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Introduction to Pro/ENGINEER Release 2001 T779-320-03 For University Use Only - Commercial Use Prohibited -

Copyright Introduction to Pro/ENGINEER Copyright © 2001 Parametric Technology Corporation. All Rights Reserved. This Introduction to Pro/ENGINEER Training Guide may not be copied, reproduced, disclosed, transferred, or reduced to any form, including electronic medium or machine-readable form, or transmitted or publicly performed by any means, electronic or otherwise, unless Parametric Technology Corporation (PTC) consents in writing in advance. User and training documentation from Parametric Technology Corporation (PTC) is subject to the copyright laws of the United States and other countries and is provided under a license agreement that restricts copying, disclosure, and use of such documentation. PTC hereby grants to the licensed user the right to make copies in printed form of this documentation if provided on software media, but only for internal/personal use and in accordance with the license agreement under which the applicable software is licensed. Any copy made shall include the PTC copyright notice and any other proprietary notice provided by PTC. This documentation may not be disclosed, transferred, modified, or reduced to any form, including electronic media, or transmitted or made publicly available by any means without the prior written consent of PTC and no authorization is granted to make copies for such purposes. Information described herein is furnished for general information only, is subject to change without notice, and should not be construed as a warranty or commitment by PTC. PTC assumes no responsibility or liability for any errors or inaccuracies that may appear in this document. The software described in this document is provided under written license agreement, contains valuable trade secrets and proprietary information, and is protected by the copyright laws of the United States and other countries. UNAUTHORIZED USE OF SOFTWARE OR ITS DOCUMENTATION CAN RESULT IN CIVIL DAMAGES AND CRIMINAL PROSECUTION. Registered Trademarks of Parametric Technology Corporation or a Subsidiary: Advanced Surface Design, CADDS, CADDShade, Computervision, Computervision Services, Electronic Product Definition, EPD, HARNESSDESIGN, Info*Engine, InPart, MEDUSA, Optegra, Parametric Technology, Parametric Technology Corporation, Pro/ENGINEER, Pro/HELP, Pro/INTRALINK, Pro/MECHANICA, Pro/TOOLKIT, PTC, PT/Products, Windchill, and the InPart logo. Trademarks of Parametric Technology Corporation or a Subsidiary 3DPAINT, Associative Topology Bus, Behavioral Modeler, BOMBOT, CDRS, CounterPart, CV, CVact, CVaec, CVdesign, CV-DORS, CVMAC, CVNC, CVToolmaker, DesignSuite, DIMENSION III, DIVISION, DVS, DVSAFEWORK, EDE, e/ENGINEER, Electrical Design Entry, e-Series, Expert Machinist, Expert Toolmaker, Flexible Engineering, ICEM, Import Data Doctor, Information for Innovation, i-Series, ISSM, MEDEA, ModelCHECK, NC Builder, Nitidus, PARTBOT, PartSpeak, Pro/ANIMATE, Pro/ASSEMBLY, Pro/CABLING, Pro/CASTING, Pro/CDT, Pro/CMM, Pro/COMPOSITE, Pro/CONVERT, Pro/DATA for PDGS, Pro/DESIGNER, Pro/DESKTOP, Pro/DETAIL, Pro/DIAGRAM, Pro/DIEFACE, Pro/DRAW, Pro/ECAD, Pro/ENGINE, Pro/FEATURE, Pro/FEM -POST, Pro/FLY-THROUGH, Pro/HARNESS-MFG, Pro/INTERFACE, Pro/LANGUAGE, Pro/LEGACY, Pro/LIBRARYACCESS, Pro/MESH, Pro/Model.View, Pro/MOLDESIGN,Pro/NC-ADVANCED, Pro/NC-CHECK, Pro/NC-MILL, Pro/NCPOST, Pro/NC-SHEETMETAL, Pro/NC-TURN, Pro/NC-WEDM, Pro/NC-Wire EDM, Pro/NETWORK ANIMATOR, Pro/NOTEBOOK, Pro/PDM, Pro/PHOTORENDER, Pro/PHOTORENDER TEXTURE LIBRARY, Pro/PIPING, Pro/PLASTIC ADVISOR, Pro/PLOT, Pro/POWER DESIGN, Pro/PROCESS, Pro/REPORT, Pro/REVIEW, Pro/SCAN-TOOLS, Pro/SHEETMETAL, Pro/SURFACE, Pro/VERIFY, Pro/Web.Link, Pro/Web.Publish, Pro/WELDING, Product Structure Navigator, PTC i-Series, Shaping Innovation, Shrinkwrap, The Product Development Company, Virtual Design Environment, Windchill e-Catalog, Windchill e-Series, Windchill ProjectLink, CV-Computervision logo, DIVISION logo, and ICEM logo.

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PRINTING HISTORY Document No. Date

Description

T779-320-01

05/18/01

Initial Printing of Introduction to Pro/ENGINEER for Release 2001

T779-320-02

08/15/01

Revisions to Introduction to Pro/ENGINEER for Release 2001

T779-320-03

11/08/01

Revisions to Introduction to Pro/ENGINEER for Release 2001

Order Number DT-779-320-EN Printed in U.S.A


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T r aining Agenda Introduction to Pro/ENGINEER Day 1

Day 4

Introduction to Pro/ENGINEER

Principles of Top-Down Design

The Pro/ENGINEER Interface

Additional Datum Features and Skeletons

Pick-and-Place Features

Layers and Suppression

Sketcher Basics

Creating Surfaces with Freeform

Sketched Features

Day 2

Day 5

Default Datum Templates

The Resolve Environment

Parent/Child Relationships

Information Tools

Sweeps and Blends

Configuring Pro/ENGINEER

Relations and Parameters

Modeling Philosophy

Day 3 Appendix A: Review Questions Behavioral Modeling

Appendix B: Project Laboratory

Drawings and Drawing Templates

Appendix C: Precision Learning

Duplication Features: Patterns and Copy

Appendix D: PTC Help

Creating Assemblies

Appendix E: Technical Support


PTC Telephone and Fax Numbers The following is a list of telephone and fax numbers you may find useful:

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In addition, you can find the PTC home page on the World Wide Web can be found at: http://www.ptc.com. The Web site contains the latest training schedules, registration information, directions to training facilities, and course descriptions, as well as information on PTC, the Pro/ENGINEER product line, Consulting Services, Customer Support, and Pro/PARTNERS.


Table of Contents Introduction to Pro/ENGINEER INTRODUCTION TO PRO/ENGINEER

1-1

PRO/ENGINEER CORE CONCEPTS ........................................................................1-2 Solid Modeling Benefits .................................................................................................................1-2 Designing Feature-based Models ..................................................................................................1-3 Designing with Parametric Features .............................................................................................1-4 Taking Advantage of Associativity...............................................................................................1-5

THE PRO/ENGINEER INTERFACE

2-1

ELEMENTS OF THE INTERFACE...........................................................................2-2 The Base Window............................................................................................................................2-2 Accessing Commands with Pull-Down Menus ..........................................................................2-2 Accessing Frequently-used Commands with the Toolbar.........................................................2-3 Manipulating Your Designs in the Display Area........................................................................2-3 Viewing Information in the Message Area..................................................................................2-4

WORKING WITH MODELS.....................................................................................2-4 Working with Dialog Boxes...........................................................................................................2-5 Retrieving Models ............................................................................................................................2-6 Using the Model Tree......................................................................................................................2-7 Using the Menu Manager...............................................................................................................2-8 Obtaining Additional Information with Help ..............................................................................2-8 Retrieving Multiple Models ...........................................................................................................2-8 Working with Multiple Sub-Windows .........................................................................................2-8 Saving Changes ................................................................................................................................2-9 Closing Windows...........................................................................................................................2-10 Deleting Files ..................................................................................................................................2-10

LABORATORY PRACTICAL................................................................................. 2-11 EXERCISE 1: Using the Pro/ENGINEER Environment........................................................2-12 EXERCISE 2: Manipulating Model Size and Orientation......................................................2-15 EXERCISE 3: Interrogating the Model Tree.............................................................................2-18 EXERCISE 4: Challenge Exercise..............................................................................................2-21

MODULE SUMMARY ........................................................................................... 2-25


PICK-AND-PLACE FEATURES

3-1

DEFINING PICK-AND-PLACE FEATURES ............................................................ 3-2 Generic Method of Creation........................................................................................................... 3-2 Shell Features ................................................................................................................................... 3-2 Creating Edge Chamfers................................................................................................................. 3-3 Creating Simple Rounds................................................................................................................. 3-3 Specifying Radius Values for Simple Rounds ........................................................................... 3-5 Hole Features.................................................................................................................................... 3-6 Creating the Straight Hole Feature................................................................................................ 3-6

LABORATORY PRACTICAL .................................................................................3-10 EXERCISE 1: Shell and Automatic Round Features.............................................................. 3-11 EXERCISE 2: Creating Chamfers and Rounds ....................................................................... 3-14 EXERCISE 3: Exploring the Straight Hole Feature ................................................................ 3-21 EXERCISE 4: Challenge Exercise............................................................................................. 3-29

MODULE SUMMARY ............................................................................................3-31

SKETCHER BASICS

4-1

THE SKETCHER INTERFACE ................................................................................ 4-2 The Intent Manager......................................................................................................................... 4-3 Accessing Commands with Pop-Up Menus................................................................................ 4-3

THE SKETCHER MODE.......................................................................................... 4-4 Accessing Commands with Sketcher Menus.............................................................................. 4-4 Specifying References .................................................................................................................... 4-5 Creating Geometry........................................................................................................................... 4-6 Dimensioning Sketches .................................................................................................................. 4-7 Adding Constraints.......................................................................................................................... 4-9 Other Sketcher Tools ....................................................................................................................... 4-9 Setting Sketcher Preferences ....................................................................................................... 4-13

TAKING ADVANTAGE OF SKETCHER MODE ....................................................4-14 LABORATORY PRACTICAL .................................................................................4-17 Goal.................................................................................................................................................. 4-17 Method............................................................................................................................................. 4-17 Tools ................................................................................................................................................ 4-17 EXERCISE 1: Sketching Basics ................................................................................................. 4-18 EXERCISE 2: Sketching in Steps .............................................................................................. 4-24 EXERCISE 3: Sketching a Hexagon.......................................................................................... 4-31

MODULE SUMMARY ............................................................................................4-34

SKETCHED FEATURES

5-1

DEFINING SKETCHED FEATURES........................................................................ 5-2


Sketching Cuts and Protrusions.....................................................................................................5-2

USING THE SKETCHER TOOLS .............................................................................5-5 Dimensioning Sections ...................................................................................................................5-5

LABORATORY PRACTICAL................................................................................. 5-10 EXERCISE 1: Creating a Cut ......................................................................................................5-11 EXERCISE 2: Creating a Protrusion..........................................................................................5-20

MODULE SUMMARY ........................................................................................... 5-24

DEFAULT DATUM TEMPLATES

6-1

USING DATUM PLANES AS BASE FEATURES .....................................................6-2 Base Features ....................................................................................................................................6-2 Defining a Datum Plane..................................................................................................................6-2 Using a Default Datum as the Base Feature ................................................................................6-2 Creating Datum Planes....................................................................................................................6-3 Creating Internal Datum Planes.....................................................................................................6-3

LABORATORY PRACTICAL...................................................................................6-4 EXERCISE 1: Creating a New Part ..............................................................................................6-5 EXERCISE 2: Creating an Internal Datum Plane ....................................................................6-11

MODULE SUMMARY ........................................................................................... 6-15

PARENT/CHILD RELATIONSHIPS

7-1

PARENT/CHILD RELATIONSHIPS IN PRO/ENGINEER.........................................7-2 Pick-and-Place Feature Parent/Child Relationships ..................................................................7-2 Sketched Feature Parent/Child Relationships.............................................................................7-2

LABORATORY PRACTICAL...................................................................................7-8 EXERCISE 1: Using Feature Reroute..........................................................................................7-9 EXERCISE 2: Using Feature Redefine......................................................................................7-14

MODULE SUMMARY ........................................................................................... 7-20

SWEEPS AND BLENDS

8-1

SWEEP AND TRAJECTORIES.................................................................................8-2 Creating Sweeps and Trajectories .................................................................................................8-2 Creating Parallel Blends .................................................................................................................8-3

LABORATORY PRACTICAL...................................................................................8-7 EXERCISE 1: Creating Parallel Blend Features ........................................................................8-8 EXERCISE 2: Create a Simple Sweep Protrusion...................................................................8-14

MODULE SUMMARY ........................................................................................... 8-17


RELATIONS AND PARAMETERS

9-1

RELATIONS AND PARAMETERS.......................................................................... 9-2 Parametric Relations ....................................................................................................................... 9-2 Representing Relations: Types and Symbols .............................................................................. 9-4 Incorporating Your Design Intent Using Relations ................................................................... 9-4 Order of Relations ........................................................................................................................... 9-6 Design Changes ............................................................................................................................... 9-8

LABORATORY PRACTICAL .................................................................................. 9-9 EXERCISE 1: Creating Relations .............................................................................................. 9-10 EXERCISE 2: Creating Parameters for Feature-Control........................................................ 9-15

MODULE SUMMARY ............................................................................................9-18

BEHAVIORAL MODELING

10-1

BEHAVIORAL MODELING...................................................................................10-2 Behavioral Modeling Features..................................................................................................... 10-2

USING BEHAVIORAL MODELER .........................................................................10-4 Defining the Behavioral Modeler Components ........................................................................ 10-8

LABORATORY PRACTICAL ...............................................................................10-13 EXERCISE 1: Creating a Datum Analysis Feature to Measure Mass Properties ............10-14 EXERCISE 2: Analyze Fluid Volume in a Cup.....................................................................10-20 EXERCISE 3: Crankshaft Optimization..................................................................................10-26

MODULE SUMMARY ..........................................................................................10-36

DRAWINGS AND DRAWING TEMPLATES

11-1

DRAWING FUNDAMENTALS...............................................................................11-2 Creating a Drawing........................................................................................................................ 11-2 Adding Drawing Views ................................................................................................................ 11-2 Types of Views............................................................................................................................... 11-2 Using the View Type Menu......................................................................................................... 11-3 Adding a Cross-section................................................................................................................. 11-4 Manipulating Views ...................................................................................................................... 11-5

DEFINING DRAWING TEMPLATES .....................................................................11-6 DETAILING THE DRAWING.................................................................................11-7 Creating Feature Dimensions ...................................................................................................... 11-8 Creating Driven Dimensions ....................................................................................................... 11-8 Manipulating Dimensions............................................................................................................ 11-8

LABORATORY PRACTICAL ...............................................................................11-10 EXERCISE 1: Creating a Drawing...........................................................................................11-11 EXERCISE 2: Modifying Created Views and Testing for Associativity ..........................11-17 EXERCISE 3: Detailing the Gear Part Drawing....................................................................11-20


MODULE SUMMARY ......................................................................................... 11-24

DUPLICATING FEATURES: PATTERNS AND COPY

12-1

CREATING PATTERNS......................................................................................... 12-2 Patterning Benefits.........................................................................................................................12-2 Pattern Types ..................................................................................................................................12-2 Pattern Options...............................................................................................................................12-3

COPYING FEATURES ........................................................................................... 12-7 Specifying Copy-To Locations....................................................................................................12-8 Copying Methods...........................................................................................................................12-8 Specifying Copied Feature Dependencies .................................................................................12-9 Choosing Features to Copy ........................................................................................................12-10 Specifying Dependency Options ...............................................................................................12-10

LABORATORY PRACTICAL............................................................................... 12-12 EXERCISE 1: Creating and Modifying a Dimension Pattern..............................................12-13 EXERCISE 2: Creating a Reference Pattern ...........................................................................12-15 EXERCISE 3: Creating Rotational Patterns of Sketched Features .....................................12-18 EXERCISE 4: Copying Features ..............................................................................................12-22 EXERCISE 5: Building the Steering Column .........................................................................12-24

MODULE SUMMARY ......................................................................................... 12-28

CREATING ASSEMBLIES

13-1

OVERVIEW ........................................................................................................... 13-2 The Surface Normal Vector..........................................................................................................13-2 Constraining Component Parts ....................................................................................................13-3 Placing Components......................................................................................................................13-6 Packaging Under-Constrained Components .............................................................................13-7

MODIFYING ASSEMBLIES................................................................................... 13-7 Modifying Your Design Intent ....................................................................................................13-8

OTHER ASSEMBLY OPTIONS.............................................................................. 13-8 Generating Bills of Material.........................................................................................................13-8 Creating Exploded Views .............................................................................................................13-9

LABORATORY PRACTICAL............................................................................... 13-10 EXERCISE 1: Create a Subassembly of Three Parts ............................................................13-11 Exercise 2: Create the Machine Assembly ..............................................................................13-18

MODULE SUMMARY ......................................................................................... 13-22

PRINCIPLES OF TOP-DOWN DESIGN

14-1

INTRODUCTION ................................................................................................... 14-2


Definition......................................................................................................................................... 14-2 Stages of Top-Down Design........................................................................................................ 14-2 The Approach................................................................................................................................. 14-2 Comparing Top-Down Design to Traditional Approaches .................................................... 14-3 Benefits of Top-Down Design Methodology ........................................................................... 14-4

THE SIX STEPS OF TOP-DOWN DESIGN..............................................................14-4 Step 1 - Defining Design Intent................................................................................................... 14-5 Step 2 - Defining Preliminary Product Structure ..................................................................... 14-5 Step 3 - Skeleton Models ............................................................................................................. 14-5 Step 4 - Communicating Design Intent...................................................................................... 14-6 Step 5 - Continued Population of the Assembly....................................................................... 14-6 Step 6 - Managing Part Interdependencies................................................................................ 14-6

PRO/ENGINEER TOP-DOWN DESIGN TOOLS .....................................................14-7 Layouts ............................................................................................................................................ 14-7 Skeletons......................................................................................................................................... 14-8 Data Sharing Features .................................................................................................................14-10 Managing References / Interdependencies..............................................................................14-12

MODULE SUMMARY ..........................................................................................14-15

ADDITIONAL DATUM FEATURES AND SKELETONS

15-1

ADDITIONAL DATUM FEATURES.......................................................................15-2 Datum Axes .................................................................................................................................... 15-2 Datum Curves................................................................................................................................. 15-2 Datum Points .................................................................................................................................. 15-3 Datum Coordinate Systems .......................................................................................................... 15-4

LABORATORY PRACTICAL .................................................................................15-5 EXERCISE 1: Creating Additional Datum Features............................................................... 15-6 EXERCISE 2: Creating a simple skeleton ................................................................................ 15-9 EXERCISE 3: The Link Skeleton in an assembly .................................................................15-14 OPTIONAL EXERCISE 4: The Vice Grip .............................................................................15-16

MODULE SUMMARY ..........................................................................................15-19

LAYERS AND SUPPRESSION

16-1

DEFINING LAYERS...............................................................................................16-2 Functionality................................................................................................................................... 16-2 Working With Layers.................................................................................................................... 16-2

CREATING LAYERS..............................................................................................16-3 Selecting the Object....................................................................................................................... 16-3 Creating Layers .............................................................................................................................. 16-4 Associating Items to a Layer........................................................................................................ 16-4


Setting the Display Status of a Layer..........................................................................................16-5 Manipulating Layer Display Status ............................................................................................16-7

SUPPRESSION FUNCTIONALITY ........................................................................ 16-8 Using Suppression .........................................................................................................................16-8 Suppressing Parent/Child Relationships....................................................................................16-9 Saving and Resuming Suppressed Features ..............................................................................16-9

LABORATORY PRACTICAL............................................................................... 16-10 EXERCISE 1: Using Layers in Part Mode..............................................................................16-11 EXERCISE 2: Using Layers in Assembly Mode ...................................................................16-14 EXERCISE 3: Suppressing in Part Mode................................................................................16-20 EXERCISE 4: Suppressing Components in Assembly Mode..............................................16-22

MODULE SUMMARY ......................................................................................... 16-26

CREATING SURFACES WITH FREEFORM

17-1

DESIGNING WITH INTERACTIVE SURFACES.................................................... 17-2 THE STYLE FEATURE.......................................................................................... 17-2 HYBRID MODELING ............................................................................................ 17-3 CREATING SURFACES WITH ISDX..................................................................... 17-4 Creating 2-D and 3-D Curves ......................................................................................................17-4 Using COS.......................................................................................................................................17-6 Creating Styling Models ...............................................................................................................17-6 Creating Freeform Surfaces with Parametric Controls ............................................................17-7 Creating Blends and Transitions .................................................................................................17-8 Applying Style Surfaces to Engineering Models ......................................................................17-8 Reverse Styling...............................................................................................................................17-9

CREATING STYLE SURFACES............................................................................. 17-9 LABORATORY PRACTICAL............................................................................... 17-10 EXERCISE 1: Interrogating the STYLE Interface.................................................................17-11 EXERCISE 2: Creating a Handle on the Flashlight...............................................................17-16

MODULE SUMMARY ......................................................................................... 17-23

THE RESOLVE ENVIRONMENT

18-1

REGENERATION FAILURES ................................................................................ 18-2 Starting the Resolve Environment...............................................................................................18-2 Resolving Regeneration Failures.................................................................................................18-2

LABORATORY PRACTICAL................................................................................. 18-6 EXERCISE 1: Resolving a Regeneration Failure.....................................................................18-6

MODULE SUMMARY ......................................................................................... 18-10


INFORMATION TOOLS

19-1

MODEL INFORMATION........................................................................................19-2 Obtaining Information about a Specific Feature....................................................................... 19-2 Obtaining Regeneration Information.......................................................................................... 19-2 Accessing Information about Part Features .............................................................................. 19-2 Obtaining Information about Assemblies .................................................................................. 19-3

MEASUREMENT, INTERFERENCE, AND MASS PROPERTIES ...........................19-3 Calculating Mass Properties ........................................................................................................ 19-3

LABORATORY PRACTICAL .................................................................................19-5 EXERCISE 1: Using Information Tools .................................................................................... 19-5

MODULE SUMMARY ............................................................................................19-9

CONFIGURING PRO/ENGINEER

20-1

CUSTOMIZING PRO/ENGINEER...........................................................................20-2 Defining Configuration Files ....................................................................................................... 20-2 Creating Mapkeys.......................................................................................................................... 20-4

CUSTOMIZING YOUR TOOLBAR.........................................................................20-5 Adding Icons to Existing Toolbars ............................................................................................. 20-5 Creating Pull-down Menus .......................................................................................................... 20-6

THE MODEL TREE ................................................................................................20-7 LABORATORY PRACTICAL ...............................................................................20-10 EXERCISE 1: Setting Up a Configuration File......................................................................20-11 EXERCISE 2: Creating a Mapkey............................................................................................20-16

MODULE SUMMARY ..........................................................................................20-19

MODELING PHILOSOPHY

21-1

DESIGN INTENT....................................................................................................21-2 Recording Your Design Criteria.................................................................................................. 21-3 Using Pro/ENGINEER as a Parametric Tool............................................................................ 21-3 Creating Parent/Child Relationships.......................................................................................... 21-3 Advantages of Pro/ENGINEER Associativity ......................................................................... 21-4 Changing Design Intent................................................................................................................ 21-5

LABORATORY PRACTICAL .................................................................................21-6 Part I: Part Level Design Intent................................................................................................... 21-6 Part II: Assembly level Design Intent ......................................................................................21-10 Decision Process Questionnaire ................................................................................................21-10

MODULE SUMMARY ..........................................................................................21-13


REVIEW QUESTIONS

A-1

DAY 1: REVIEW QUESTIONS................................................................................A-2 DAY 2: REVIEW QUESTIONS................................................................................A-6 DAY 3: REVIEW QUESTIONS.............................................................................. A-10 DAY 4: REVIEW QUESTIONS.............................................................................. A-14 DAY 5: REVIEW QUESTIONS.............................................................................. A-17

PROJECT LABORATORY

B-1

INTRODUCTION .................................................................................................... B-2 PART CREATION ................................................................................................... B-3 SECTION 1: Creating the Motor Part ......................................................................................... B-3 SECTION 2: Creating the Lower Housing Part......................................................................... B-5 SECTION 3: Creating the Snap Ring Part .................................................................................. B-9 SECTION 4: Creating the Upper Housing Part .......................................................................B-11

CREATING ASSEMBLIES .................................................................................... B-18 SECTION 1: Creating the Motor Assembly.............................................................................B-18 SECTION 2: Concurrent Design of the Motor Housing........................................................B-22 SECTION 3: Creating the Blower Assembly...........................................................................B-23 SECTION 4: Creating the Motor Part Drawing.......................................................................B-26

INTERROGATING YOUR MODELS..................................................................... B-29 SECTION 1: Designing the Cover Part.....................................................................................B-30 SECTION 2: Completing the Motor Part..................................................................................B-34 SECTION 3: Completing the Blower Assembly .....................................................................B-36 SECTION 4: Completing the Motor Assembly .......................................................................B-40

COMPLETING THE PROJECT.............................................................................. B-43 SECTION 1: Developing the Motor Part ..................................................................................B-43 SECTION 2: Finishing the Lower Housing.............................................................................B-45 SECTION 3: Completing the Drawing .....................................................................................B-47

USING THE PRO/FICIENCY EVALUATOR

C-1

TECHNOLOGY-BASED LEARNING @ PTC.......................................................... C-2 TBLS: Necessity and Advantages ................................................................................................ C-2 TBLS Components ......................................................................................................................... C-2

THE PRO/FICIENCY EVALUATOR ....................................................................... C-3 Measurable Training Outcomes.................................................................................................... C-3 A Powerful Planning Tool............................................................................................................. C-3

COMPLYING WITH EQUAL OPPORTUNITY EMPLOYMENT REQUIREMENTS.................................................................................................... C-4 EXERCISE 1: Completing Evaluator Assessments .................................................................. C-5

MODULE SUMMARY ............................................................................................ C-8


USING PTC HELP

D-1

PTC HELP OVERVIEW .......................................................................................... D-2 PTC Help Features.......................................................................................................................... D-2

USING Pro/ENGINEER HELP ................................................................................. D-2 Launching Help: Four Methods................................................................................................... D-2

PTC HELP MODULES............................................................................................ D-7

PTC GLOBAL SERVICES: TECHNICAL SUPPORT

E-1

FINDING THE TECHNICAL SUPPORT WEB PAGE ...............................................E-2 OPENING TECHNICAL SUPPORT CALLS .............................................................E-2 Opening Technical Support Calls via E-mail..............................................................................E-2 Opening Technical Support Calls via Telephone.......................................................................E-3 Opening Technical Support Calls via the Web...........................................................................E-3 Sending Data Files to PTC Technical Support ...........................................................................E-3 Routing Your Technical Support Calls ........................................................................................E-4 Technical Support Call Priorities ..................................................................................................E-5 Software Performance Report Priorities ......................................................................................E-5

REGISTERING FOR ON-LINE SUPPORT ...............................................................E-5 ONLINE SERVICES.................................................................................................E-6 FINDING ANSWERS IN THE KNOWLEDGE BASE ...............................................E-6 Terminology used by Technical Support.....................................................................................E-7

GETTING UP-TO-DATE INFORMATION ...............................................................E-8 CONTACT INFORMATION ....................................................................................E-9 PTC Technical Support Worldwide Electronic Services..........................................................E-9 Telephone........................................................................................................................................E-10

ELECTRONIC SERVICES ..................................................................................... E-14

INDEX

I-1


For University Use Only - Commercial Use Prohibited -Module

1 Introduction to Pro/ENGINEER In this module you learn about the core Pro/ENGINEER features and concepts.

Objectives After completing this module, you will be able to: •

Describe how to use Pro/ENGINEER as a solid modeling design tool.

