &todays_date is an internal Pro/E parameter, it needs to be placed in a Table in order for it to be evaluated when the format is placed on a drawing. If &todays_date is placed as a free note on a format, the parameter will not be evaluated. The note will appear as "&todays_date". 6. In order for a user-defined parameter to update with information from the model, the parameter must be placed inside a Table. Placing the parameter inside a Table is a cue for Pro/E to search the current model for a parameter of the appropriate name. If the parameter is not placed inside a Table, the parameter will not update with information from the model, but will be treated as a regular note. However, if a parameter name is entered into a Table, and this parameter does not exist in the model, Pro/E will prompt to "Enter text for the parameter "parameter name" [NONE]:". This is a good method of having Pro/E prompt for a value, such as "&drawn_by", when a format is placed on a drawing. As seen in Figure 4, the user defined parameters "&mat" and "&drawn_by" have been place inside of the Table on the format.

Figure 4

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Large Assembly Drawings

Large Assembly Drawings Config Options The following are configuration file options that relate specifically to large assembly drawings. Making use of these options can significantly improve drawing productivity.

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Large Assembly Drawings

Assembly Manipulation Techniques The following suggestions can be used in Assembly mode prior to Drawing creation:

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Create the simplified reps you need for the drawing. Don't mix up several simplified reps in one drawing because you'll have to load all parts again. If its necessary to have several representations in one drawing, create first for each rep one drawing and merge them later together to a multiple sheet drawing. Use Simplified Representations to prevent Pro/ENGINEER from retrieving unnecessary models into memory. Replace models that are not referenced in a drawing view with Geometry Reps. Geometry Reps take approximately half the time to retrieve as the master model. Use as few assembly features as possible because intersecting components creates hidden copies of the model and this uses additional memory. When sketching assembly features, use closed sections and manually select the components to be intersected. This will prevent Pro/ENGINEER from intersecting extraneous components and will speed up drawing performance.

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Large Assembly Drawings

Increasing Performance when Working with Large Assembly Drawings The following methodologies can be utilized in drawing mode to increase drawing productivity: ❍

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Set the line display of all views to Wireframe. Regeneration time will be faster than if the display of the views are set to Hidden or No Hidden. Erase views that are not being used when detailing the drawing. By erasing a view the display will not be calculated by Pro/ENGINEER and this will decrease regeneration time. Use Views, Resume View to resume the views before plotting. Move views, which are complete to separate sheets of the drawing. The views can be moved back to the original sheet prior to plotting. Use Z-Clipping to reduce graphical information displayed in an assembly view. All geometry behind the Z-Clipping plane will be removed from the display. Use Views, Dwg Models, Add Model for adding subassemblies to the drawing. Create views of the subassemblies instead of creating views of simplified representations of the master assembly. Create separate drawings whenever possible, as this will prevent Pro/ENGINEER from retrieving unnecessary models into memory. Use Pro/BATCH so all plotting can be performed outside of Pro/ENGINEER To minimize retrieval time when plotting, use View Only retrieve. The config.pro option "save_display" must be set to "yes" prior to saving the drawing. The display of components in an assembly can be blanked in a drawing. Create layers to blank the display of many components in an assembly. Use Views, Disp Mode, Memb Disp and Blank to also blank the display of assembly components.

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Large Assembly Drawings

Tips & Tricks When working in a drawing and changing the part (or assembly), all views of the drawing are unregenerated. After switching back to the drawing, all views of the current sheet are regenerated automatically. This could last up to 1 hour and more. By setting the config option auto_regen_views to no, the views are not regenerated automatically. So the user has control using Views - Regenerate View to regenerate the view, which he currently needs to go ahead with his work (Often the user is doing a change in the model and he needs only one view to be updated at the moment). Exception: When changing display of a layer, the views are regenerated regardless of this option setting. PTC development is working on this problem. If it hurts too much, use these workarounds: ● ●

Erase views before using layer Add an additional empty sheet to the drawing, switch to this sheet before using layer

If you find a better solution, please inform me.

To speed up working in drawings you can ● ● ● ●

suppress features in the part use wireframe display erase views in the drawing use simpl. Rep. in assembly drawings (e.g. work as much as possible with skeleton part, while real part is suppressed)

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Large Assembly Drawings

This regeneration of the views takes most of the time, when retrieving a drawing. Example cylinderheaddrawing: Load of files takes 1 min., regeneration of views takes 20 min. To speed up retrieval time, you can either ●

Save the display of views when saving the drawing: If you set Environment, Save Display (or use config option SAVE DISPLAY), then the display of the drawing is stored in the drawing file. Second advantage is, that you can retrieve the drawing very quickly without model (View only) for inspecting or plotting. Attention: Views, which are not regenerated (see upper chapter) when saving the drawing, are automatically regenerated, when retrieving the drawing (regardless of SAVE DISPLAY setting). Example: Drawing and model is in session; then the model is modified. After switching back to drawing, only some views are regenerated (using Views - Regenerate View), all other views stay unregenerated. Additionally when retrieving this drawing with View only, then the unregenerated views are not displayed (only a rectangle is visible). It may be makes sense to regenerate all views before saving the drawing.

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Erase views before saving the drawing. The erased views are not regenerated while retrieval. The user has to resume the views, which he needs for work. This could maybe also done with new Representation functionality in Rev 2000i. When setting the config option INTERFACE_QUALITY to "0", the creation time of plotfiles is accelerated enormous. Pro/E doesn’t check the output, so check the plots, whether there are problems or not. Set the Frame when you have placed at least one view. Then the parameters will be filled in automatically. Customers complained about dimensions, which moved in the drawing without any reason. We recognized that every drawing view has got a "bounding box" which influences the position of the dimensions. If the outer geometry is modified (for example additional features), the dimensions will change their positions. Workaround: create a bounding box made of surface features around your part which will not be exceeded.

The config.pro option FORCE_WIREFRAME_IN_DRAWINGS is probably too confusing for working with complex models. Everybody should be aware, that all views should be regenerated before plotting.

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The option CREATE_DRAWING_DIMS_ONLY should be set to yes. If you don’t do this, the dimensions, which you create in your drawing will be saved in the .prt file. If you create a drawing with created dimensions and you forget to save the model as well you will loose all the created dimensions. If you work parallel with y our model and the drawing in different windows you shouldn’t modify you environment settings. If you do this all views will be regenerated. A workaround is to set the fast hlr option. Another way to avoid long waiting times is to modify the display mode of the different views separately by using the DISP MODE, DISP VIEW command.

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The command VIEWONLY RET can save a lot of time during the retrieval of a drawing. But if you did not regenerated all views before you saved the drawing, you’ll see at the next retrieval with this command only bounding boxes for the views which are not regenerated. The workaround is to create a mapkey which regenerates all views, saves the current drawing and quits Pro/E. Activate this mapkey in the evening before you leave. If you set the SAVE_DISPLAY option to YES, you’ll get the views immediately if you retrieve a drawing. But be aware that this happens only to views, which have been regenerated before saving it. The rest will be regenerated. This causes sometimes nevertheless long waiting times. Avoid regenerating. Do it before you go for lunch or at the end of the day before you leave.

http://www.ptc-mss.com/Tutorial/Advdraw_site/Large_Assembly/Large_assy_D.htm (6 of 6) [28.11.2002 13:01:45]

collaboration

innovation

global solutions

Pro/ENGINEER Tips and Tricks

5 December 2001 © 2001 PTC

Agenda

© 2001 PTC

ƒ

Introductions

ƒ

Goals for Today

ƒ

General ProE Tips

ƒ

Drawing Tips

ƒ

Questions

2

Tips & Tricks – Goals

ƒ

A Bunch of Things You Probably Knew

ƒ

Some Things You Didn’t Know

ƒ

Maybe One Thing That Works Great That You Didn’t Know

© 2001 PTC

3

Tips & Tricks – General ProE

© 2001 PTC

ƒ

Middle Mouse Button to Accept

ƒ

Right Mouse Button for Pop-up Redefine/Info/Etc.

ƒ

File Preview

ƒ

Use Fast Hidden Line Removal

ƒ

Renaming Features

ƒ

Display Datums While Spinning

ƒ

Component Display States

ƒ

Explode States

ƒ

Assembly – move component using CTRL-ALT 4

Tips & Tricks – Model Tree

© 2001 PTC

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Right Mouse Features from Model Tree

ƒ

Drag and Drop Re-Order

ƒ

Drag and Drop Insert Mode

ƒ

Right Mouse in Model Tree

ƒ

Custom Model Tree Setups

ƒ

Rename/Modify Features in Model Tree

5

Tips & Tricks – Sketcher

© 2001 PTC

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Cheat Sheet (Handout)

ƒ

Middle Mouse Button to get Pick Arrow

ƒ

Configure Screen & Icons

ƒ

Mapkeys – Create & Iconize

6

Pro/ENGINEER 2000i2 Sketcher Cheat Sheet

Line

Sketcher Tools Toolbar

Circle

Sketcher Preferences

Select Item (hold SHIFT to gather more) Rectangle

Arc Tool tangent & 3-point

Concentric Arc

This menu appears when you have nothing selected and click the Right Mouse Button

Concentric Circle

Ellipse

Arc Center & Ends

Conic Arc

Fillet

Elliptical Fillet

Reference Csys

Create Point

Use Edge

Offset Edge

Dynamic Trim

Trim

Divide

Mirror

Scale & Rotate

Copy

Complete Section

Quit Section

Spline

Create Dimension

Centerline

Modify (dimensions, splines & text)

Sketcher Constraints

This menu appears when you have an item selected and click the Right Mouse Button Pressing the DELETE key will delete selected items

Create Datum Plane Create Datum Axis Create Datum Curve Create Datum Points Create Datum Csys Create Analysis Feature

Asynchronous Datum Creation Toolbar (Used Anytime out of Sketcher Mode)

Sketcher Toolbar

Undo Redo

Toggle Vertices

Reorient to Sketch View

© 2001 PTC

Toggle Dims

Toggle Constraints

Toggle Grid

Ethan Meyer - PTC MSS 7

Tips & Tricks – Drawings (Clarity)

© 2001 PTC

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Z-Clipping (also decreases repaint time)

ƒ

Member Display

ƒ

Relating Draft Items to a View

ƒ

Quilt Hidden Line Removal

ƒ

Fonts

ƒ

Use @o to attach leader to multi-line text

8

Tips & Tricks – Drawings (Ease of Use)

© 2001 PTC

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Right Mouse Modify

ƒ

Align Views / Unalign Projected Views

ƒ

Copy from other Drawing

ƒ

Template Drawings

ƒ

Word Wrap (2001)

9

Tips & Tricks – Drawings (Speed) ƒ

© 2001 PTC

General Tips: ƒ

Turn off datum displays

ƒ

Work in wireframe

ƒ

Set auto_regen_views to no

ƒ

No View Open (open_simplified_rep_by_default=yes)

ƒ

Erase/Resume Views

ƒ

Snapshot of View

ƒ

Merge Drawings

10

Untitled Document

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/view_disp_mode.htm [28.11.2002 13:04:43]

http://www.kinetivision.com/freevids/comp_disp.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/comp_disp.htm [28.11.2002 13:05:01]

http://www.kinetivision.com/freevids/drip_loop.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/drip_loop.htm [28.11.2002 13:05:21]

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Design Animation

Table of Contents: 1) Overview 2) Tutorial 3) Key Vocabulary 4) Tutorial Evaluation

Page 1 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Overview: Pro/ENGINEER Design Animation provides engineers with a simple yet powerful tool for conveying complex information about a product or process through animation sequences. Now communication with groups as diverse as customers, suppliers, sales and marketing, management, and design is easier than ever. Animation sequences also serve to provide exceptional communication value in design reviews or as a method for remote communication of information. Tools to communicate design sequences Pro/ENGINEER Design Animation enables the creation of animation sequences within Pro/ENGINEER, using parts, assemblies, and mechanisms. Using key frames, drivers and inherited mechanism joints, animations can be created and manipulated with ease. As a simple yet powerful way to convey complex information about a product or process, these animation sequences can be used as animated guides to assembly, disassembly, and maintenance procedures or to provide useful concept communication tools for sales and marketing, management meetings, design reviews, and as a method for remote communication of information. Capabilities: Integrated and associative Design Animation is an integrated part of Pro/ENGINEER, so there are no data transfer problems usually found with 3rd party animation packages, and users benefit from full associativity and interoperability with other PTC products and data management tools. If the designs of parts or assemblies change, the animation will update automatically. Key frame sequences The user defines the key frame sequences, which describe the position, and orientation of parts and assemblies at specified times, and Design Animation interpolates between these key frames to produce a smooth animation. Key frames can be easily created by simply 'snapping' current positions and orientations in Pro/ENGINEER. Animation specific tools Pro/ENGINEER Design Animation delivers powerful assembly manipulation functionality to help quickly set up key frames by allowing the user to specify geometric constraints, translational and rotational dragging, body locking and other tools. This allows rapid manipulation of part positions to quickly build key frame sequences and animations. Animation manager Events, key frames, and sub-animations are displayed and controlled by the easy-to-use animation manager. From this one panel, users can quickly and easily define, manipulate, and change any aspect of the animation. Page 2 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Design intent re-use The mechanism joints used to create and move assemblies in Pro/ENGINEER Mechanism Design are re-used by Pro/ENGINEER Design Animation where they can be selectively activated and de-activated at any stage during animation sequences.

Page 3 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Tutorial: For this introduction to Design Animation, we will take you through the basics of developing an animation process, controlling camera angles and component displays. The model that we will be using in this tutorial is a Pedal Mechanism Assembly, as shown below:

Step one: Change your working directory to the folder called design_animation. Once you have navigated to that location, open the model called, top_level.asm. This will open the model that we will be using for Design Animation. Since Design Animation is a floating module, we need to grab the floating license. Click on the pull-down menu called, Utilities and click on Floating Modules.

Page 4 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

This will open the Floating Modules GUI, were you can select the license for Design Animation, and then click OK.

Know hat you have attained a license for Design Animation; we can begin to build our animation. To access the tools for Design Animation, we need to click on the pull-down menu called, Applications, and select Animation.

Page 5 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

This will open the new Design Animation toolbars: Animation Animation Icon Display Body Definition in Animation Drag Model and Create Snapshots Create New Keyframe Sequence Create New Body – Body Lock Create New Driver Create New View @ Time Create New Display @ Time Edit Selected Animation Object Undo Redo Remove Selected Entity Start Animation Playback Export the Animation And open the Sequencer Window:

Sequencer Window

Page 6 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

The Sequencer Window is the area that we capture the details for our animation. Step Two: Click on the Saved View List icon, , and select ISO. Know that we have orientated the model to the right angle, we can begin to capture component states, as we move object apart. Some parts of the assembly will need to become separate bodies, to allow for them to be disassembled. If components are assembled with static constraints, then they will need to be defined as separate bodies to move them. Click on the Body Definition in Animation icon,

. This will open the Body Definition GUI:

You can select each of the defined bodies and see particular object highlighted. When you click on body2, you will notice that it highlights both the Shaft_Spring and Knob_Spring. As well, if you click on body 3, you will notice it highlights both the Shaft_Spring and Knob_Clutch. These object need to be broken up if we plan on moving each of the knobs separately. From the Bodies GUI, choose Add. This will open the Bodies Add GUI:

Page 7 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Select on the Knob_Clutch, Done/Sel and click OK. Click Add again, and select the Knob_Spring, Done/Sel and click OK, Close the Bodies GUI. Step Three: Know that we have defined the particular bodies that we will be moving in the assembly, we can start to capture their translated states. Click on the Drag Model and Create Snapshot icon,

. This will open the Drag GUI:

In the viewing window, you can see the central coordinate system for the assembly. This will be used to help us move components in a particular direction.