•

Describe the three main Pro/ENGINEER design concepts.

Page 1-1

NOTES

PRO/ENGINEER CORE CONCEPTS You use Pro/ENGINEER to create solid models of your designs. The three-dimensional work environment enables you to take advantage of: •

Feature-based modeling

•

Associativity

•

Parametric relationships

Solid Modeling Benefits Solid modeling enjoys benefits not obtained in two-dimensional design: •

Solid models have volumes and surface areas.

•

You can calculate mass properties directly from the geometry you create.

•

When you manipulate a solid model, the model itself remains a solid.

1. Wireframe 3. No Hidden Line

2. Hidden Lines 4. Solid Shade

Figure 1: Solid Model Display

For University Use Only - Commercial Use Prohibited P a g e 1- 2


NOTES

Designing Feature-based Models The models you create in Pro/ENGINEER are feature-based. This means that the geometry of your part model is composed of one or more features. A feature is the smallest building block in a part model. Pro/ENGINEER enables you to build a model incrementally by adding individual features one at a time. As you construct your model, you choose your building blocks, as well as the order in which to create them. Creating models in Pro/ENGINEER involves incorporating your “design intent” into the model. Design intent is the reason for adding every feature. For example, you add hole features to a model because the resulting part must be assembled to another part, and the holes are needed for the screws. The following figure shows how a typical part can be designed by adding one feature after another to a base model.

Base Feature

Protrusion Added

Thru-All Cuts and Holes Added

Blind Cut Added

Chamfer Added

Chamfers Added

Rounds Added

Figure 2: Building Models Feature by Feature

For University Use Only - Commercial Use Prohibited Introduction to Pro/ENGINEER

P a g e 1- 3

NOTES

Designing with Parametric Features The designs you create in Pro/ENGINEER can be parametric. This means that their dimensions are controlled by parameters, which are related dimensions. Parametric modeling has many advantages: •

Modifying dimensions can change model geometry.

•

Designated features can be related to each other.

•

Modifications to certain features propagate changes to other features.

•

Parent/child relationships can be developed between features.

5

10

Figure 3: Protrusion and Hole Follow Side of Block



NOTES

Taking Advantage of Associativity Pro/ENGINEER models usually consist of several parts, assemblies, and drawings. All of these objects are fully associative. This means that changes made at one level will propagate to all the levels. For example, if you change dimensions on a drawing, the change will be reflected in the associated part. The following figure shows associativity between a part and an assembly.

5

Original shaft before length modification

Shaft associated to assembly

10

Modification of shaft length Assembly automatically updates

Figure 4: Associativity

For University Use Only - Commercial Use Prohibited Introduction to Pro/ENGINEER

P a g e 1- 5


For University Use Only - Commercial Use Prohibited - Module

2 The Pro/ENGINEER Interface In this module you learn how to use the Pro/ENGINEER interface to enhance your design sessions.


Describe how to use the Pro/ENGINEER interface.

•

Describe the different Pro/ENGINEER file types.

•

Retrieve, save, erase, and delete files in Pro/ENGINEER.

•

Describe how to use the Model Tree and the Menu Manager.

•

Describe the parametric, associative, and feature-based characteristics of Pro/ENGINEER models.

P age 2-1

NOTES

ELEMENTS OF THE INTERFACE

Figure 1 Sample Model Display in Main Window

The Base Window When you start Pro/ENGINEER, the base window opens on your desktop. You create your designs in this window. This window has four main parts: •

Pull-down menu

•

Display area

•

Toolbar

•

Message area

Accessing Commands with Pull-Down Menus The following Pro/ENGINEER pull-down menu options are available in all the different modes of the software: •

File –

File manipulation commands

•

Edit –

Object manipulation and action commands

•

View –

Model display commands



NOTES

•

Insert

•

Analysis –

•

Info –

•

Applications

•

Utilities –

Working environment customization commands

•

Window –

Window manipulation commands

•

Help

– Creates features like protrusions, cuts, holes, and rounds

Model, surface, curve, motion, and sensitivity and optimization commands Query and report commands – Launch commands for other Pro/ENGINEER modules

– Help commands

Accessing Frequently-used Commands with the Toolbar The Pro/ENGINEER toolbar contains icons for frequently used commands. Toolbar buttons are provided as an alternative to menu commands. You can customize you toolbar.

Figure 2: Pro/ENGINEER Toolbar

Manipulating Your Designs in the Display Area Pro/ENGINEER displays parts, assemblies, drawings, and models on the screen in the display area. An object’s display depends on the current environment settings. When you select the model on the screen, the system distinguishes between an edge and a surface of the model by highlighting them in two different colors.

Note: Surfaces of models are valid in Pro/ENGINEER regardless of the model display.

For University Use Only - Commercial Use Prohibited The Pro/ENGINEER Interface

P a g e 2- 3

NOTES

Viewing Information in the Message Area The message area: •

Displays status information for every operation performed.

•

Displays queries and hints to simplify the task you are working on.

•

Prompts you for additional information (the text message is accompanied by an optional audible signal).

•

Displays icons that represent different kinds of information, such as warnings or status prompts.

To view old messages, you can use the scrollbar located on the right.

Note: When Pro/ENGINEER requires data input, it temporarily disables all other functions until you enter the required data.

WORKING WITH MODELS File Types Every type of Pro/ENGINEER object has a different file extension. Typical file extensions are described next.. •

PRT – Part files allow you to create 3-D models consisting of many

features. •

ASM – Assembly files contain information on how 3-D parts and

assemblies are assembled together. •

DRW – Drawing files contain 2-D fully dimensioned drawings of parts

or assemblies. •

SEC – Sketch files contain 2-D non-associative sketches that can be imported while in sketcher mode.

In addition, there is also a SKETCHER mode that allows you to create twodimensional sketches that are parametric.



NOTES

Note: When you create new files and save them you do not have to add the file extensions. The system automatically associates the correct file extension to the file that you are saving.

Working with Dialog Boxes Dialog boxes in Pro/ENGINEER are used for model manipulation, feature creation, and saving. There are two kinds of dialog boxes: general and model.

The General Dialog Box A general dialog box performs general software environment functions such as setting display options for the model. The following figure represents some of the common elements in a regular dialog box.

Title Tabs

Drop-down arrow Check boxes

Text box

Command buttons

Figure 3: Example of a Dialog Box


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NOTES

The Model Dialog Box A model dialog box creates and modifies model geometry by prompting you for required and optional elements from the user. Required elements are modifiable properties of a Pro/ENGINEER feature that must be specified to completely define a feature. Optional elements are additional operations that you may perform; but they are not necessary for completing the feature. The following figure illustrates a model dialog box that defines a ROUND feature.

Figure 4: A Model Dialog Box

The option buttons in a model dialog box are: •

Define

•

Refs

•

Info

•

OK

•

Cancel

•

Preview

– Defines and/or changes selected elements in the dialog box.

– Displays the external references of the current selected element. – Generates a listing of the properties of the feature that you are creating. – Completes the definition of the elements, creating the feature or model entity. – Cancels the current feature or model entity. – Checks geometry before completing the feature definition.

Retrieving Models When you retrieve files into a working session by clicking File > Open , Pro/ENGINEER also opens up a model tree window and a menu manager that allow you to create, manipulate, and modify model geometry.



NOTES

Using the Model Tree The MODEL TREE presents the model structure feature by feature. You can select features from the MODEL TREE for modification and deletion. MODEL TREE icons indicate the corresponding item type and its current status.

Figure 5: Model Tree with Added Parameters


P a g e 2- 7

NOTES

Using the Menu Manager The MENU MANAGER displays a list of menus that you can use to create, modify, and duplicate model geometry. Using the MENU MANAGER, you drive along a certain path to complete a task by making choices from menus. Each time you choose an option from a submenu, Pro/ENGINEER opens another submenu until you have finished making selections.

Obtaining Additional Information with Help When you hold your mouse over any menu option, an on-line help message displays on the bottom of the current active window. If you need additional help, you can right-click [ from the pop-up menu.

] the menu option and select G e t

Help

Note: The system administrator must install and setup the online documentation for you to be able to access this functionality.

Retrieving Multiple Models You can have multiple models in session at one time—each window containing a model—making it possible to refer to one model while working on another. However, Pro/ENGINEER only allows you to work on one active window at a time.

Note: To activate a window, you must click Window > Activate .

Working with Multiple Sub-Windows If the main window currently contains a model, Pro/ENGINEER automatically opens a new main window each time you open another model. The new main window contains the same toolbars and message area as the first main window.



NOTES

Figure 6: A New Window over the Main Window

Saving Changes As you work on your design, is a good practice to save your file often. The File > Save option creates a new version of the file with an incremental version number. To retrieve an old version, you must specify the version number in the retrieval name. The All Versions option in the FILE OPEN dialog box displays the version numbers of a file.


P a g e 2- 9

NOTES

Figure 7: Opening a Version of a Model

Closing Windows To close a window, you use the Window > Close or the File > Close Window options. However, this does not remove the model from the current session of Pro/ENGINEER. The model still occupies RAM space on the computer. If the model is no longer required, you erase it from memory with the F i l e > Erase > Current option. You can erase all models that are in session but not displayed in the active windows with the Erase > Not Displayed option.

Deleting Files The File > Delete option removes old versions of a model. The Delete > All Versions option deletes all versions of the model from the system memory, as well as from the hard drive.

For University Use Only - Commercial Use Prohibited P a g e 2- 1 0


NOTES

LABORATORY PRACTICAL Goal In this laboratory you will get first-hand experience to see how Pro/ENGINEER is a parametric, associative, and feature-based solid modeler.

Method In Exercise 1, you learn the Pro/ENGINEER environment. In Exercise 2: you learn how to manipulate the size and orientation of the model. In Exercise 3, you learn how to interrogate the MODEL TREE. In Exercise 4, you how to investigate the associativity between an assembly component and an incomplete drawing.

Tools Table 1: Pro/ENGINEER Toolbar Icons

Icons

Description Datum planes on/off Shading Wireframe display Hidden line display Zoom in Zoom out Refit Orient view Saved view list File save


P a g e 2- 1 1

NOTES

EXERCISE 1: Using the Pro/ENGINEER Environment Task 1.

Open the master assembly.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 02_interface. 3. Click

[File open].

4. In the FILE OPEN dialog box, select Assembly for the TYPE dropdown list. Only the assembly files become visible. 5. Select MASTER.ASM and click Preview >>> . This will show a preview of the model before opening it. 6. Click [No hidden line] icon to see the graphical preview of the assembly. 7. Click O p e n to open MASTER.ASM.

Figure 8: The Master Assembly

Task 2.

Manipulate the display of the assembly.

1. Click Utilities > Environment . 2. In the ENVIRONMENT dialog box, clear the Datum Planes and Datum Axes check boxes.



NOTES

3. Click Apply. Do not close the dialog box. 4. Select H i d d e n Line from the DISPLAY STYLE drop-down list. 5. Click Apply. Task 3.

Change the orientation of the assembly.

1. Select Isometric from the DEFAULT ORIENT drop-down list. 2. Click Apply. 3. Change the orientation back to Trimetric. 4. Click OK to close the dialog box.

Figure 9: Hidden Line Display of Assembly

Task 4.

Use the toolbar to manipulate the model.

1. Toggle the display of datum planes. Click the Datum Plane icon in the toolbar on top of the screen. The datum planes reappear. Datum planes on/off

Datum axes on/off

Datum coordinate system on/off

Datum points on/off

Figure 10: Datum Display Section of Toolbar


P a g e 2- 1 3

NOTES

2. Click

[On/Off ] to turn off the datum planes.

3. Shade the model. Click

Wireframe display

[Shading] on the toolbar.

No Hidden Line display

Shading display

Hidden Line display

Figure 11: Changing the Model Display

4. Click [Wireframe display] to revert back to the hidden line display mode. 5. Click View > Shade to cosmetically shade the model. Note: Wireframe remains selected on the toolbar because the model

is only cosmetically shaded and is not switched to a shaded display mode.

6. Click View > Repaint .



NOTES

EXERCISE 2: Manipulating Model Size and Orientation Task 1.

Change the size and orientation of the model using the toolbar.

1. Click

[Zoom in]. Refit

Zoom In Orient the model Repaint

Zoom Out

Saved Views

Figure 12: Model Orientation Options 2. Select a location in the model. Then select a second location to create a zoom box. The model zooms in. 3. Click

[Zoom out].

4.

[Refit] to resize the model.

Task 2.

Click

Orient the model so that the bracket faces front.

1. Click

[Orient view].

2. The ORIENTATION dialog box opens with the Orient by Reference already selected as shown in the following figure.


P a g e 2- 1 5

NOTES

Figure 13: Orientation Dialog Box

3. In OPTIONS, Reference 1 refers to what is parallel to the screen, and Reference 2 refers to what orients that parallel reference. 4. Leave the default Front in the REFERENCE 1 drop-down list and select the front surface of the bracket part as shown in the following figure.

Select this surface to face front for Reference 1.

Select this surface as the top for Reference 2.

Figure 14: Surface Selection for Orientation



NOTES

5. Select the other surface of the bracket part as Reference 2. The model changes its orientation as shown in the following figure.

Figure 15: Model after Orientation 6. Select the SAVED VIEWS bar towards the bottom of the dialog box. Type [SIDE] in the NAME text box. 7. Click Save to save the new orientation. 8. Click OK in the ORIENTATION dialog box. Task 3.

Change the model back to the default orientation.

1. Click . [Saved views list]. Toggle between the DEFAULT and the saved SIDE views from the saved view list to observe the model in two different orientations. Tips & Techniques: You can also manipulate the model orientation by using the mouse buttons and key. The left mouse button zooms the model, the middle spins it, and the right pans it.


P a g e 2- 1 7

NOTES

EXERCISE 3: Interrogating the Model Tree Task 1.

Modify dimensions of model using the MODEL TREE.

1. If the MODEL TREE is not active, click View > Model Tree to view the model tree on the left. 2. Modify the offset value of the master shaft part. In the model tree, right-click on the MASTER_SHAFT.PRT, and select Modify from the pop-up menu. 3. Select the 76 dimension that appears. 4. In the message area, type [90] and press . 5. Click Done in the MODIFY menu of the MENU MANAGER. 6. Click Done/Return in the ASSEM MOD menu. Task 2.

Regenerate the assembly.

1. In the ASSEMBLY menu, click Regenerate . 2. In the PRT TO REGEN menu, click Automatic. 3. The shaft moves to its new location. The gear and crank parts follow the shaft. This proves the parametric nature of the assembly. Task 3.

Test the associativity by modifying length of the shaft part.

1. Click File > Open. Open MASTER_SHAFT.PRT. 2. Click

> Default

to see model in default view.

3. Click Modify in MENU MANAGER. 4. Select the shaft as shown in the following figure.



NOTES

Select the shaft.

Select this dimension to modify.

Figure 16: Modifying the Shaft

5. Select the 152 dimension. 6. Type [250] and press . 7. Click Regenerate in the PART menu. 8. Save the shaft model. Click

[Save].

9. Accept the default name of MASTER_SHAFT.PRT. Task 4.

Check for associativity between the shaft and the assembly.

1. Close the SHAFT window. Click Window > Close . 2. Make the ASSEMBLY window active. Click Window > Activate . 3. Regenerate the assembly. From the MENU MANAGER, click Regenerate > Automatic. 4. The regenerated assembly appears with modified shaft dimensions, as shown in the following figure.


P a g e 2- 1 9

NOTES

Figure 17: Assembly after Modification and Regeneration

5. A modification made to a part automatically modifies the whole assembly. This proves the associativity of Pro/ENGINEER.



NOTES

EXERCISE 4: Challenge Exercise Task 1. Investigate the associativity between an assembly component and an incomplete drawing. 1. Open the drawing DRAW_CRANK2. DRW. 2. Turn on the datum planes if they are not on, then repaint the screen. 3. Click Edit > Value . 4. Select the 60.50 dimension. 5. Type [90.5] as the new dimension.

Modify this dimension

Figure 18: Crank2 Drawing

6. Click Regenerate from the DRAWING menu. 7. Click Model from the REGENERATE menu. 8. Save the drawing model. Click File > Save and press .


P a g e 2- 2 1

NOTES

9. Click File > Close Window . 10. Click Windows > Activate . This activates the assembly window. Notice that the crank is updated in the assembly. This shows the associativity between the part drawing and the assembly. Task 2. Check for interference between the solid models of the assembly. 1. Click Analysis > Model Analysis. The MODEL ANALYSIS dialog box appears, as shown in the following figure.

Figure 19: Analyzing Global Interference 2. The default type is set to Assembly Mass Properties. Select Global Interference from the TYPE drop-down list.



NOTES

3. Accept defaults and click Compute . 4. In the RESULTS window, the system indicates that two parts are interfering. Use the arrow to toggle between the interfering part models. This also highlights the volume of interference on the screen. 5. Close the dialog box. 6. Click name. Task 3.

to save the ASSEMBLY model. Accept the default

Determine the results of closing the master assembly window.

1. Click Window > Close . Notice the BASE Pro/ENGINEER window cannot be removed as indicated in the message area. 2. Open CRANK2.PRT, which is still in the memory. In the FILE OPEN dialog box, click

[In Session].

Figure 20: Using the IN SESSION Option


P a g e 2- 2 3

NOTES

3. Select CRANK2. PRT. Click O p e n. The system retrieves this model from the system memory, not from the computer hard drive. Task 4. Remove the master assembly models that are not displayed in a window from the session memory. 1. Erase the models that are not displayed. Click File > Erase > Not Displayed. 2. A dialog box appears with all the selected models that are in session highlighted. Click OK to complete the operation. Task 5. Retrieve “in-session” models again to determine which ones remain in session. 1. Click

. Click

. Note that only CRANK2.PRT is listed.

2. Click Cancel . Task 6.

Erase the crank model from system memory to conserve RAM.

1. Erase the current file. Click File > Erase > Current . Confirm the operation.



NOTES

MODULE SUMMARY In this module you have learned that: •

Pull-down menus, toolbars, the display area, and the message area are the four important elements of the Pro/ENGINEER user interface.

•

Models can be oriented and displayed on the screen in various ways.

•

Pro/ENGINEER models such as parts, assemblies, and drawings exhibit feature-based, parametric, and associative characteristics.

•

Pro/ENGINEER automatically opens a new main window each time you open an additional model, so that you can work with multiple windows.

•

Erasing models that are not in use will free up the system memory.


P a g e 2- 2 5


Module

3


Pick-and-Place Features Certain Pro/ENGINEER features need not be built with great effort. They are freely provided and can simply be utilized whenever needed. These features are called Pick-and-Place features.


Identify and define the different types of Pick-and-Place features.

•

Create, delete, and modify the three Pick-and-Place features.

•

Navigate among the various options of the HOLE dialog box to capture the intent of the hole element in the lab practical.

Page 3-1

NOTES

DEFINING PICK-AND-PLACE FEATURES The Pick-and-Place features discussed in this module are: •

Shell

•

Edge chamfer

•

Edge round

•

Hole

Generic Method of Creation To create any of these Pick-and-Place features, you specify the appropriate placement references on your model and provide the required dimensions. Pro/ENGINEER places the feature on that location.

Note: Pick-and-Place features behave parametrically with respect to their placement references. That is, if the placement reference moves, the feature also moves.

Choosing Hidden References Using Query Select When you click Query Select and then select on a surface, a dialog box appears with various reference options.

Shell Features The Shell option removes a surface or surfaces from a solid and hollows out the inside of the solid, leaving a shell of a specified wall thickness.

Figure 1: The Shell Feature



NOTES

When Pro/ENGINEER makes a shell, all the features that were added to the solid before you chose the Shell option are hollowed out. Therefore, the order of feature creation is very important when considering the shell feature.

Creating Edge Chamfers An edge chamfer feature removes a flat section of material from a selected edge or edges to create a beveled surface between the two original surfaces common to the edges. The Pro/ENGINEER dimensioning schemes for edge chamfers are shown in the following figure.

Figure 2: Edge Chamfer Dimensioning Schemes

Note: When selecting circular edges for chamfers, Pro/ENGINEER only highlights one half of the edge. Since the system places the chamfer on the entire circular edge, you do not have to select the other half of the edge.

Creating Simple Rounds Round features create a rounded smooth transition between two adjacent surfaces. An edge round smoothes the hard edges between adjacent surfaces.

For University Use Only - Commercial Use Prohibited Pick-and-Place Features

P a g e 3- 3

NOTES

Pro/ENGINEER offers two types of rounds: simple and advanced. Simple rounds employ the default round shape and transitions. Advanced rounds employ user-defined round shapes and transitions.

Radius Options for Simple Edge Chain Rounds •

Constant

•

Variable

– Assigns the same radius value to every selected edge.

– Specifies radii at every selected edge at the endpoints and, optionally, at intermediate vertices along the edge being rounded.

Figure 3: Constant and Variable Radius Rounds

•

Full Round

– Creates a round that completely removes a model

surface.

Full Round

Figure 4: Full Round

Note: Do not dimension other features to the edges or tangent edges of round features. Round features make unstable parents.



NOTES

Tip: You should create round features on your model as late in the design process as possible.

Figure 5: Cut Feature Dimensioned to the Edge Round

Specifying Radius Values for Simple Rounds •

Enter

•

Select On Surf

•

Thru Pnt/Vtx

•

Default Values –

– (default) Specifies a new radius value that does not appear in the menu. Use the key to select other radius type options. – Specifies a point on the adjacent surface that determines the radius value. – Specifies a datum point, vertex, curve, or edge end through which the radius of the round should pass. Specifies a radius value as the system default value or a previously entered radius value in the SEL VALUE menu. Select on this surface.

Round created tangent

Original model

Figure 6: Using the Select On Surf Option


P a g e 3- 5

NOTES

Select this vertex.

Original Model

Figure 7: Using the Thru Pnt/Vtx Option

Hole Features There are three types of Holes: •

Straight Holes

•

Standard Holes

•

Sketched Holes

This module primarily deals with the Straight Hole feature and its many options.

Creating the Straight Hole Feature Pro/ENGINEER creates all straight holes with a constant diameter. The hole feature always removes material from your model.

Placement Options To place a hole on your model, you can choose from the following options in the PLACEMENT menu. •

– Places the hole on a plane. Dimensions the center of the hole from two surfaces or edges using linear dimensions. Linear



NOTES

Figure 8: Linear Hole

•

– Places the hole with respect to an axis using polar dimensions on a plane, cylinder, or cone. Radial holes placed on a plane have a diameter, radius, or linear dimensioning scheme. Radial

Figure 9: Radial Holes on a Plane

•

– Places the hole co-axially using an existing axis. Does not create placement dimensions, but creates only a diameter dimension for the hole itself. Coaxial

Figure 10: Coaxial Hole


P a g e 3- 7

NOTES

•

– Places the center of the hole directly on an on surface datum point. The axis of the hole is normal to the placement surface. On Point

Figure 11: On Point Hole

Depth Options You can also create the hole from either side of the placement plane or from both sides using the Depth One and Depth Two options in the HOLE dialog box.

Figure 12: Side Options

The system determines how deep to create the hole based on your depth specification. The following figure illustrates the various depth options listed in the HOLE dialog box.



NOTES

Thru All

Variable

To Reference

Thru Next Thru Until

Figure 13: Hole Depth Options


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NOTES

LABORATORY PRACTICAL Goal In this laboratory, you will learn how to create and implement the important Pick-and-Place features.

Method In Exercise 1, you add a shell feature and a simple tangent chain round feature to a base model by using the automatic round creation functionality. In Exercise 2, you add chamfers and rounds to a model. In Exercise 3, you explore the straight hole feature and its many options. In Exercise 4, you create a straight radial hole placed on a planar surface.

Tools Table 1: Icons for Pick-and-Place Features

Icons

Description Shading Hidden line display Repeat feature Select geometric entities



NOTES

EXERCISE 1: Shell and Automatic Round Features

Figure 14: The Start Model

Task 1.

Create a shell feature.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 03_pick_place. 3. Retrieve the AUTOMATIC.PRT from the working directory. 4. Click Insert > Shell . 5. Select the front surface of the part as shown in the following figure.

Select the front surface

Figure 15: Selecting the Shell Reference

6. After the surface has been selected, click Done Sel > Done Refs.


P a g e 3- 1 1

NOTES

7. Enter [0.25] as the shell thickness and press . 8. Click OK from the SHELL dialog box to complete the shell feature.

Figure 16: Completed Shell

Task 2.

Add an automatic round feature using the right mouse button.

1. Click [Select geometry] and select the outer arc-shaped edge as pointed out in the following figure. 2. Click

> Round Edges from

the pop-up menu.

Select the outer arc-shaped edge

Figure 17: Selecting the Round Edges

3. Click on the green icons on the round feature and drag it dynamically to modify the size of the round. Click the left mouse button anywhere on the screen to complete the round creation. 4. Notice that the system automatically selected the edges that were tangent to the arc-shaped edge to create the simple round feature.



NOTES

Tangent edges were selected automatically as round references.

Figure 18: Completed Round

5. Click File > Save . Accept the default name and press to save the model. 6. Click File > Close Window to close the current working window. 7. Erase all objects from memory. Click File > Erase > Not Displayed. Click OK .


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NOTES

EXERCISE 2: Creating Chamfers and Rounds


Task 1.

Adding the 45 x d edge chamfer to a cylinder.

1. Retrieve the CHAMFERS.PRT from the working directory. 2. Click Insert > Chamfer > Edge Chamfer. 3. Click 45 x d from the SCHEME menu. 4. Type [1.0] as the value for the chamfer dimension. 5. Select the two circular edges on either end of the cylindrical protrusion as shown in the following figure. Selecting the edges highlights them in blue.



NOTES

Select these two circular edges

Figure 20: Selecting the Circular Edges

6. Click Done Sel > Done Refs. 7. Click OK to complete the chamfer.

Figure 21: The Edge Chamfer Dialog Box

8. The completed chamfer is shown in the following figure.


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NOTES

Figure 22: Completed Chamfer

Task 2. model.

Add the d1 X d2 chamfer to the four edges at the bottom of the

1. Click Insert > Chamfer > Edge Chamfer. 2. Select d1 x d2 from the SCHEME menu. Type [1] as the value for d1 and [2] as the value for the d2 dimension. 3. Switch to a H i d d e n Line view by clicking Pro/ENGINEER toolbar.

[Hidden line] in the

4. Click Query Sel , then select the hidden bottom surface as the reference surface for the d1 dimension.

Select the hidden bottom surface.

Figure 23: Selecting the Bottom Surface

5. Select the front edge and right side edge as edge references. 6. Click Query Sel , then select the two hidden bottom edges.



NOTES

Note: Make sure to click Accept from the query bin after picking each edge when using Query Sel.

Select these two hidden bottom edges.

Select front and right side edges

Figure 24: Selecting the Hidden Edges

7. Click Done Sel > Done Refs. 8. Click OK to complete the chamfer. 9. Click

[Shading] to see the shaded model.

Figure 25: Completed Chamfer


P a g e 3- 1 7

NOTES

Task 3.

Create a simple round with a variable radius value.

Figure 26: Simple Edge Round with Variable Radius

1. Click Insert >Round > Simple > Done . 2. Click Variable > Edge Chain > Done . 3. Switch to the hidden line display by clicking

[Hidden line]

4. Click One By One in the CHAIN menu to define the single edge references one by one. 5. Select the three visible vertical edges of the base and the invisible edge as shown in the following figure.



NOTES

Select the fourth (hidden) edge here.

Select these three edges

Figure 27: Selecting the Variable Round References

6. To select the hidden vertical edge, click Query Sel and click Accept in the Query bin. 7. The system highlights eight vertices. 8. Click Done in the CHAIN menu. 9. The system now highlights eight vertices. Click Done once again. Task 4. Define radius values for the variable edge round, keeping track of the vertices that Pro/ENGINEER highlights. 1. As the system highlights each end of every edge in green, type [0] as a value for the top of the edge; type [2] as a value for the bottom of the edge. Repeat for all four edges. 2. Click OK to complete the round feature. 3. Click

[Shading].


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NOTES

Figure 28: Completed Round

4. Click File > Close Window . 5. Click File > Erase > Not Displayed. Click OK .



NOTES

EXERCISE 3: Exploring the Straight Hole Feature Four cooling fins Base feature

270-degree flange Fluid pipe


Task 1. Create a linear placed hole with a variable depth of 30 on the top of the base feature of the model shown in the preceding figure. 1. Open STRAIGHT_HOLES.PRT. Change display to Hidden Line from the toolbar. 2. Click Insert > Hole . The HOLE dialog box appears, shown in the following figure.


P a g e 3- 2 1

NOTES

Figure 30: Hole Dialog Box

3. Leave the default hole type as Straight . 4. Type [7.5] as the diameter value . Press . 5. Leave the depth one default as Variable and depth two as None . 6.

Type [30] as the depth value . Press .

7. The Primary Reference defines hole location. Click the top surface of the base feature as the placement plane as shown in the following figure.



NOTES

First dimension reference (hidden side surface)

Placement plane for Primary Reference

Second dimension reference

Figure 31: Creating a Linear Placed Hole

8. For the first linear reference, click Query Sel to select the hidden side of the base feature. Type [10] as the distance for this reference. Press . 9. For the second linear reference again click Query Sel once again and select the visible front surface. Type [15] for the distance from this reference. Press . 10. Click

.

Figure 32: The First Completed Hole


P a g e 3- 2 3

NOTES

Task 2.

Add a linear hole that runs through the cooling fins.

1. Click Insert> Hole . 2. In the HOLE dialog box, leave the default hole type as Straight . 3. Type [12.5] for the hole diameter. Press . 4. Click Thru All as the DEPTH ONE option and None as DEPTH TWO. 5. Select the top surface of the first cooling fin near the right back corner as the placement plane, as shown in the following figure.

First dimension reference (hidden back surface)

Second dimension reference (visible thin surface of fin) Placement plane

Figure 33: Creating the Second Straight Hole Feature

6. For the first linear reference, click Query Sel and then select the hidden back surface of the base feature. 7. Type [10] as the distance for this reference. Then press . 8. For the second reference, click Query Sel and select the side surface (not the edge) of the top cooling fin. If selecting the side surface of the fin is difficult zoom in the model. 9. Type [10] for the distance for the second reference. Then press . 10. You may preview the hole feature but do not close the HOLE dialog box.



NOTES

Note: You will be creating another hole feature. You may use the repeat button

in the HOLE dialog box.

Figure 34: The Second Hole Placed

Task 3. Use the TO REFERENCE depth option to create another linear hole through the top three fins. 1. In the HOLE dialog box, leave the default Straight hole type. Type [12.5] as the diameter. Press . 2. Click To Reference in the Depth One option dropdown menu. 3. Click Query Sel , then select the bottom surface of the third fin. By this, you are specifying that the hole has to end at the bottom surface of the third fin.


P a g e 3- 2 5

NOTES

Select the hidden underside surface

Figure 35: The To Reference Hole 4. For the Primary Reference, select the top surface of the first fin as shown in the following figure. Select this surface as the placement plane Second dimensional reference

First dimensional reference

Figure 36: Creating the Third Hole

5. For the first Linear Reference, select the front part of the base feature and type [10] for the distance. Press . 6. For the second Linear Reference, select the visible side surface of the cooling fin. Type [10] for the distance. 7. Complete hole feature.



NOTES

Task 4.

Create a coaxial hole to the cylindrical feature.

1. Click Insert > Hole 2. In the HOLE dialog box, leave the default hole type as Straight . 3. Type [5] as a value for the hole diameter.

Axis line (A_3)

Depth surface to extrude up to Select here for the placement pl ne

Figure 37: Creating a Coaxial Straight Hole 4. Make Depth One to be a To Reference . Click Query Sel and select the visible front surface of the base feature as shown in the preceding figure. 5. Select the front surface of the cylindrical protrusion as the primary reference. 6. Select Coaxial from the PLACEMENT TYPE drop-down list. 7. Select the A_3 axis of the cylindrical protrusion as the axial reference. If you cannot see the axis, turn it on by clicking [Datum axes on/off]. 8. Click

to complete the coaxial hole feature.


P a g e 3- 2 7

NOTES

Figure 38: The Completed Co-Axial Hole Feature



NOTES

EXERCISE 4: Challenge Exercise Task 1.

Create a straight radial hole placed on a planar surface.

Figure 39: The Completed Model

1. Set the hole specifications. Diameter = 15mm Depth One = To Reference Depth Two = None Depth Reference = Invisible surface of the circular flange as shown in the next figure. 2. Set the hole placement. Primary Reference = Visible front surface of the circular flange Placement Type = Radial Axial Reference = A_3 of the fluid pipe Distance = 25 mm Angular Reference = Front face of the flange near the angled cut.


P a g e 3- 2 9



4 Sketcher Basics In this module you learn how to sketch and define complex parts. You also learn how to use Pro/ENGINEER in Sketcher mode, and how to take advantage of the Intent Manager to improve your designs.


Start a design in Sketcher.

•

Create various types of geometry.

•

Constrain sketched entities.

•

Modify section sketches.

P a ge 4-1

NOTES

THE SKETCHER INTERFACE The Sketcher interface consists of: •

A menu bar with pull-down menus that include Sketcher-specific menus EDIT and SKETCH.

•

A standard Pro/ENGINEER toolbar.

•

An additional Sketcher toolbar with Sketcher-specific options.

•

A message area below the toolbars.

•

An INTENT MANAGER with fly-out icons on the right to perform frequently used actions.

•

An additional Sketcher-specific message area at the bottom left of the window describing INTENT MANAGER’s fly-out icons.

Figure 1: Sketcher Interface



NOTES

Selecting Sketched Entities Using the mouse, you can select individual or multiple-specific sketched entities, or all entities that fall within a swept box. Selected entities highlight in red.

The Intent Manager The INTENT MANAGER appears automatically on the right side of the screen when you enter the Sketcher mode. It includes fly-out icons which are logically grouped together based on capability. These icons provide access to the most frequently used sketching tools.

Default cursor to pick entities

Icons to create different kinds of geometry

To create dimensions To modify dimensions To impose constraints To trim Entities

Figure 2: INTENT MANAGER Flyout Icons

Accessing Commands with Pop-Up Menus You access Pop-up menus by right-clicking in the SKETCHER display area. These menus offer short-cuts for sketching, modifying, dimensioning, deleting, and undoing steps.

For University Use Only - Commercial Use Prohibited Sketcher Basics

P a g e 4- 3

NOTES

Figure 3: A Typical Sketcher Pop-Up Menu

THE SKETCHER MODE Accessing Commands with Sketcher Menus EDIT and SKETCH are top-level menus specific to the SKETCHER mode.

They contain all the commands needed in the sketching environment.

Figure 4: Edit Menu

The INTENT MANAGER commands and the T e x t option are also available in the SKETCH menu.



NOTES

Figure 5: Sketch Menu

Specifying References In the SKETCHER mode you specify the references of the section when you: •

Create a new feature.

•

Redefine a feature with missing or insufficient references.

•

Provide references to place a section.

It is good practice to reference before sketching. This provides the sketched entities a location to automatically align to and dimension from.

Note: The references that you select for a section create Parent/Child relationships.


P a g e 4- 5

NOTES

Creating Geometry SKETCHER mode enables the creation of geometrical shapes and entities.

The basic ones—lines, arcs, and circles—are discussed below. •

Lines –

Using the Line fly-out icons in the INTENT MANAGER, you create two types of sketched lines: Straight lines from point to point. Centerlines for referencing or constraining entities.

Figure 6: Lines Fly-Out Icons

•

– Using the Arcs fly-out icons in the INTENT MANAGER, you create four types of arcs: Arcs

An arc by 3 points or tangent to an entity at its endpoint. A concentric arc. An arc by selecting its center and endpoints. A conic arc.

Figure 7: Arcs Fly-Out Icons

•

Circles –

Using the Circle fly-out icons in the INTENT MANAGER, you can create three types of circles: A circle by selecting the center and a point on the circle. A concentric circle. A full ellipse.

Figure 8: Circle Fly-Out Icons



NOTES

Sketched circle

Concentric to this edge

Figure 9: Sketching a Concentric Circle to an Edge

Dimensioning Sketches Once a sketch is complete, you dimension it. An orderly arrangement of dimensions helps visual clarity, particularly when the sketch gets complex. To place dimensions in SKETCHER, you left-click to select the entity and middle-click to place the dimension. You can place a dimension at any point during or after sketching. The following figure illustrates the simple dimensioning of a rectangle.

Figure 10: Creating Dimensions for a Rectangle


P a g e 4- 7

NOTES

Figure 11: Grabbing and Moving Dimensions

Modifying Dimensions You can modify the dimensions values of a sketch in the MODIFY DIMENSIONS dialog box. You also have the options to Regenerate and Lock Scale the sketch. You can also double-click on a specific dimension in a sketch to dynamically change the value of the dimension. The SENSITIVITY scrollbar allows you to adjust the sensitivity of the control wheels when changing dimensions dynamically.

Figure 12: Modify Dimensions Dialog Box



NOTES

Adding Constraints Sketcher applies system default constraints to a sketch to establish the initial design intent. You can override the default constraints from the CONSTRAINTS dialog box.

Figure 13: Sketcher Constraints Dialog Box

You can use the constraint options to: 1. Make a line or two vertices vertical. 2. Make two entities tangent. 3. Make two points or vertices symmetrical about a centerline. 4. Make a line or two vertices horizontal. 5. Place a point on the middle of the line. 6. Create equal lengths, equal radii, or same curvature constraint. 7. Make two entities perpendicular. 8. Creates same points or points on entities. 9. Make two lines parallel.

Other Sketcher Tools Edge The Edge tool has two instances represented by its two fly-out icons in the Intent Manager, as shown below:


P a g e 4- 9

NOTES

Figure 14 Edge Fly-Out Icons

•

– Uses an existing model edge to create sketched entities. Automatically selects the edge as a specified reference. Use Edge

Figure 15: Using Existing Model Edge to Create Sketched Entities

•

– Uses existing model edge to create sketched entities at an offset distance. Offset Edge

Figure 16: Creating Sketched Entities at an Offset Distance

Note: The Use Edge and Offset Edge options create parent/child relationships with the referenced feature.

Copy The Edit > Copy option copies 2-D drafts and imports entities from a drawing. You can move and scale a section, making legacy data easier to manipulate.



NOTES

Mirror You can mirror sketched entities from one side of a centerline to the other using the Edit > Mirror option.

Move The MOVE ENTITY menu displays the following options: •

Drag Item

•

Drag Many

•

Rotate90

•

Dimension

– Moves an entity or its vertex to a new location. – Translates selected entities within a sketch.

– Rotates sketched entities about a specified point by multiples of 90 degrees. – Repositions a dimension within a sketch.

Trim The Edit > Trim option shortens or extends an entity in three different ways corresponding to the three fly-out icons shown below:

Figure 17: Trim Fly-Out Icons

•

The first dynamically trims section entities

•

The second cuts or extends entities to other entities or geometry.

•

The third divides an entity at the point of selection, replacing the original with two new entities.

Replace Replaces a sketched entity from the original section with a newly sketched entity.

Section Analysis The Analysis > Section Analysis option provides you with information about: •

Intersection and tangency points.

•

Angles and distances.

•

Dimensioning references.


P a g e 4- 1 1

NOTES

•

Entity curvature display.

Sketcher Points Sketcher points force coincidence among sketched entities and allow slanted dimensions between sketched entity end-points.

Figure 18: Midpoint Definition Using Sketcher Point

Figure 19 Defining Theoretical Sharps Using Sketcher Points



NOTES

Setting Sketcher Preferences The SKETCHER PREFERENCES dialog box in the UTILITIES menu modifies the Sketcher environment.

Figure 20 Sketcher Preferences Dialog Box

Use the SKETCHER PREFERENCES dialog box to: •

Modify the display options of various sketcher entities.

•

Set constraints preferences by enabling or disabling constraints assumed by Sketcher.

•

Set grid, grid spacing, and accuracy parameters.

•

Click the Default button to reset the preferences.

Sketching in 3-Dimensions (3-D) When you select the Use2D Sketcher option from the ENVIRONMENT dialog box, Sketcher starts in a 2-D orientation (that is, with the sketching plane parallel to the computer screen). When you do not select this option, the Sketcher starts in a 3-D orientation. You can change the view orientation at any time and sketch in


P a g e 4- 1 3

NOTES

3-D. Using View > Sketch View , you can re-orient a Sketcher section into the 2-D view while in Sketcher mode.

Figure 21: The Environment Dialog Box

TAKING ADVANTAGE OF SKETCHER MODE Your work sessions will be more productive if you apply the following rules when working with Sketcher:



NOTES

1. Keep sketches simple.

This makes the final model flexible and helps regeneration. 2. Use the Undo option

The Undo option restores a sketched section to its prior state. This is extremely useful when sketching features incrementally. 3. Do not sketch to scale.

Concentrate on getting your geometry straight by sketching large. Resolve the sketch by modifying dimensions. This rule is particularly helpful when the sketched entities are small. 4. Use the grid. Create lines equal, parallel, or perpendicular. Align sketched entities. Align centers horizontally and vertically. 5. Do not extend the sketch outside of the part. There is no need to sketch sections that extend outside the part, as is required with some solid modeling packages. 6. Make effective use of Sketcher's accuracy.

The range for the accuracy is 1.0 e-9 through 1.0 (default). To prevent Sketcher from making constraints, you can increase Sketcher accuracy by changing it from 1.0 to a lower number. 7. Use open and closed sections appropriately. When sketching an open section, you cannot have more than one open section per feature. If you use an open section, you must explicitly align its open ends to the part. When in doubt over whether you should use an open or closed section, you should use a closed one since it is easier to regenerate, and is less prone to failure.


P a g e 4- 1 5

NOTES

Protrusion A

Protrusion B

Cut

Figure 22: Open and Closed Sections



NOTES

LABORATORY PRACTICAL Goal In this laboratory you practice the basic sketching procedures such as entering sketcher mode, creating straight lines, creating arcs, applying constraints, dimensioning, and generating solid models.

Method In Exercise 1, you practice basic sketching procedures. In Exercise 2, you create a snap ring by sketching in steps. In Exercise 3, you create a hex section using construction entities.

Tools Table 1: Sketcher Basic Tools

Icons

Description Impose sketcher constraints Perpendicular constraint Tangent arc Create circle Create rectangle Create dimension Dynamic trim Modify dimension


P a g e 4- 1 7

NOTES

EXERCISE 1: Sketching Basics

Figure 23 Completed Sketch after Exercise 1

Task 1.

Create a new sketch named ROUND_RECTANGLE.

1. Click

[File new] in the toolbar.

2. In the NEW dialog box, select Sketch . 3. Type [ROUND_RECTANGLE ] for the name and click OK . 4. Sketcher mode activates. Task 2. Sketch four lines with a horizontal bottom line, as shown in the following figure.

1. Click 2. Click

[Sketch line] and place by clicking

.

to end line creation.



NOTES

Figure 24: Sketching a Quadrilateral

Task 3.

Apply the constraint to make the lines perpendicular.

1. Click [Impose sketcher constraints], then click [Perpendicular constraint], then select two lines to make them perpendicular, as shown in the following figure.

Figure 25: Perpendicular Constraint on One Side

2. Select the other two lines to make them perpendicular.


P a g e 4- 1 9

NOTES

Figure 26: Perpendicular Constraint on the Other Side

3. Close the CONSTRAINTS dialog box. Task 4.

Delete the two vertical lines.

1. Click the P o i n t e r icon, and select the left vertical line. 2. Press and hold and select the right vertical line. 3. Right-click and select Delete from the pop-up menu. Task 5.

Sketch a tangent end arc on the left side of the section.

1. Click

[Tangent arc ].

2. Select and drag the top left vertex out of the left quadrant of the circle to get a tangent end arc. 3. Select the end point to be the bottom left end point, as shown in the following figure.



NOTES

Figure 27 Sketching a Tangent End Arc

Task 6.

Repeat the process on the right side of the section.

Figure 28 Sketching Tangent End Arcs on Both Sides

Task 7.

Add the proper dimensions.

1. Click

[Create dimension].

2. Select each arc, then middle-click to place the dimension. 3. Select Tangent > Accept and Horizontal > Accept for type and orientation.


P a g e 4- 2 1

NOTES

Figure 29 Dimensioning the Arcs

Task 8.

Create a diameter dimension on the left arc.

1. Select twice the left arc, and then

to place it.

Figure 30 Dimensioning the Left Arc

Task 9.

Modify both dimensions.

1. Click

and select the horizontal and the diameter dimensions.

Press and hold and click

[Modify dimension].

2. Modify the diameter to [2 ] and the linear dim to [4].



NOTES

Figure 31: Modify Dimensions Dialog Box

3. Click

to complete the feature.

4. Save and close the MODIFY DIMENSIONS dialog box.

Figure 32: Sketch with Modified Dimensions


P a g e 4- 2 3

NOTES

EXERCISE 2: Sketching in Steps

Figure 33 Completed Snap Ring after Exercise 2

Task 1.

Create a new sketch called SNAP_RING.

1. Click

.

2. Select Sketch . 3. Type [SNAP_RING] as the name of the sketch. Task 2.

Create two offset circles aligned horizontally.

1. Click [Create circle] and draw two circles, as shown in the following figure.



NOTES

Figure 34 Two Offset Circles Aligned Horizontally

Task 3. Create a rectangle that snaps to the inside circle on both upper vertices. 1. Click [Create rectangle]. Click in the Sketcher to start the sketch, and then click again to end the sketch. 2. Then use the dynamic trim to create intersections. Click [Dynamic trim]. Drag from below the bottom horizontal line and to above the top horizontal line, as shown in the following figure.


P a g e 4- 2 5

NOTES

Stop cursor here

Delete

Start dynamic trim here

Figure 35 Sketching a Rectangle Inside Circles 3. Highlight each item. If all the crossed items are not highlighted, continue to drag over the lines until they do highlight. 4. The result is shown in the following figure.

Figure 36 Using Dynamic Trim



NOTES

5. The results of trimming are shown in the following figure.

Figure 37: Section after Trimming

Task 4.

Sketch another rectangle.

1. Snap to the outside circle and the bottom of the two vertical lines, as shown in the following figure. Do not snap through any of the arc's vertices.


P a g e 4- 2 7

NOTES

Figure 38: Sketching a Second Rectangle

Task 5.

Use the dynamic trim to remove the final lines and arc.

1. Click 2.

to trim the unwanted entities.

The result is shown in the following figure.



NOTES

Figure 39: Capturing Intent with Dynamic Trim

Task 6.

Dimension the entities.

1. Click

to create the dimensions.

2. Select each entity, and then middle-click to place the dimensions. Refer to the preceding figure to determine the dimensioning scheme (the format of the dimensions and not the actual value) required for capturing design intent. 3. Click

to modify the six dimension values.


P a g e 4- 2 9

NOTES

Figure 40: Modifying Dimensions

4. Save and close.



NOTES

EXERCISE 3: Sketching a Hexagon Task 1.

Create a new sketch called HEX.

1. Click Task 2.

. Select Sketch and type [HEX] as the name.

Create a sketcher point

1. Click the point button

.

2. Place a point in the center of the screen. Task 3.

Add vertical centerlines passing through the sketcher point.

1. Click the centerline button

.

2. Create a vertical centerline that passes through the point. 3. Create two additional centerlines that pass through the point at an angle. Task 4.

Modify the angles to 60°.

1. Modify the angle between centerlines to 60°, as shown in the following figure.

Figure 41: Modifying Angles between Centerlines


P a g e 4- 3 1

NOTES

Task 5.

Create a circle centered on the Sketcher point.

1. Click 2.

to draw a circle.

and select Toggle Construction to convert it to a construction circle.

Figure 42: Creating a Construction Circle

Task 6. Create a hexagon by sketching 6 lines from the intersection points of the circle and the centerlines.

Figure 43: Creating a Hexagonal Sketch



NOTES

1. Add a diameter dimension to the construction circle and modify it's value to [1.0] 2. Click File > Close Window . 3. Click File > Erase > Not Displayed. Click OK .


P a g e 4- 3 3

NOTES

MODULE SUMMARY In this module, you learned that: •

The Sketcher interface consists of the main sketcher area, pull-down menus, toolbars, message areas, the INTENT MANAGER with fly-out icons and pop-up menus.

•

Sketched geometry must be dimensioned and constrained.

•

You can create lines, arcs, circles, rectangles, splines, and many other geometrical entities using the Intent Manager.

•

The EDIT and SKETCH menus contain most of the tools that are unique to Sketcher mode such as Copy , Mirror , Move , and Trim .

•

Default dimensions can be modified at any stage of model generation.

•

The system notifies you when a model has conflicting constraints.

•

Sketcher preferences can be set using the SKETCHER PREFERENCES dialog box.




5 Sketched Features In this module you learn how to create sketched features by defining their size, shape, and location in a model.


Sketch cuts and protrusions.

•

Created extruded and revolved forms.

•

Set up sketching planes.

•

Dimension sketched features.

Page 5-1

NOTES

DEFINING SKETCHED FEATURES Sketching Cuts and Protrusions •

Protrusion

•

Cut

– adds material to a model in any desired shape.

– removes material from an open or closed cross-section in a model.

Figure 1: Protrusion versus Cut

Created Extruded and Revolved Forms •

Extrude

•

Revolve

– adds or removes material linearly from the sketching plane.

–creates a feature by revolving the sketched section around a sketched centerline.



NOTES

Sketched centerline

Figure 2: Extruded versus Revolved Features

Selecting a Sketching Plane To create a new feature on a model, begin the sketch on the surface where you intend to place the feature. The surface you choose defines the sketching plane.

Selecting a Reference Plane Once you create and dimension the sketch, then you orient the new feature to a reference plane. The reference plane must be perpendicular to the sketching plane.

Changing the Default Reference Plane You can change the default orientation and manually select a new reference plane. The default orientation of the sketching plane orients it parallel to the screen and chooses one of the default datums as a reference plane. For example, you may want to manually select the top surface of the model for a perpendicular reference orientation.

For University Use Only - Commercial Use Prohibited Sketched Features

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NOTES

Top orientation plane

Direction of feature creation

Sketching plane

Sketcher Orientation -- Protrusion

Resulting Protrusion

Sketcher Orientation -- Cut

Resulting Cut

Figure 3: Two Features Defined by the Same Cross-section



NOTES

USING THE SKETCHER TOOLS Whenever you create a sketch, Pro/ENGINEER automatically assumes a dimensioning scheme. Since all sketches are parametric, you can create them in a convenient scale and later modify their dimensions. In SKETCHER main window toolbar, the Sketch option pull-down menu contains all the necessary sketching tools. Another additional toolbar containing the sketching options and constraints appears on the right side of the SKETCHER window.

Dimensioning Sections To override weak dimensions with strong ones, you select the entity, then middle-click [

] to place the dimension at the desired location.

Completes or aborts geometry creation

Creates section entities by selecting points

Opens pop-up menu

Figure 4: Sketcher Mouse Button Functions


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NOTES

Linear Dimensions Linear dimensions indicate the length of a line segment or the distance between two entities. The different types of linear dimensions are illustrated in the following figure.

Figure 5: Linear Dimensions in Sketcher Mode

Note: You cannot dimension the length of a centerline.



NOTES

Diameter Dimensions Diameter dimensions measure the diameters of sketched circles and arcs. To create a diameter dimension, select the arc or circle twice and place the dimension. Select twice on the circle

to

Place the dimension

Figure 6: Diameter Dimension on Circle

To create a diameter dimension for a revolved section, Select the entity to dimension and the centerline to use as the axis of revolution. Then select the entity again and place the dimension. Finally, place the diameter dimension.

Second, select the sketched centerline

Third, select the sketched entity once again. First, select the sketched entity

Figure 7: Diameter Dimension for Revolved Section in Sketcher Mode


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NOTES

Note: The diameter dimension for a revolved feature extends beyond the centerline, indicating that it is a diameter dimension rather than a radius dimension.