Before we begin moving objects, lets capture the present state, click the camera icon, , to take a snapshot. The snapshot will be given a default name, Snapshot1. Page 8 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Highlight Snapshot1 and this will give you the opportunity to rename the snapshot. In the name field give it a detailed name, step_one.

Lets start to move a component, select Translate in X icon, . Pick on the Knob_Spring component and move it to the right, away from the assemble. When you get it to be were you want it, click the first mouse button (FBM).

Page 9 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Click the camera icon, , to take a new snapshot. The snapshot will be given a default name, Snapshot2. Highlight Snapshot2 and this will give you the opportunity to rename the snapshot. In the name field give it a detailed name, step_two. Repeat this process for the Knob_Clutch. Select Translate in X icon, , click the component and move it to the left, away from the assembly. Click the FMB to place the , to take a new snapshot. The component were you like it. Click the camera icon, snapshot will be given a default name, Snapshot. Highlight Snapshot3 and this will give you the opportunity to rename the snapshot. In the name field give it a detailed name, step_three.

Mechanism Constraint

Step Four: Know that we have translated the knobs. We can start to move the other components. In the assembly, we see mechanism constraint symbols on the components we want to move. Since they were assembled with these special types of constraints (see Mechanism Tutorial to learn more about mechanism constraints), we need to disable them to translate the component. Still in the Drag GUI, select the Constraint tab. This will open new options to select from.

Page 10 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

We can perform a variety of tasks from this window, however we are concerned with disabling the existing constraints. Select the Enable/Disable Constraint icon, will allow you to select a constraint, select the following pin-joint:

. This

Once you have highlighted it red, click done/Sel, this disable the constraint and show it in the list.

Page 11 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Select the Snapshots tab again and select the Translate in X icon, . Pick the Shaft_Spring component were we disabled the constraint and move it to the right away from the assembly. Click the camera icon, , to take a new snapshot. The snapshot will be given a default name, Snapshot4. Highlight Snapshot4 and this will give you the opportunity to rename the snapshot. In the name field give it a detailed name, step_four.

Page 12 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Lets move the other knob. Still in the Drag GUI, select the Constraint tab. This will open new options to select from.

Select the Enable/Disable Constraint icon, constraint, select the following pin-joint:

. This will allow you to select a

Once you have highlighted it red, click done/Sel, this disable the constraint and show it in the list.

Page 13 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Select the Snapshots tab again and select the Translate in X icon, . Pick the other Shaft_Spring component were we disabled the constraint and move it to the left away from the assembly. Click the camera icon, , to take a new snapshot. The snapshot will be given a default name, Snapshot5. Highlight Snapshot5 and this will give you the opportunity to rename the snapshot. In the name field give it a detailed name, step_five.

Page 14 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Only one more component to move, the pedal. We will need to disable one last constraint. Still in the Drag GUI, select the Constraint tab. This will open new options to select from. Select the Enable/Disable Constraint icon, select a constraint, select the following pin-joint:

. This will allow you to

Once you have highlighted it red, click done/Sel, this disable the constraint and show it in the list.

Select the Snapshots tab again and select the Translate in X icon, . Pick the other Pedal component were we disabled the constraint and move it up away from the assembly. Click the camera icon, , to take a new snapshot. The snapshot will be given a default name, Snapshot6. Highlight Snapshot6 and this will give you the opportunity to rename the snapshot. In the name field give it a detailed name, step_six.

Page 15 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Step Five: Know that we have disassembled the components into there individual steps; we can capture the steps in time. Select the Create New Keyframe Sequence icon, ; this will open the Key Frame Sequence GUI. Under name, change the default KF1 to Disassemble. Rename sequence to Disassemble.

Page 16 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Under Key Frame, click he pull down menu and select step_six, with a time of zero. Click the Add Keyframe icon, sequence window.

; this will add the Keyframe to the list, as well as, the

Next click the Keyframe pull down menu again and select step_five. This time we are going to edit the time. By default the time will have changed to 1 sec., we are going to put 2 sec. Once you have made the changes click the Add Keyframe icon, the previous steps to add the keyframes until you have added all the steps. When you are done it should look like the following, every step will be 2 seconds apart. Click OK to exit the GUI.

Page 17 of 20

. Repeat

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Step Six: Know that we have defined the Keyframe in the sequence window; lets play the sequence to see what it looks like, click the Start the Animation icon,

. How does that look?

Lets add another level of detail, by capturing camera angles at specific times. Click the Create a New View @ Time icon,

; this will open View @ Time GUI.

Under the Name pull down menu select the predefined view called Right, click Apply, this will add the view to the sequence window.

Click the Name pull down menu and select ISO. Under the Time area put 3 in the value field, click Apply. Repeat adding the following views; Angle and ISO2, at 3-second intervals. When you are done it should look something like this:

Play the sequence; click the Start the Animation icon, . If the camera angles are not were you want them, you can click on the camera object in the sequence window and move it to were you want it.

Page 18 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Step Seven: Lets view the animation, click the Playback icon, it looks like a VCR control panel.

. This will open the Playback GUI;

Click the icon to play the animation; you can even control the speed by moving the toggle switch. If you want to save the animation to a movie file (MPEG), click capture.

Leaving everything as default, click ok, this start to create the movie. Save the file in Pro/E. You are done the tutorial! There are other details you can add to the animation, like Display settings and render output. If this is of interest, please contact you local Design Animation export. Open the file called Final_Top_Level.asm to see the advance details.

Page 19 of 20

Title: Design Animation Date: 8/8/2002 PTC-MSS Services

Tutorial Evaluation: Name:

Title:

… Engineer

… Designer

… Foundation

… Draftsmen

… Mfg. Engr.

… Advanced Assembly Extension

PTC Products Used:

… Behavioral Modeling

Time using Pro/E:

… 0-6 months

… Intralink

… 6-12 months

… Analyst

… Advanced Surface Extension

… Modelcheck

… 1-2 years

… Tech. Pubs.

… All

… 2-5 years

… 5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

…………………………

1

2

3

4

5

2.

The exercise was easy to understand:

…………………………

1

2

3

4

5

3.

This tutorial will help me on current projects:

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1

2

3

4

5

4.

These techniques make Pro/E a more effective tool:

…………………………

1

2

3

4

5

5.

These techniques will increase my speed using Pro/E:

…………………………

1

2

3

4

5

What concepts/techniques learned from this tutorial will you apply on the job? 1) 2) 3) What would you like to see as a future tutorial at your company? 1) 2) 3) What can be done to improve these tutorials for your company? 1) 2) 3)

Additional Comments:

Page 20 of 20

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Pro/ECAD Benefits, Techniques and Best Practices Tutorial

Table of Contents: 1) Objective 2) Overview 3) Metric 4) Tutorial 5) Key Vocabulary 6) Tutorial Evaluation

Page 1 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Objective: At the end of this tutorial, you will be able to: • Repeat the steps necessary to ensure a smooth exchange of data between the Electrical and Mechanical department. • Formulate an internal process for managing changes between the Electrical Engineer & the Mechanical Engineer. • Improve product quality. • Promote a concurrent design environment w/ out fear of design ramifications downstream and from design issues w/in your team members.

Overview: In the typical design process, the Mechanical Designer defines the board shape, specifies important “keep in” and “keep out” areas, and places critical components such as connectors, switches, displays, and LED’s using Pro/Engineer. This information is exported via an IDF file to the PCB designer to use as the basis for the board layout in the PCB layout system. After placing the remaining components, the fully placed board assembly is passed back through the IDF file to the Mechanical Designer to make sure the board assembly fits into the final product package. Multiple iterations of this basic flow typically occur during the product design phase. Why is it beneficial to the Electrical Engineer? The electrical engineer can communicate design requirements effortlessly to the Mechanical Engineer. This information includes, hole placement, pin hole placement, keep in/keep out areas, and board size. Why is it beneficial to the Mechanical Engineer? Mechanical Engineers can specify mechanical requirements and transmit them directly to an electrical engineer’s PCB layout program. Most all PCB layout programs have an export capability called an IDF file. This is similar to exporting an IGES file. The difference is that exact component information (placement and size) is contained within the file. This information is transmitted effortlessly to the Mechanical Engineer. With other translation methods, such as IGES, data is often lost in the conversion. What are the mechanical aspects that are critical to the Mechanical Engineer? 1) Interference Checking- Accurate assemblies are created and can be joined with other assemblies to check interference between mating parts. 2) Mass Properties can be calculated automatically by using a library of ECAD component part files that contain accurate mass property information. 3) Static, dynamic, thermal analysis can be performed.

Page 2 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Metric: The following example illustrates the immediate impact on utilizing Pro/ECAD to automate Printed Wiring Assembly (PWA) design information exchange between the PCB design group and the mechanical engineering group. This is done to: 1. Increase accuracy 2. Enhance efficiency And removing need of interface drawing creation: 1. Translates in 1-2 man-days saving per PWA assembly 2. Immediate communication of design changes to Mechanical Engineering upon import of PCB design data 3. Eliminates need for change documents The previous practice of exchanging drawings and DXF data resulted in longer effort and inaccurate results as exact component placements were difficult to establish.

4 3.5 3

DXF/Drawings

2.5 2

Pro/ECAD

1.5 1 0.5 0

Data Exchange

Page 3 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Tutorial: What is the best way to use Pro/ECAD? You can import parts from an ECAD database in two ways: 1. Let the Pro/ECAD translator automatically create basic 3-D extrusions of the part outlines as they are read in, or 2. Use a map file to reference a library of ECAD part files you have set up beforehand. If you use the automatic method, a separate .prt file for each component is automatically created and added to the session. These files can be saved and customized in Pro/E as necessary to more accurately show the true shape of the component. After they are customized, you can use the import map file (ecad_hint.map) to substitute them for the automatically generated parts if you run the import process again. If you already have custom part files for ECAD components (ECAD Library), you can set up the map file in advance to substitute them for the automatically generated parts. Using this method you get a more accurate representation of the components. You will see examples below showing with a library and with out. A. How do I use existing PCB files with Pro/ECAD? STEP 1: Create a New Model w/ the .emn file: File > Open > To create a new model > Change your type to ECAD IDF (*.emn) Select an .emn file and provide a name for the board. The following dialog box will then appear:

Page 4 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Select Options near the bottom of the screen: Under the options tab you will see a listing of holes that will be imported. You may want to shut the holes off depending on the number. Some times you will see a number (say for this example 460). This represents the pin holes in the PCB board. Pro/Engineer will generate a hole for every type listed. To reduce regeneration times turn on only the holes that are needed. Uncheck the first option to filter out the 460 PIN holes since they are not needed for our design.

Page 5 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

The imported PCB board with holes and keep out/keep in areas is shown below:

Step 2: Create a new assembly File > New > Assembly > (give it a name) Component > Assemble > (In Session) > Select the PCB board part (Select the default constraint to assemble automatically.) Step 3: Add the components from the .emn file. Insert > Data From File… > Change your type to ECAD IDF (*.emn) and select the same .emn file > Open The following options will appear in the menu: • • • •

• •

Components: Import component library Placement: Import component placement Other Outline: Import other outline(s) which are volumes representing non-electrical items that would not have reference designators Investig Plc: Imports component placements in investigate mode. This option lets you selectively accept or reject the placements of new or changed components Investig Geom: Investigate component’s geometry changes Use Def Template: Use default template for new Components Page 6 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Accept the default options and select Done. The file will import all the components creating new part files. View the model tree to verify this. Below is the imported assembly: 1) w/out ECAD library

2) w/ ECAD library

B. How do I use start the board design in Pro/E? STEP 1: Create an ECAD Area in the model: W/ a board already modeled, Insert > Cosmetic > ECAD Area… The following menu will appear: • • • • • •

Regular Sec: Feature will regular sketching plane Project Sec: Feature will use projection of section on selected surface. Xhatch: The created feature will be meshed No Xhatch: The created feature will not be meshed 3D Volume: The created feature will be 3D quilt Two Sides: Create two areas w/ the same section on both sides of the board.

Refer to Key Vocabulary section for remaining definitions.

Page 7 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Let’s select Xhatch > 3D Volume and select any surface for the feature to be created on. Sketch your area:

And enter the height values to get the following result:

STEP 2: Export the board outline and component information: File > Save A Copy Ensure that the type is set to ECAD IDF (*.emn) and select from the following options:

Now you are ready to import the file into your ECAD package. Page 8 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Workflow That Enables The Best Use Of Pro/ECAD 1) The Mechanical Engineer creates a PCB board inside an assembly that mounts to their existing hardware. 2) Mounting holes are created. 3) Keepin/Keepout areas are created. 4) Connectors (from the ECAD library) are placed on the PCB board. 5) File is exported to an IDF 3.0 file. 6) The IDF file is read into the PCB layout program. 7) Components are added observing the keep in and keep out areas on the board. 8) The file is exported out of the PCB layout program back to an IDF 3.0 file. 9) The Mechanical Engineer opens up their existing PCB board and appends the new IDF file. New components are added and existing components are automatically moved because of the PCB layout engineer’s design change. This is a single iteration, but this can continue until the board is fully designed. Interference checks can be run and thermal analysis is one step away because of a fully designed PCB board.

Page 9 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Key Vocabulary for Pro/ECAD: ECAD: Electrical Computer Aided Design ecad_hint.map file: an ASCII file you use to control the following functions in the ECAD import-export process: · Substituting custom made Pro/E parts for automatically extruded parts on import. · Allowing or disallowing specified parts on import. · Allowing or disallowing specified parts on export. · Changing an ECAD reference designator to a different string for import (If for example the ECAD reference designator uses characters that are illegal in Pro/E). · Changing an ECAD 'other outline' string for import (If for example the ECAD reference designator uses characters that are illegal in Pro/E). Pro/ECAD searches the working directory for ecad_hint.map and references it every time import occurs. If the file is empty or has no relevant information it is ignored. You can use the configuration option ECAD_MAPPING_FILE <path> to set a default location for the ecad_hint.map file. If you set a path with this config option, the working directory is not searched. Sample excerpt: # # A template for ecad_hint.map # map_objects_by_name-> ECAD_NAME "CSTCS1" ECAD_ALT_NAME "N7414N" ECAD_TYPE "" MCAD_NAME "CSTCS1_PN-" MCAD_TYPE "part" END # map_objects_by_name-> ECAD_NAME "GF-1" ECAD_ALT_NAME "SC1A17.53-ND" ECAD_TYPE "" MCAD_NAME "GF-1_PN-" MCAD_TYPE "part" END # map_objects_by_name-> ECAD_NAME "J1_10" ECAD_ALT_NAME "A2099-ND" ECAD_TYPE "" MCAD. . . . . .

Page 10 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

IDF: Intermediate Data Format PCB: Printed Circuit Board. Place Keepin: region of board within which components are placed. Place Keepout: region of board where components cannot be placed. Place Region: region of board to place similar components within. Pro/ECAD: an interface tool that is available with every Pro/Engineer Foundation seat. This functionality enables communication between the Electrical Engineers creating PCB layouts and Mechanical Engineers creating packaging for the electrical components. This technology enables 3D models of the PCB board, components, and connectors to be created and placed automatically for the Mechanical Engineer. It also allows communication of keep in/keep out areas, board size, and hole placement between both Mechanical and Electrical Engineers. Pro/ENGINEER: the leading 3D product development solution, enabling designers and engineers in 31,000 companies to bring superior products to market faster. Spanning the entire product development process, from creative concept through detailed product definition to serviceability, Pro/ENGINEER delivers measurable value to companies of all sizes and across all industries. Route Keepin: region of board where routing is allowed. Route Keepout: region of board where routing is not allowed. Via Keepout: region of board within which vias are not allowed.

Page 11 of 12

Title: Pro/ECAD Techniques, Benefits & Best Practices Date: 12/05/01 PTC-MSS Services

Tutorial Evaluation: Name:

Title:

… Engineer

… Designer

… Foundation

… Draftsmen

… Mfg. Engr.

… Advanced Assembly Extension

PTC Products Used:

… Behavioral Modeling

Time using Pro/E:

… 0-6 months

… Intralink

… 6-12 months

… Analyst

… Advanced Surface Extension

… Modelcheck

… 1-2 years

… Tech. Pubs.

… All

… 2-5 years

… 5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

…………………………

1

2

3

4

5

2.

The exercise was easy to understand:

…………………………

1

2

3

4

5

3.

This tutorial will help me on current projects:

…………………………

1

2

3

4

5

4.

These techniques make Pro/E a more effective tool:

…………………………

1

2

3

4

5

5.

These techniques will increase my speed using Pro/E:

…………………………

1

2

3

4

5

What concepts/techniques learned from this tutorial will you apply on the job? 1) 2) 3) What would you like to see as a future tutorial at your company? 1) 2) 3) What can be done to improve these tutorials for your company? 1) 2) 3)

Additional Comments:

Page 12 of 12

http://www.kinetivision.com/freevids/neut_plane_draft.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/neut_plane_draft.htm [28.11.2002 13:09:55]

collaboration

Pro/ENGINEER 2001 innovation

Update Reference global solutions

© 2001 PTC

Tool Relocation Matrix OLD LOCATION File > W orking Directory File > Export File > Import > New File > Import > Append Edit > Modify Edit > Reroute Edit > Redefine Edit > Find View > Default View > Spin/Pan/Zoom View > Orientation View > Model Display View > Datum Display View > Performance View > Advanced > Visibilities Utilities > Colors > System Utilities > Colors > Entity View > Analysis Display View > Advanced > Photorender Utilities > Model Tree Settings > Load Utilities > Model Tree Settings > Save Datum menu ( on menu bar) Utilities > Compare Part Info > BOM Info > Pro/Engineer Objects Info > Regen Info Utilities > Trail/Training File Utilities > Distributed Computing Utilities > Preferences W indow > Open System Help > Pro/E Help System Help > I-Site Preferences Help > Round Tutor Help > Customer Services Info © 2001 PTC

NEW LOCATION (*New Label Only) File > Set W orking Directory* File > Save A Copy* File > Open* Insert > Data From File Edit > Properties* Edit > References* Edit > Definition* Edit > Find in Model Tree* View > Default Orientation* This command has been removed View > Reorient* View > Display Settings > Model Display View > Display Settings > Datum Display View > Display Settings > Performance View > Display Settings > Visibilities View > Display Settings > System Colors View > Display Settings > Entity Colors View > Model Setup > Analysis Display View > Model Setup > Photorender View > Model Tree Setup > Open Settings File View > Model Tree Setup > Save Settings File Insert > Datum Analysis > Part Comparison Info > Bill of Materials Info > Session Info > Pro/Engineer Objects Utilities > Model Player Utilities > Play Trail/Training File* Utilities > Processing Distribution* Utilities > Options* W indow > Open System W indow* Help > Contents and Index* Help > PTC I-Site* Help > Rounds Tutorial* Help > Technical Support Info* 2

Pro/E 2001 - File > AKA Import New

AKA Export

© 2001 PTC

3

Pro/E 2001 - Edit >

© 2001 PTC

4

Pro/E 2001 - View >

© 2001 PTC

5

Pro/E 2001 - Insert >

AKA Import Append

© 2001 PTC

6

Pro/E 2001 - Analysis >

© 2001 PTC

7

Pro/E 2001 - Info >

© 2001 PTC

8

Pro/E 2001 - Applications >, Utilities >, Window >, Help >

© 2001 PTC

9

Pro/E 2001 - Select Primary Items

RMB

© 2001 PTC

10

Pro/E 2001 - Select Geometry

RMB

© 2001 PTC

11

collaboration

innovation

Automated Surface Cleanup Import Data Doctor

global solutions

© 2000 PTC

Import Procedure Create

New file from Template Append imported file Select Csys Check Import Log Info-Geom Check Redefine Import feature  

Automatic

 

Manual

Perform

Manual Surface

Cleanup Collapse Features

© 2000 PTC

2

Import Data Doctor

Automated

Surface Cleanup Constraint

Manager Zip

Gaps

Compare

Surfaces Collapse

Geometry

© 2000 PTC

3

Benefits Automated Surface Cleanup: Faster Repair of Imported Geometric Data Fixed models are closer to original design intent Visual Feedback of repair process Preview of Changes Better data reuse (customers, internal, suppliers) Collapse Features: Reduced feature count = faster regeneration Improved Reference handling

© 2000 PTC

4

Constraint Manager Modify      

Exclude Include Suspend

Modify          

Wireframe

Constraints

Frozen Frozen w/ boundary Master Tangent Split

Display          

© 2000 PTC

Options

Frozen Higher Order Surfs Master Tags Fixed Surfs 5

Constraint Manager - Modify Wireframe

Exclude: Removes selected surfaces, curves and vertices from automatic surface cleanup computation Suspend: Edge chains may be suspended Example: Two complex quilts intersect each other. Intersection edge can be suspende to individual quilts will be fixed without adjusting their intersection

© 2000 PTC

6

Constraint Manager - Modify Constraints Frozen: Allows computation to manipulate the surface boundary in the plane of the surface’s original shape. Frozen w/boundary: Does not allow for surface intersection. Master: Allows for master edge between unfrozen surfaces to be selected as their intersection. (Pro/E will normally compute a middle edge between the two boundaries.) Split: Allows for a single surface to be split into two separate surfaces (Ex: Most of a surface is good, but small portion needs reworking)

© 2000 PTC

7

Constraint Manager - Display Options Tangent Edge

Frozen w/boundary Frozen Surface

Master Edge

Split Surface

© 2000 PTC

8

Analyze Changes - Compare Surfaces Available

after Compute has been selected from CM Shows Color Plot of change in surface from IGES data Display Options: Color Selection (Linear, Logarithmic, Two Color) Limits Accuracy

© 2000 PTC

9

Manual Repair - Collapse Geometry Not

all problems can be automatically fixed. Pro/Engineer’s powerful surfacing tools to repair or replace problem surfaces.

Collapse Geometry Capabilities: Reduce Feature count Simplify Parent/Child Relationships Deletes history of imported feature repair without invalidating references.

© 2000 PTC

10

Advanced Surfacing Course Length: - 2 Days Topics: ‹Datum

curves ‹Variable section sweeps ‹Merging surfaces ‹Extending surfaces ‹Surface Analysis ‹Ensuring tangency between neighboring surfaces ‹Creating solid features from surfaces ‹Creating surfaces from IGES files ‹Surface information ‹Surface creation method z © 2000 PTC

blended, swept, revolved, flat, boundaries 11

Importing/Exporting 3D Data Course Length: - 1 Day Topics: ‹Setting

up for Export ‹Setting up for Import ‹Importing Surfaces ‹Repair of Import Surfaces ‹Importing Wireframe Data ‹Development of solids using foreign surface data ‹Correction of surface data to generate solids ‹Generation of parametric features with relation to imported data ‹Using wireframe information to create solids

© 2000 PTC

12

Pro/ENGINEER 2001 Drawing Cheat Sheet

Drawing Sketcher Toolbar

Enable Sketching Chain

See Icon Definitions

Crossed Construction Lines

Sketch Lines

Remember Parametric Sketching References Select Items (hold SHIFT to gather more) Sketch Arc by Center and Endpoints

Construction Lines Ellipse by Center and End Points

Sketch Construction Circle

Sketch Circle

Ellipse by End Points

Sketch 3 Point or Tangent Arc Sketch a Fillet Sketch a Spline Curve thru several points Sketch a Point Sketch a Chamfer

Select Dimension and rightclick popup menu

Insert a Datum Point Cut Draft Entities, Notes and Tables

Paste Draft Delete 1 or Entities, Notes Show/Erase more drawing Dialog Box and Tables objects

Cleanup dimensions

Drawing Toolbar

Insert a Datum Axis

Insert a Coordinate System

Select View and rightclick popup menu Copy Draft Entities, Notes and Tables

Move/Align Set current drawing model Several Objects

Switch detail items to another view

Toggle between Drawing Sheets

Courtesy of James Paschetto - PTC

collaboration

Pro/Process For Assemblies & Round Tutor innovation

global solutions

© 2000 PTC

PRO/PROCESS FOR ASSEMBLIES

© 2000 PTC

2

Pro/Process For Assemblies ‹ You’ll see how to quickly create a fully annotated assembly process

plan by referencing, but never affecting, the original design assembly. ‹ You’ll see how tools and fixtures can be added to the process plan

data-base required for fabrication purposes without affecting the design BOM. The benefits of using Pro/PROCESS for ASSEMBLIES are: ‹ ease-of-use ‹ speed ‹ associativity back to the design assembly ‹ ability to regroup design components independently from the design

structure. © 2000 PTC

3

Pro/Process For Assemblies Unlike traditional methods, Pro/PROCESS for ASSEMBLIES uses the information already available in the design assembly such as component placement and parameter information and automatically updates the process plan when this information changes. Furthermore, the process plan and service documentation can be created concurrently while the design assembly is still being developed - as components are added to the design assembly, they can be added to the process plan. The benefit, again, shorter time to market.

NOTE: PRO/PROCESS FOR ASSEMBLIES ALLOWS FOR MULTIPLE EXPLOSION STATES VERSUS A SINGLE ONE W/OUT THIS MODULE. © 2000 PTC

4

Creating a Process Plan 1. Please name the process plan accordingly i.e. _pp

© 2000 PTC

5

Creating a Process Plan 2.

© 2000 PTC

3.

6

Creating a Process Plan 4. Your assembly will come in hidden-line. Now you may select the models you want to add to the first sequence. © 2000 PTC

7

Creating a Process Plan

Your selected models will become shaded to graphically inform you of which models have/have not been added to an assembly sequence. © 2000 PTC

8

Creating a Process Plan 5. Once you hit Æ DONE then double-click any of the options to fill in these parameters in the dialogue box. DESCRIPTION : Input a one or two line sentence to describe this sequence

‹

SIMPLFD REP : Create/select a pre-defined simplified representation if required ‹

‹ © 2000 PTC

EXPLODE STATE : Create/select an explosion state 9

Explosion Position

© 2000 PTC

10

Explosion Offset Lines

© 2000 PTC

11

Creating a Process Plan ‹

© 2000 PTC

VIEW : Create/specify a view for this step

12

Creating a Process Plan

‹ TIME ESTIMATE : Enter a time estimate in hours if req’d

‹ COST ESTIMATE : Enter a cost estimate if req’d

Repeat/redefine creation of sequences as necessary … © 2000 PTC

13

Creating a Process Plan Document 1.

© 2000 PTC

14

Creating a Process Plan Document

Automatically all information that you have specified earlier fills into the table.

© 2000 PTC

15

Creating a Process Plan Document 2. Specify the state that you would like to place onto the next sheet 4. Add your view & balloons …

3. Now add another sheet to place the steps … © 2000 PTC

16

Creating a Process Plan Document 5. You also have the ability to modify the display of newly added components for your current state as well as how you wish to represent components that were already specified in previous steps.

© 2000 PTC

17

Creating a Process Plan Document

© 2000 PTC

18

ROUND TUTOR

© 2000 PTC

19

How to Activate The Round Tutor

© 2000 PTC

20

Create A Round …

Once you’ve enabled the “Round Tutor” then when you begin to create a round, an applet will fire up and guide you through the entire Round creation process.

© 2000 PTC

21

Round Tutor Contents

To see a listing of contents, activate the CONTENTS icon.

As you will notice, each line is a hyperlink to a document for that topic.

© 2000 PTC

22

Tutor Map To see a User Interface Map for Round Creation, activate the TUTOR MAP icon. And also each step is a hyperlink w/ a more detailed description of that round type. Refer to the next page for the entire Round Map.

© 2000 PTC

23

http://www.kinetivision.com/freevids/simp_pro_program.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/simp_pro_program.htm [28.11.2002 13:26:02]

collaboration

Pro/ENGINEER Tips & Tricks innovation

Terry Amundson Mark Fischer global solutions

August 13, 2002

© 2000 PTC

Agenda ƒ

Introductions

ƒ

Goals for Today

ƒ

General ProE Tips

ƒ

Drawing Tips

ƒ

Questions

© 2000 PTC

2

Tips & Tricks – Goals

ƒ

A Bunch of Things You Probably Knew

ƒ

Some Things You Didn’t Know

ƒ

Maybe One Thing That Works Great That You Didn’t Know

© 2000 PTC

3

Tips & Tricks – General ProE ƒ

Middle Mouse Button to Accept

ƒ

Right Mouse Button for Pop-up Redefine/Info/Etc.

ƒ

Use Fast Hidden Line Removal

ƒ

Renaming Features

ƒ

Display Datums While Spinning

ƒ

Component Display States

ƒ

Explode States

ƒ

Assembly – move component using CTRL-ALT

ƒ

Drag & Drop Files – from File Explorer

© 2000 PTC

4

Tips & Tricks – Model Tree ƒ

Right Mouse Features from Model Tree

ƒ

Drag and Drop Re-Order

ƒ

Drag and Drop Insert Mode

ƒ

Right Mouse in Model Tree

ƒ

Custom Model Tree Setups

ƒ

Rename/Modify Features in Model Tree

© 2000 PTC

5

Tips & Tricks – Drawings (Clarity) ƒ

Z-Clipping (also decreases repaint time)

ƒ

Member Display

ƒ

Relating Draft Items to a View

ƒ

Quilt Hidden Line Removal

ƒ

Fonts

ƒ

Use @o to attach leader to multi-line text

© 2000 PTC

6

Tips & Tricks – Drawings (Ease of Use) ƒ

Right Mouse Modify

ƒ

Align Views / Unalign Projected Views

ƒ

Copy from other Drawing

ƒ

Template Drawings

ƒ

Word Wrap (2001)

© 2000 PTC

7

Tips & Tricks – Drawings (Speed) ƒ

General Tips: ƒ

Turn off datum displays

ƒ

Work in wireframe

ƒ

Set auto_regen_views to no

ƒ

No View Open (open_simplified_rep_by_default=yes)

ƒ

Erase/Resume Views

ƒ

Snapshot of View

ƒ

Merge Drawings

© 2000 PTC

8

BOM Graph

© 2000 PTC

9

File Open Create a Table Display in your workspace with 2 columns: Model Name, Description

© 2000 PTC

10

File Open Create “Fly Outs” to sort for commonly used objects: Parts, Assemblies, Drawings

© 2000 PTC

11

File Open Preview Config.pro Options: z save_model_display z save_drawing_picture_file

shading_low embed

NOTE: “shading_low” will take longer to process than “shading_high”, but takes up less disk space, and is “lighter” when working with “graphics reps”.