Radial Dimensions Radial dimensions measure the radii of circles or arcs. To create a radial dimension, select the circle or arc and place the dimension.

Select on the ARC (left)

Place dimension (middle)

Figure 8: Radial Dimension in Sketcher Mode



NOTES

Angular Dimensions Create an angular dimension between lines by selecting two lines. to place the dimension. Where you place the dimension determines how the system measures the angle.

Select the two lines in any order.

Place dimensions in indicated positions.

Figure 9: Angular Dimensions in Sketcher Mode

To create an arc angle dimension, select one endpoint, then the other endpoint, and finally the arc.

to place the dimension.

Select 1 - endpoint Select 2 -endpoint

Select 3 - on arc

Place dimension

Figure 10: Arc Angle Dimension in Sketcher Mode


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NOTES

LABORATORY PRACTICAL Goal In this laboratory you add and remove material to a solid part using protrusion and cut features.

Method In Exercise 1, you create a cut feature. In Exercise 2, you create a protrusion.

Tools Table 1: Icons for Sketched Features

Icons

Description Sketch centerline Toggle grid on/off



NOTES

EXERCISE 1: Creating a Cut

Figure 11: Start and Finished Models

Task 1.

Sketch a cut feature within a closed section.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 05_sketch_feat. 3. Open SKETCHED_FEATURES.PRT. 4. Change to Hidden Line display. 5. Click Insert > Cut > Extrude . 6. Click One Side > Done .


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NOTES

Select the top planar surface

Sketching plane

Figure 12: Selecting Sketching Plane Task 2.

Define the front surface as the sketching plane.

1. Leave defaults and Query Sel to select the planar front surface of the block as the plane to sketch the shape of the cut. 2. The feature should extrude into the part. Click O k a y from the DIRECTION menu. Task 3.

Orient the model by selecting the orientation references.

1. Click Top from the SKET VIEW menu. 2. Select the top planar surface to begin the SKETCHER. Note Instead of manually orienting the model, you can usually click Default in the SKET VIEW menu to enter the default sketcher mode.

Task 4. Define the references. The design intent of the cut is to be at a specified distance from the right side and the bottom of the model. 1. Note that Pro/ENGINEER automatically assumes two references. To delete these two references from the REFERENCES dialog box, highlight and click Delete .



NOTES

2. Select the bottom surface and the right side surface as references. Note that the REFERENCE dialog box entries are both SURF:F4 (Protrusion). Click Close .

Select this bottom surface as the first reference (selecting it on edge)

Select this side surface as the second reference

Figure 13: Specifying References

Task 5.

Define the section for the cut.

1. Click

. Select in the Sketcher to start the line and drag it from

left to right. Left-click [ finish the line.

] to end the line. Right-click [

] to

2. Click . Click the right end point of the line as the start point for the arc and drag a 180-degree arc. Click to end the arc creation. Note: If you did not sketch what you wanted, you can undo the operation by selecting Undo.


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NOTES

Figure 14: Creating a 3 Point/ Tangent End Arc

3. From the endpoint of the arc sketch another horizontal line segment. 4. Finally complete the section by sketching another tangent end arc that connects the open end of the second line to open end of the first line.



NOTES

Figure 15: Completing Section Sketch

Task 6.

Make the two horizontal lines equal in length.

1. Impose the Equal Length Sketcher constraint. Click

and

.

2. Select the two horizontal lines you want to make equal. 3. If the sketch is over-constrained, the RESOLVE SKETCH dialog box appears.

Figure 16 Resolve Sketch Dialog Box


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NOTES

4. Retain the Equal Lengths constraint and delete any other constraint. Task 7. Override existing weak dimensions and constraints with your own strong dimensions and constraints. 1. Click . Select a point approximately half way between the two arc centers. When the centerline snaps to vertical, click again. 2. Check for the symmetric constraint symbols—two arrows indicating a symmetric constraint located about the centerline. If INTENT MANAGER added a dimension, click Undo and re-create the centerline. Or, force it using the CONSTRAINT menu. 3. Click

. Create the dimensions of the cut section.

4. To create the radius dimension, select the perimeter of the left arc and


5. To create the arc center-to-center dimension, select the each of the arc centers and


6. To create the location dimension from the right surface to the centerline, select the centerline and then select the right surface and


7. To create the location dimension from the bottom surface to the left arc center, select the arc center and the bottom surface and to place the dimension.



NOTES

Figure 17: Specifying Constraints and Dimensions.

8. Complete dimensioning the size and location of the cut section. Task 8.

Modify the dimensions of the cut.

1. Change the dimension values. Click

. Select a dimension.


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NOTES

Figure 18: MODIFY DIMENSION Dialog Box

2. Type in the correct number and press . 3. Repeat the above step to modify all the other dimensions of the cut.

Figure 19: Modified Dimensions



NOTES

Task 9.

Finish defining the cut.

1. Click

.

2. Click O k a y to accept the arrow pointing towards the inside of the section to define the direction of the cut. 3. To define the depth, click Thru All > Done . 4. Click OK . Note: Note that the system placed a circle with an X in the center of the part to indicate the direction of feature creation. It represents a 2-D arrow perpendicular to the screen in the direction that is into the screen (away from you). A circle with a dot in the center represents a 2-D arrow perpendicular to the screen in the direction that is out of the screen (toward you).

5. View your new cut feature in different views.

Figure 20: Finished Cut


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NOTES

EXERCISE 2: Creating a Protrusion Task 1.

Create a cylindrical protrusion on the right side of the model.

TOP orientation reference Sketching plane

Create this protrusion

Figure 21: The Completed Protrusion

1. Click Insert > Protrusion > Extrude . 2. Click One Side > Done from the ATTRIBUTES menu. 3. Select the right side of the block as the sketching plane. 4. The arrow points outward from the block. Click O k a y from the DIRECTION menu. 5. Click Top and select surface shown in the preceding figure. Task 2.

Specify two references for Sketcher in the DEFAULT view.

1. Click View > Default Orientation . 2. Click block.

[Toggle grid on/off], so that you can clearly see the

3. Delete the two references in the REFERENCE dialog box.



NOTES

4. Select the top surface of the model as reference. and select Query Select from the pop-up menu to select the back hidden surface. 5. Close the REFERENCES dialog box.

Select this top surface as a reference

Select the back surface as a reference

Figure 22: Selecting Section References

6. Click View > Sketch Orientation . Task 3.

Define the section for the protrusion.

1. Click

.

2. Select in the Sketcher to begin a sketch of a small circle. 3. Select again to finish the circle. Task 4.

Strengthen dimensions.

1. Click 2. Select the circle twice and



P a g e 5- 2 1

NOTES

3. Select the center of the circle and the left reference surface. place the dimension.

to

4. Place the dimension between the center of the circle and the left reference surface. Task 5.

Change the dimension values to reflect the design


1. Click and select each of the three dimensions consecutively while holding . 2. Click Edit > Modify . The MODIFY DIMENSIONS dialog box appears. 3. Change dimension values for each as shown in the preceding figure. 4. Click

to close the MODIFY DIMENSIONS dialog box.



NOTES

5. Click Task 6.

in the INTENT MANAGER to complete the section.

Define a blind depth value for the protrusion.

1. Click Blind > Done from the SPEC TO menu. 2. Type [3] in the ENTER DEPTH window and press . 3. Click OK . 4. View your model in different displays. 5. Click File > Save and press . 6. Click File > Erase > Current ; then click Yes from the dialog box.

Figure 24: The Completed Model


P a g e 5- 2 3

NOTES


Cut and Protrusion are two important features that can be sketched using the Sketcher Mode

•

Both of these sketched features can be created in extruded and revolved forms

•

When sketching a new feature, you can always sketch it as convenient and later alter the dimensions

•

In a new sketch, lines, arcs, and circles can be constrained to different properties such as equal lengths, concentricity, perpendicularity, parallelism and symmetry.

•

For a sketched feature, you not only have to dimension it properly but also have to orient it in relation to reference planes (usually the side surfaces of the base feature).




6 Default Datum Templates In this module you learn how to use datum planes to create parts.

Objectives After completing this module you will be able to: •

Describe the purpose of using datum planes as base features.

•

Describe the difference between internal and external datum planes.

•

Start new designs with default or offset datum planes as base features.

•

Align sketched sections to parts.

•

Orient additional datum planes within your model.

Page 6-1

NOTES

USING DATUM PLANES AS BASE FEATURES Base Features A base feature is the first feature that you create when starting a new part. It is the foundation for the rest of the model. Features that are added to the model later depend on the base feature for many or all of their references. The following figure shows an example where a cylinder is used as the base feature for a part.

Figure 1: Base Feature

Defining aDatum Plane A datum plane is an imaginary plane on which you use as a reference for orienting your parts and assemblies. Datum planes are infinite, twodimensional, and perfectly flat. They have no mass or volume. By default, datum planes have two sides: yellow (the active side) and red (the passive side). In the default mode, the system displays datum planes with a yellow side and a text name such as FRONT, TOP , and RIGHT.



NOTES

Using a Default Datum as the Base Feature When creating new models, Pro/ENGINEER automatically provides a default datum plane as the first feature. This is done because datum planes enable you to: •

Develop parent/child relationships between different features.

•

Use planar (flat) surfaces as references, especially useful when designing models that do not have any flat surfaces.

Creating Datum Planes You can create a datum at any time. You can create additional datum planes as reference features for a model where references do not already exist. When creating a datum, you can define it using several different methods. Though methods of creation differ, the Datum Plane constraints are the same: •

Parallel

•

Angle

•

Through

•

Normal

•

Offset

•

Blend Section

•

Tangent

Creating Internal Datum Planes If you do not want datum planes to be a feature of your model, you can create an internal datum, on the fly, when specifying sketching or reference planes. Sometimes, it is beneficial to construct internal datums because the system builds their dimensions into your sketched feature, while displaying the datums only temporarily. Consider the following rules for datum planes created on-the-fly: •

Datum planes created during feature creation are internal to and belong to that feature.

•

Datum planes on-the fly become invisible after you create the feature. Any associated dimensions positioning the datum plane are included with those of the feature. This gives you more choices for varying dimensions when you create a feature pattern.

For University Use Only - Commercial Use Prohibited Default Datum Templates

P a g e 6- 3

NOTES

•

When you use Copy/Mirror to copy features and use datum planes onthe-fly as the mirror plane, this datum plane stays visible because it can be referenced by more than one feature.



NOTES

LABORATORY PRACTICAL Goal In this laboratory you create new part models in Pro/ENGINEER using the default templates.

Method In Exercise 1, you create an extruded and a revolved feature using the default datum planes built into the default template. In Exercise 2, you create a datum plane during the creation of a solid feature to establish good parent-child relationship.

Tools Table 1: Interface Icons

Icons

Description Saved views Draw circle Done section Zoom in Modify dimension Create dimension


P a g e 6- 5

NOTES

EXERCISE 1: Creating a New Part Task 1.

Create a new part model using the default template.

1. Click File > New . Name the part. Type [MOTOR_SHAFT]. Accept the Use default template option and click OK . 2. A default coordinate system and three orthogonal default datum planes, FRONT, RIGHT and TOP, appear with their yellow sides facing you. 3. Click [Saved views]. Notice the list of pre-defined saved views that have been created by using the default template. 4. From the MENU MANAGER click Setup > Units > millimeter Newton Second (mmNs) > Set. Click O K from the WARNING dialog box, then click Close . 5. Click Done to exit from the SETUP menu.

Figure 1: Default Datum Planes and Coordinate System



NOTES

Task 2. feature.

Use the default datums as your sketching reference for the first

1. Select the datum tag FRONT to make it the sketching plane. 2. Click Insert > Protrusion > Extrude . 3. Notice that the system automatically selected the reference plane and placed you in the Sketcher mode. If you want to change the attributes of the protrusion you can always use the Redefine option. 4. Notice that the INTENT MANAGER places references (RIGHT and TOP) for the intended protrusion automatically. Click Close . 5. Click [Draw circle]. Select the intersection of the default datum planes. Drag the diameter out of a circle and place it. The INTENT MANAGER adds a weak diameter dimension. Middleclick to complete the circle creation.

Figure 2: Sketched Circle at Center of Datums


P a g e 6- 7

NOTES

Task 3. Modify the diameter dimension and regenerate the section to see the change. 1. Change the diameter. Double-click the diameter dimension. Type [14.5]. 2. Press . 3. Click . Notice that the system automatically assigns a depth and completes the protrusion. 4. Change the view to the default view. Click Task 4.

and Default.

Modify the depth to 240mm.

1. Click > Dynamic Modify after selecting the protrusion id in the model tree. Notice that you can use the yellow icon in the middle of the protrusion to dynamically modify the depth by dragging. 2. From the PART menu, click Modify > Value and select on the protrusion that you just created. Select the depth value and type [240]. Click Regenerate from the PART menu. Task 5. Add a revolved cut feature to the protrusion you created. As section references, use the default datums. 1. Click Insert > Cut > Revolve . 2. Click One Side > Done . 3. Query Sel the RIGHT datum plane as the sketching plane. Click OKAY to confirm the direction of creation. 4. Select LEFT from the SKET VIEW menu and Query Sel the FRONT datum plane as the reference plane. 5. Now the RIGHT datum plane is the sketching surface.



NOTES

Task 6. In a revolved section you need to use a centerline in the sketch to define an axis of revolution. Create a centerline and proceed to define the section.

1. Click

[Zoom in] and on the left end of the shaft.

2. If the REFERENCES dialog box accidentally closes before you define references. Click Sketch > References to access it 3. Delete the two references that the INTENT MANAGER automatically provides. 4. Select the TOP datum plane as the first reference. Then select the silhouette edge of the protrusion and the left end surface of the protrusion as the second and third references as shown in the following figure.

Select the silhouette edge as the second reference.

Select the end surface as the third

Select the TOP datum plane as the first reference.

Figure 3: Selecting References for the Cut

5. Close the REFERENCES dialog box. 6. Sketch a centerline that coincides with the TOP datum plane. 7. Sketch three line segments.


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NOTES

Figure 4: Sketch for Revolved Cut (dimensions not shown for clarity)

Task 7.

Create the diameter dimension.

1. Click

.

2. In order to get the dimension scheme shown, select the horizontal line you sketched. Select the centerline. Select the horizontal line again. Middle-click to place the dimension.

Figure 5: Creating the Diameter Dimension



NOTES

3. Modify the dimensions of the section. Click dimension] and change the dimensions.

[Modify


Task 8.

Finish defining the revolved cut on the model.

1. Click

.

2. If necessary, flip the arrow to remove material from the inside of the section. Otherwise, click O k a y. 3. Select 360 and click Done in the REVOLVE TO menu. 4. Click OK to finish the feature. 5. Change to the default view. Click View > Default. 6. Save the model. 7. Click File > Erase > Current > Yes.


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NOTES

EXERCISE 2: Creating an Internal Datum Plane In this exercise, you add a protrusion to the model by creating an internal datum plane feature on the fly.

Add this protrusion.

Figure 7: The Start and Finished Models

Task 1. Add a datum plane to the part to use as the sketching reference for the cylindrical protrusion you want to create. 1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 06_templates_datum_planes. 3. Open the part model INTERNAL_DTM.PRT. 4. Click Insert > Protrusion > Extrude . 5. Click One Side > Done in the ATTRIBUTES menu. 6. Click Make Datum > Offset in SETUP PLANE menu. Select the planar front surface of the block as a reference for the new plane.



NOTES

Offset from this front surface

Figure 8: Creating a Sketching Plane

7. In the OFFSET menu, click Enter Value . 8. Type [1] as the offset value. Click Done . Task 2. Finish defining the protrusion by using the datum plane as a sketching plane. 1. Flip the direction of the intended protrusion to point towards the model. Click O k a y to accept the direction of feature creation. 2. Click Top and select the top planar surface of the block as the reference plane. 3. Delete the two default references. Make the A_2 axis of the first cylinder as the first reference. Make the visible vertical surface of the block from which the cylinder protrudes as the second reference. Close the REFERENCES dialog box. 4. Click . Sketch a circle on the cylinder with its center coinciding with the A_2 axis. 5. Modify the dimension of the circle’s diameter to 0.88. 6. Modify the distance from the left vertical surface of the base block feature to 1.5.


P a g e 6- 1 3

NOTES

. Figure 9: Modified Dimensions

7. Click

.

8. Click Thru Next > Done in the SPEC TO menu. 9. Complete the feature. 10. Shade and save the model.

Figure 10: Completed Model



NOTES



P a g e 6- 1 5

NOTES


Datum planes are infinite, two-dimensional, flat references that have no mass or volume.

•

Datum planes act as the ideal base feature to create new parts and models.

•

Additional datum planes can be created in Pro/ENGINEER while creating a model.

•

There are different kinds of datum planes; such as those that are created as Through/Plane, Offset/Plane, Offset/Coord Sys, and Blend Section.

•

You can build internal datum planes when you do not want the datums to be a feature of your model.




7 Parent/Child Relationships In this module you learn how to work with parent/child relationships in Pro/ENGINEER. The order that features are created and the references that they provide creates hierarchical relationships. These parent/child relationships determine feature interaction. You will learn how to manage parent/child relationships to achieve the desired behavior in your models.


Describe parent/child relationships in Pro/ENGINEER.

•

Describe sketched feature parent/child relationships.

•

Describe Pick-and-Place feature parent/child relationships.

•

Change the parents of a feature in a model using the Reroute , Redefine and Reorder options to change the original design intent.

Page 7-1

NOTES

PARENT/CHILD RELATIONSHIPS IN PRO/ENGINEER Solid modeling is a cumulative process where the creation of certain features must, by necessity, precede others. When creating a new feature, Pro/ENGINEER references it to previously defined features for information on size, shape, location, and orientation. This forms the basis for a parent/child relationship. The feature used as the reference becomes the parent to the new feature, the child. Parent/child relationships determine how features react when other features in the model change.

Pick-and-Place Feature Parent/Child Relationships Pick-and-Place features also have parent references because they use existing geometry for location and orientation. Any selection of a surface or edge for this purpose generates a parent/child relationship. The system supplies different options to select a reference, resulting in different parents for the feature. •

Tangent Chain

•

One by One

•

Surf Chain

– specifies a reference only to the selected edge, but developing the feature along all edges that are tangent to the selected one. – specifies a reference for each selected edge.

– specifies a reference to the surface that is selected and a single edge. It also can create references to selected edges if the option From-To is used.

Sketched Feature Parent/Child Relationships When sketching a feature, the sketching plane and the reference plane become parents of the new feature. If the sketching plane moves, the feature moves along with it. Similarly, if the reference plane that determines orientation changes, the orientation of the feature changes as well.


Introduction to ProENGINEER

NOTES

Figure 1: Example of Parent/Child Relationship

Modifying a Feature’s Parents You can alter the parents of a feature by rerouting or redefining it.

Rerouting Parent Features With the Reroute option in the FEAT menu, you can change the parents of a feature including sketching planes, reference planes, and anything specified as a reference in Sketcher. When rerouting a feature, Pro/ENGINEER highlights its external references one at a time and identifies each reference in the message area. You have two choices. You can click Alternate and select a new reference, or click Same Ref and retain the current reference.

Note: Pro/ENGINEER considers references that you use for alignment to be dimensioning references.

For University Use Only - Commercial Use Prohibited Parent/Child Relationships

P a g e 7- 3

NOTES

Figure 2: Bracket with Datums

Redefining Features The Redefine option in the FEAT menu also changes the parents of a feature. When you select a feature to redefine, the same feature dialog box appears that is visible during initial feature creation.

Figure 3: Feature Dialog Box



NOTES

Working with Sketched Features When sketching a section, you can change the sketch plane or the sketch itself. The features that you created after sketching a section temporarily disappear. When you select the Section element for a sketched feature, the menu displays the following options: – Prompts you to specify a sketching plane and reference. You can select and redefine all of the elements listed in the dialog box. Therefore, in addition to being able to change the parents of a feature, you can also change other elements such as direction and material-side-plane before entering Sketcher mode. For each, you can select an alternate reference or retain the same reference. Sketch Plane

– Allows you to use Sketcher mode to change sketched entities, add/remove constraints, and create and delete dimensions. The system warns you if you try to delete an entity that is referenced by another feature. Sketch

Resolving Regeneration Problems Pro/ENGINEER bases the definition of a feature on the parent feature. If parent features are missing, the system automatically brings you into the RESOLVE environment.

Note To remove a feature from the regeneration process, you must also decide what to do with the child features, if they exist.

Regenerating Parent/Child Features When regenerating a model, Pro/ENGINEER regenerates features one at a time, following the order in which they appear in the MODEL TREE. As you create new features, it adds them to the bottom of the list in the MODEL TREE.


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NOTES

Using the Feature Reorder and Insert Modes The R e o r d e r or Insert Mode options in the FEAT menu modify the order of the features. Or you can simply drag and drop the features in the model tree to reorder their positions.

Note You must regenerate a parent feature before you regenerate its children. Therefore, you cannot reorder a parent to be after its children; nor can you reorder a child to be before its parents.

Using the Insert Mode option, you can create one or more features at a selected position in the regeneration process. You can insert features at any point, except before the first feature or after the last feature. After you click Activate , you select the feature after which to insert features. The system suppresses any features after it in the regeneration process. If you click Cancel to stop inserting features, you must then specify if you want to resume the features that were suppressed when you activated insert mode. If you resume them, the system places them after the inserted features.



NOTES

Rectangular base added Base caps hole

Cylindrical protrusion with hole added

Rectangular Base Added

Finished model

Figure 4: Reordering the Hole

Insert mode activated before hole

Protrusion added

Figure 5: Inserting the Protrusion


P a g e 7- 7

NOTES

LABORATORY PRACTICAL Goal In this laboratory you learn to alter the existing parent/child relationships in a model and create new parent/child relationships to capture the changed design intent.

Method In Exercise 1, you move the cylindrical protrusion on the base protrusion and place it on the cut feature by using the Reroute feature. This involves creating new parent/child relationships for the cylindrical protrusion. In Exercise 2, you delete the second protrusion and modify the shape of the slot feature by using the Redefine feature.

Tools Table 1: Interface and Sketcher Icons

Icons

Description No Hidden Create constraint Create dimension Shading



NOTES

EXERCISE 1: Using Feature Reroute

Second protrusion

Cylindrical protrusion Cut

Base protrusion

Slot feature

Figure 6: Original Model

Figure 7: Finished Models after Exercises 1 and 2

Task 1. feature.

Reroute the half cylinder protrusion to the surface of the cut

1. Click File > Set Working Directory. 2. Set the working directory to \ intro_proe_320 \ 07_pc_relationships . 3. Retrieve the P_C_EXERCISE.PRT. 4. Click

[No hidden].


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NOTES

5. Click Feature > Reroute in the menu manager and leave the default selections. 6. Do not roll back the part model. Click No from the message area. 7. Select the half-cylindrical protrusion. 8. Specify a new reference for the sketching plane. Leave the default Alternate . 9. Click Query Sel to select the top surface of the cut. Select this surface as the sketching plane

Select this surface as the second dimension

Figure 8: Rerouting References for the Protrusion

10. Leave DTM3 as the horizontal reference. Click Same R e f. 11. Leave the back surface as the dimensional reference. Click S a m e R e f. 12. Change the second dimensional reference. Leave the default Alternate.

13. Click Query Sel to select the side of the model, as shown in the preceding figure. Task 2. The model enters the Resolve environment because the changes that you have made created a problem. Investigate the problem and resolve it. 1. Read the INFORMATION window that appears. It indicates that a slot feature needed to regenerate the model is missing references.



NOTES

2. Click Undo Changes > Confirm . Task 3.

Investigate the parent/child relationships of the slot feature.

1. Click Info > Parent/Child. Select the slot on the front side of the block. 2. In the REFERENCE INFORMATION WINDOW dialog box, select the Parent’s List to highlight it. 3. Click Tree > Expand > All .

Figure 9 References Information Window

4. Select SURFACE ID 16. The front surface of the block highlights as the sketching plane. 5. Select SURFACE ID 64. The top of the cylinder highlights as the horizontal reference plane. This is an unwanted relationship. 6. Select EDGE ID 73. The bottom edge of the cylinder highlights as a dimensional reference. This reference caused the reroute to fail. 7. Select EDGE ID 47. The right edge of the second protrusion highlights as a dimensional reference. This edge was used as an alignment reference.


P a g e 7- 1 1

NOTES

8. Click Close . Task 4. Break the parent/child relationship between the slot and the cylindrical protrusion. 1. Click Edit > References. 2. Do not roll back the part model. Click No . 3. Click Same Ref. Read the message window. 4. Leave the default Alternate . 5. Click Query Sel to select the top surface of the large protrusion as the new horizontal reference plane. Second protrusion

New horizontal reference

New dimensional reference

Figure 10: Rerouting the Slot

6. Leave the dimensional reference to the second protrusion. Click Same R e f.

7. Change the edge of the cylinder's dimensional reference. Leave the default Alternate . 8. Click Query Sel and select the top surface of the large protrusion as shown in the preceding figure. 9. The message area displays the message: “Feature rerouted successfully.”



NOTES

Task 5.

Reroute the cylindrical protrusion as planned.

1. Select PROTRUSION ID 58 in the MODEL TREE and click Edit > Preferences. 2. Do not roll back the model. 3. Query Sel and select the top surface of the cut as the new sketching plane. 4. Do not change the horizontal reference. Click Same R e f. 5. Do not change the dimensional reference. Click S a m e Ref. 6. Query Sel and select the side of the model as the second dimensional reference. 7. The successfully rerouted cylindrical feature appears as shown in the following figure.

Figure 11: The Re-routed Cylindrical Feature


P a g e 7- 1 3

NOTES

EXERCISE 2: Using Feature Redefine Task 1. The new design intent of this model dictates you should remove the second protrusion from the model by deleting it. 1. Right-click PROTRUSION ID 29 in the MODEL TREE, then select Delete .

Figure 12: Warning Dialog Box

2. Click Cancel in the WARNING window. 3. The slot highlights because it is a child of the second protrusion. Task 2. Break the parent/child relationship between the slot and the protrusion. In addition, change the section of the slot.

1.

the slot feature in the MODEL TREE and select Redefine .

2. Click Section > Define > Sketch from the FEATURE dialog box. Tips & Techniques: You can also double-click on an element to change its definition, instead of highlighting and clicking Define .



NOTES

3. To change the section, select the left vertical sketched line, as shown in the following figure. Click Edit > Delete . 4. Create a tangent end arc.