© 2000 PTC

12

Open Rep Set config.pro option so that Open Rep dialog box comes up by default Open_simplified_rep_by_default

© 2000 PTC

YES

13

Hide / Un Hide Hide / Unhide available from: ‹RMB

in working window

‹RMB

from model Tree

‹View

menu in pull down

‹Assembly ‹Part

– works on Components, Features

– works on Datums, Curves, and Surfaces

z

Turn off 1 datum at a time

z

No need to create excess layers

© 2000 PTC

14

Datum Tag Display You have the ability to turn off labels for: Datum Planes, Coordinate Systems, Axis, Points

© 2000 PTC

15

Intent Manager (Sketcher) Learn How to Use the tool ! Turn on these Config.pro options:

© 2000 PTC

sketcher_readme_button

yes

sketcher_overview_alert

yes

16

Tips & Tricks – Sketcher

Middle Mouse Button to get Pick Arrow

Mapkeys – Create & Iconize

© 2000 PTC

17

Sketcher Ability to reference an entity that intersects the sketch plane

Pick XSEC button Select SURFACE

© 2000 PTC

18

Pro/ENGINEER 2001 Sketcher Cheat Sheet

Line

Sketcher Tools Toolbar

Circle

Sketcher Preferences

Select Item (hold SHIFT to gather more) Rectangle

Arc Tool tangent & 3-point

Concentric Arc

This menu appears when you have nothing selected and click the Right Mouse Button

Concentric Circle

Ellipse

Arc Center & Ends

Conic Arc

Fillet

Elliptical Fillet

Reference Csys

Create Point

Use Edge

Offset Edge

Dynamic Trim

Trim

Divide

Mirror

Scale & Rotate

Copy

Complete Section

Quit Section

Spline

Create Dimension

Centerline

Modify (dimensions, splines & text)

Sketcher Constraints

This menu appears when you have an item selected and click the Right Mouse Button Pressing the DELETE key will delete selected items

Create Datum Plane Create Datum Axis Create Datum Curve Create Datum Points Create Datum Csys Create Analysis Feature

Asynchronous Datum Creation Toolbar (Used Anytime out of Sketcher Mode)

Sketcher Toolbar

Undo Redo

Toggle Vertices

Reorient to Sketch View

© 2000 PTC

Toggle Dims

Toggle Constraints

Toggle Grid

Ethan Meyer - PTC MSS 19

ISDX Tutorial D:\Pro/E Loadpoint\apps\tutorials

© 2000 PTC

20

Flatten Quilt Create flat pattern of Any* Part *NOTE: All surfaces must be tangent

© 2000 PTC

21

“Trace Sketch” “Scan” sketches, apply to Surface Can be used as a sketching aid

© 2000 PTC

22

Performance Options Turn off display of datums For BEST performance while SPINNING and FLY THROUGH Of LARGE Assemblies

(Blanking Datums with LAYERS or turning Off DISPLAY of DATUMS with icon is NOT The same!)

© 2000 PTC

23

Performance Options Fly Through – from inside Pro/E

© 2000 PTC

24

Intent Rounds

Pick in 1 Location All 4 Edges are selected! © 2000 PTC

25

Increased understanding of the design Design Insight z Model Player z VCR-like controls over the regeneration of the model z Clear understanding of how the model was constructed

© 2000 PTC

26

Compare Part Shape Comparison z z View different versions of same model z z Comprehensive graphical display of feature and geometric differences z z

Compliments Shape Indexing and offers text report of feature differences

© 2000 PTC

27

BMX Optimization Features z Capture critical design requirements persistently within the model itself z Ensure that these requirements are ALWAYS met, even as the design changes

always persistently continually

Ensure container holds exactly 5 liters. Maintain balanced crankshaft. Minimize design’s mass. Maximize critical clearance. © 2000 PTC

28

Import/Export of board & components 2001 Features z z

Geometry

z z

Attributes

z z

ECAD Areas

z z

Direct Interfaces z z

Allegro Boardstation

z z

Visula

z z

z z

Industry standard interfaces z z z z

z z

Investigation of modifications on re-import z z z z

© 2000 PTC

IDF2.0 IDF3.0

Board geometry Component placement 29

External Copy Geom ‹A

great way to create Castings & Machined Parts

‹Use

External Copy Geoms – not Copy Geoms in Assembly -NO dependence on Assembly hierarchy

© 2000 PTC

30

Sheet metal Hints Create all sheet metal parts with “Absolute Accuracy” (.001) Create all “Form Tools” at same “Absolute Accuracy” Config.pro options: enable_absolute_accuracy

yes

accuracy_lower_bound

0.0000100

HINT: you may have to sketch a small datum curve in your “Template Part” in order to set the “Accuracy” low enough!

© 2000 PTC

31

CCS Composites Benicia, CA.

The Company z z Specialists in Compression Molding for custom and production molding of high performance carbon fiber and glass reinforced composites. z z Provides complete design thru manufacturing capabilities. Needs for collaboration • A majority of molded products are jointly designed with the customer to reduce component & associated tooling costs. • Early inclusion of the tool makers to streamline cost and schedule. Benefits z z “Since we started using Pro/Collaborate, we have reduced the time to create a customer product” z z “Our customers are very pleased with the ability to collaborate with us on new projects”

© 2000 PTC

32

PTC Customer Care Portal http://www.ptc-mss.com Links to: z Tips & Techniques z Tutorials z FAQ z Customer Support z User Groups z Documentation z Training z And Much Much MORE!

© 2000 PTC

33

http://www.kinetivision.com/freevids/relpattern.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/relpattern.htm [28.11.2002 13:34:11]

collaboration

innovation

How To Use Layers

global solutions

© 2000 PTC

Layers ‹Reasons

for Using Layers ‹Creating Layers ‹Associating Items to Layers ‹Default Layers ‹Display Status ‹Tips and Tricks

© 2000 PTC

2

Reasons For Using Layers

Layers provide a means of organizing items such as features, components, draft items, and other layers, so you can perform operations on them collectively. Reduce Display Clutter! Reduce Graphics Display Time Suppress by Layer to Quickly Simplify Geometry Delete & Plot Items by Layer

© 2000 PTC

3

Is this what most of your models look like?

Would this be easier to work with?

© 2000 PTC

4

Creating Layers ‹Use

the “Layer Display” icon. ‹Use the “Create Layer” icon. ‹Default Layer: optional, choose if you’d like to set.

© 2000 PTC

5

Adding Items to a Layer ‹Use

the “Add Item” icon. ‹Choose the items to add. ‹Select the items. Notes: ‹Items can be associated to more than one layer. ‹Pro/E does not automatically place items on layers.

© 2000 PTC

6

Wouldn’t you rather have it automatic? Specifying default layers in your config.pro is an effective way to automate layering schemes. With it you can: ‹Automatically

add items to layers as you build your model (i.e. datum planes, datum curves, coordinate systems, etc.) ‹Establish common naming conventions ‹Allow other users to understand what your layers represent

© 2000 PTC

7

Editing your config.pro To create a default layer, edit your config.pro file. Specify the value of the “def_layer” option as type-option layername. The type-option is the type of item that you want to place on that layer. The layername is the name of the layer. Config Option

type-option layername

For the first line, Pro/E automatically assigns all new datum planes to the 1_ALL_PLANES layer automatically as the they are created. © 2000 PTC

8

Manually setting Default Layers

Alternately, you can assign default layers during the creation of a new layer by using the “Default Layer Types” option in the New Layer dialog box. The drawback to this is that once you exit and bring the model into a new session, the Default Layer Type is not retained. The reason is because when you specify default layer types in this manner, it does not write it to the config.pro file. To permanently keep the default layering scheme, update your config.pro file.

© 2000 PTC

9

Default Layers in Session To see the default layers in the current session, click on the Default Layers command in the Layer Pull Down Menu

© 2000 PTC

10

Setting the Display Status One of the primary reasons to use layers is to control what information is displayed on the screen. From the Layers dialog box, you can perform the following on layers: Show Displays items on screen. Blank Removes items from screen. Isolate Displays items on screen while removing all non-isolated layers from screen Hide

Removes items from screen when when working in No Hidden mode. In Hidden Line mode, it displays the component entirely in hidden lines. No effect when in Wireframe and Shade mode.

Link

Makes an independent drawing view dependent.

Note: Blanking or Isolating a layer does not increase regeneration time. Pro/E still regenerates blanked items. © 2000 PTC

11

Display Status Tips Display status only affects non-solid geometry. For example, if you associate a hole to a layer and set the display status to Blank, only the non-solid geometry, or axis of the hole, is removed from the screen. Only exception is blanking components in an assembly removes the components from the screen. Isolate has priority over Blank status. If an item is associated to two layers, one Isolate and one Blank, then the item will be displayed on the screen. Display has priority over Blank. If an item is associated to two layers, one Display and one Blank, then the item will be displayed on the screen.

© 2000 PTC

12

Display Status Tips The following tips apply when in Assembly mode: If a layer is set to Isolate, Pro/E blanks all other layers and all other items not associated to any layer. Isolate affects the level of the object and all levels above it. Blank affects the level of the object and all levels below it. By assigning common names to the layers throughout the levels of the assembly, you can control the display status on layers in lower-level models. When you change the display status of an upper-layer level, the change will propagate down through to all layers with the same name.

© 2000 PTC

13

© 2000 PTC

14

Example: Part Mode Only three items have been applied to three separate layers: Datum A, Datum C, Hole.

Layer Hole Datum A Datum C

© 2000 PTC

Status Show Show Show

Layer Hole Datum A Datum C

Status Blank Show Blank

Layer Hole Datum A Datum C

Status Show Show Isolate

15

Example: Assembly Mode Only three items have been applied to three separate layers: Comp B, Comp C, ADTM A.

Layer Comp B Comp C ADTM A

© 2000 PTC

Status Show Show Show

Layer Comp B Comp C ADTM A

Status Blank Show Blank

Layer Comp B Comp C ADTM A

Status Isolate Show Show

16

http://www.kinetivision.com/freevids/simp_extr_prot.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/simp_extr_prot.htm [28.11.2002 13:38:05]

http://www.kinetivision.com/freevids/setup_units.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/setup_units.htm [28.11.2002 13:41:54]

Title: “Name of Tutorial” Date: 7/16/01

“Simplified Reps”

Table of Contents: 1) Objective 2) Overview 3) Topic Value 4) Tutorial 5) Test for Retention 6) Key Vocabulary 7) Tutorial Evaluation

Page 1 of 13

Title: “Name of Tutorial” Date: 7/16/01

Objective: At the end of this tutorial, you will be able to: • Definitions: Commonly used selection criteria • How to Create a Simplified Rep o Set and Unset Components • Differentiate between common Graphics Settings • Substitute a Lower Level Simplified Rep into a Top Level Assembly • Restate the concept of when to use a Simplified Rep

Overview: The purpose of this module is to understand how to create, modify and manage usage of Simplified Representations. In addition, leverage existing Simplified Reps into higher-level Assemblies.

Topic value: Due to proper usage of Simplified Representations, Lam Research has been able to reduce the amount of time needed to open one of their Top Level Assemblies from

20 minutes to less then 2 minutes or 90% faster.

Page 2 of 13

Title: “Name of Tutorial” Date: 7/16/01

Simplified Rep Tutorial To begin creation of a Simplified Rep select 1) Simplified Rep/Create

2) Select the Default Rule. In general Master Rep and Exclude Component will be the two most commonly chosen options.

NOTE: For this tutorial Master Rep will be chosen as the default Definitions: Master Rep: • Master Rep defines that initially all components are shown and the user must select the items to be removed. • Mater Rep allows for all future assembled components to be added to ALL Simplified Reps with the default Rule as Master Rep. To avoid this use Exclude Comp instead. Exclude Comp: • Exclude Comp defines that the initial state of components are all blanked and the user must select the items to be shown • Exclude Comp prevents all future assembled components to be added to any Simplified Reps with the default Rule as Exclude Comp. Graphics Rep • Graphics Rep reduces the amount of data that is pulled into Ram. (25%) • Not as commonly used • Cross Section Not allowed • No Mass prop Geometry Rep Page 3 of 13

Title: “Name of Tutorial” Date: 7/16/01 • •

Geometry Rep reduces even more data (50%) Not commonly used

3) Enter Name for Simplified Rep:

4)

Edit Rep Options. If needed change from Master Rep to Graphics Rep or Geometry Rep. Master Rep is the most common selection. Master Rep: • Which ever was chosen in Step 2 will be displayed here Graphics Rep: • Replaces THE SELECTED parts with a lightweight version approximately 25% of original size. Mass Prop and Cross Section functionality cannot be calculated. Geometry Rep: • Replaces THE SELECTED parts with a slightly larger weight model at approximately 50% of the original size. Mass Prop and Cross Section functionality can be calculated. Substitute: • In the Context of an Assembly: Allows the user to replace a component with a part level Simplified Rep Default • Removes selected components off of the Simplified Rep that is being defined

Page 4 of 13

Title: “Name of Tutorial” Date: 7/16/01 5) Selecting Components: Now select the components that need to be displayed on the Sim Rep. The parts on the model can be directly selected or the model tree can be used. See below for description on the two techniques. Model Tree • •

While in the Creation menus of a Simplified Rep, the Model tree adds a column to display the components that are affected by the Sim Rep being defined. Removal of components can be selected off the model tree by selecting the model name

Working Window • •

Components can be selected from the working window (Part to be removed is selected in red) Reflects in Model Tree

Page 5 of 13

Title: “Name of Tutorial” Date: 7/16/01 Notes on Part Selection: Regardless of where the part is selected, the model tree will reflect the removed components. Sim Rep Name

Even though components are selected to be removed from the Sim Rep, nothing will change until you either • Update Screen • Complete the Sim Rep When Update Screen is selected the screen will show the resultant display based on the selected items. Note the difference between original Assembly and new Sim Rep shown here.

Page 6 of 13

Title: “Name of Tutorial” Date: 7/16/01 After Update Screen is selected and the components removed are not as expected, you may unselect the them as follows: • Select DEFAULT under EDIT REP • Pick in the model tree the components that were not intended for the Sim Rep • Update Screen • Components are Returned to original state

Page 7 of 13

Title: “Name of Tutorial” Date: 7/16/01 5) Substituting Components: In many cases, a Simplified Rep of a lower level Sub assembly is needed to be displayed in a respective higher-level assembly. In the picture on right, there exists a Subassembly of the front panel including all the gauges, levers, hinges etc. A Simplified Rep has initially been created of the front panel as shown below

Sub Assembly in Master Rep view:

Simplified Rep named Next_ASSY:

Instead of individually removing all the unwanted components such as Gauge, Bracket and Door Hinge, at the top level, we can select the Simplified Rep on the preexisting lower level subassembly. In this example we will remove components at the high level simplified rep by substituting a Simplified Rep of a lower level assembly. Page 8 of 13

Title: “Name of Tutorial” Date: 7/16/01 PROCEDURE: 1) Select Substitute from EDIT REP Menu:

2) Select the Sub Assembly from the model tree

3) Choose By Simplified Rep and then Browse:

Page 9 of 13

Title: “Name of Tutorial” Date: 7/16/01

4) Select the appropriate Simplified Rep name and select OK:

5) Choose OK again and then Update Screen:

Page 10 of 13

Title: “Name of Tutorial” Date: 7/16/01

6) The Simplified Rep is included in the top level Assembly. Notice simplified version of front panel:

7) Finish the Simplified Rep by selecting DONE

END OF TUTORIAL: Thank You for Coming!!

Page 11 of 13

Title: “Name of Tutorial” Date: 7/16/01

Key Vocabulary for “Simplified Reps”: Interchange Assembly: function that allows the switching out of functionally equivalent models. Common usage is a “simplify interchange” where a completed, complex assy is replaced with a simple part representation for faster regeneration. Regeneration: the mathematical updating of CAD geometry and their associated objects when dimensional changes take place. This can be as simple as individual part values updating or as complex as an entire toplevel assembly changing. Simplified Reps: advanced Pro/E tools to limit the amount of models needed to be in session (and thus regenerated).

Page 12 of 13

Title: “Name of Tutorial” Date: 7/16/01

Tutorial Evaluation: Title:

Engineer

PTC Products Used:

Foundation

Designer

0-6 months

Mfg. Engr.

Advanced Assembly Extension

Behavioral Modeling Time using Pro/E:

Draftsmen

Intralink

6-12 months

Analyst

Advanced Surface Extension

Modelcheck 1-2 years

Tech. Pubs.

All 2-5 years

5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

………………………………………………

1

2

3

4

5

2.

Time was utilized effectively:

………………………………………………

1

2

3

4

5

3.

The exercise was easy to understand:

………………………………………………

1

2

3

4

5

4.

This tutorial will help me on current projects: ………………………………………………

1

2

3

4

5

………………………………………………

1

2

3

4

5

………………………………………………

1

2

3

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5

5. 6.

These techniques make Pro/E a more effective tool: These techniques will increase my speed using Pro/E:

What 3 concepts/techniques learned from this tutorial will you apply on the job? 1. 2. 3.

What, if anything can be done to improve this tutorial for your company?

Additional Comments:

Thank you for filling out this evaluation! Your comments will be used to improve the quality of future tutorials.

Page 13 of 13

Title: ModelCHECK Date: 8/22/01

ModelCHECK – Helping to Ensure Quality Deliverables:

Table of Contents: 1) Objective 2) Overview 3) Using ModelCHECK 4) Checks Available

1

Title: ModelCHECK Date: 8/22/01

Objective: At the end of this tutorial, you will know how ModelCHECK: • can help you adhere to your company’s standards (Parameters, Layers, etc) • facilitates Reuse of Models • can assist with Problem Resolution, Education, and Online Advice • can monitor improvement

Overview:

ModelCHECK evaluates Pro/ENGINEER parts, assemblies, and drawings to ensure that they adhere to a company's modeling standards and best practices. If an exception to these conventions is detected, users are notified of the inconsistency, given tools to identify the problem within the solid model, and can often make a correction 2

Title: ModelCHECK Date: 8/22/01 automatically from the familiar web-based ModelCHECK interface. ModelCHECK facilitates the work of design team engineers by letting users create superior models that are well suited for reuse in downstream applications. Facilitating Reuse of Models As companies continue to embed Pro/ENGINEER into their design process, reusing the model becomes increasingly important. To facilitate reuse, models have to be created in accordance with common and accepted design philosophies and must contain all necessary information. However, users are often unaware of the design standards, or the company has difficulty enforcing them. ModelCHECK helps designers use correct modeling practices by letting them constantly monitor the Pro/ENGINEER model as design features are added, much as they would use a spell checker for a word processing application. In this manner, variations from accepted practices can be detected and corrected early in the design process, before they affect downstream users of the model and incur additional costs. Detecting Existing Designs As the volume of models being created and stored in databases continues to grow, the opportunity to reuse existing designs increases. The problem is that with an increased number of models stored, it becomes progressively more difficult to identify similar designs. Often previously designed and released models are re-created from scratch simply because the user had no ability to determine if the model already existed somewhere in the database. ModelCHECK introduces powerful new patent pending Shape Indexing™ technology that enables rapid detection of existing designs. While a user is building a model, ModelCHECK is constantly scanning the model's geometry to determine if a model with similar shape has been previously created. As soon as a similar model is detected, ModelCHECK informs the user of this opportunity and displays to them the degree of similarity between the two models and from where the existing model can be retrieved. Problem Resolution, Education, and Online Advice The first step in guaranteeing the quality of any finished solid model is making sure users are aware of information missing in their model. ModelCHECK offers tools beyond simple notification. It will not only identify the feature in question but also actually make corrections to the model. In addition, users can easily access online help pages specific to the problem identified. This type of immediate feedback will advance user knowledge of Pro/ENGINEER modeling practices and help avoid the same types of mistakes in the future. Automated Tracking of Model Quality As ModelCHECK is run on Pro/ENGINEER models, a database is created to track the types of problems found and their frequency. Tools provided with ModelCHECK sort and graph this data for trend analysis. The result is an engineering management organization that better understands the training needs and challenges of their Pro/ENGINEER users. 3

Title: ModelCHECK Date: 8/22/01

Using ModelCHECK: Much of the effort in implementing ModelCHECK is done by the system administrator. He or she is responsible for configuring the checks to adhere to your company’s standards. Once the configuration is established, the use of ModelCHECK becomes part of the Pro/ENGINEER users everyday workflow. The reports are easy to read and many of the problems found in models can be fixed with a single button pick from the report window. ModelCHECK runs in four ways: • Interactively (as shown below) • When the model is regenerated • When the model is saved • In batch mode

4

Title: ModelCHECK Date: 8/22/01 The ModelCHECK report displays the items in the model that have failed during the check. A sample check is shown below.

This section gives information about the model, how ModelCHECK was run and which configuration files were used

Errors and Warnings are reported

Selecting Report will reformat the window as shown below to allow corrective action

Shows indented Bill of Material with the number of errors and warnings for each part listed. A sample window is pictured below. Page 8

Compiles total list of errors for the assembly, Tells how many parts fail each check. A sample window is pictured below. Page 7

5

Title: ModelCHECK Date: 8/22/01

Window shown when “report” is chosen in the initial summary window

This section gives information about the model, how ModelCHECK was run and which configuration files were used Each tab will list all relevant checks run, with a status of ok, error or warning The summary tab shows all warnings and errors from all of the checks. It does not list checks that have passed

For many checks (like the parameter check shown) selecting on the red buttons will correct the problem detected. Others may need to be corrected manually

6

Title: ModelCHECK Date: 8/22/01

Window shown when “Assembly BOM failed checks” is chosen in the initial summary window

Results are listed for all checks that have failed in the assembly or any of its’ models. The number of models which have the particular failure are listed.

7

Title: ModelCHECK Date: 8/22/01

Window shown when “Assembly Bill of Material” is chosen in the initial summary window

An indented BOM is shown with the tally of errors and warnings for each component

Users are able to navigate to the reports for a given component through this window and where appropriate, fix the errors

Some of the general check capabilities are shown below. These are taken from the list of all checks which follows on page 10. Conformance to Standards Use of start part Parameters Layers Views Model naming convention Proper use of family tables Version of Pro/ENGINEER the model was created in or last stored in

• • • • • • •

8

Title: ModelCHECK Date: 8/22/01 Use of Proper Modeling Techniques • Buried features • Geometry problems (Geom. Checks) • Poor feature creation order • Improper dimensioning of features • References to external models Manufacturability and Translatability • Short edges • Sharp edges • Small holes and fillets • Non standard hole sizes • Non standard sheet metal wall thickness • Irregularities in curves, edges and surfaces Drawing Checks • Spell checker • Faked dimensions • Views out of bounds • Unused models • Drawing formats • Use of standard fonts and drawing tags (.dtl info)

9

Title: ModelCHECK Date: 8/22/01

Types of Checks: This is a complete list of checks available in 2001. For some of these checks the problem can be highlighted on the Pro/ENGINEER model and some of the problems can be automatically fixed from the ModelCHECK report window.

ModelCHECK 2001 List of Checks Highlight Fix

INDEX Problem can be highlighted from ModelCHECK ModelCHECK can fix the problem

CHECK

CONFIG TAG

HIGHLIGHT

FIX

COMMENT

Datum Checks 1

Datum axes (list of and come from a standard list)

2 3

Datum coordinate systems (list of and come from a standard list) Datum curves (list of and come from a standard list)

4 5

Datum features are the correct feature number Datum planes (list of and come from a standard list)

8 9 6

Datum planes built through other datum planes Datum planes without children (not including start features) Datum points (list of and come from a standard list)

7

Datum rename (for legacy models)

STARTCHECK DTM_AXES_INFO STARTCHECK DTM_CSYS_INFO STARTCHECK DTM_CURVE_INFO STARTCHECK STARTCHECK DTM_PLANE_INFO DATUM_PARENT DATUM_CHILD STARTCHECK DTM_POINT_INFO DATUM_RENAME

✔ ✔

✔

Parameter Checks 8 9 10 11 12 14 15 16 17 18 19 20 21 22

Check drawing parameters Create a parameter that stores the results of a check (material name, model units etc) Extra parameters (those that are not listed in the start part) Parameter notes used are from approved lists Parameter rename (for legacy models) Parameter values match required syntax and values Parameters are not empty Parameters are of correct type Parameters are PDM designated Parameters used (list of) Parameters with spelling mistakes Required parameters exist Unacceptable text in parameter notes Parameters not used in family tables or relations

DRAWING_PARAMS ADD_CHK_PARAM

✔

EXTRA_PARAMS PARAM_NOTE_REQ PARAM_RENAME PARAMCHECK PARAMCHECK PARAMCHECK PARAMCHECK PARAM_INFO PARAM_SPELL PARAMCHECK PARAM_NOTE_UNACC PARAM_UNUSED

✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔

10

Title: ModelCHECK Date: 8/22/01 CHECK

CONFIG TAG

HIGHLIGHT

FIX

COMMENT

Feature Checks 23 24 25 26 27 28 29 30 33 34 35 36 37 38 39 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56

Ability for users to ignore problems Buried features Calculate suggested minimum short edge length Chamfers which are created too early in the model Children of chamfers Children of drafts Children of rounds Children of the default datums (number of features) Cosmetic features (list) Cosmetic features which are too early in the model Cuts and slots which should be modeled as holes Cuts with non-standard diameters Draft features which are too early in the model Draft features with non-standard angles Features that are dimensioned to edges Features with names (number of) Freeform surfaces (number of) Geom Checks Holes with non-standard diameters Imported (IGES) features (list) Incomplete features List and quantity of feature types used Maximum number of entities per sketched feature Merged or cutout features are in the model Resumed features (number of) Round features which are too early in the model Sharp edges Short edges Small cylindrical surfaces Suppressed features (number of) Surfaces with gaps or overlaps

IGNORE_FEAT BURIED_FEAT Set in constant file EARLY_CHAMFER CHAMFER_CHILD DRAFT_CHILD ROUND_CHILD DEFAULT_CHILD COSMETIC_FEAT EARLY_COSMETIC CYL_CUT_SLOTS CYL_DIAMS EARLY_DRAFT DRAFT_ANGLES EDGE_REFERENCES NAMED_FEAT FREEFORM GEOM_CHECKS HOLE_DIAMS IMPORT_FEAT INCOMPLETE_FEAT FEATURE_INFO SKETCH_ITEMS MERGE_FEAT REG_FEATURES EARLY_ROUND SHARP_EDGES SHORT_EDGES SMALL_CYLSRF SUP_FEATURES SRF_EDGES

✔ ✔

✔

✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔

✔ ✔

✔ ✔ ✔ ✔ ✔ ✔ ✔

Model information 57 Absolute accuracy is within acceptable range 58 Create new custom checks from the outcome of existing checks 59 Cross sections (list of) 60 Disk space used to store the model 61 External references 62 Fully regenerate the model and report any errors 63 64 65 66 67 68 69 70 71

Insert mode is still active Layouts associated with the model (list of) Material used is from an approved list Memory space used to retrieve the model Model density is 1.00 (default) Model name meets required syntax and values Named dimensions Overall size of model (LxWxH) Regenerate all cross sections of a model

ACCURACY_INFO CHK_* XSEC_INFO FILE_SIZE EXT_REF_INFO Auto on MC_REGEN if REGEN_ERRS and REGEN_WRNS enabled INSERT_MODE LAYOUT_INFO MATERIAL_INFO MEMORY_SPACE DENSITY_INFO MODEL_NAME RENAMED_SYMBOLS OVERAL_SIZE Auto on MC_REGEN

MC REGEN, Batch mode with REGEN_ERRS ✔ ✔ Batch mode only ✔ ✔ MC REGEN only

11

Title: ModelCHECK Date: 8/22/01 72 73 74 75 76 77 78 79 80 81 82 83 84 85 86 87

CHECK Regenerate all simplified reps of a model Relative accuracy is within acceptable range Report the name of the model RuleCHECK rules (list of) RuleCHECK rules that are still pending Shape Indexing for duplicate models Simplified rep names (follow standard) Simplified reps (list of) STL can be made successfully (yes / no) UDF’s (list of) Units used (report) Units used for length are from a standard list Units used for mass are from a standard list Version of Pro/ENGINNER the model was last saved in Views (list of) Views (standard view names exist)

CONFIG TAG Auto on MC_REGEN ACCURACY_INFO MODEL_NAME_STR RULECHECK_INFO RC_INCOMPLETED DUPLICATE_MODELS SIMPREP_NAME SIMPREP_INFO STL_INFO UDF_INFO UNIT_INFO UNIT_LENGTH UNIT_MASS PRO_VERSION VIEW_INFO STARTCHECK

HIGHLIGHT

FIX COMMENT MC REGEN only

✔

✔

Relations 88 89 90 91 92 93

Check if any relations have multiple assignments Check that all relations have comments Check that there are no relation errors List all relations Update relations Standard relations exist

RELATION_MULT RELATION_COMM RELATION_ERRS RELATION_INFO RELATION_UPDATE RELATION_MISS

✔ ✔

Family Tables 94 95 96 97 98

Check if a standard list of parameters is in the table Identify if the model is a generic or instance Instance names meet required syntax and values Table cells with default values (* in the table) Verify all instances in the table

FT_STD_PARMS FAMILY_INFO INSTANCE_NAME FT_DEF_VALS Auto on MC_REGEN

✔

DRAWING_LAYERS LAYER_PLACE EXTRA_LAYERS LAYER_DISPSTAT LAYER_STATUS LAYER_INFO LAYER_MOVE REPT_LAYR_ALWAYS

✔ ✔ ✔

LAYER_ITEMS STARTCHECK

✔ ✔

✔ MC_REGEN only

Layer Checks 99 100 101 102 103 104 105 106

Check drawing layers Check that standard items are on standard layers Extra layers (those that are not listed in the start part) Layers stored in “isolate” (display) mode Layers with improper display status List all layers in the model Move items on ‘old’ layers to ‘new’ layer names Only report missing layers if there are features that belong on them in the model (default layers) 107 Report any features on multiple layers 108 Required layers exist

✔ ✔

Tolerancing 109 Check that tolerances are properly defined as either ANSI STARTCHECK or DIN/ISO 110 Minimum and maximum tolerance used in the model MINMAXTOL_INFO 111 Tolerances below allowable minimum LOW_TOLERANCE

✔ ✔

Sheetmetal Checks 112 113 114 115

Check that the bend table is from an approved list Check that the flat pattern feature exists Check that the Y-factor is from a standard list Report if the wall thickness is a non-standard dimension

SHTMTL_BENDTAB SHTMTL_FLAT SHTMTL_YFACTOR SHTMTL_THICK

No Batch mode No Batch mode

12

Title: ModelCHECK Date: 8/22/01 CHECK 116 Report if there are any consecutive unbend/bend back features

CONFIG TAG SHTMTL_UNBENDS

HIGHLIGHT

FIX

COMMENT

Assembly Checks 117 118 119 120 121 122 123

Assembly features other than datums exist Bill of materials (list) Bulk items Family table generic components exist Frozen components Global Interference - has it been run recently Missing components

ASM_FEATURES ASM_BOM BULK_ITEMS GEN_COMPONENTS FRZ_COMPONENTS GLOBAL_INTF MIS_COMPONENTS

124 125 126 127

Number of parts and sub-assemblies Number of unique parts and sub-assemblies Packaged components Suppressed components