Delete this line segment.

Sketch this arc.

Figure 13: New Section for Slot

Task 3.

Change the dimensioning scheme of the slot.

1. Click

> Explain .

2. Read the message area. 3. Select the vertical bar constraint, as shown in the following figure. 4. Read the message area.


P a g e 7- 1 5

NOTES

select this edge

select this vertical bar constraint symbol

Figure 14: Interrogating a Constraint

5. Click Sketch > References in the MAIN MENU. 6. Select EDGE: F6. Click Delete > Close > Yes. Tips & Techniques: You can easily determine external references to edges and surfaces by looking for the brown dashed line.

7. Click View > Default. 8. Click . Add a dimension from the left side of the base protrusion to the center of the left arc, as shown in the following figure.



NOTES

Figure 15: Dimensioning the Slot

Tips & Techniques: It is always good practice to dimension in the default view to avoid unwanted parent/child relationships.

9. Click Task 4.

> OK .

Remove the second protrusion from the design.

1. Highlight Protrusion id 29 in the MODEL TREE. Right-click and select Delete . 2. Click OK to confirm the deletion of the second protrusion.


P a g e 7- 1 7

NOTES

Figure 16: Second Protrusion Deleted

Task 5. model.

Change the design so that the slot passes completely through the

1. Click Feature > Redefine in the menu manager. 2. Select the slot. 3. Click Depth > Define > Thru All > Done > OK. Task 6.

Analyze the model using shading.

1. Click

[Shading]. Spin the model.

2. Click View > Saved Views >BACK > Set > Close . Tips & Techniques: You can also select named views directly by clicking [Saved view list].



NOTES

Figure 17: Slot Redefined Using the Thru All Option

Task 7.

Change the holes to have a collar.

1. Look in the MODEL TREE and confirm that the hole pattern (listed as PATTERN ) is the last feature in the model. 2. Select SHELL from the MODEL TREE and drag it below PATTERN. 3. Note that the holes now all have a collar.

Figure 18: Reordered Shell Feature

4. Close the model without saving the changes. 5. Click File > Erase > Current > Yes.


P a g e 7- 1 9

NOTES


Parent/child relationships are hierarchical relationships within a model whose features are cumulatively built beginning with a base feature.

•

During regeneration of a model, Pro/ENGINEER strictly follows the order in which the features were built while accounting for parent/child relationships among them. A child feature can never be regenerated before its parent feature.

•

To capture changing design intent, parent-child relationships between various features of a model have to be re-negotiated. For this, Reroute , Redefine , and Reorder are used as needed.

•

By using the Insert Mode option, new features can be inserted in between features of an existing model.




Module

8 Sweeps and Blends In this module, you learn how to add and remove material using sweeps and parallel blends.


Create swept features.

•

Create parallel blend features.

Page 8-1

NOTES

SWEEP AND TRAJECTORIES Creating Sweeps and Trajectories Sweeps consist of two features—the trajectory and the cross-section. The trajectory is the path along which you sweep the cross-section. The first step in defining a sweep is to creating a trajectory. The second step is to create the cross-section. You must locate the cross-section with respect to the trajectory. A sweep can add material when defined as a protrusion, or remove material when defined as a cut. A sweep trajectory can be sketched as either open or closed; that is the section does not have to end at the point of origin. To illustrate this point, the following figure provides three different combinations of trajectories and sections.



NOTES

Open trajectory, closed section

Closed trajectory, closed section (No Inn Fcs)

Closed Trajectory, Open Section (Add Inn Fcs)

Figure 1: Sweep Trajectories and Section

Creating Parallel Blends A Blend feature combines at least two planar sections joined together at their edges with transitional surfaces to form a continuous feature. You can use blends as forms for either protrusions or cuts. You create a parallel blend from a single section that contains multiple contours, called subsections. In the following figure, each segment is matched to the subsequent segment, creating the blended surfaces between the corresponding segments. Therefore, each section or subsection must always have the same number of segments/vertices.

For University Use Only - Commercial Use Prohibited Sweeps and Blends

P a g e 8- 3

NOTES

Straight transition

Smooth transition

Figure 2: Parallel Blends

When blending the sections together, Pro/ENGINEER connects the start point of each section and continues to connect the vertices of the sections in a clockwise manner. The Feature Tools option in the SKETCH pull down menu changes the start point for any section to control the blend or twist of the blended surfaces. Or you can use the pop-up menu to select a different start point.

Figure 3: Start Points and Twisted Blend



NOTES

Figure 4: Start Points and Blend Shape

When creating a parallel blend, you create all of the sections for the blend in the same sketch. You toggle between sections to distinguish between each sections. The feature attribute for parallel blends is smooth or straight. •

The straight attribute blends the transitional surfaces from one section straight to the next.

•

The smooth attribute connects the section with spline surfaces.

Subsections can be located with respect to the other subsections via dimensions or constraints. If you begin your part with three default datum planes, all subsections can be dimensioned to them. As with any feature, the dimensioning scheme is important, since it captures the design intent of the model.


P a g e 8- 5

NOTES

Figure 5: Dimensioning Parallel Blend Sections



NOTES

LABORATORY PRACTICAL Goal In this laboratory you will create parallel blends and simple sweeps.

Method In Exercise 1, you create a parallel blend by first retrieving a section to be used for subsections. This is an effective technique to use for common sections, especially if they are complex. In Exercise 2, you create a swept protrusion.


Icons

Description Toggle grid Refit Toggle datum planes


P a g e 8- 7

NOTES

EXERCISE 1: Creating Parallel Blend Features Task 1.

Start a new part without using the default datum template.

1. Create a new part and name it PARALLEL_BLEND.PRT. 2. Uncheck the Use default template option, as shown in the following figure.

Figure 6: Creating Part without using Default Template

3. Click Empty > OK in the NEW FILE OPTIONS dialog box. 4. Click Insert > Datum > Plane . Task 2.

Create a parallel blended protrusion.

1. Click Insert > Protrusion > Blend 2. Accept all the defaults in the BLEND OPTS menu and click Done . 3. Leave the default Straight in the ATTRIBUTES menu and click Done . 4. Select DTM3 as the sketching reference and click O k a y for direction.



NOTES

5. Click Top and select DTM2 as the reference plane. 6. Toggle

to show the gridlines.

7. Zoom in (about 4 X 4 grid squares) at the intersection of DTM1 and DTM2. Task 3.

Retrieve the first section from disk and place it.

1. DTM1 and DTM2 as section references are placed. Close the REFERENCES dialog box. 2. Click Sketch > Data from File . 3. Select BLEND.SEC and click O p e n. A small blend section and the SCALE ROTATE dialog box will appear. 4. For the Scale option, type [3 . 0] and press . For Rotate , leave the default [0 . 0] value. Do not close the dialog box. 5. Select the center point of the section; move and place it so that your vertical and horizontal centerlines snap to DTM1 and DTM2 respectively. Place center point of section at intersection of datums

Figure 7: Placing the First Section

6. Click 7. Click

in the SCALE ROTATE dialog box. [Refit].


P a g e 8- 9

NOTES

Task 4. Add the second section to the sketch using the same sketch, but a different scale value. 1. Click Sketch > Feature Tools > Toggle Section . Notice the first subsection gets deactivated and turns gray. 2. To retrieve the BLEND.SEC section again, click Sketch > Data from file . 3. For Scale, type [1.0] and press . 4. Leave the default [0.0] as the rotating angle. Do not close the SCALE ROTATE dialog box. 5. Place the sections so that the centerlines are coincident with the previous section centerlines. 6. Click

in the SCALE ROTATE dialog box.

Task 5. Use the same sketch again for the third section of the blend assigning it a scale factor of 2. 1. Click Sketch > Feature Tools > Toggle Section . Make sure both the sections are gray before bringing in the final section. 2. Retrieve the same BLEND.SEC section again and assign a scale factor of [2.0]. 3. The three sections should look as shown in the following figure. 4. Change the view to default.



NOTES

Figure 8: Creating the Third Section

Task 6.

Define the feature.

1. Click

to get out of the intent manager.

2. Type [30.0] as the depth for the second section and press . 3. Type [20.0] as the depth for the third section and press . 4. Click OK . 5. The blend should look as shown in the figure below except the dimensions will not be visible.


P a g e 8- 1 1

NOTES

Figure 9: Completed Blend

Note: Note that Pro/ENGINEER uses straight lines as transitions to attach the vertices of the subsections.

Task 7. Change the shape of the transitional surfaces from a straight line transition to a spline transition by using Redefine . 1. Right-click on the blend protrusion in the model tree and select Redefine . 2. Click Attribute > Define > Smooth > Done . 3. Finish the definition. Click OK . 4. Save the file and close the window.



NOTES

Figure 10: Straight and Smooth Surfaces


P a g e 8- 1 3

NOTES

EXERCISE 2: Create a Simple Sweep Protrusion Task 1. Create a part, starting with default datum planes. Create the base feature protrusion as a sweep. 1. Start a new part and name it SWEEP.PRT. 2. Clear the Use the default template option in the NEW dialog box and check Empty in the NEW FILE OPTIONS dialog box followed by OK . 3. Click Insert > Datum > Plane to create the default datum planes or click 4. Toggle

[Insert datum] to turn on the datum planes.

5. Click Insert > Protrusion > Sweep. Note: A sweep is a two-part sketch: the trajectory is first and the cross-section follows.

Task 2. Sketch the trajectory on DTM2 using DTM3 as the bottom reference. 1. Click Sketch Traj from the SWEEP TRAJ menu. 2. Select DTM2 and click O k a y for the direction. 3. Click Bottom and select DTM3 as the reference. 4. Check to see if DTM3 and DTM1 are the default references and close the REFERENCES dialog box. 5. Sketch an open trajectory section consisting of a line, a tangent arc; and then two lines as shown in the following figure. Place the correct dimensions.



NOTES

Sketched lines Sketched arc fillet

Figure 11: Showing Sketch and Dimensions

6. When you have completed the trajectory, click INTENT MANAGER.

from the

7. The system has placed you in another Sketcher session. Task 3. Note that the centerlines provided by the system at the start point of the trajectory. The system defines the sketching plane as a plane normal to the trajectory, located at the start point. Sketch the cross-section of the sweep. 1. Sketch an inverted T cross-section, as shown in the following figure. You may want to turn the Sketcher grid off. Trajectory starts here

Figure 12: Sketching an Inverted “T”


P a g e 8- 1 5

NOTES

The default view appears as follows:

Start point

Trajectory

Cross-section

Figure 13: Default View

2. Click

to complete the section.

3. Click OK to complete feature. The sweep is rounded where there was an arc in the trajectory, and mitered where there was a corner (nontangent segment) in the trajectory. 4. Save the file and erase it from memory.

Figure 14: The Completed Sweep



NOTES

MODULE SUMMARY In this module, you learned that •

When defining a Swept Feature, you must define its trajectory and its cross-section.

•

Sweeps can either add or remove material depending on whether they are defined as protrusions or cuts.

•

A parallel blend is created from a single section that contains multiple contours called subsections.

•

The parallel blend feature can have either a straight attribute or a smooth attribute.


P a g e 8- 1 7



9 Relations and Parameters In this module you learn to drive the design of a model by using relations. Relations create explicit parent-child relationships.


Describe the purpose of relations.

•

Describe the four types of relations pertaining to models.

•

Create relations that allow your child features to drive their parent features.

•

Re-order relations.

•

Delete and update invalid relations to accommodate changes to the design intent.

Page 9-1

NOTES

RELATIONS AND PARAMETERS Parametric Relations Relations are user-defined equations written between symbolic dimensions and parameters. They can be used to control the effects of modifications on models, to define values for dimensions in parts and assemblies, and to act as constraints for design conditions. The following figure represents a simple relation between the two dimensions of a rectangular feature, where d0 is always twice the size of d1.

Figure 1: Part Relation - Relation: d0 = 2*d1

The four types of model relations are: •

Assembly relations – Relate different component parameters to one another using a coding symbol to designate different components.

•

Part relations – Relate

different feature parameters to one another in

a single part.



NOTES

•

Feature relations –

Relate parameters specific to one feature in the

model. •

Pattern relations –

Relate specific pattern parameters within a

pattern.

Feature relations: Cam slot shape driven by relation /*hole centered in plate d5=d2/2 d6=d3/2

Part relations Hole centered in plate

Assembly relations Bracket centered on plate

Figure 2: Different Relation Types

For University Use Only - Commercial Use Prohibited Relations and Parameters

P a g e 9- 3

NOTES

Representing Relations: Types and Symbols The table below presents the various elements that you can include in relations. Table 1: Elements of Relations Relation Types:

Equality: d0=2*

Comparison:

Constraint: d1>= 2.67 if (d4>.25) endif

d1 d12 = 1.5 else d12=1

Dimension Symbols

d# – Part dimensions d#:# – Dimensions in Assembly mode rd# – Reference dimensions sd# – Sketcher dimensions

Tolerance Symbols

tm# – Minus tolerance tp# – Plus tolerance tpm# – Plus/minus tolerance

Instance Symbols

Integer parameter for instances in each direction of a pattern: p0, p1, p2, etc.

User Parameters

Numeric parameter (i.e., 3.67) Character string parameter (i.e., 32-A24-67B) Yes or no parameter Model note parameter

Incorporating Your Design Intent Using Relations Relations enable you to capture sophisticated levels of design intent for your models. They are an integral part of any advanced design of parts and assemblies. Relations allow one feature to drive another. You can take advantage of this unique capability and use child features to drive the parent features. In a traditional parent/child relationship, it is the parent feature which always takes precedence (whether in dimensioning or regeneration). Parametric relations allows you to craft your model in such as way as to reverse the parent/child hierarchy.

Note: Do not create relations using reference dimensions.



NOTES

In the following figure, you could write a relation that drives the placement of the hole so that it is centered top to bottom: /*center hole top to bottom d5=d2/2

Figure 3: Plate Showing Parameters

You could then write another relationship to keep the hole centered from left to right: /*center hole left to right d6=d3/2 Once you have added these relations, Pro/ENGINEER automatically centers the hole in the plate and retains it at the center, even when you modify the height or width of the plate later on.

Note: You can change the symbolic name of a dimension by using Modify > DimCosmetics > Symbol .


P a g e 9- 5

NOTES

Figure 4: Relations that Drive Hole Location

Tips & Techniques: It is good practice to add a relation as soon as you realize that you need it in your design. Do not wait until the end of the design process. It is also good practice to comment your relations using the /* to document the design intent of the relations. You should always test your relations to be sure that they function correctly.

Order of Relations Pro/ENGINEER evaluates relations in sequential order. Therefore, the order that you enter them in is important. During regeneration of the model, the system evaluates the relations and checks to see if all of them are still valid. If not, it issues a warning.



NOTES

The following figure illustrates the consequences of entering relations improperly:

Relations added: d5=d4 d4=d2/2

After first regeneration

Figure 5: Reordering Relations

The design intent is to center the hole on the plate. The two relations, d5 = d4 and d4 = d2/2, are added in that order. After the first regeneration of the model, the relations do not capture the desired intent. Design intent is captured by reversing the order of relations. Relations can be deleted or edited using the Edit Rel option. The final regenerated model is shown in the following figure.

Figure 6: Model Regenerated with Relations Sorted


P a g e 9- 7

NOTES

Design Changes As a design cycle progresses, the design intent of a model tends to change. This may invalidate existing relations in the model. Whenever Pro/ENGINEER encounters invalid relations during regeneration, it automatically highlights the problem and prompts you to correct it. You can either delete the relation or update it. If you have to modify or delete a relation because of a design change or an error, you can edit the relation in the model using a system text editor. The editor that your system uses depends on the type of workstation that you have.



NOTES

LABORATORY PRACTICAL Goal In this laboratory you create relations and manipulate their defining parameters.

Method In Exercise 1, you create relations to capture the design intent of a part, test the relations. In Exercise 2, you create parameters to control features using relations.


P a g e 9- 9

NOTES

EXERCISE 1: Creating Relations Task 1. feature.

Center the straight hole on top of the rectangular base solid

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 09_relations . 3. Open RELATIONS.PRT. 4. Change to wireframe display.

Figure 7: Symbolic Dimensions of RELATIONS.PRT

5. Click Relations from the PART menu. 6. Select the hole to display its dimensions. 7. The dimensions appear in their symbolic form (i.e., d5, d6, d7). 8. Select the block to display its symbolic dimensions. Task 2.

Start adding a relation.

1. Click Add from the RELATIONS menu.



NOTES

2. Enter a comment to describe the function of the relation. Type [/* center hole front to back]. Press . 3. Type [d6 = d4/2], then press. 4. For the second relation, type [/* Center hole left to right], then press. 5. Type [d5 = d2/2], then press. 6. Press on a blank prompt line to finish adding relations. Task 3.

Toggle between the numeric and symbolic values.

1. Click Switch Dim from the RELATIONS menu. 2. Click Done from the MODEL REL menu. 3. Click Regenerate . The hole should move to the center of the block. Note If your relation contains an error, click Relations > Edit.

Task 4. depth.

Test the two relations by modifying the base feature width and

1. Click Modify from the PART menu. 2. Select the rectangular base. 3. Select the width of the block and change it to [70.0] from 50. 4. Click Modify from the PART menu. Select the depth of the block and change it to [90.0] from 50. 5. Regenerate the model. Task 5.

Show the dimensions of the hole.

1. Click Modify from the PART menu. 2. Select the straight hole to display its dimensions.


P a g e 9- 1 1

NOTES

3. Confirm that the two locating dimensions are 35 and 45. 4. Change the base back to the original dimension values. Select each dimension, and type [50.0]. 5. Regenerate the model. Task 6. Add a relation that limits the diameter of the hole to be less than or equal to 11.25. 1. Click Relations from the PART menu. 2. Select the hole feature. Identify the symbolic name given to the hole diameter, (d7). 3. Click Add from the RELATIONS menu. 4. Type an appropriate comment. 5. Type [d7 <= 11.25]. 6. Press on a blank line. 7. Click Done from the MODEL REL menu. Task 7.

Test the relation by modifying the diameter dimension.

1. Click Modify > Dimension from the PART menu. 2. Click the diameter dimension followed by Done Sel . The DIMENSION PROPERTIES dialog box appears. 3. Type [15 ] as the nominal value and then click OK .



NOTES

Figure 8: Dimension Properties Dialog Box

4. Click Regenerate from the PART menu to update the model. 5. Note the warning in the information window; then close it. 6. Continue the regeneration regardless of the warning. 7. Type [Y] to continue the regeneration, and press . Task 8.

Review the relations via the information window.

1. Click Relations > Show Rel . 2. Close the window and click Done . 3. Modify back to a smaller diameter. Click Modify , select the hole select the diameter dimension, then type [10.0]. 4. Regenerate the model.


P a g e 9- 1 3

NOTES

Task 9. Resume a hole and counterbore that were previously suppressed. 1. Click Feature > Resume . 2. Retrieve only the last set of features that were suppressed. Click Last Set > Done from the RESUME menu followed by Done from the FEAT menu.

Figure 9: The Resumed Hole



NOTES

EXERCISE 2: Creating Parameters for FeatureControl Task 1. Add a parameter to the model then control the counterbore depth using the parameter. 1.

Click Relations from the PART menu.

2.

Click Add Param .

3. Define a real number so the depth can vary infinitely. Click R e a l Number . 4. Type [depth_ratio] in the message area followed by . 5. Type [.10] followed by . Task 2.

Start to add a relation.

1. Click Part Rel from the MODEL REL menu. 2. Select the surface of the counterbore hole. 3. Click Add . 4. Type [/*control the counterbore depth], then press .

5. Enter a relation to have the conterbore as deep as the hole minus the thread depth. Type [d23 = depth_ratio*d22], then press .

6. Press on an empty line. 7. Click Done from the MODEL REL menu. 8. Regenerate the model. Task 3.

Test your relation .

1. Increase the total depth of the hole. Click Modify and select on the counterbore hole. 2. Click the depth dimension and type [30].


P a g e 9- 1 5

NOTES

3. Regenerate the model. Task 4. Edit the ratio parameter to change the relationship between the counterbore and hole. 1. Click Set Up from the PART menu, then click Parameters from the PART SETUP menu. 2. Leave the default part and click Modify from the MODEL PARAM menu. 3. Select DEPTH_RATIO and type [.5]. 4. Click Done from the PART SETUP menu. 5. Click Regenerate . Task 5. Change the symbolic name of the entire depth of the hole and the counterbore depth to document the design. 1. Click Modify > Dim Cosmetics. 2. Select the depth dimension and type [entire_depth]. 3. Select depth dimension of the counterbore, then type [cbore_depth]. 4. Click Done from the DIM COSMETIC menu, then click Done from the MODIFY menu. Task 6.

Inspect the parameter in the model using various methods.

1. Click Setup > Parameters > Info from the MODEL PARAMS menu. 2. Read the INFORMATION window; then click Close . 3. Click Done from the PART SETUP menu. 4. Click Relations > Show Rel .



NOTES

Figure 10: Relation Information Window

5. Notice that the system lists the relations you have defined along with the parameters. Also notice that the new symbolic names are now displayed. 6. Click Close > Done . 7. Save the model and click File > Close Window . 8. Click File > Erase > Not Displayed. Click OK .


P a g e 9- 1 7

NOTES

MODULE SUMMARY In this module you learned that: •

Relations are user-defined mathematical equations composed of symbolic dimensions and parameters, which capture design relationships within a part or among the many component parts of an assembly.

•

There are four different kinds of relations: Assembly Relations, Part Relations, Feature Relations, and Pattern Relations.

•

The ordering of relations is crucial in capturing design intent as Pro/ENGINEER evaluates relations in consecutive order.

•

During model regeneration, invalid or conflicting relations are highlighted by prompts for resolution.

•

The user should always plan ahead to make relations an integral part of the design of parts and assemblies.

•

Relations can be intelligently used to make child features drive their parent features.




Module

10 Behavioral Modeling CAD technology has matured through four distinct stages: 2-D drafting, 3-D wireframe modeling, 3-D solid modeling, and 3-D solid modeling with associative, parametric, and feature-based characteristics. The latest state-of-the-art, 5th generation CAD technology is called Behavioral Modeling. In this module you learn about the behavioral modeling capabilities of Pro/ENGINEER.


Describe the purpose of Behavioral Modeling.

•

Describe various Behavioral Modeling components and their uses.

•

Analyze mass properties.

•

Create model and relation analysis features.

•

Conduct sensitivity, feasibility, and optimization studies.

P age 10-1

NOTES

BEHAVIORAL MODELING Product requirements are becoming increasingly volatile and products are being custom-tailored more and more. In such a scenario, the requirements for a mechanical design automation technology that automates mundane design tasks so that the designer can concentrate on creative work becomes apparent. Behavioral Modeling is such a technology.

Figure 1: CAD Evolution

Behavioral Modeling Features The power of Behavioral Modeling derives from three factors: 1. Smart Models 2. Objective-Driven Design Capabilities 3. Open Extensible Environment

For University Use Only - Commercial Use Prohibited P a g e 1 0- 2


NOTES

Figure 2: Cornerstone of Behavioral Modeling

Smart Models •

Smart models are intelligent designs that adapt to their environment.

•

They contain all the specifications and process information they need within them.

•

As smart models are “aware” of their contexts and purposes, the designer can develop innovative, differentiated, and customerresponsive products.

Figure 3: Smart Model Adapting to Changing Needs

For University Use Only - Commercial Use Prohibited Behavioral Modeling

P a g e 1 0- 3

NOTES

Objective-Driven Design Capability •

The objective-driven design approach automatically optimizes designs to meet any number of objectives captured in a smart model.

•

It can simultaneously resolve conflicting objectives, a task that was often impossible using traditional approaches.

•

In addition to defining a problem with standard types of measurements such as the center of gravity or an edge length, more complex requirements can be captured in features such as surface or curve analysis or complex equations.

For example, perhaps you want to place a hole coincident with the axis of the center of gravity of a design. Capturing the center of gravity in a feature and parametrically tying it to the hole will ensure that the features remain coincident, even as other design changes are made and the center of gravity moves to reflect these changes.

Open Environment •

Smart models can accommodate features that link to information in other applications.

•

These external features make the design solution infinitely extensible.

•

External features reside within smart models and link to other applications.

USING BEHAVIORAL MODELER The following are the uses of the Behavioral Modeler: •

Create feature parameters based on measurements and analyses of the model.



NOTES

No Overall Height Dimension

Figure 4: Creating Parameters •

Create datum geometry based on measurements and analyses of the model.

Figure 5: Creating Datum Features

•

Create new types of measurements tailored to your specific needs. Surface Area normal to the centerline of the pipe at any given location. All geometry needed for the calculation is part of the measurement.

Figure 6: Creating New Types of Measurements


P a g e 1 0- 5

NOTES

•

Analyze the behavior of measured parameters as dimensions vary.

Y-Axis = volume of tank

X-Axis = width of tank

Figure 7: Analyze Varying Measurements •

Automatically find the dimension values that achieve a desired behavior of the model. Center of Gravity and Axis of Rotation must line up vertically.

Size of the crank can vary to achieve the goal while also minimizing the mass.

Figure 8: Finding the Correct Distance and Size

•

Allow information to be passed between external programs and Pro/ENGINEER.



NOTES

•

Spreadsheet programs: Differential equation solvers Technical computing environments in numeric computation and highlevel programming languages Computational Fluid Dynamics (CFD) Light or optics analysis Piping or HVAC analysis. Solve model configuration that best satisfies multiple goals and constraints.

Two pipes in heat exchangers that cannot intersect; that have a minimum allowable bend radius; and whose length must be minimized.

Figure 9: Solving Complex Problems

•

Perform graph matching.

Measured Curve - Graph of analysis feature of current model

Ideal Curve - Match model to this curve

Figure 10: Graph Matching


P a g e 1 0- 7

NOTES

•

Perform motion analyses. Analyze the angle through the full motion range

Analyze the distance between these two points through the full range of motion

Figure 11: Analyzing Motion

Defining the Behavioral Modeler Components •

Analysis Features – A datum feature that measures or evaluates

geometry and produces parameters and geometry as result. Analysis features

Figure 12: Analysis Features Symbols

Note: Analysis features are evaluated every time the model is regenerated. The system establishes a parent-child relationship between the analysis features and their predecessors in the regeneration cycle.

•

Field Points – A datum point that is partially constrained and free to

move within that constraint.



NOTES

Figure 13: Field Points •

User-Defined Analysis (UDA) – An analysis that is customized to

the users need, and is defined by a set of features.