NUM_COMPONENTS UNQ_COMPONENTS PACK_COMPONENTS SUP_COMPONENTS

✔

✔

MC REGEN and Batch mode only ✔

Drawing Checks 128 129 130 131 132 133 134 135 136 137 138 139 140 141 142 143 144 145 146 147 148 149 150 151 152 153

Differences between .dtl file in use and the standard one Dimensions which cannot be regenerated Dimensions which have been overridden using @O Draft geometry not attached to a view Drawing name conforms to standard syntax Drawing parameters - list any that exist Drawing text that is not a standard font Drawing text that is not standard height Erased views Format used is from a standard list Ignore a given sheet List of symbols Model names used on each sheet (list of) Notes on the drawing (list of) Number of drawing sheets is below defined maximum Number of sheets and their sizes Required parameters exist on the drawing Spelling errors in notes Spelling errors in symbols Spelling errors in tables Symbols used in the drawing are from an approved list Text in drawing that is not allowed Text in the Title Block that is not parameter-driven Unused drawing sheets Unused models on the drawing Verify that certain table cells contain approved information 154 Views with display status set to default 155 Views that are out of bounds 156 Views that overlap

STD_DTL_SETUP REGEN_DIMS DIM_OVERWRITE DRAFT_GEOM DRAWING_NAME PARAMS_EXIST NOTE_FONT NOTE_HEIGHT ERASED_VIEWS FORMAT_NAME IGNORE_SHEETS SYMBOL_INFO MODELS_USED NOTE_INFO NUM_DRAW_SHEETS SHEET_SIZE_INFO PARAMS_USED NOTE_SPELL SYMBOL_SPELL TITLE_SPELL STD_SYMBOLS NOTE_UNACCEPT TITLE_INFO UNUSED_SHEETS UNUSED_MODELS TABLE_CELLS

No batch mode MC_REGEN only ✔

✔ ✔

✔

✔ ✔

✔ ✔

✔

DEFAULT_VIEWS BOUND_INFO OVERLAP_INFO

✔ ✔ ✔

M1_TINY_ELMNT M2_IDENTICAL_ELEMNT M3A_POSITION_CONT M3B_TANG_CONT

✔ ✔ ✔ ✔

GeomIntegrityCHECK 157 158 159 160

Small elements (curves, faces and surfaces) Identical elements (curves, faces and surfaces) Positional continuity (curves, faces and surfaces) Tangential continuity (curves, faces and surfaces)

13

Title: ModelCHECK Date: 8/22/01 CHECK 161 Curvature continuity (curves, faces and surfaces) 162 Curves and surfaces defined by equations with high polynomial degrees 164 Wavy elements (curves and surfaces) 165 Small distance between knot vectors (curves and surfaces) 166 Self intersecting curves 167 Non IGES-compliant text 168 Small edge segments 169 Small radius of curvature 170 Small angle between edges 171 Reversal of normals 172 Poor patch distribution 173 Unoccupied patch rows 174 Small distance between edges 175 High edge-surface deviation 176 Non parallel path / dissimilar orientation 177 High edge-segment concentration 178 More than two surfaces per edge 179 Dissimilar normal distribution 180 Knife edge 181 High vertex-edge deviation 182 High vertex-surface deviation 183 Features without history 184 Auxiliary geometry 185 Cavities 186 Multi-body solids 187 Multi-solid parts

CONFIG TAG M3C_CURV_CONT M4_POLYN_DEG

HIGHLIGHT ✔ ✔

M5_WAVINESS M6_KNOT_DIST C7_SELF_DIST D28_IGES_TEXT SU8_TINY_SEG_EDGE SU9_TINY_CURV_RAD SU10_BOUND_ANGLE SU11_NORM_REVERSAL SU12_PATCH_DIST SU13_UNOC_PATCH_ROW F14_BOUND_DIST F15_SURF_DIST F16_SIM_ORIENT F17_NUM_SEG T18_NUM_FACE T19_NORMAL_ORIENT T20_KNIFE_EDGES SO21_DIST_VERT_EDGE SO22_DIST_VERT_FACE SO23_HIST_DELETE SO24_EXTRA_GEOM SO25_CAVITIES SO26_MULT_BODY SO27_MULT_SOLID

FIX

COMMENT

✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔ ✔

Batch Mode Auto Correcting Capability Add items to layers Add relations and comments Change layer display status Create layers Create parameters (if the values are known) Fully regenerate the model from the first feature on and report any problems Move items between layers Designate parameters for PDM use Rename datums Rename layers Rename parameters Save the model

14

Title: ModelCHECK Date: 8/22/01

Tutorial Evaluation: Title:

… Engineer

… Designer

… Foundation

… Draftsmen

… Mfg. Engr.

… Advanced Assembly Extension

PTC Products Used:

… Behavioral Modeling

Time using Pro/E:

… 0-6 months

… Intralink

… 6-12 months

… Analyst

… Advanced Surface Extension

… Modelcheck

… 1-2 years

… Tech. Pubs.

… All

… 2-5 years

… 5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

…………………………

1

2

3

4

5

2.

The exercise was easy to understand:

…………………………

1

2

3

4

5

3.

This tutorial will help me on current projects:

…………………………

1

2

3

4

5

4.

These techniques make Pro/E a more effective tool:

…………………………

1

2

3

4

5

5.

These techniques will increase my speed using Pro/E:

…………………………

1

2

3

4

5

What concepts/techniques learned from this tutorial will you apply on the job? 1) 2) 3) What would you like to see as a future tutorial at your company? 1) 2) 3) What can be done to improve these tutorials for your company? 1) 2) 3)

Additional Comments:

15

http://www.kinetivision.com/freevids/mech_gears_sync.htm

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/mech_gears_sync.htm [28.11.2002 13:59:10]

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Shared Data Menu: Communicating Design Intent Throughout Designs

Table of Contents: 1) Objective 2) Overview 3) Metric 4) Tutorial 5) Key Vocabulary 6) Tutorial Evaluation

Page 1 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Objective: Describe the use of the new Shared Data menu for communicating geometry from one model to another. These options first debuted in Pro/ENGINEER 2000I and have been expanded in Pro/ENGINEER 2001. After reading this tutorial you will be able to: • Describe how this functionality can be used to describe process variants • Build simplified geometry for subsystem installation and routing • Create associative simplified models to share with co-workers or sub contractors • Explain how Shared Data features simplify Top Down Design

Overview: There are many times when a designer must share geometry from one model into one or more other models. One example is the creation of process variants: “as machined” versus “as cast.”

As Machined

As Cast

You may also want to create a simplified version of an assembly for subsystem mounting or cable/pipe routing. Shared Data shrinkwrap features are useful in this instance. Most new design work is created using a Top Down Design Process. A typical Top Down Design process consists of six fundamental steps: 1. Defining Design Intent 2. Defining Preliminary Product Structure 3. Introducing Skeleton Models 4. Communicating Design Intent Throughout Assembly Structure 5. Continued Population of the Assembly 6. Managing Part Interdependencies Shared Data features are central to topics four and six.

Page 2 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

This document will explain the use of the following types of shared data features: • Copy Geometry from other model • Shrinkwrap from Other Model • Inheritance features • Cutout from other model • Merge from other model • Publish Geometry

Metric: There are many benefits to using the new Shared Data features. •

When used to communicate surface shapes in Top Down Design these features are 50% smaller than surface copies made at the assembly level.

•

Geometry can be communicated between models without creating and managing an assembly

•

Pro/INTRALINK manages all dependencies created using the Shared Data Menu

•

Shrinkwrap features retrieve >70% faster than the models that they represent

Page 3 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Tutorial: We will look at each type of shared data feature separately. All are accessed the same way. With a part or assembly open select #Insert;# Shared Data.

Note: You may also select #Feature;#Create;#Data Sharing.

Copy Geometry from Other Model: In this example we will copy the required references from a skeleton model into a part model to ensure that a mouse button corresponds to the proper shape and size defined in the master model. The master model is shown below:

Page 4 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

To design the part for the left mouse button I need the master surface definition, the Pivot axis, and the curves denoting the perimeter of the button. We will use Copy Geometry from Different Model to get started. • •

Create a new part with three datum planes and a coordinate system for the left mouse button. Select #Insert;#Shared Data;# Copy Geometry from Different Model. You will see the following elements of the feature, most of them are optional.

Page 5 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Ext Model: Retrieve a model that you need references from. I’ll call this model the source model. Select Open or pick a model that is visible. Location: Locate the source model relative to your target model. You have two options: Use the default location or align coordinate systems. In this case I have chosen the default location. Surface Refs: Allows the selection of surfaces and quilts. The typical surface collection menus are available.

I have used the Indiv Surfs option and selected the top surface of the mouse.

Page 6 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02 Curve Refs: Will allow the selection of curve features. I have used the option to select the bounding curves of the mouse button.

Misc Refs: Allows the selection of Datum features’ intent chains and other references. I have used the option to select the button pivot axis.

Page 7 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02 Publish Geom: Allows the selection of references that have been pre-bundled in the source model. Rather than picking features and references individually, you reference a Publish Geometry feature in the source model. Publish geometry features are chosen from a list of available features. An example of creating a Publish geometry feature in a source model appears in this document. Dependency: One of the most interesting things about Data Sharing features is that you can choose whether or not the features update automatically; You can determine associativity. I have selected dependent. My reference geometry will automatically update if the source geometry is available in session. You can toggle between dependent and independent at will.

The resulting feature is shown below. I now have all the references needed to build the left mouse button without requiring a merge of the entire master model, or unnecessary assembly references. I can also choose when my model updates to external changes.

The Model tree shows on feature for the six references that were added.

Page 8 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Note the icon used for external copy geom features. The Feature name can be changed

Shrinkwrap from Other Model: In this example we will create a simplified version of a Printed Circuit Board. This will allow us to place a single part file in assemblies to represent the Circuit Board Assembly. Only this file would need to be checked out of Intralink instead of all the components on the circuit board. Other uses of this function would be to create simplified versions of assemblies to route cables or pipes. You could also share information with other project workers or other companies in a manner that would allow associative updates. This is the original board:

• • •

Create a new blank part Select #Insert;#Data Sharing;#Shrinkwrap from Other Model The following dialog shows the elements for the feature

Page 9 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Ext Model: Retrieve a model that you need references from. I’ll call this model the source model. Select Open or pick a model that is visible. I chose the board assembly pictured above. Location: Locate the source model relative to your target model. You have two options: Use the default location or align coordinate systems. In this case I have chosen the default location. Attributes: Defines the behavior of the shrinkwrap feature.

Quality varies from 1-10. Controls the number of surfaces selected to represent the source model (part or assembly) Holes can be optionally filled to further simplify the model Quilts can be optionally included to further define the model

I chose a quality of 5. The higher the quality the longer the feature takes to regenerate. Additional Surfs: Allows you to manually select surface to be included in the shrinkwrap feature. Use this when your chosen quality setting does not automatically select a surface that you want included. Include Datums: Datum features are not included in shrinkwrap features. Remember that we are trying to create a simplified model. There are occasions when you would like to include datums, particularly as future assembly references. Use this option to select the desired datums.

Page 10 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Dependency: One of the most interesting things about Data Sharing features is that you can choose whether or not the features update automatically; You can determine associativity. I have selected independent. My model will not update until I toggle dependency back on.

The resulting feature is shown below shaded and in wireframe.

Inheritance feature

: In this example we will derive an “as-cast” design model from an "asdesigned” or “as-machined model.” We need to be able to toggle features on and off as well as modify feature dimensions

Page 11 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

As Machined

As Cast

In the past users might have used merge model techniques or family tables for this type of task. This method is not only more straightforward and useful; it also reduces data management concerns since the person creating the manufacturing variant does not change the original mode. Also, some of the change required would not be possible in a merge model scenario. This feature could also be used to copy in an entire skeleton or master model if desired. • • •

Create a new model. This will be the manufacturing variant or the “as-cast” model. The model uses a start part and has three datums and a coordinate system. Note: the units used must agree with the model that you are referencing. Select #Insert;#Shared Data;#Inheritance The following options are available

Base Model: Retrieve a reference model. Select Open or pick a model that is visible. I chose the final version of the connecting rod pictured above. By default this entire model will show as a single feature in the target model. Location: Locate the source model relative to your target model. You have two options: Use the default location or align coordinate systems. In this case I have chosen the default location. Var Dims: feature dimensions can be modified in the current model. Select “Add”; select the feature to be modified then the dimension to be changed.

Page 12 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Selecting features and using the right mouse button to modify them can also modify dimensions. You will be prompted to add the dimension to the var dim table. Var Feats: Features may be suppressed in the current model. Select “Add;” select the features to be suppressed; select suppress.

Features can also be suppressed by expanding the feature list in the model tree, selecting features and using the right mouse button to suppress. Copy notes: Copy 3-D notes if desired Dependency: One of the most interesting things about Data Sharing features is that you can choose whether or not the features update automatically; You can determine associativity.

Page 13 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Cutout and Merge from Other Model

: Cutout and merge models can now be created without an assembly. The menus are similar and shown below.

Base Model: Retrieve a reference model. Location: Locate the source model relative to your target model. You have two options: Use the default location or align coordinate systems. Dependency: One of the most interesting things about Data Sharing features is that you can choose whether or not the features update automatically; You can determine associativity.

Publish Geometry: In the copy geometry example shown above (collecting references for the left mouse button), the user selected multiple references from a source model. It may make sense for the originator of the source model to pre-select these references for you. The references (surfs, curves, datums, etc) can be collected in a Publish geometry providing the following benefits: • Sometimes the source model may be very complex and hand picking the references may be difficult. • Some items that are needed may be on layers and not visible and you may not be familiar with the model. • The originator of the source model would be in a better position to select the necessary references for you. He/she would also know which references will stay in their model. • This is particularly useful when the references will be used in many models. You can select them once in the publish geometry and reference the Publish Geometry feature in many models. The Publish Geometry functionality is described below. This example will build a Publish Geometry feature in the Master Model of the Mouse used above. This feature will pre-select features need to create the mouse buttons. Select #Insert;#Shared Data;#Publish Geometry. The following options are presented.

Page 14 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Name: Name the feature. This name will appear in lists when other models reference the feature Surface Refs: Allows the selection of surfaces and quilts. The typical surface collection menus are available.

I have used the Indiv Surfs option and selected the top surface of the mouse.

Page 15 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02 Curve Refs: Will allow the selection of curve features. I have used the option to select the bounding curves of the mouse button.

Misc Refs: Allows the selection of Datum features’ intent chains and other references. I have used the option to select the button pivot axis.

The icon used in the model tree of the originating model is shown below.

Page 16 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Publish Geometry Feature

Key Vocabulary for Shared Data Features: Copy Geometry Feature: A Pro/ENGINEER feature allowing geometry from one model to be replicated in one or many other models Cutout: Remove the volume of one model from another. Like creating a mold cavity Inheritance Feature: A Pro/ENGINEER feature allowing one part model to appear as a single feature in another part model. Useful for creating/documenting manufacturing process variants. Merge: Combine two part models into one. Publish Geometry Feature: A Pro/ENGINEER feature allowing a user to collect references in a source model to make it easier for other users to reference the geometry. Shrinkwrap: A lightweight version of a part or assembly. Used in this document as an associative surface shrinkwrap. Skeleton Model: A Top Down Design tool used to communicate shape and interfaces throughout a model Source model: The model from which references are needed. Top Down Design: A method of designing a product by specifying top level design criteria and passing those criteria down from the top level of the product’s structure to all of the affected sub systems.

Page 17 of 18

Title: Shared Data Menu: Communicating Design Intent Throughout Designs Date: 2/21/02

Tutorial Evaluation: Title: PTC Products Used: Time using Pro/E:


Engineer


Designer


Foundation


Mfg. Engr.


Advanced Assembly Extension


Behavioral Modeling
0-6 months


Draftsmen


Intralink


6-12 months


Analyst


Advanced Surface Extension


Modelcheck


1-2 years


Tech. Pubs.


All


2-5 years


5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

…………………………

1

2

3

4

5

2.

The exercise was easy to understand:

…………………………

1

2

3

4

5

3.

This tutorial will help me on current projects:

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1

2

3

4

5

4.

These techniques make Pro/E a more effective tool:

…………………………

1

2

3

4

5

5.

These techniques will increase my speed using Pro/E:

…………………………

1

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4

5

What concepts/techniques learned from this tutorial will you apply on the job? 1) 2) 3) What would you like to see as a future tutorial at your company? 1) 2) 3) What can be done to improve these tutorials for your company? 1) 2) 3)

Additional Comments:

Page 18 of 18

Sheetmetal Pocket Demo

Page 1 of 5

Pro/ENGINEER Sheetmetal - Pocket Tutorial Ethan Meyer - PTC [email protected] SUMMARY This pocket tutorial is intended to highlight the basic functionality of the sheetmetal module. Specifically, topics covered include: flat patterns, deformation allowance, bend tables, working in both flat and "as designed" states, and full associativity between part, drawing and flat state. Ensure you have the sheetmetal module attached to your license of Pro/ENGINEER before beginning. PICKS 1. Create a part (sub-type sheetmetal) with extruded wall as first feature; sketch as in following figure: FEATURE / CREATE / WALL / EXTRUDED / DONE / ONE SIDE / DONE / select your planes etc...

HINT: Sketch the outer "solid line" first, then use SKETCH / FEATURE TOOLS / THICKEN / FLIP / OKAY / 0.25 / / Now place the 0.50 Radial dimension on the inside "dotted line radius. This will simulate the thickness of the sheetmetal. It is best practice to dimension sheetmetal bends on the inside radius. Thickness = 0.25, Depth = 20

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2. Unbend the part. Pro/ENGINEER allows you to work in the formed or flate states. CREATE / UNBEND / REGULAR / DONE / select the top surface as fixed plane / UNBEND ALL / DONE / OK Observe the model in wireframe and shown axes mode, you can now see the bend lines and the bend tangents. If you modify the first feature you will see the developed length of the bends as a modifiable feature. The default is fine for design purposes but we will drive this by a manufacturing specified bend table in the next step. 3. Assign bend table. Important if you have manufacturing bend table specifications, not necessary if you don't. SET UP / BEND ALLOW / BEND TABLE / SET / CONFIRM / FROM FILE / TABLE1 4. Now view the table that you applied. These tables from the machinists handbook and are customizable if necessary. SHOW / FROM PART / TABLE1 (for soft copper and soft brass) 5. Create a cut across the bend. This will make apparent the realistic deformation that is show in Pro/ENGINEER sheetmetal. CREATE / CUT / DONE / select the top plane / DEFAULT ; sketch and align cut to axis as in following figure:

Make the cut THRU ALL / OK 5. Add a sketched flat wall. There are a variety of ways to create sheetmetal walls.

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CREATE / WALL / FLAT / NO RADIUS / DONE / PART BEND TBL / DONE / select the edge of the part to attach to / OKAY / sketch as shown in the following figure:

6. Bend the part back up and notice the deformation created at the cut. CREATE / BEND BACK / select the top surface as fixed plane / BEND BACK ALL / DONE / OK 7. Set up the flat state. This will be a fully associative family table instance for use in manufacturing drawings and tool paths. Having the two models allows users to design in the formrd state (add cuts, tabs, features, etc.) while having a fully accurate flat pattern for mfg. SET UP / FLAT STATE / CREATE / (this names the instance, the default is Pro/E industry standard) / FULLY FORMED / select top flat surface / OK This creates a family table intance that is always fully flat. This instance can then be used for flat pattern drawings and Manufacturing. Remember to do all design work in the bent state or generic, so your model will be correct. 8. Create drawing, showing bent and flat states on the same page. Show the dimensions on the bent part, create ordinate dimensions on the flat state.

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Sheetmetal Pocket Demo

Page 4 of 5

9. Now retrieve the part. Change the bend allowance from Table 1 to Table 3. (Refer to step 3) This alters the part's flat state to meet a new manufacturing requirement and shows the associativity of the model. Notice the effect on the developed length dimensions. 10. Create swept wall. It will be an additional flange. CREATE / WALL / SWEPT / USE RADIUS / DONE / DONE/RETURN / select green curvy edge (will highlight entire edge) / DONE / OKAY / sketch horizontal 2" line / DONE / ENTER VALUE / 0.5 / OK 11. Note the change in the flat state family table instance. Either: FILE / OPEN / IN SESSION / select the flat state or SETUP / FLAT STATE / SHOW / select the flat state 12. Return to drawing; notice changes have been incorporated due to change in bend allowance table and swept wall.

Final part:

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Sheetmetal Pocket Demo

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Page 5 of 5

8/8/2002

Title: Shrinkwrap Date: 8/22/01

Shrinkwrap

Table of Contents: 1) Objective 2) Overview 3) Metric 4) Tutorial 5) Tutorial Evaluation

1

Title: Shrinkwrap Date: 8/22/01

Objective: At the end of this tutorial, you will: • Know three types of shrinkwrap parts. • Know how the use of shrinkwrap parts affect regeneration times • Know how shrinkwrap parts can be used for Vendor supplied component library parts.

Overview: Many parts, especially Outside Plant (or Vendor) assemblies, contain much more detail and many more parts than are necessary to ensure proper space allocation in Pro/ENGINEER assemblies. Additionally, it is often not desired to submit assemblies with non-standard hardware to Pro/INTRALINK. Pro/ENGINEER techniques exist to reduce the file size of these assemblies greatly and represent them as simple piece parts. When this shrinkwrap capability is used the files are not only smaller but the vendor hardware does not need to be submitted to Intralink. There are four types of shrinkwrap: Surface Subset, Faceted, Solid Merge, and Data Sharing (Data Sharing available in 2000i2 and beyond).

Solid Merge type. Accurate mass properties, not associative.

Surface subset type. Accurate Mass Properties, not associative.

Faceted Shrinkwrap. Accurate Mass Properties, not associative.

2

Title: Shrinkwrap Date: 8/22/01

Data Sharing Shrinkwrap. Can toggle between associative and stand-alone. Created using Data Sharing functionality available in Pro/ENGINEER 2000i2 and beyond.

Metric: Shown below are the types of file size reduction that can be achieved when assemblies are simplified using Shrinkwrap. Actual data taken from a typical oilfield equipment assembly.

25 Full Assembly 20 15 10 5 0

File Size MB

Solid Shrink Wrap Surface Shrink Wrap Data Share Shrinkwrap Faceted Shrinkwrap

Corresponding improvements in retrieval time of the resulting part are also achieved. See below:

3

Title: Shrinkwrap Date: 8/22/01

45 40 35 30 25 20 15 10 5 0

Full Assembly

Retrieval Time (sec)

Solid Shrink Wrap Surface Shrink Wrap Data Share Shrinkwrap Faceted Shrinkwrap

Tutorial: To create non-associative, exported shrinkwraps follow the steps below. File; Open the part or assembly that you need to shrinkwrap. To create non-associative shrinkwraps in 2000i and 2000i2: Choose File;Export;Model:

4

Title: Shrinkwrap Date: 8/22/01

From the resulting right hand menu choose Shrinkwrap:

In Pro/ENGINEER 2001 select File;Save a Copy:

5

Title: Shrinkwrap Date: 8/22/01

Then select Shrinkwrap from the File Open Browser:

At this point you should see the shrinkwrap menu for exported shrinkwrap types. The options are shown below, descriptions follow.

6

Title: Shrinkwrap Date: 8/22/01 For Surface Subset types: Shrinkwrap Type selection

Quality selection. Determines amount of surfaces chosen to represent the design. Scale is 1-10, 10 being the highest. Higher quality results in longer creation.

Holes, Skeletons, Quilts and Small Surfaces can be automatically removed. The current Mass Properties of the parent assembly can be assigned to the resulting shrinkwrap part.

By default, no datums are included in the new part. Desired datums can be selected here for inclusion. It is often useful to see which surfaces will be included in a surface shrinkwrap upon completion. When the Gray-Orange option is chosen, unselected surfaces are shown in orange. Desired surfaces which are not chosen by default can be added manually. Name of resulting file

Create the new shrinkwrap part

Preview the resulting geometry from the current settings

7

Title: Shrinkwrap Date: 8/22/01

For Faceted Solid types:

Shrinkwrap Type selection Quality selection. Determines # of triangular surfaces created to represent the design. Scale is 1-10, 10 being the highest. Higher quality results in longer creation.

Holes, Skeletons, and Quilts can be automatically removed. The current Mass Properties of the parent assembly can be assigned to the resulting shrinkwrap part.

By default, no datums are included in the new part. Desired datums can be selected here for inclusion.

Choose your desired output type: Pro/ENGINEER part Stereo Lithography file (STL) VRML Name of resulting file

Create the new shrinkwrap part

Preview the resulting geometry from the current settings

8

Title: Shrinkwrap Date: 8/22/01

For solid subtypes:

Shrinkwrap Type selection Quality selection. Determines parts chosen to represent the design. Scale is 1-10, 10 being the highest. Higher quality results in longer creation.

Holes, Skeletons, and Quilts can be automatically removed. The current Mass Properties of the parent assembly can be assigned to the resulting shrinkwrap part.

By default, no datums are included in the new part. Desired datums can be selected here for inclusion. Components not selected by the quality setting can be chosen manually Name of resulting file

Create the new shrinkwrap part

Preview the resulting geometry from the current settings

The Data Sharing Shrinkwrap method is covered in the Data Sharing Tutorial document. It has the added benefit of being associative. Even better, the user has the capability to toggle between associative and independent at will.

9

Title: Shrinkwrap Date: 8/22/01

Some uses: This functionality can be used any time a model needs to be simplified prior to use. Some benefits: • The files are smaller • No vendor hardware needs to be maintained in INTRALINK • Retrieval time is very fast. • When sharing data with suppliers, proprietary data can be masked Be aware of the following. • Cross sections will not fill for the surface subset method • The exported types are not associative. Changes to shrinkwrap parts will need to be handled manually (except for the “data sharing shrinkwrap” covered in the data sharing paper). Use the data sharing type where possible.

10

Title: Shrinkwrap Date: 8/22/01

Tutorial Evaluation: Title:

… Engineer

… Designer

… Foundation

… Draftsmen

… Mfg. Engr.

… Advanced Assembly Extension

PTC Products Used:

… Behavioral Modeling

Time using Pro/E:

… 0-6 months

… Intralink

… 6-12 months

… Analyst

… Advanced Surface Extension

… Modelcheck

… 1-2 years

… Tech. Pubs.

… All

… 2-5 years

… 5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

…………………………

1

2

3

4

5

2.

The exercise was easy to understand:

…………………………

1

2

3

4

5

3.

This tutorial will help me on current projects:

…………………………

1

2

3

4

5

4.

These techniques make Pro/E a more effective tool:

…………………………

1

2

3

4

5

5.

These techniques will increase my speed using Pro/E:

…………………………

1

2

3

4

5

What concepts/techniques learned from this tutorial will you apply on the job? 1) 2) 3) What would you like to see as a future tutorial at your company? 1) 2) 3) What can be done to improve these tutorials for your company? 1) 2) 3)

Additional Comments:

11

http://www.ptc-mss.com/Tutorial/2Ki2%20sketcher%20cheat%20sheet.pdf

Embedded Secure Document The file http://www.ptc-mss.com/Tutorial/2Ki2%20sketcher%20cheat%20sheet.pdf is a secure document that has been embedded in this document. Double click the pushpin to view.

http://www.ptc-mss.com/Tutorial/2Ki2%20sketcher%20cheat%20sheet.pdf [28.11.2002 14:14:39]

http://www.ptc-mss.com/Tutorial/ProE%202001%20Sketcher%20Quick%20Reference%20Card.pdf

Embedded Secure Document The file http://www.ptcmss.com/Tutorial/ProE%202001%20Sketcher%20Quick%20Reference%20Card.pdf is a secure document that has been embedded in this document. Double click the pushpin to view.

http://www.ptc-mss.com/Tutorial/ProE%202001%20Sketcher%20Quick%20Reference%20Card.pdf [28.11.2002 14:16:21]

ModelCHECK Quick Reference for Self-Installation

This document is intended to give a brief overview of the requirements to run and install ModelCHECK. It should enable users and administrators to get a head start in installing and achieving the return on investment ModelCHECK can give to customers. We recommend that our Global Services Organization perform the installation, but if that is not an option this guide should help with the installation. For more information and guidance please refer to the customer support website located at http://www.ptc.com/

2000 Parametric Technology Corporation

PTC Customer Care Program: Boesiger

Table of Contents MODELCHECK ................................................................................................................ 1 ABOUT MODELCHECK................................................................................................... 3 RUNNING MODELCHECK............................................................................................... 3 ABOUT MODELCHECK TEACHER ................................................................................ 4 CONFIGURING MODELCHECK...................................................................................... 4 Location of configuration files:.............................................................................................................. 5

INTEGRATING MODELCHECK WITH A PDM SYSTEM ................................................ 6 CONFIG_INIT.MC............................................................................................................. 6 SETCONF.MCC FILE ....................................................................................................... 7 CONDITION.MCC FILE .................................................................................................... 8 CHECK CONFIG (FILENAME.MCH) ............................................................................... 8 START CONFIG (FILENAME.MCS) ................................................................................ 8 CONSTANT CONFIG (FILENAME.MCN) ........................................................................ 9 RULECHECK.................................................................................................................... 9 DUPLICATE MODELS IN MODELCHECK...................................................................... 9 CONFIGURING YOUR WEB BROWSER ...................................................................... 10

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PTC Customer Care Program: Boesiger

About ModelCHECK ModelCHECK is an integrated application that runs transparently inside Pro/ENGINEER. It analyzes parts, drawings, and assemblies and recommends proper Pro/ENGINEER modeling techniques. ModelCHECK promotes the use of standard design practices to improve the effectiveness of downstream users and design reuse.

Running ModelCHECK To Start ModelCHECK: 1. Set the Pro/ENGINEER configuration option modelcheck_enabled to yes 2. Start Pro/ENGINEER 3. Click Analysis > ModelCHECK.

You can run ModelCHECK in four ways, depending on how it is configured. •

Interactively, using a Pro/ENGINEER menu command. This is performed by selecting Analysis >ModelCHECK > MC inside Pro/ENGINEER

•

Automatically after every regeneration. This is the most effective use of ModelCHECK. Set MODE_RUN to Y in the Regenerate Mode column of the config_init.mc file. Upon regenerating any Pro/ENGINEER model, ModelCHECK will generate a report if there are errors or warnings found with the model.

•

Automatically after every save. Set SAVE_MC_PRE in the config_init.mc to Y in order to run ModelCHECK before you save, and N to run ModelCHECK after you save. Save the Model

•

Batch Mode. There are a number of automatic corrections that are performed in batch mode: i. Add Items to Layers ii. Add relations and comments iii. Change Layer Display iv. Create Layers v. Create Parameters (if their values are known) vi. Fully regenerate the model from the first feature and report any problems vii. Move Items between layers

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PTC Customer Care Program: Boesiger

viii. Designate Parameters for PDM Tools ix. Rename Datums x. Rename Layers xi. Save the Model

About ModelCHECK Teacher You may not always know what causes the problems or errors identified by ModelCHECK. ModelCHECK Teacher is a series of Web pages containing information about common modeling errors and how to fix them. To access it, click the question mark to the left of each item in a report. This loads a web page with information specific to the check. If your company has its own standards or rules to follow, you can modify the Teacher pages to include this information, or you can add links to your company’s Intranet. ModelCHECK’s Teacher pages also have links to Pro/HELP and Cadtrain COAch. You can use these links if the software is installed on your network.