Figure 14: User-Defined Analysis


P a g e 1 0- 9

NOTES

•

Sensitivity Analysis – An analysis that plots how a change to

particular parameter affects the results of an analysis. In the following figure, the X-axis measures the width dimension and the Y-axis volume dimension.

Figure 15: Sensitivity Plot

For University Use Only - Commercial Use Prohibited P a g e 1 0- 1 0


NOTES

•

Feasibility Study – A study that determines if a specified constraint

or goal can be achieved by varying certain model parameters within specified ranges.

Figure 16: Feasibility Dialog Box


P a g e 1 0- 1 1

NOTES

•

Optimization – If there are multiple solutions to a specified set of

constrains or goals, then optimization is used to determine which solution provides the minimum or maximum value of a specified goal. You can incorporate optimization into a model as a feature so that modifications to the model will be incorporated automatically.

Figure 17: Optimization Dialog Box



NOTES

LABORATORY PRACTICAL Goal In this laboratory your learn the diverse practical applications of behavioral modeling functionality.

Method In Exercise 1, you create a datum analysis feature to measure mass properties by designing a new propeller blade for underwater applications. In Exercise 2, you create three analysis features. It is shown that the position of each analysis feature in the MODEL TREE is critical in order to ensure that the proper parameter is calculated. In Exercise 3, you create and use Sensitivity, Feasibility and Optimization Studies.

Tools Table 1: Behavioral Modeling Icons

Icons

Description Build feature Build feature and repeat the same feature type creation Go to next page Preview feature geometry Create an analysis feature


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EXERCISE 1:Creating a Datum Analysis Feature to Measure Mass Properties Task 1.

Change the working directory and open the blade part.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 10_behavioral_modeling. 3. Click

> BLADE.PRT.

4. Clear the display of datum planes. 5. Click Utilities > Environment to remove the spin center from the ENVIRONMENT dialog box. The model appears as shown in the following figure.

Figure 18: The Blade Part

Note: The model’s design cycle is partially completed. The model’s state shown on the screen represents the model with the preliminary machining step. Not only do you want to find the mass of the model, but also you want a datum coordinate system that represents the center of gravity to be created at the current location in the regeneration cycle.



NOTES

Task 2.

Create a datum analysis feature that measures mass.

1. Click Insert > Datum > Analysis. 2. Type [MASS_PROPS] in the NAME box and press . 3. Select MODEL ANALYSIS as the type of analysis, and click [Next Page]. 4. Leave the default Model Mass Properties as the TYPE. 5. Click Compute. 6. If prompted for density in the message window, type [.75]. (The current model units are lbs/in3 ) 7. Close the MODEL ANALYSIS dialog box. Task 3.

Create the VOLUME and MASS parameters.

1. In the RESULT PARAMS section of the ANALYSIS dialog box, check that VOLUME is set to YES. Scroll down and set the Mass parameter name to Yes. Click CREATE section. 2. Click Task 4.

[Next Page].

Create a COORDINATE SYSTEM at the center of gravity.

1. With CSYS_COG_95 highlighted, click Yes. 2. Click [Preview]. The following figure displays the created coordinate system.


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NOTES

Figure 19: Created Coordinate Analysis Feature

3. Click

[Build Feature].

Task 5. View the values of the newly created parameters as columns in the MODEL TREE. 1. Click View > Model Tree Setup > Column Display. 2. Select Feat Params as the TYPE. 3. Type [MASS] in the NAME box, then press . 4. Type [VOLUME] in the NAME box, then press and click OK. 5. Notice the parameter values in the MODEL TREE. (If necessary, widen the model tree or change the width of the columns.)



NOTES

Figure 20: Parameter Values Reflected in Model Tree

6. Click View > Model Tree Setup > Item Display > Suppressed Objects > OK . 7. Select the cut in the MODEL TREE and click > Resume . Notice the MASS and VOLUME parameters have updated.

Figure 21: Updated Parameter Values in Model Tree

Task 6. Create a copy of the analysis feature and reorder it to confirm that the measurement regenerates in the order of creation.

1. Click Feature > Copy > click

>

, select the MASS PROPS feature, and

.

2. Expand the group in the MODEL TREE to view the new analysis feature. Then select the group and click > Ungroup . Notice that both are indicating the same MASS and VOLUME parameters.


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NOTES

3. Select the new analysis feature, then click > Redefine . Modify the name to MASS_PROPS_2, press and click .

Figure 22: Creating a New Analysis Feature

4. Drag the first MASS_PROPS analysis feature above the cut. Notice the changing values and COG coordinate system location.

Figure 23: Dynamic Value Changes in Mass Property Calculations

Note: An Analysis feature’s results are governed by its position in the model tree. If you were to continue with this model, additional features could be created that are based on the results of these analysis features.



NOTES



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NOTES

EXERCISE 2: Analyze Fluid Volume in a Cup Task 1. plane.

Measure the volume before the shell feature up to a ‘fluid-level’

1. Open STYROFOAM.PRT.

Figure 24: Start Model

2. In MODEL TREE, click and drag the red insert marker above the shell feature. 3. Click

> Offset and select DTM2. Click Enter Value ,

type [4.0] and click

.

4. Click Setup > Name , select the newly created plane from the MODEL TREE and enter [FLUID_LEVEL]. Click Done from the PART SETUP menu to return to the highest level. 5. Click

[Analysis Feature] > Model Analysis.

6. Type [VOL_SOLID] for the name and press . 7. Click

[Next Page].



NOTES

8. Select One-Sided Volume from the TYPE drop-down menu in the MEASURE dialog box. 9. Select the FLUID_LEVEL datum plane from the model tree. 10. Click Flip (so that the arrow faces downward) and O K A Y. 11. Notice the calculated volume in the Results section, and click Close . 12. Ensure that the volume parameter is set to Yes, edit the name to [VOL], and press . 13. Click

[Build Feature].

14. Click View > Model Tree Setup > Column Display. 15. Select Feat Params as the Type . 16. Type [Vol] in the name box, then press and click OK.

Figure 25: Model Tree with Volume Parameter

Task 2.

Measure the one-sided volume after the shell feature.

1. Click and drag the Insert marker below the shell feature. 2. Click


3. Type [VOL_SHELL] for the name and press .


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NOTES

4. Click

[Next Page].

5. For the TYPE, select One-Sided Volume . 6. Select the FLUID_LEVEL datum plane. 7. Click Flip (so that the arrow faces downward) and OK. Notice the calculated volume in the RESULTS section, and click Close. 8. Ensure that the volume parameter is set to Yes, edit the name to [VOL], and press . 9. Click

[Build Feature].

Task 3. Create relation type analysis feature. This relation will calculate the difference between the previous one-sided volumes. 1. Click

[Analysis Feature] > Relation from the type button.

2. Type [VOL_FLUID] for the name and press . 3. Click

[Next Page].

4. When the text editor appears, type the relation on one line as [vol=vol:fid_vol_solid - vol:fid_vol_shell] 5. Click [Build Feature], and observe the volume calculations as shown below.

Figure 26: Volume Calculations of Styrofoam Cup



NOTES

Task 4.

Investigate the fluid volume when the model is modified.

1. Modify the height of the Fluid_Level plane to [5.0] and Regenerate . 2. Toggle the model tree display off and on to refresh its display. The volume values should update as shown below.

Figure 27: Updated Volume Values

3. Modify the height of the Fluid_Level plane to [2.50], Regenerate, and refresh the Model tree. 4. Select the first protrusion from the model tree, and click Modify.

>

5. Modify the dimensions as shown in the following figure, Regenerate , and refresh the Model tree.

Figure 28: Modified Styrofoam Model


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NOTES

6. The new fluid volume with the modified dimensions is 43.15in3 and is shown in the model tree. Task 5. Use behavior modeling capabilities to solve for a fluid volume of an even 50.0 1. Click Add > Analysis > Feasibility/Optimization in the main menu. 2. Refer to the following figure and set Study Type to Feasibility . 3. Set the design constraint to solve for a vol_fluid = [50.0] . Click Add from the design constraints area and select VOL: VOL_FLUID. 4. From the parameter drop-down in the DESIGN CONSTRAINTS dialog box, click S e t and enter [50] as the value followed by OK . 5. Click Add Dimension and select the dimension corresponding to the Fluid Plane (2.5 dimension). 6. Click Done Sel and enter [2 . 0] and press for the minimum value and enter [3 . 0] for the maximum value.

Figure 29: Conducting a Feasibility Study



NOTES

7. Click Options > Preferences followed by Run and edit the Convergence % to [0.001] as shown in the following figure and click OK.

Figure 30: Setting Convergence Value

8. Click Compute. 9. After notification of a feasible solution, click Close > Confirm. 10. Refresh the model tree and observe that the vol_fluid is [50.0] with a fluid level of [2.788].

Figure 31: The “Feasible” Solution

11. Click

> File > Close Window .


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NOTES

EXERCISE 3: Crankshaft Optimization Task 1. Create an analysis feature to measure the mass properties of the part. Output a MASS parameter and a datum coordinate system at the center of gravity. 1. Open CRANKSHAFT.PRT.


2. Click


3. Type [Mass_Props ] for the name, press and click [Next Page] .

4. If necessary, select Model Mass Properties as the Type, and click Compute > Close.

5. Toggle the Volume parameter to NO , and the Mass parameter to YES to create only the Mass parameter. 6. Click

[Next Page] .

7. Toggle the Csys creation to YES , edit the name to [COG ], press , and click .



NOTES

8. Click > Side and note that the current COG is well below the axis of revolution. Create another analysis feature that measures the distance between the center of gravity coordinate system and the crankshaft’s axis of rotation, A_1. 9. Click

[Analysis Feature] > Measure .

10. Type [ COG_DIST ] for the name, press and click [Next Page] .

11. Select Distance as the Type, and select A_1 and COG to measure between them as shown. (The distance should be approximately 0.35)

. Figure 33: Distance Measurement 12. Click Close , verify the Distance parameter is set to YES , and click Task 2. Use a sensitivity study to determine which dimension modification (height or width) has the most impact on the COG. 1. Set the following config option which will use Excel to create graphs instead of the Pro/E graph window. Ask your instructor if you need assistance.


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NOTES

Figure 34: Setting Configuration Option

2. Click Analysis > Sensitivity Analysis > Dimension , and select the main lobe of the crank as shown below. Note that dimensions d28 and d27 are the main height and width dimensions. If necessary, click Info > Switch Dimensions to see dimensions in their symbolic form.

Figure 35: Selecting Main Lobe of Crank

3. Select d27 and notice that the system by default has placed Min and Max values for the Variable range at +/- 10%. 4. Click plot.

> DISTANCE:COG_DIST > Ok

to set the parameter to

5. Click Compute . After a few moments, the following graph should appear:



NOTES

Figure 36: Sensitivity Plot

Note: This is an Excel spreadsheet running inside of Pro/E. on the graph will allow you to Open, Edit, or Delete the graph.

6. Record the difference between the high and low values on the vertical graph scale. (0.404 - 0.304 = 0.1) Therefore, changing this dimension by +/-10% would move the COG by [0.1]. 7. Select the graph and > Delete . Then click Dimension , select d28 , and click Compute .

Figure 37: Modified Sensitivity Plot


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NOTES

8. Again, record the difference between the high and low values on the vertical graph scale. (0.529 - 0.229 = 0.3) Therefore, changing this dimension by +/-10% would move the COG by [0.3]. 9. In conclusion, the Sensitivity Study has determined that the height dimension (d28) has more of an impact on the COG than the width dimension (d27). 10. Click Close . Task 3. Create a FEASIBILITY STUDY to get the center of gravity and axis of revolution to equal zero. There are certain dimensions that you already know you can change. 1. Click Analysis > Feasibility/Optimization > Feasibility . 2. Click Add, select the DISTANCE:COG_DIST parameter, Set the value to [0 ], and click OK > Cancel. 3. Click Add Dimension , and select dimensions d27, d28, and d31, then click

.

4. Enter the Min and Max values as shown.

Figure 38: Minimum and Maximum Values

5. Click Options > Preferences, check only Graph constraints and click OK . Click Compute for the results.



NOTES

Figure 39: Optimization Limit Convergence Graph

6. Notice the COG distance quickly dropped from 3.5 to a value very close to zero with only two iterations. 7. Compare the before and after dimension values as shown below. Note that the radius value hardly changed, and therefore could be removed from future studies.

Figure 40: Comparing Dimension Values

8. Click > Side and notice that if these new values were kept, the COG Csys would coincide with the rotation axis. Conclusion: balancing this model is feasible. 9. Undo the changes and close the dialog box for now. Click Undo, then Close from the OPTIMIZATION/FEASIBILITY dialog box.


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NOTES

Task 4. Create a third analysis feature so that the material between the main shaft and the balancing body stays above a certain value.

1. Click

[Analysis Feature] > Measure .

2. Type [MATL_DIST ] for the name, press and click [Next Page] .

3. Select Distance as the Type, and select the two edges shown.

Figure 41: Selecting Edges

4. Click Close , verify the Distance parameter is set to YES , and click . Task 5. Redo the Feasibility study to see if a feasible solution can be found when this new distance parameter is added as another design constraint. 1. Click Analysis > Feasibility/Optimization . Notice that the previous values are maintained. 2. Click Add > DISTANCE:MATL_DIST . Set the parameter value to be ‘> = ’ a set value of [0.25]. Then click OK > Cancel . 3. Click Options > Preferences, and uncheck any available graph options. 4. Compute the results. (A feasible solution should be found)



NOTES

TASK 6. For the final criteria, check that the mass of the part is minimized, as well as all the other constraints by running an OPTIMIZATION STUDY.

1. Click Optimization from the top of the dialog box. 2. Leave Minimize and Mass:Mass_Props as the goal. 3. Compute the results. Notice the reduction of mass on the graph and that the dimensions are now varied differently.

Figure 42: Observing Graph and Model


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NOTES

Task 7. Next, incorporate the Optimization into the model as a feature so that modifications to the model will be incorporated automatically. Modify the model to confirm this. 1. From the Optimization/Feasibility dialog, click File > Make . Then click Close and repaint the screen. Notice Feature > the Optimization feature in the model tree. 2. Select the Optimization feature from the model tree and click > Suppress > OK . 3. Display suppressed features in the model tree. Click View > Model Tree Setup > Item Display and select Suppressed Objects. 4. Modify the diameter dimension as shown in the following figure from [ 1.25 ] to [0.75 ] and Regenerate.

Figure 43: Modifying Diameter Dimension

5. Add the distance parameter column to the model tree and switch to a side view. Notice that now the COG is slightly below center (0.077).

Figure 44: Side View of Model



NOTES

6. Select the Optimization feature from the model tree and click > Resume . Notice the model is now balanced again.

Figure 45: Optimized Model

7. Save the model and click File > Close Window . 8. Click File > Erase > Not Displayed. Click OK .


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NOTES

MODULE SUMMARY In this module, you have learned that: •

Behavioral Modeling gives you the tools you need to design product models that are driven by your requirements and specifications.

•

In traditional design systems, you need to manually iterate the geometry of designs. Now with Behavioral Modeling tools, you can now explore optimal solutions with a complete understanding of the performance and behavior of your design.

•

Analysis features allow you to measure geometric properties of the model at specific points in the list of features or components of the model. These measurements produce parameters and logical datums that you can use to determine geometric properties such as mass, volume, curvature, the center of gravity, and many others. You can even create your own parameters as the result of a relation or a userdefined analysis.

•

A Feasibility Study searches for a solution within the range of chosen dimensions to meet a set of constraints. You specify the constraints by means of one or more analysis feature parameters.

•

An Optimization Study solves a feasibility problem with an additional condition, a goal. The goal is to minimize or maximize some analysis feature parameter.




11 Drawings and Drawing Templates You can use the Drawing mode in Pro/ENGINEER to create detailed drawings of all Pro/ENGINEER models. You can also import drawings from other systems into Pro/ENGINEER. Pro/ENGINEER associates drawings with their parent models. The model automatically reflects any changes that you make to a drawing. Conversely, drawings also reflect any changes that you make to a model in Part, Sheetmetal, Assembly, or Manufacturing modes.


Describe the different types of drawing views in Pro/ENGINEER.

•

Create a production drawing for an existing part model.

•

Explore the associativity that exists between a model and its drawing.

•

Create dependency between certain drawing views.

•

Create a simple production drawing that will detail dimensions and notes.

Page 11-1

NOTES

DRAWING FUNDAMENTALS Creating a Drawing After selecting Drawing from the NEW dialog box and assigning it a name, the NEW DRAWING dialog box will open. This dialog box gives you multiple options in which you can assign an associated model, select the sheet size, and specify an orientation: •

With a portrait orientation, the system uses the larger sheet dimension as the height and the smaller one as the width.

•

With a landscape orientation (the default setting), the system uses the larger sheet dimension as the width and the smaller one as the height.

•

With a variable orientation, the system uses values that you specify for the height and width of the drawing sheet.

You also have the ability to assign a predefined company format. The format that you select will automatically define the sheet size and orientation.

Adding Drawing Views After selecting a format or specifying a sheet size, you can add views to your drawing using the V i e w s option. The first view must be a general view. When first placed, it appears in the default view orientation. Using the ORIENTATION dialog box, you can reorient it during placement.

Note: You should always use default datums to orient a general view.

Types of Views The five primary view types available in the VIEW TYPE menu are: •

Projection

•

Auxiliary

– An orthographic projection of an object as seen from the front, top, right, or left. – A view created by projecting 90 degrees to an inclined surface, datum plane, or along an axis.



NOTES

•

General

•

Detailed

•

Revolved

– A view that you orient and is not dependent upon any other view for its orientation. – A view that you create by taking a portion of an existing view and scaling it for dimensioning and clarification purposes. The boundary for the detailed view can be a circle, ellipse (with or without a horizontal or vertical major axis), or a spline. – A planar area cross-section revolved 90 degrees about the cutting plane line and offset along its length.

Figure 1: The Five Main Types of Views

Using the View Type Menu Using other options in the VIEW TYPE menu, you can specify how much of the model is visible in the view, as shown in the following figure. •

Full View

•

Half View

•

Broken View

•

Partial View

– Shows the entire model.

– Shows only the portion of the model on one side of a datum plane. – Removes sections from large objects between two points and moves the remaining sections close together. – Shows only the portion of the view that is contained within a boundary.

For University Use Only - Commercial Use Prohibited Drawings and Drawing Templates

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NOTES

Figure 2: Specifying How Much of the Model to Make Visible

Adding a Cross-section To determine if a view is a single surface or a cross-section, you use the VIEW TYPE menu options: •

Section

– Displays a cross-section for a particular view.

•

No Xsec

– Does not display a cross-section.

•

Of Surface

– Displays only the selected surface of a particular view

orientation. The following figure illustrates the various types of cross-sectional views that you can create using the XSEC TYPE menu.



NOTES

Figure 3: Cross-Sectional Views

Manipulating Views Using the Move View option, you can move general and detailed views anywhere on the sheet. However, you can move projection, auxiliary, and revolved views only along their line of projection. Using the Delete View option, the PARENT views—views used to create projection views—cannot be deleted. Instead, they have to be erased with the Erase View option. Restore erased views using Resume View . Using the Disp Mode option, you display views independently of the ENVIRONMENT dialog setting such as Wireframe , Hidden line , and No Hidden. For example, you can show some views with hidden lines and others with no hidden lines. Any views that you establish with this option remain at the same setting regardless of any changes that you make to the ENVIRONMENT dialog box settings. Using the Scale option, you can place certain views. Those views have their own scale parameters that you can change using the Modify option. When you modify them, only those views and their children change; the change does not affect the other views in the drawing.


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NOTES

DEFINING DRAWING TEMPLATES Drawing templates are provided by the system to automatically generate drawings of models. Drawing templates: •

Automatically create views.

•

Set desired view display.

•

Create snap lines

•

Show model dimensions based on the template.

Drawing templates contain three types of information for creating new drawings. •

Basic information

•

Instructions

•

Parametric notes –

– makes up a drawing but is not dependent on the drawing model. This information is copied from the template into the new drawing. – used to configure drawing views and the actions that are performed on that view, also to build a new drawing with a new drawing object (model). update to new drawing model parameters and dimension values. The notes are re-parsed or updated when the template is instantiated.

Use drawing templates to: •

Define the layout of views

•

Define tables

•

Set view display

•

Create snap lines

•

Place notes

•

Show dimensions

•

Place symbols



NOTES

Customizing Drawing Templates You can also create customized drawing templates for the different types of drawings that you create. The advantage of this is the template allows the creation of portions of drawings automatically. For example, you can create a template for a machined part versus a cast part. The machined part template can define the views that are typically placed for a drawing of a machined part. You can: •

Set the view display of each view.

•

Place company standard machining notes.

•

Automatically create snap lines for placing dimensions.

DETAILING THE DRAWING Detailing is important as a method for communicating design intent to machinists, mold makers, and other production personnel. Once the views are created on a drawing, showing the dimensions are usually just a click of a button. Therefore the redundancy involved in both the designer and the draftsman duplicating the same dimensions is eliminated. In manufacturing, additional dimensions in the drawing will need to be created to convey additional information. Once the driving dimensions in the drawing are in place, they are fully modifiable and changes are immediately reflected in the model. This associativity allows fast and efficient design development.


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NOTES

Creating Feature Dimensions Feature dimensions are created in the actual part and assembly models. In the drawing, they only appear in a single view to prevent double dimensioning. Feature Dimensions have many options: •

Show All

•

View

•

Feature

•

Feature & View

– Shows all dimensions for the model.

– Shows all dimensions of a selected view. – Shows the dimensions of a selected feature. – Shows all dimensions of a selected feature in a

selected view. •

Part

•

Part & View

– Shows the dimensions of a selected part. – Shows the dimensions of a selected part in a selected

view.

Creating Driven Dimensions Dimensions that you actually create in Drawing mode are known as Driven dimensions. To create them, click Create from the DETAIL menu and Dimension from the DETAIL ITEM menu; then select the desired geometry.

Modifying and Deleting Driven Dimensions In contrast to feature dimensions, you cannot modify driven dimensions in a production drawing because their values are based on the part model. However, you can delete them from a drawing.

Manipulating Dimensions Once you have displayed dimensions in a drawing, you can use options in the DETAIL menu to manipulate them in various ways: •

Use Move Text to relocate the dimension text along the dimension or leader elbow line.

•

Use Mod Attach to locate dimensions of rounds and chamfers on another reference of the same feature.

•

Use Switch View to move a dimension to another view.



NOTES

•

Use Flip Arrows to flip arrows inside or outside the extension lines.

•

Use Clip to clip extension lines to a selected location.

•

Use B r e a k to break an extension line.

•

Use Align to align dimensions.

Creating Drawing Notes Use the Note option in the DETAIL ITEM menu to create drawing notes by either typing them in or pasting from a text file. The NOTE TYPES menu allows you to specify leaders, text justification, and text styles.

Parametric Notes When you include a dimension or parameter in a note, it is referred to as a Parametric Note. To change a dimension value in a Parametric Note, choose Modify from the DRAWING menu and select the value. To specify parameter information, use the following format: •

Dimensions

•

Instance number

– &d#, where # is the dimension ID. – &p#, where # is the parameter ID (for example,

&p0). •

User-defined parameters

– &xxxxx, where xxxxx is the symbolic

name of the parameter


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NOTES

LABORATORY PRACTICAL Goal In this laboratory you create detailed drawings of solid parts and explore the associativity between drawings and part models.

Method In Exercise 1, you create a drawing of a gear part from a default template. You explore various options available and create additional views. In Exercise 2, you modify the views in the drawing in different ways and regenerate it to explore its associativity with the solid gear part. In Exercise 3, you retrieve the gear part drawing that you started earlier, manipulate its dimensions and create notes.

Tools Table 1: Drawing and Interface Icons

Icons

Description Select icon Wireframe display Dimension



NOTES

EXERCISE 1: Creating a Drawing

Fourth view Second view 3-D view from template

First view Third view

Figure 4: Completed Gear Part Drawing

Task 1.

Create drawing called gear from the default ptc_std template.

1. Click

.

2. In the NEW dialog box, click Drawing , type [gear], and click O K . 3. In the NEW DRAWING dialog box, click Browse in the Default Model section and browse to GEAR.PRT in \ intro_proe_320 \ 11_drwgs_drw_templates. 4. Click Browse in the TEMPLATE section and browse to PTC_STD.DRW as shown in the following figure.


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NOTES

Figure 5: The New Drawing Dialog Box

5. Click OK . 6. The drawing is created with the 3-D view automatically. Task 2. Create and orient the first view of the gear model using a general view. 1. Click V i e w s from DRAWING menu. 2. Click General > Done to accept the default selections in the menu manager. 3. Select in the drawing window towards the left for the general view. Do not be too concerned with the placement; you can move the view later. 4. Select DTM3 for the FRONT REFERENCE and DTM2 for the TOP REFERENCE in the ORIENTATION dialog box. 5. Click OK to finish view creation.



NOTES

Task 3.

Move the general view that you just created.

1. Click

from the INTENT MANAGER.

2. Select on the view to activate it and place it at a new location. 3. Experiment with moving the view. Finally, position the view toward the left side of the sheet. Task 4. Add the second view as a projection view using the general view as its parent. 1. Click Add View from the VIEWS menu. 2. Leave the defaults Projection > Full View > No Xsec > No Scale . 3. Click Done . 4. Place the projection view by selecting a location above the view you just added (General View) near the top of the sheet as shown in the first figure of this exercise. 5. Read the message area and note that there is a conflict in the parent view. Select the first view you added. Task 5.

Add the auxiliary view with a cross section displayed.

1. Click Add View > Auxiliary > Full View > Section > No Scale > Done . 2. Define a cross section through the entire view. Click Full > Total Xsec > Done . 3. Select a location to the lower right of the first view to place the cross section view. 4. Read the message area and select DTM4 as shown in the following figure.


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NOTES

Select DTM4

Figure 6: Orienting the Auxiliary Reference

5. The auxiliary view appears to the lower right of the general view. Note: This part has a previously created cross section named “C.” The system allows you to use cross sections that have been defined in part mode.

6. Select C from the XSEC NAMES menu. 7. Read the message area. 8. Now once again click on the general view you created. This displays the cutting arrow. 9. Click Done/Return from the VIEWS menu. Note: You can create cross sections in the drawing if you have a license for the optional add-on module Pro/DETAIL.

Task 6. Change the cross-hatching to improve its display on the drawing. 1. Click

in the INTENT MANAGER if its not already selected.

2. Select the cross-hatching line as shown in the following figure.



NOTES

Figure 7: Selecting Cross-Hatching

3. Click Edit > Properties. 4. Click Spacing > Half. 5. Click once again H a l f. 6. Click Angle > 0 > Done . The resulting modified cross-hatching is shown in the following figure.