Configuring ModelCHECK You can configure ModelCHECK to run different checks at different times. For example, the MC option allows you to check the currently active model; with MC Regen you can regenerate the active model and then check it; using Load Config you can select a configuration to use manually.

A series of text files store the configuration options. These files are located in the config directory, a subdirectory of the ModelCHECK loadpoint. The following files apply: •

Config_init.mc: specifies initialization settings. This file is read when Pro/ENGINEER starts and ModelCHECK initializes. If any changes are made to the file you must restart Pro/ENGINEER.

•

Condition.mcc: specifies the conditions that determine what set of configuration files to read when you have the ModelCHECK config option CNFG_SELECT_AUTO in config_init.mc set to Y. This is read each time you run ModelCHECK

•

Setconf.mcc: When the ModelCHECK configuration option CNFG_SELECT_AUTO is set to N or A in config_init.mc this file determines what configuration files you can select from the Pro/ENGINEER Load Config menu (Info>MC>Load Config).

•

.mch: Configures the checks and specifies how problems are reported. There can be several of these files. This file determines which check file to use each time you run ModelCHECK. You can give any name to a check file but it must have the extension .mch

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PTC Customer Care Program: Boesiger

•

.mcs: Start config file is used to specify the start part information for which ModelCHECK checks. You can have several .mcs files and use more than one at a time. The condition file determines which start file to use each time you run ModelCHECK. You can give any name to a start file but it must have the extension .mcs

•

.mcn: Constant file is used to specify constant values such as the length of a short edge. There can be several of these files. The condition file determines which constant file to use 3each time you run ModelCHECK. You can give any name to a constant file but it must have an extension of .mcn

Location of configuration files: All configuration files must be kept in the <modchk>/config directory for release 3.0 and 2000i. In ModelCHECK 2000i2 and greater, the path to the config file directory is <proe>/modchk/language/<English>/config

Use $MCDIR to specify an alternative location for the config directory. If $MCDIR exists, any file in that location overrides the default setting.

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PTC Customer Care Program: Boesiger

Figure 1 Example workflow using ModelCHECK configuration files

Integrating ModelCHECK with a PDM System You can configure ModelCHECK to add four parameters to the model file each time it is run on the model:

MODEL_CHECK – (string) indicates the date and time that ModelCHECK was last run MC_ERRORS – (integer) indicates the number of errors found MC_CONFIG –(string) indicates the names of the configuration files used MC_MODE –(Interactive, Regenerate, Save, Batch or MC_regen) indicates the mode in which ModelCHECK was run.

To see these parameters from within Pro/INTRALINK, attributes with the same names and types (as shown in the parentheses above) must be created from within Pro/INTRALINK’s commonspace. You can program Pro/INTRALINK to allow check-in only of models that have the above parameters set to specified values. For example, a trigger can be written to deny the check in of models with errors (MC_ERRORS is greater than 0).

Config_init.mc Initialization settings for ModelCHECK are set in the config_init.mc file. 1. Using a text editor, open config_init.mc. This file is in <proe>/modchk//config or in the directory you have specified with the environment variable $MCDIR 2. For the options you want to set, set a value for each ModelCHECK mode. In the config_init.mc file each mode is in a separate column. The modes are abbreviated as follows: a. I – Interactive b. B – Batch c. R – Regenerate d. S – Save

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PTC Customer Care Program: Boesiger

To specify a directory in config_init.mc you can includes spaces in the name of any directory. You do not need to include quotes around a directory name that contains spaces. Example: ! ---------------------------------------------------------# Options "I" "B" "R" "S" ! ---------------------------------------------------------# Enable ModelCHECK Y=enable, N=disable, A=Ask user MC_ENABLE YNA Y # View ModelCHECK Report Y=applet reports, N=html reports w/applet buttons, MODE_VIEW YN Y # Enable/Disable ModelCHECK in specific modes MODE_RUN YN Y Y

N

N

Setconf.mcc File You can allow users to decide what config files ModelCHECK uses during a Pro/ENGINEER session or have it automatically set. 1. In config_init.mc set CNFG_SELECT_AUTO to N or A to allow users to decide what config files to use. If this is set to Y the config files to use are chosen automatically. N: requires the user to choose the config files to run. A: prompts the user whether to load the configuration files or let ModelCHECK select them automatically. 2. Using a text editor open setconf.mcc. Edit the file to set up the Load Config choices. For example: PDM = (checks/pdm.mch) (start/pdm.mcs) (start/default_start.mcs) (constant/mm.mcn) NoStart = (checks/default_checks.mch) (start/nostart.mcs) (constant/mm.mcn) 3. Save setconf.mcc. All the configuration files you list in this file must be in their respective directories. 4. If CNFG_SELECT_AUTO is set to N or A, click Info > MC > Load Config in Pro/ENGINER. The Load Config menu appears. If setconf.mcc is set as in the above example then the following are listed on the Load Config menu: PDM, Light, NoStart 5. Click the configuration you want to use.

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PTC Customer Care Program: Boesiger

You can us3 mc_msg.txt to customize the configuration names that are listed in the Load Config menu. Mc_msg.txt is in the ModelCHECK text directory and is used to build the Pro/ENGINEER meny commands when ModelCHECK is initializing. Be careful when editing this file. If you edit the wrong lines, you may have to reinstall ModelCHECK. The default configuration names are Heavy, Medium, and Light. If you want to rename them so that the users see other names, edit the file.

Condition.mcc File When ModelCHECK runs, it reads a file called condition.mcc to determine the combination of configuration files (start, check and constant) to use. This files is located in the config directory of the ModelCHECK load point directory. You can use condition.mcc to override check settings. Prior to ModelCHECK version 3.0 all configuration options were stored in one file, config.mc. It is still possible to use config.mc. The condition.mcc file has a SET CONFIG FILE section and an OVERRIDE CHECKS section

Check Config (filename.mch) The check config file, or check file has an extension of .mch and is used to determine when to run checks and how to report problems when they are found. It is located in <proe>/modchk/language/engligh/config/check. You can set a value for the Interactive (I), Batch (B), Regenerate ®, and Save (S), modes for each checks. The available values for each check are: -N – Do not perform the check -Y – Perform the check but do not report any problems in the summary report, only in the full report, which is the second one you see. Y should be used for minor problems or for information only checks. -

E – Perform the check and report an error if it fails. Errors are reported in the summary report and in the full report. When errors are found a model parameter is created that has a value of the number of errors found in the model. Pro/INTRALINK can be set to track models with errors or to even reject their submission.

-

W – Does the same as E except no model parameter is created. W should be used for less serious problem.

Save the edited file with the extension .mch

Start Config (filename.mcs)

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PTC Customer Care Program: Boesiger

The start config file is where start part information is kept. In the start config file you can initialize part mode features, assembly mode features, drawing mode features and external files. It is located in the <proe>/modchk/language/English/config/check directory. In the file you list the parameters to add to the model. Save the file with the extension .mcs. You can have more than one .mcs files and they can be used at the same time.

Format: PRT_ADD_CHK_PARAM

[PARAMETER]

[CHECK_OUTPUT]

Where: [PARAMETER] is the name of the parameter that will be created [CHECK_OUTPUT] is the name of the check with output that will be used Example: PRT_ADD_CHK_PARAM

MATERIAL

MATERIAL_INFO

Constant Config (filename.mcn) The constant config file contains the values of constants that ModelCHECK uses. It is located in the <proe>/modchk/language/English/config directory. You can have multiple constants files.

RuleCHECK RuleCHECK, a component of ModelCHECK is designed to allow companies to easily document and enforce engineering rules. It can be used to develop a Design Advisor for Pro/ENGINEER users. Rules can be defined to describe a company’s engineering rules, design process steps, required deliverables, and Pro/ENGINEER best practices. Each type of part and assembly that a company designs may have specific rules assigned for it. You can have Engineering Rules, Design Process Steps, Required deliverables and Pro/ENGINEER best practices. It is accessed by selecting Analysis > ModelCHECK > RuleCHECK inside Pro/ENGINEER

Duplicate Models in ModelCHECK ModelCHECK can search for duplicate parts by examining a model’s shape and then searching the database for similar models. A line item in the ModelCHECK report indicates if duplicate models are found. You can then click on the line item a table with the names of the models found, and the following items appear:

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PTC Customer Care Program: Boesiger

•

Percent match

•

Model units

•

Number of features

•

Number of datums

•

Size of the model

Configuring your Web Browser ModelCHECK runs on any web browser that supports Java (Netscape 2.01 or greater and IE 3.0 or greater). Netscape 4.03 or higher is recommended.

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Title: Surface Transforms (for large patterns) Date: 7/22/01

Surface Transforms: For Large Patterns

Table of Contents: 1) Objective 2) Overview 3) Metric 4) Tutorial 5) Key Vocabulary 6) Tutorial Evaluation

Page 1 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01

Objective: At the end of this tutorial, you will be able to: • Explain why a surface transform is useful for large patterns. • Describe why a large pattern model would regenerate faster using this technique. • Identify a current project where this method can be applied.

Overview: Patterning a feature on a model can be a powerful away to leverage the parametric nature of Pro/E. There are times however when the size of pattern becomes so large that regeneration times become unacceptably long or you run into situations where a feature is created without proper references to allow it to be patterned at all using the conventional commands available. Surface transforms leverage the power of Pro/E surfacing by both reducing regeneration times as well as allowing you to create patterns of features that were previously impossible to pattern.

Metric: The example used in this tutorial was of a carrier for a semiconductor chip. Before surface transforms were used, this model took 25 minutes to regenerate. After the surface transform technique was applied, regeneration went down to 5 minutes. This is an 80% reduction in regeneration time!

25 20 15

Regular Pattern

10

Surface Transforms

5 0

Regeneration time on large pattern

Tutorial: Page 2 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01 A pin receptacle cutout has been created (Picture #1) in this model and it consists of 5 features: 2 cuts and 3 rounds. We need a 10x10 grid array of these features which would normally consist of (10x10 = 100, 100x5 = 500) 500 individual features that would be regenerated. We will reduce this to approximately 25 using surface transforms.

Picture #1

Page 3 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01 Step 1: Create a surface copy of the geometry to be transformed. a) Menu Picks: FEATURE, CREATE, SURFACE, COPY, DONE b) Select all of the surfaces that comprise the feature (hint: use SURF & BND for quick selection). Surf & Bnd method (Picture #2) a) Select a seed surface (bottom of cut) b) Select a bounding surface (top plane of part) c) Pro/E will automatically “gather” all of the inside surfaces between this seed surface and the bounding surface. “Seed” surface

“Bound” surface

Picture #2

Step 2: Transform the surface copy just created. a) Menu Picks: FEATURE, CREATE, SURFACE, TRANSFORM, MOVE, DONE b) Select the previously created surface c) TRANSLATE, PLANE d) Select a plane that the direction will be perpendicular to (flip if necessary). e) Enter in the dimension to translate, DONE MOVE. You will now have a new surface that is an exact copy, just shifted. This “Transformed” surface now has a linear dimension associated with it that we can use to pattern.

Page 4 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01 Step 3: Pattern the transformed surface. a) Menu Picks: FEATURE, PATTERN, select the transformed surface, DONE. b) Select the first direction, enter increment, DONE, enter total number in this direction, enter 2, DONE. This will now give us a single row of three surface copies. Step 4: Create solid cut using the surfaces. a) Menu Picks: FEATURE, CREATE, SOLID, CUT, USE QUILT, DONE, select the first transformed surface, select the check box to finish. b) Now pattern this solid cut using the reference pattern option. Step 5: Create a surface copy of all the solid cutouts of the geometry that we want. c) Menu Picks: FEATURE, CREATE, SURFACE, NEW, COPY, DONE (hint: used SOLID SURFS option for fast selection). Solid Surfs method a) Select part, all of the external surface geometry is included in the surface copy. b) Select EXCLUDE, a pick all of the outside geometry you don’t want to copy c) Select SHOW, MESH to get a visual on which surfaces are actually selected (Picture C) .

Picture #3

Page 5 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01

Step 6: Transform the entire row of surfaces by repeating Step 2. Step 7: Pattern the entire row of surfaces by repeating Step 3.

Picture #4 Step 8: Create a solid cut using the row of surfaces by repeating Step 4.

Page 6 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01

Finished! Now you have two very clean transformed surfaces that control the number of cutouts in rows and columns (Picture #5). Now you simply change the number of patterned transformed surfaces in each direction to control your X, Y grid. Instead of having to regenerate 5 features for each cutout, Pro/E is now only cutting out one surface feature for an entire row!

Picture #5 Quick Summary of Steps 1) Create a surface copy of all required features 2) Create surface transform 3) Select “Move” “Copy” 4) Select the surface copy to pattern 5) Select “Translate” or “Rotate” 6) Select appropriate reference (plane, axis, coord) 7) Enter in values for movement 8) Pattern the newly transformed surface 9) Create solid feature (cut or protrusion) from surface 10) Ref pattern the new solid feature.

Page 7 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01

Key Vocabulary for Surface Transforms: Bound Surface: The surface that “caps” off the automatic gathering of surfaces by Pro/E during a “Surf & Bnd” operation. Imagine trying to gather all of the surfaces internal to a drinking glass, the boundary would be the top rim. Copy (surface): a method to create a new surface feature by copying previously created surfaces or individual surfaces on a solid. Pattern: any geometry that occurs in a regular, repeatable fashion. Common examples are linear patterns (i.e. a grid array) or radial patterns (i.e. a bolt circle on a flange). Seed Surface: Any surface that is internal to the geometry that you want to gather during a “Surf & Bnd” operation. Imagine trying to gather all of the surfaces internal to a drinking glass, the seed would be the inside bottom. Surface: The exterior “skin” of a solid part or feature. A solid feature is comprised of many surfaces, each one can individually be selected. A surface is the “skin” geometry bounded by a continuous loop of edges. Transform: A function in which you can take an existing surface feature and move it in either a linear or radial direction. This operation can do two things, either move the existing surface geometry or make a copy and then move the copied surface geometry.

Page 8 of 9

Title: Surface Transforms (for large patterns) Date: 7/22/01

Tutorial Evaluation: Title:

… Engineer

… Designer

… Foundation

… Draftsmen

… Mfg. Engr.

… Advanced Assembly Extension

PTC Products Used:

… Behavioral Modeling

Time using Pro/E:

… 0-6 months

… Intralink

… 6-12 months

… Analyst

… Advanced Surface Extension

… Modelcheck

… 1-2 years

… Tech. Pubs.

… All

… 2-5 years

… 5+ years

1 – Strongly Disagree 3 – Agree 5 – Strongly Agree 1.

This tutorial content met my expectations:

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The exercise was easy to understand:

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This tutorial will help me on current projects:

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These techniques make Pro/E a more effective tool:

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These techniques will increase my speed using Pro/E:

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What concepts/techniques learned from this tutorial will you apply on the job? 1) 2) 3) What would you like to see as a future tutorial at your company? 1) 2) 3) What can be done to improve these tutorials for your company? 1) 2) 3)

Additional Comments:

Page 9 of 9

Untitled Document

KinetiVision Presents Pro/ENGINEER Release 2001 Tips and Techniques

http://www.kinetivision.com/freevids/an_mass_props.htm [28.11.2002 14:23:10]