Figure 8: The Modified Cross-Hatching

Task 7.

Add an isometric view.

1. Click Views > Add View > General > Scale > Done . 2. Select a location toward the upper right of the drawing to place the view. 3. Scale the view to [.75]. 4. Select DTM3 for FRONT REFERENCE and DTM2 for the TOP REFERENCE in the ORIENTATION dialog box. Do not close the dialog box.


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NOTES

5. If you make a mistake, click Undo . 6. Click Angles from the TYPE drop-down menu 7. Click Horizontal from the REFERENCE drop-down list. 8. Type [45] for the angle followed by Apply. 9. Click Edge/Axis from the REFERENCE drop-down list. 10. Select the vertical left edge of the gear. 11. Type [30] for the angle followed by Apply. 12. Finish the orientation. Click OK from the ORIENTATION dialog box.



NOTES

EXERCISE 2:Modifying Created Views and Testing for Associativity

Fourth view Second view 3-D view from template

First view Third view

Figure 9: Completed Gear Part Drawing

Task 1. Modify the display of hidden and tangent edges from the default settings. 1. Click Views > Disp Mode > View Disp from the MENU MANAGER. 2. Change the display of the projected and AUXILIARY view by selecting the SECOND view and the THIRD view shown in the preceding figure. Click Done Sel . 3. Click No Hidden > Tan Solid > Done from the VIEW DISP menu. 4. Change the display of the general and isometric views (First and Fourth views). Click the two views followed by Done Sel . 5. Cick Hidden Line > Tan Solid > Done .


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NOTES

6. Click [Wireframe display]. Click [Repaint]. Notice that there is no change in the display of the views. 7. Click

[Hidden line] to revert to hidden line display. Click

.

Task 2. Projected and auxiliary views are children of their parent view. Experiment with moving these view types 1. Click

in the INTENT MANAGER.

2. Select the PROJECTED view or SECOND view and move to new location. 3. Place the view. 4. Click Done/Return to return to the highest menu. 5. Now select the GENERAL view or FIRST view and move to new location. Observe how the PROJECTED view and SECTION views move in relation to the GENERAL view. Task 3.

Modify the scale value for the sheet.

1. Click Edit > Value and select the sheet scale value 1.000 on the lower left corner of the screen, shown in the following figure.

Figure 10: Modifying Drawing Scale

2. Type [.625]. 3. Change scale back to 1.000. Click Edit > Value , type [1.000]. 4. Save the drawing file. Do not erase the drawing. Task 4. Create a feature on the gear part to view the associativity between the part model and the drawing. 1. Click

and open GEAR.PRT.

2. Create a straight hole on the flat surface of the slot feature.



NOTES

Note: You can choose the dimension and attributes of the hole, since you are going to delete it later.

3. Activate the DRAWING window and select GEAR.DRW. Note that the hole appears in all of the views. 4. Return to the gear part. Click Window and select GEAR.PRT. 5. Delete the hole feature. Task 5.

Erase the drawing and the part without saving the hole feature.

1. Close the GEAR PART window. Click File > Close Window . 2. Activate the GEAR DRAWING window again. Click Window and select GEAR.DRW. 3. Save before erasing both files from memory. GEAR.DRW is used again in the next exercise. 4. Click Erase > Current > Select All > OK . The system erases the gear drawing. Note: Pro/ENGINEER does not automatically save to disk any change that you have made to the model. A simple way to revert back to the last saved version is to erase the model from memory without saving.


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NOTES

EXERCISE 3: Detailing the Gear Part Drawing

Figure 11: Detailed Gear Drawing with Dimensions

Task 1.

To begin the detailing process, show the model dimensions.

1. Retrieve the gear drawing GEAR.DRW. 2. Click View > Show/Erase . 3. In the SHOW/ERASE dialog box, click the SHOW BY options.

and select View in

4. Now select the lower left general view (First view) on the screen. Click Done Sel . 5. Close the SHOW/ERASE dialog box.



NOTES

Task 2.

Clean up the display of dimensions.

1. Click Tools > Clean Dims in the DETAIL menu. 2. Select the first view again; then click Done Sel . 3. Clear the Create Snap Lines check box. 4. Click Apply > Close . 5. Click Done/Return in the TOOLS menu. 6. Select the 76.66 dimension with the select cursor to another location.

and move it

7. Select other dimensions and adjust them similarly. 8. Click Task 3.

to repaint the screen.

Erase extra dimensions in the drawing

1. Click View > Show/Erase > Erase . 2. Click

.

3. Select the two extra 6.3mm dimensions shown in the following figure and click Done Sel from the GET SELECT menu.


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NOTES

Figure 12: Erasing Dimensions

4. Click Close . 5. Click

to view the results.

Task 4. Enable the display of dimensions for the section view and clean up their display. 1. Follow the same procedure to do this task as for the FIRST view. Task 5. Create a parametric note that displays the value of the pin hole diameter. Note: The system allows for notes to be displayed with the parametric dimension within the text. This allows the note to automatically update with changes in the dimensions.



NOTES

Figure 13: Creating a Parametric Note

1. Click Insert > Note . 2. Click Leader > Normal Ldr > Make Note leaving alone all the other defaults from the NOTE TYPES menu. 3. In the cross section view, select the edge of the small hole as the entity to which the system should attach the note. Use Query Sel , if necessary. 4. Select a location for the note. All the dimensions and parameters change to their symbolic form. 5. Look at the lower right or cross section view and identify the symbolic dimension representing the diameter of the small hole (for example: symbol:d26). 6. Select the ∅ symbol from the SYMBOL PALETTE window. 7. Type [&d26 drill thru ] in the message area, then press . 8. Type [one place] and press . 9. Save the drawing. 10. Click File > Close Window . 11. Click File > Erase > Not Displayed. Click OK


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NOTES


There are five primary Drawing View types—Projection, Auxiliary, General, Detailed, and Revolved.

•

General views are not dependent on any other view.

•

General views can have their own scale.

•

General views can be in any orientation and placed using the default view, and saved views from part mode.

•

Default datum planes should always be used to orient the first general view.

•

View types have four further sub-options: Full View, Half View, Broken View, and Partial View.

•

Views can be moved and deleted; their display modes can be changed and scale values modified.

•

The principle of associativity works between solid part models and their drawings.

•

Cross-sections can be created in part mode or drawing mode during view placement.

•

The majority of dimensions included on the drawing come from the part model.

•

There are two types of dimensions: Feature Dimensions and Driven Dimensions.

•

Dimensions can be manipulated.

•

Drawing notes can be created to provide other information and for documentation.




12 Duplicating Features: Patterns and Copy In this module you will learn how to duplicate features using Pro/ENGINEER. When creating complex parts and assemblies, often a need arises for duplication. The design intent in these cases specifies identical features or parts to be placed at separate locations in the same model.


Duplicate features using two different methods: Patterning and Copying.

•

Differentiate between Dimension Patterning and Reference Patterning.

•

Implement patterns with three different options: Identical, Varying, and General.

•

Specify different location options for the Copy feature.

•

Establish dependence among various copied features.

•

Use various copying techniques.

•

Select features for copying.

•

Specify the dependency of copied features.

•

Use the Transform option to duplicate surfaces and datum curves.

Page 12-1

NOTES

CREATING PATTERNS You can use patterns to create multiple instances of a single feature. The original feature that you base the pattern on is referred to as the “pattern leader.” There are two ways to define patterns: •

Increment the pattern leader’s dimensions.

•

Reference an existing pattern.

If you do not increment a dimension value, the system assigns the dimension value of the pattern leader to all instances in the pattern.

Patterning Benefits The patterning method of feature duplication offers numerous benefits: •

A pattern behaves as a single feature.

•

The pattern is parametric. Therefore, you can change pattern parameters and regenerate.

•

When you modify the dimensions of the pattern leader, the system automatically updates the whole pattern.

•

The system automatically groups all entities belonging to a pattern together in the model tree for ease of selection.

Pattern Types Dimension Patterns With dimension patterning, you increment existing dimension values of the leader in one or two directions to specify the pattern instances. If you use the second direction, the system takes all instances that are created by the first direction and increments them in the second direction.

Reference Patterns With reference patterning, you reference an existing pattern to define the locations of the new instances. This pattern type is only available if the leader feature for the new pattern references the leader feature of the existing pattern. This is illustrated in the following figure.



NOTES

Note: In contrast to a dimension pattern, the system does not provide parameters for the number of instances or increment values in a reference pattern. It obtains this information from the pattern that it references. A reference pattern updates automatically when the pattern that it references changes.

A reference pattern of a counterbore hole

Figure 1: Reference Pattern

Pattern Options There are three patterning options: Identical, Varying, and General.

Identical

Varying

General

Figure 2: Pattern Options

Pro/ENGINEER places certain restrictions on pattern options; these restrictions are listed in the following table.

For University Use Only - Commercial Use Prohibited Duplicating Features: Patterns and Copy

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NOTES

Table 1: Patterning Restrictions

Pattern Option

Regeneration Varying Speed Instances

Allowing Instance Intersections

Identical

Fastest

No

No

Varying

Moderate

Yes

No

General

Slowest

Yes

Yes

1st

1st 1st

II

I

III

Figure 3: Pattern Parameters

I

II

III

Figure 4: Pattern Parameters



NOTES

1st

1st

2nd

2nd

Figure 5: Pattern in Two Directions

A

B

Figure 6: Pattern in Two Directions

Creating Rotational Patterns To create a rotational pattern for a hole, you must increment an angular dimension using radial placement. However, for a sketched feature (such as a protrusion, cut, or rib), you must create an internal datum plane at an angle.


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NOTES

Figure 7: Rotational Pattern of a Sketched Feature



NOTES

Figure 8: Rotational Pattern of a Sketched Feature

Note: Do not use a sketched centerline to create the rotational dimension. A sketched centerline has no direction associated with it, so the pattern results may not be consistent.


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NOTES

COPYING FEATURES Once you have created a feature, it is often more efficient to reuse it rather than re-create it. Copying is an effective technique for duplicating multiple features. Once you have created a feature, it is often more efficient to reuse it rather than re-create it. Copying is an effective technique for duplicating multiple features. The Copy feature allows you to create new features by copying existing features to a new location. You must specify a location for the copy, Select the features to copy, and then establish dependence or independence for the copied feature’s dimensions.

Specifying Copy-To Locations To select a location for the copy, click one of these options from the COPY FEATURE menu: •

New Refs

•

Same Refs

•

Mirror

•

Move

– Specifies new feature references. You can retain each reference or click an alternate. – Retains the same feature references.

– Mirrors the features about a planar surface or datum plane.

– Specifies rotation and/or translation.

Copying Methods You can copy a feature by specifying new references, using the same references, mirroring, and moving. Using any of these techniques, you can specify whether the copy and the original features should share dimensions. Copying by Translating and Rotating Features

When copying a feature by translating or rotating it, you must specify a reference for the direction of translation or rotation: a plane normal; a straight curve, edge, or axis; or a coordinate system.



NOTES

Arrow shows positive rotation using the right-hand rule.

Figure 9: Rotation

Specifying Copied Feature Dependencies You can control the level of design intent that you capture in your model by making the copied features dependent or independent. •

–the system assigns each copied feature its own dimensions so you can modify them without affecting the original. Likewise, any changes that you make to the original do not affect the copy. Independent

Note: If you copy a feature from a different model or version, the system automatically makes the geometry independent.

Change to rib height does not affect others.

Figure 10: Independent Copies


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NOTES

•

– any dimensions that were unchanged at the time of the copy creation become dependent on the original feature. In this example, the two dimensions specified when the copy was made are independent. Changing one of them on the second rib only affects the second rib. The other dimensions are dependent, so changing the value affects both ribs. Dependent

Change to rib height affects all dependent features.

Figure 11: Dependent Copies

Tips & Techniques: If you create a copy as dependent, you can break that dependency using the Make Indep option in the MODIFY menu. You can make individual dimensions or the entire section independent.

Choosing Features to Copy To select which features to copy, select one of these options from the COPY FEATURE menu: •

Click

•

All Feat

•

FromDifModel

•

FromDifVers

– Selects features to copy from the current model.

– Selects all features in the current model. This option is available when you select Mirror or Move . – Selects the features to copy from a different model. This option is available when you select New Refs. – Selects the features to copy from a different version of the current model (for example, xxxx.prt.3 when the current model is xxxx.prt.5). This option is available when you select New Refs or Same Refs.



NOTES

Specifying Dependency Options To make the copied feature dimensions independent of their parent dimension, use the Independent option. Copies that you create using the FromDifModel and FromDifVers options are automatically independent. To specify that copied feature dimensions (that you have not changed) depend on the parent feature for their values, click the Dependent option. When you create a dependent copy, you can make the entire section or individual dimensions independent by clicking Modify and Make Indep.

Tips & Techniques: If you use the Mirror Geom option instead of Copy , you can mirror all of a model’s geometry about a plane without creating new features. The system adds a Merge reference to the Model Tree.

Before copy operation

3. Move copy

2. Same Ref copy

4 New ref copy 1. Original model

5. Mirror copies

After copy operation

Figure 12: Instances of the Copy Feature


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NOTES

LABORATORY PRACTICAL Goal The goal of this lab is to duplicate geometry using patterns and copy features.

Method In Exercise 1, you create a dimension pattern. To produce the end result, you pattern the cut and then modify the angle of the slot. In Exercises 2 and 3, you create a reference pattern and a rotational pattern respectively. In Exercise 4, you work on a model using the copy feature and mirror geometry options. In Exercise 5, you create mounting tabs on the steering column support shaft by using various copy options.


Icons

Description Hidden line display Datum Plane Datum axis



NOTES

EXERCISE 1: Creating and Modifying a Dimension Pattern

Start model

Model after patterning and modifying

Figure 13: Dimensional Pattern of a Cut

Task 1.

Open an existing part to be used for creating a pattern.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 12_duplication_features. 3. Click

and open DIM_PATTERN.PRT.

4. Click

[Hidden line].

Task 2.

Create a varying pattern of cuts.

1. Click Feature > Pattern and select the cut. 2. Click Varying > Done . 3. Select the 10 dimension on the cut. 4. At the prompt, type [4] as the incremental value between pattern members and press . 5. Click Done from the EXIT menu.


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NOTES

6. Type [12] as the total number of instances in this direction and press . 7. Click Done from the EXIT menu once again. Click Done from the FEAT menu.

Figure 14 Varying Pattern

Task 3. pattern.

Modify the angle of the leader to change the angle of the entire

1. Click Modify . Select the cut. Select the 45- degree dimension and type [-45] as the new value and press . 2. Regenerate the model. 3. Save the model and erase it from memory.



NOTES

EXERCISE 2: Creating a Reference Pattern

Finished Model

Start model

Figure 15: Reference Pattern

Task 1.

Start creating the reference pattern.

1. Open file REF_PATTERN.PRT. Task 2.

Create an identical pattern of holes in two directions.

1. Click Feature > Pattern and Select the hole. 2. Click Identical > Done . 3. Select the 20 dim ension and type [20] as the new value and press . 4. Click Done from the EXIT menu. 5. Type [3] as the total number of instances. 6. Now Select the 10 dimension and type [20] and press . 7. Since this is the only dimension that you are going to increment in the second direction, click Done from the EXIT menu. 8. Type [2] as the total number of instances in this direction.


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NOTES

Figure 16: Identical Hole Pattern in Two Directions

Task 3. Create a square cut on the leader feature of the pattern, so that you can create a reference pattern of it. 1. Click Insert > Cut > Extrude . 2. Click One Side > Done . 3. Select the top surface of the protrusion as the sketching plane. 4. Click O k a y from the DIRECTION menu. 5. Click Default for orientation. 6. Delete the current references in the REFERENCE dialog box. 7. Specify the axis A_1 as a reference. Task 4.

Sketch the section shown in the following figure.

1. Work on the leader figure shown, so that it can act as the reference feature later. 2. Sketch vertical and horizontal centerlines passing through axis A_1. This should be the only reference in the dialog box. Should you have selected any other references by accident, delete them. 3. Sketch a square centered on axis A_1 making sure Intent Manager makes the assumption of equal line lengths and symmetry.



NOTES

Figure 17: Section for Slot

4. Modify the width to 10mm. The model regenerates automatically. 5. Click

to exit from sketcher.

6. Remove the material to the inside of the cut by selecting O k a y. 7. Click Blind > Done . Type [2.5] as the depth value. 8. Complete the feature. Click OK . Task 5.

Create a reference pattern of the cut feature.

1. Click View > Model Tree , hold mouse over the feature Cut id 1205

and

. Select Pattern in the pop-up menu.

2. Define the pattern using the leader reference. Click Ref Pattern > Done . 3. Save the part and erase it from memory.


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NOTES

EXERCISE 3: Creating Rotational Patterns of Sketched Features Task 1.

Start creating the rotational pattern

1. Open BLOWER.PRT. 2. Click [Datum plane] and and axes.

[Datum axes] to display datum planes

Figure 18: Blower Base with Dimensions Shown

Task 2. Create a horizontal/vertical reference plane for sketching, with an angle associated with it. 1. Click Insert > Protrusion > Extrude . 2. Click One Side > Done . 3. Select the top face of the disk as the sketching plane for blower blades. 4. Click Okay to accept the default direction. 5. Click Bottom from the SKET VIEW menu. 6. Click Make Datum from the SETUP PLANE menu. 7. Click Through ; then Query Sel to Select axis A_1.



NOTES

8. Click Angle , then Select DTM3 and click Done . 9. Click Enter Value and type [30]. 10. Specify the references as the outer edge of the circular protrusion and the datum you just created. Make sure you do not specify DTM3 or DTM1 as a reference. 11. Sketch the section as shown in the following figure. Make sure that the bottom straight edge has a constraint of perpendicular to the outer edge of the base protrusion. Pick Datum for horizontal reference

Section

Figure 19: Sketching the Section

Tips & Techniques: To help aid you in your sketching, you should sketch your sections large, then modify the dimensions to change the size of the model.

12. Add the dimensioning scheme as shown in the following figure. Modify dimensions to the values specified and then click [Done]. 13. Accept the default Blind > Done . 14. Type [73.5] as the protrusion depth value.


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NOTES

Figure 20: Sketch of Blower Blade

Task 3. Pattern the blower blade protrusion in one direction using a varying pattern.

1. Select in model tree the protrusion you just created, Pattern .

>

2. Click Varying > Done . 3. Select dimension 30. 4. Type [60] as the increment value and press . 5. Do not define any other dimensions to increment. Click Done . 6. Type [6] as the number of instances for the pattern. 7. Do not create instances in the second direction. Click Done from the EXIT menu. 8. The final pattern of blades is as shown in the following figure.



NOTES

Pattern angle

Original angle Figure 21: Pattern of Blades

9. Close the window.


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NOTES

EXERCISE 4:Copying Features

Finished model

Start model

Figure 22: Copying Features Task 1.

Retrieve an existing model and copy some of the features.

1. Open the part file FEATURE_COPY_MIRROR.PRT. 2. Change the display to hidden line. Task 2. You can make copies either independent or dependent. The selection you make will be based on you design intent. Create a dependent copy of the lower right slot. 1. Click Feature > Copy. 2. Click Same Refs. 3. Click Dependent > Done . 4. Select the slot. Click Done from the SELECT FEAT menu. 5. Select the Dim 1 and Dim 3 check boxes, which are the 45-degree angle and the 65-inch dimension respectively. Click Done . 6. For Dim 1, type [0.00] and press . 7. For Dim 3, type [410.00] and press . 8. Click OK.



NOTES

9. Click Done twice to return to the highest level menu. Task 3. Experiment with modifying dimensions; then make the copy independent of the parent slot. 1. Click Modify and select the parent slot. 2. Select the 125.00 dimension, type [75.00] as the new value, and regenerate. 3. Modify the length of the slot back to 125.00, as described in the previous step. 4. Modify the 45-degree angle of the parent slot. Type [30.00]. Note that the angle of the copy does not change because you broke the dependence of that dimension when you modified it to create the copy. 5. Change the angle of the parent slot to back to 45 degrees. Task 4.

Break the dependency between the two slots.

1. Click Modify > Make Indep from the MODIFY menu. 2. Click Section from the MAKE INDEP menu. 3. Select the copy and click Done Sel and Done . 4. All of the copy’s dimensions are now independent of the parent slot. Task 5. You have the ability to mirror the entire model by using various options. Mirror all of the features to complete the part using Copy. 1. Click Feature > Copy from the FEAT menu. 2. Click Mirror > All Feat > Independent from the COPY FEATURE menu; then click Done . 3. Select DTM1. 4. Save the model and erase it from memory.


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NOTES

EXERCISE 5: Building the Steering Column

Figure 23: Steering Column Support Shaft

Task 1. Create a copy of the first tab at the bottom of the shaft 90 degrees to the first. To do this, use a move type copy. 1. Open STEERING_COLUMN.PRT. 2. Show axes and datum planes if the system is not already showing them. 3. Click Feature > Copy > Move > Select > Dependent > Done . 4. Select the protrusion, axis, hole, and round features that compose the first tab in the Model Tree; then click Done Sel > Done .

Round

Protrusion

Axis and hole

Figure 24: Features to Copy

5. Click Translate . 6. Toggle

to show datum planes and Select FRONT datum.



NOTES

7. Flip the arrow so that it is pointing in the appropriate direction. Click O k a y.

Figure 25: Translation References

8. Type [7.5] as the translation value. 9. Click Rotate > Crv/Edg/Axis. 10. Select axis A1 as the motion reference for the rotation. (Toggle if the axes are not visible.) 11. Point the arrow as shown in the following figure and click O k a y to accept direction. 12. Type [90] as the rotation value.

Figure 26: Rotation Direction

13. Click Done Move to complete the move. 14. Select the 2.0 length dimension and click Done from the GP VAR DIMS menu to complete definition of the feature.


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NOTES

15. Click OK . Task 2.

Mirror the copied tab about the SIDE datum.

1. Click Feature > Copy > Mirror > Dependent > Done . 2. Select the COPIED tab from the Model Tree. Click Done . Note: Because the system placed the copied tab features in a group when it copied them, you can select them as a single item.

3. Mirror the tab about the SIDE datum plane.

Figure 27: Mirrored Tab

Task 3. Make the original tab longer, and thicken the tab for strength. Because the other two tabs are dependent copies, break their dependency to create a thickness that is different from that of the original. 1. Click Modify . Select the protrusion (protrusion id 50) of the original tab. 2. Change the 2.00 length to 3.00 and the 0.25 thickness to 0.375. 3. Regenerate the model. 4. Notice that the two copied tabs also change thickness. They do not, however, change length. This is because when you copied the first one, you gave it a new length, which automatically made the length dimension independent.



NOTES

Task 4.

Break the thickness dependency between the tabs.

1. Click Modify > Make Indep > Dimension . Select the protrusion ID 50 again and the 0.375 thickness dimension. 2. Select the features to make the dimension independent. Notice the 2 highlighted copied tabs that are current and dependent. 3.

Select both of the copied tabs from the model. Click Done Sel > Done Sel .

4. Modify one of the copied tabs. Type [0.125] as the thickness. Type [60] as the new value for the 90-degree rotation angle; then regenerate. 5. Save the model.

Figure 28: Finished Steering Column Support Shaft



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NOTES


Duplication is important for capturing design intent and Pro/ENGINEER enables it through Pattern and Copy.

•

Patterning is of two kinds: Dimension Patterning and Reference Patterning.

•

There are three Pattern options: Identical, Varying, and General.

•

In the Rotational Pattern for a hole, the angular dimension must be incremented using radial placement.

•

Dependence/Independence can be established between copied entities.

•

Copies of part geometry can be created using Move and Mirror.




Module

13 Creating Assemblies In this lesson you learn how to create a functional assembly of solid components.

Objectives In this module, you will learn to: •

Create assemblies.

•

Modify assemblies.

P age 13-1

NOTES

OVERVIEW To create an assembly you must join components (parts) by selecting surfaces and features. There are several things to consider when building assemblies: •

Always begin an assembly with a base component, a component that you are unlikely to remove from the assembly later on.

•

Consider how you might break down the assembly into separate subassemblies.

•

Begin your assembly with default datums.

•

Add the first part or subassembly onto the default assembly datums.

Figure 1: Assembly Default Datum Templates

The Surface Normal Vector A surface normal vector is an imaginary vector that is perpendicular to the model surface. Pro/ENGINEER can distinguish between the outside surface and inside surfaces that comprise your solid models.



NOTES

Figure 2: A Model’s Surface Normal Vectors

Constraining Component Parts Placement constraints create parent/child relationships between the assembled components and the new component that you want to add. The following is a list of commonly used constraints: •

– Normal vectors of selected surfaces point in opposite directions and become co-planar. Mate

Figure 3: Mate Constraint

•

Mate Offset –

Normal vectors of selected surfaces point in opposite directions and are offset by a specified negative or positive value.

For University Use Only - Commercial Use Prohibited Creating Assemblies

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NOTES

Offset

Figure 4: Mate Offset Constraint

•

– Normal vectors of selected surfaces point in the same direction and are made co-planar. Align will also make two axes co-axial. Align

Note: Pro/ENGINEER does not associate any direction to the alignment of an axis.

Figure 5: Align Constraint

– Normal vectors of selected surfaces point in the same direction and are offset by a specified negative or positive value. Align Offset



NOTES

Offset

Figure 6: Align Offset Constraint

•

– Selected surfaces, utilizing their normal vector, point in the same direction and are parallel. Orient

Figure 7: A Usable Reference for Orient Constraint

•

– Selected cylindrical surfaces of revolution become co-axial. These surfaces do not need to be full 360-degree cylinders, as shown in figure below. Insert

Surfaces of revolution

Figure 8: Insert Constraint


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NOTES

Placing Components All the constraints, such as mate , align , insert , and coord sys, are available in a single component placement dialog box. As shown in the next figure, this allows for efficient component placement workflow.

Figure 9: The Component Placement Interface

The following features are available from the Component Placement dialog box: •

A consolidated list of assembly constraints beginning with Automatic provided as a drop-down list

•

A Flip button to reverse a component by 180 degrees

•

An editable offset value in the constraint list

•

A toolbar at the top of the dialog box that allows you to: Control whether the new component appears in the Assembly window or new window



NOTES

Toggle between the Constraint Placement and Move dialog box options Fix component or place it in the default position Access Component Interfaces Change Preferences

Packaging Under-Constrained Components Under-constrained components are those components which are not completed oriented into the assembly. This means that there is some ambiguity in the component placement that Pro/ENGINEER cannot resolve. This situation can be resolved with packaging. Packaging allows you to: •

Add components to an assembly without fully constraining them.

•

Add components to an assembly without defining its true or final location.

•

Allocate space in an assembly for components that will be added at a future time.

Over-Constrained Components When you over-constrain a component, you add more constraints than is necessary in order to capture additional design intent.

MODIFYING ASSEMBLIES Since Pro/ENGINEER is associative, you can make changes to all components in sub-assemblies while working in the assembly. However, the system limits the scope of those changes through the MOD ASSEM menu options listed below: •

Mod Dim

•

Mod Assem

allows you to modify any dimension in the assembly. allows you to modify only the top-level assembly

dimensions. •

Mod Subasm

•

Mod Part

allows you to modify any subassembly in the top-level assembly, which includes assembling components into the subassembly. allows you to modify parts in the assembly, which includes modifying dimensions, redefining existing features, adding new features, as well as most operations that you can perform at part level.


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NOTES

Note When creating part features at the assembly level, you should use caution to avoid creating unwanted parent/child relationships between the part and the assembly.

Modifying Your Design Intent You can modify your design intentions with the following commands: •

Reorder

•

Insert Mode

•

Reroute

•

Delete

•

Suppress

•

Resume

– Changes the order in which the system regenerates components in the assembly. – Inserts a component in between two components in the regeneration cycle of the assembly. – Changes the external references that a component has for constraints. – Removes components or assembly features from the assembly model. – Temporarily removes components from the assembly.

– Resumes components in the assembly model.

Saving Assemblies When you save an assembly, the system automatically saves any changes that you made to any of the parts in that assembly.

Note: If you rename a part in an assembly, but the assembly is not in RAM, the placement fails when you retrieve that assembly.

OTHER ASSEMBLY OPTIONS Generating Bills of Material Bills of Material (BOMs) are lists of sub-assemblies and components, including component quantities. With Pro/ENGINEER you can generate BOMs with the Info pull-down menu.



NOTES

Creating Exploded Views Using the Explode option in the View pull-down menu, you can create exploded views of the assembly model.

Note You cannot assemble components in an exploded view. If you try to do so, the system asks you to unexplode the assembly using the Unexplode option in the View pull-down menu.

Figure 10: Unexploded Machine Assembly

Figure 11 Exploded Machine Assembly


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NOTES

LABORATORY PRACTICAL Goal In this exercise you will learn how to create and modify assemblies.

Method In Exercise 1, you will assemble existing components into a subassembly by using the insert, mate, and align constraints from the component placement interface. In Exercise 2, you a machine crank assembly by using the subassembly created in Exercise 1.

Tools Table 1: Assembly Icons

Icons

Description Assemble component at default location Show component in separate window Specify new constraint Remove selected constraint Change orientation of constraint (flip)



NOTES

EXERCISE 1: Create a Subassembly of Three Parts

Figure 12 Completed Base Subassembly

Task 1.

Start creating the subassembly.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 13_creating_assemblies. 3. Click . Select Assembly and type [BASE] as the name. Make sure Use default template is checked. 4. In the menu manager, click Set Up > Units. > millimeter Newton Second > Set.

5. Click OK > Close . 6. Scroll the menu down by clicking the blue arrow and then click Done to return to the high-level menu. Task 2.

Assemble the bracket part.

1. Click Component > Assemble and open BRACKET.PRT from your working directory. 2. In the COMPONENT PLACEMENT dialog box, click [Assemble at default location].


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NOTES

3. Click OK . Task 3.

Begin to assemble the bushing part to the bracket part.

1. Click Component > Assemble and open BUSHING.PRT. 2. Toggle off the datum planes.

Figure 13: Assembly of the Bushing

Task 4. Insert the bushing into the bracket using the revolved surfaces on the models. 1. The default constraint type is Automatic in the COMPONENT PLACEMENT dialog box. 2. Click Insert from the drop-down list. 3. Select on the outside cylindrical surface of the bushing part and again on the inside revolved surface of the slot on the bracket part, as shown in the following figure.



NOTES

Figure 14: Selecting Component References for Insert

Task 5.

Mate the lip on the bushing to the back of the bracket.

1. Click Mate from the CONSTRAINT TYPE drop-down list. 2. Select on the planar flange surface on the bushing, pointed by the cursor in the following figure.

Figure 15: Selecting References for the Mate Constraint

3. Select the back surface of the bracket using Query Sel , highlighted in the preceding figure. Click Accept when the proper surface highlights.


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NOTES

4. Type [0 ] for the offset value and press . 5. You will see the results of the mate constraint. 6. Now click [Change orientation of the constraint]. You will notice that the bushing gets flipped. 7. Click

once again to the original position.

Task 6. Add a third Align constraint so that the key on the bushing lines up with the d slot in the bracket.

1. Click

[Show component in separate window].

2. The bushing part is shown in a separate window. 3. Click to add another constraint. Select the bushing key as shown in the following figure.

Figure 16: Selecting References for the Align Constraint

4. Now Select on the top surface of the bracket as shown. 5. Accept the default offset value near the message area. 6. But you don’t actually need this offset. So click on the offset value in the COMPONENT PLACEMENT dialog box to get a drop-down list.



NOTES

Figure 17: Orienting the Bushing to the Bracket

7. Click Align for the constraint type and O r i e n t e d for the offset and click OK . 8. The subassembly is fully constrained. Note: You can always delete constraints you have created by clicking and specify a new constraint by clicking .

Task 7.

Assemble the ring part to the bushing part using constraints.

1. Turn off the display of the datum planes. 2. Click Assemble ; then select RING.PRT 3. Zoom in on the bushing model so that you can see the snap ring groove more clearly, as shown in the following figure.

Figure 18: Base Zoomed In


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NOTES

Insert references

Mate references

Figure 19: Constraints for Assembling Base with Ring

4. Add an insert constraint between the inner revolved surface of the snap ring and the small, revolved surface of the recess in the bushing. 5. Add a mate constraint between the front side surface of the base and the back of the snap ring, as shown in the preceding figure. Type [0] followed by as offset. 6. Click to add another constraint. Orient the tabs so they match the orientation of the flat of the bushing. Select on the surfaces shown in the following figure.



NOTES

Figure 20: Aligning Snap Ring to the Flat of the Bushing

7. Click Align for the constraint type and O r i e n t e d for the offest in the COMPONENT PLACEMENT dialog box. 8. Click OK . 9. Click

and close window.


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NOTES

Exercise 2: Create the Machine Assembly Task 1.

Start creating the new assembly.

1. Click , select Assembly and type [MACHINE] as the name. Uncheck Use default template option. Select Empty for the template and click O K . 2. Setup the assembly to use millimeter units. Click Set Up >Units > millimeter Newton Second > Set > OK > Close . 3. Click Insert > Datum > Plane to create three default datum plane features. Task 2. Assemble the base assembly into the machine assembly using the datum planes. 1. Click Component > Assemble ; then open BASE.ASM. 2. Assemble the base subassembly to the machine assembly by clicking Task 3.

[Assemble at default placement].

Assemble the shaft component by using constraints.

1. Assemble the MASTER_SHAFT part into the machine assembly. 2. Insert the shaft into the hole in the bushing.

Figure 21: Selecting References for Align Constraint



NOTES

3. Create an Align constraint between the end surface of the shaft and the bracket surface. 4. Specify an offset value of [100 ] and press . Task 4. Add the crank part to the assembly by using the assembly constraints.

Figure 22: Assembling the Crank Part to the Machine Assembly

1. Assemble the crank part. 2. Insert the crank into the shaft.

Figure 23 Assembled Crank

3. Align the small hole on the crank with the small hole on the shaft by Selecting the axes. 4. The system says it is fully constrained, but orient the back of the crank with the end of the shaft.


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NOTES

Task 5.

Assemble the gear component to the machine.

1. Assemble the gear part into the assembly using constraints similar to those that you used for the crank part. 2. Save the assembly. Task 6. While working at the assembly level, accommodate a change in the design intent by modifying the bracket width. 1. Click Modify from the ASSEMBLY menu. 2. Click Mod Part from the ASSEM MOD menu. 3. Select the bracket part. 4. Select the base feature to display the dimensions. 5. Select the 25 dimension. Type [50.0], then press . 6. Regenerate only the part model. Task 7. Accommodate another change in the design intent by adding an edge round on the two top edges of the bracket. 1. Create a new part feature. Click Feature > Create . 2. Add a simple edge round to the bracket with a 20mm unit radius. shows the modified bracket.

Figure 24: Modified Bracket



NOTES

Task 8.

Generate a Bill of Materials for this assembly.

1. Click Bill of Materials from the INFO pull-down menu. Click O K . 2. Read the entire INFORMATION WINDOW; use the scrollbar if necessary. 3. Click Close from the INFORMATION WINDOW 4. Close the working window. 5. Erase all models that are not displayed. Click File > Erase > Not Displayed.


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NOTES


Assembly creation has to begin ideally with base components and these usually are the Default Assembly Datums.

•

There are various constraint options for adding new components to an assembly.

•

Components of an assembly can be deliberately under-constrained or over-constrained.

•

Packaged or under-constrained components are usually added to assemblies to get a spatial feel for the completed assembly. Once the look is right, the component can be fully constrained.

•

Over-constraining occurs to capture additional design intent.

•

Since Pro/ENGINEER is associative, you can make changes to all components and sub-assemblies while working in an assembly.

•

Modifying parts at the assembly level is adopting a top-down approach to design. Sometimes this is necessary to capture the higher level design intent by creating part geometry in the context of the assembly.

•

You can extract a Bill of Materials of an assembly.

•

You can create exploded views of assemblies.




14 Principles of Top-Down Design In this module you will learn the principles of top-down design. Robust models can be built only by the rigorous implementation of the principles of top-down design.


Describe the principles of top-down design.

•

List the advantages of top-down design.

•

Describe the Pro/ENGINEER tools that support the top-down design process.

•

Study reference control in relation to the top-down design approach.

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NOTES

INTRODUCTION Definition Top-down design is a method of designing a product by capturing toplevel design criteria first and then passing this information from the top level of the product’s structure to all related subsystems.

Stages of Top-Down Design •

Planning

•

Creating product structure

•

Sharing design-critical information

•

Capturing interactions between individual components

The Approach Top down design can be conceived as an ongoing process of capturing, communicating, and managing design information. It is the best methodology to harness and control Pro/Engineer’s associative design tools when conceptualizing and building large assemblies.

Figure 1: Top-Down Design Architecture


Pro/ENGINEER Advanced Top-Down Design

NOTES

Comparing Top-Down Design to Traditional Approaches In Top-down design the distribution of information happens from top design levels to lower design levels. Design Information

Component

Component

Component

Figure 2: Distribution of Information from Top to Bottom

In the traditional assembly design approach, an engineer designs individual components independent of the assembly, using a manual approach to ensure that components fit properly and meet design criteria.

Component Design

Component Design

Component Design

Assemble Components

Figure 3: Traditional Design Approach

Characteristics of the Traditional Design Approach •

The designer places components in subassemblies and then brings those subassemblies together to develop the top-level assembly.

•

Often, after creating the assemblies, a designer discovers that the models do not meet the design criteria (for example, a critical interface on two models does not match).

•

After detecting problems, the designer manually adjusts each model.

•

As the assembly grows, detecting these inconsistencies and correcting them consume a considerable amount of time.

For University Use Only - Commercial Use Prohibited Top-Down Design Overview

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NOTES

Benefits of Top-Down Design Methodology Top-down design methodology has many advantages. It can be used to manage large assemblies, organize complex designs, control motion and support more flexible assembly designs. This methodology can be used to manage large assembly designs by allowing the user to retrieve only the skeleton structure of the assembly into memory and make desired changes. The skeleton contains the important criteria of a design such as mounting locations, space requirements for subsystems and parts, and design parameters such as critical dimensions. Changes can be made to the skeleton and these changes will be propagated to the subsystems of the entire design. Top-down design organizes and helps enforce the interactions and dependencies between components of an assembly. Many interactions and dependencies exist in an actual assembly design and it is desirable to capture these in the model of the design. An example of a desirable dependency is the location of a mounting hole in one part and the corresponding location in another part. Therefore, if one of the mounting hole locations is moved, the corresponding mounting hole on the mating part also moves. Tools exist in Model Tree design to enable users to capture desirable dependencies while limiting undesirable ones. An organized assembly structure allows information to be shared between different levels of an assembly. If a change is made at one level, it is shared among all of the other related assemblies and/or components. This supports a team environment where different groups or individuals own different subsystems and components. Furthermore, a complex assembly design may be divided easily into separate tasks to be assigned to the different team members in the early stages of a design.

THE SIX STEPS OF TOP-DOWN DESIGN •

Defining Design Intent

•

Defining Preliminary Product Structure

•

Introducing Skeleton Models

•

Communicating Design Intent

•

Continued Population of the Assembly

•

Managing Part Interdependencies



NOTES

Step 1 - Defining Design Intent All products are designed with some preliminary planning. Sketches, ideas, proposals and specifications may exist to define the products' purpose, function and design. This planning helps the designer understand the product better and start the design of the system and/or detailed components. The designer can leverage this information to begin defining the structure of the design and detailed requirements of individual components within Pro/ENGINEER.

Step 2 - Defining Preliminary Product Structure The product structure consists of a list of components and their hierarchy within the assembly design. Many of the major subsystems required for the design will be determined when defining design intent. The product structure can be created easily in Pro/ENGINEER allowing the creation of subassemblies and parts without having to create any geometry. Existing subassemblies and parts can also be added to the product structure without actually having to be assembled. Defining the preliminary product structure helps to organize the assembly design into manageable tasks that can be assigned to design teams or individual designers.

Step 3 - Skeleton Models Skeleton models act as a 3-D layout of the assembly and may be used to represent space requirements, important mounting locations, and motion. Also, they can be used to share design information between subsystems and act as a means to control the references (or interactions) between these subsystems. Skeleton models serve a variety of purposes defining form, fit, and function of an assembly. Some examples are: •

Space claim (form / fit)

•

Component to component interface definition (fit)

•

Motion representation (function)


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NOTES

Step 4 - Communicating Design Intent Top-level design information such as important mounting locations and space claim requirements can be placed in the top-level assembly skeleton model. This information then can be distributed to the appropriate subassembly skeleton models as needed. This allows for each subassembly to contain a skeleton model with only the pertinent design information for that subassembly. This means that the subassembly design team can work confidently on their own design since they have local access to the toplevel design criteria. Consequently, many separate design teams can be working on their subassembly and referencing the same top-level design information. The result is an assembly developed concurrently that fits together the first time. The recommended Pro/ENGINEER tool for storing design intent at different levels of the product structure is the skeleton model. Various data-sharing features such as Copy Geometry and Shrinkwrap can be used to communicate and propagate the design intent from level to level and from model to model.

Step 5 - Continued Population of the Assembly Once the skeletal representation of the assembly has been defined, and the top-level design criteria have been distributed, individual component design can begin. Many methods exist for populating the assembly structure with detailed parts. Existing components can be assembled, or components can be created in the context of the assembly. These individual parts can be related to each other using other functionality such as assembly relations, skeleton models, layouts, and merge features to further capture design intentions.

Step 6 - Managing Part Interdependencies One of the greatest benefits of parametric modeling is the ease with which designs can be changed. Methods can be used to manage the many desired interdependencies between components of a design in an organized manner. Managing interdependencies allows components from one design to be used in another and provides a means for controlled change and update of the entire assembly design.



NOTES

Tools exist in Pro/ENGINEER to help guide users in setting up the dependencies between parts and subassemblies that will propagate the desired changes throughout the entire design. Reference control can be configured to limit undesired dependencies and allow desirable ones. Furthermore, a Global Reference Viewer tool has been provided to help users investigate and understand existing interdependencies between components.

Note: As the design evolves and the designers are able to obtain more information about the design, they may need to further define the design intent, edit the skeletons, pass the critical data to other models and continue to populate the assembly. This is an iterative process—one in which the design becomes more detailed and specific throughout the project. You should, therefore, expect to perform the sequence of steps listed above more than once in order to complete the project.

PRO/ENGINEER TOP-DOWN DESIGN TOOLS The following Pro/ENGINEER tools enable you to successfully capture design intent using the top-down design approach:

Layouts Layouts are central locations in which you can capture non-geometrical top-level design criteria. A layout is an especially useful tool in cases where you do not have exact information about the geometry. Dimensions, parameters, and relations defined in a Layout can be parametrically linked to skeletons or part models.


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NOTES

Figure 4: Layout for a Race-Car Model

Figure 5: Using Layouts as a Top-Down Design Tool

Skeletons Skeletons are central locations in which you can capture geometrical central design information for a model. You can use skeleton models to represent the design information in a layout in a 3-D representation. There are three typical uses for skeletons: •

Space claim (form / fit)



NOTES

Figure 6: Using Skeletons for Space Claimes

•

Component to component interface definition (fit)

Figure 7: Using Skeletons for Fit

•

Motion representation (function)


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NOTES

Figure 8: Using Skeletons for Motion Representation

Data Sharing Features •

Publish Geometry – A Pro/ENGINEER feature that allows a

designer to document the design information, making it easier for others to later use the Copy Geometry function.

Figure 9: The Publish Geometry Dialog Box

•

Copy Geometry – A Pro/ENGINEER feature that allows you to

transfer design information such as surfaces, datum planes, and datum axes from one model to another.



NOTES

Figure 10: Accessing the Copy Geometry Feature

•

– A Pro/ENGINEER feature that allows you to ‘shrinkwrap’ a model or assembly with a surface, thereby dramatically reducing regeneration time in the recipient model. Shrinkwrap


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NOTES

Figure 11: Accessing the Shrinkwrap Feature

Managing References / Interdependencies Two functions that help the user in the sixth and ongoing step of top-down design are Reference Control and the Global Reference Viewer

Reference Control The Reference control dialog box allows users to define the allowable scope for external references that the system will create. This function is particularly useful when designing in an assembly, or when creating Copy Geometry features.



NOTES

Figure 12: Reference Control Dialog Boxes


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NOTES

Global Reference Viewer The Global Reference Viewer is a very powerful tool that gives you the ability to find any type of external reference between models in an assembly. This tool is useful to ensure that only desired references have been created, or for troubleshooting of existing assemblies.

Figure 13: Model and Global Reference Viewer Dialog Boxes



NOTES


Top down design can be conceived as an ongoing process of capturing, communicating, and managing design information.

•

There are six steps in the Top-Down Design process: Defining Design Intent, Defining Preliminary Product Structure, Introducing Skeleton Models, Communicating Design Intent, Continued Population of the Assembly, Managing Part Interdependencies.

•

Layouts, Skeletons, Publish Geometry, and Copy Geometry tools enable the Top-Down Design approach.

•

Managing references and interdependencies using reference control options and the global reference viewer are an important part of the ongoing cycles of working in models built with the Top-Down Design principles.


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15 Additional Datum Features and Skeletons In this module you learn how to create additional datum features like datum axes, datum curves, datum points, and datum coordinate systems. In addition you will be introduced to skeleton features and their uses.


Describe all available additional datum features in the software

•

Create additional datum features using different methods.

•

Employ additional datum features as robust references for solid geometry

•

Create a basic skeleton feature

Page 15-1

NOTES

ADDITIONAL DATUM FEATURES Datum features are mass-less, non-solid features that can be used as references and as parents to solid geometry. All datum features serve the purpose of construction type geometry.

Datum Axes Datum axes appear as dashed yellow lines that often have name-tags such as A_1 , A_2 , and A_3 .

Uses •

As centers of coaxial holes

•

As references for assembly constraints

•

As aids for the creation of other datum features

Methods of Creation •

Thru Edge

•

Normal Pln

•

Pnt Norm Pln

– Created through a straight edge of the model

– Normal to a selected surface with linear dimensions to two references – Normal to a selected surface and though a datum

point •

Thru Cyl

•

Two Planes –

•

Two Pnt/Vtx

– Created through the “imaginary” center of any surface of revolution Created at the intersection of two planes

– Created through two datum points or two vertices of

the model •

Point on Surface

•

Tan Curve

– Goes through a point normal to the surface

– Created tangent to a datum curve or at the end point of a model’s edge

Datum Curves Datum curves appear on the model as orange lines. They can be straight or curved and open or closed loops.



NOTES

Uses •

As trajectories for swept features

•

To help define the shape of assembly skeletons

•

To aid in surface creation

•

To measure features of a model


Sketch

– Uses sketcher functionality to create the curve on a flat

surface. •

Intr . Surf

•

Thru Points

•

Projected

•

Formed

•

2 Projection

•

From Equation

– Creates a curve at the intersection of two surfaces. – Create a curve through a series of datum points.

– Projects a 2D curve onto a solid surface.

– Transfers a datum curve onto a surface as a formed curve. The formed curve preserves the length of the original curve. – Creates a projected datum curve from two sections on non-parallel sketching planes. – Creates a curve based of mathematical equations.

Datum Points Datum points appear as small yellow “x ”s on the model, with name tags such as PNT1

Uses •

Help in creating datum curves and datum axes.

•

Used when creating holes that are placed on point.

•

Used as references for assembly constraints.


On Surface

•

On Vertex

•

Offset Csys –

•

At Center

– Creates a point on a selected surface using linear dimension to two references – Point is defined at a vertex on the solid model

Points are defined offset from a coordinate system using Cartesian, cylindrical, or spherical coordinates – Creates a point at the center of an arc or a circle

For University Use Only - Commercial Use Prohibited Additional Datum Features and Skeletons

P a g e 1 5- 3

NOTES

•

•

– Creates a point along a datum curve or model edge with the following dimensional options. On Curve

Offset – Places a point on the curve offset at a distance from a planar surface.

– Places a point on the curve as a percentage of the overall length (0.0 and 1.0 are the start and end points of the curve). Length Ratio

Actual Length – Places the point using the actual arc length distance of the curve. Field Point – Places a free-floating point on a selected reference such as a surface or a curve.

Datum Coordinate Systems Datum Coordinate Systems appear yellow on the model and usually have nametags, such as CS1. Each axis on the coordinate system is also labeled (x,y,z).

Uses •

Ability to define a zero position for datum points read in from file.

•

Orientation for manufacturing procedures.

•

References for assembly constraints.


3 Planes

•

Pnt + 2Axes –

•

2 Axes –

•

Default

– Origin at the intersection of three planes.

Origin at a datum point, vertex, or origin of another datum coordinate system. Origin at the intersection of two axes, straight edges or straight datum curves. – Origin at the first vertex of the base feature.



NOTES

LABORATORY PRACTICAL Goal The goal of this lab is to create additional datum features and use them as references to solid geometry.

Method In Exercise 1, you start with the default datums and a datum coordinate system included in any new part. Then you create datum points and a datum curve to create a door handle. In Exercise 2, you use several datum features to create a simple skeleton. In Exercise 3, you open and ‘flex’ an assembly with a skeleton.

Tools Table 1: Additional Datum Features

Icons

Description Insert datum coordinate system Insert datum points Insert sketched curve Insert datum curve Insert datum axis


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NOTES

EXERCISE 1: Creating Additional Datum Features. Task 1.

Create a new part and define the control points for the handle.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 15_addtl_dtm_feats_skels . 3. Create a new part with the name DOOR_HANDLE. Task 2. Since we already have a coordinate system, we will create points at x, y, z positions relative to it. 1. Click

[Insert datum points] from the sidebar and click Offset Csys from the DATUM POINT menu.

2. Select the PRT_CSYS_DEF coordinate system from the model tree. 3. Click Cartesian as the coordinate type. 4. Click Enter Points and type [0] for x, [0] for y, and [0] for z. Task 3. Once the first datum point’s x, y, z positions have been defined, enter in the x, y, z data for the other points. 1. Create a second datum point at 4,0,0. Enter [4], [0], [0] at the prompt. 2. Create a third datum point at 4,16,0. Enter [4], [16], [0] at the prompt. 3. Create a fourth datum point at 0,16,0. Enter [0], [16], [0] at the prompt. 4. Once the coordinates of the last point have been entered, type on a blank line. 5. Click Done to complete the feature. The part should look as shown in the following figure.



NOTES

Figure 1: Datum Points

Task 4. Create a datum curve through these points. The order the points are created does matter because the curve will connect them in that order. 1. Click Task 5. point.

[Insert datum curve], click Thru Points > Done .

Define a specific radius that the curve will take through each

1. Click Single Rad, and select PNT1. Type [1.0]. 2. Click Done Sel > Done . 3. Click OK to finish the feature Task 6. Create a swept protrusion as the door handle geometry. The trajectory is the datum curve that you created. 1. Click Insert > Protrusion > Sweep. 2. Click Select Traj > Curve Chain. 3. Select the datum curve; then click Select All > Done > Okay. 4. Define a 1.0 inch diameter circle as the cross-section, centered at the intersection of the centerlines.


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NOTES

5. Click 6.

.

Click OK to finish the feature. The final part should look as shown in the following figure.

Figure 2: Final Solid Geometry



NOTES

EXERCISE 2: Creating a simple skeleton Task 1.

Create a datum curve.

1. Create a new part called LINK_SKEL using the default template. 2. Select the FRONT datum plane and click datum curve].

[Insert sketched

3. Sketch the following three line segments.

Figure 3: Sketching Three Lines

4. Click Task 2.

.

Create points at the vertices

1. Click [Insert datum points] > On Vertex , then select the vertices shown in the following figure.


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NOTES

Figure 4: Selecting Vertices

2. Click Done Sel > Done . Task 3.

Create axes through the points

1. Click [Insert datum axis] > Pnt Norm Pln and select the FRONT datum plane and PNT0. Then click Done Sel > Done . 2. Click [Insert datum axis] > Pnt Norm Pln and select the FRONT datum plane and PNT1. Then click Done Sel > Done . Note: To accept default selections that the system provides such as Done Sel and Done , you may also use

for ease of use.

3. The model is as shown in the following figure. (The tags for the points and axes have been turned off for clarity)



NOTES

Figure 5: Sketched Preliminary Model

Task 4.

Create two additional datum planes

1. Click [Insert datum plane] > Though and select the curve shown in the following figure.

Figure 6: Creating a Through Datum Plane

2. Click Parallel and select the RIGHT datum plane and click Done . 3. Click

> Though

and select the diagonal curve.


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NOTES

4. Click Normal and select the FRONT datum plane and click Done . Task 5.

Create a coordinate system

1. Click [Insert datum coordinate system] > Orig+Zaxis > Then select the vertex as shown in the following figure.

.

Figure 7: Selecting Vertex

2. Select DTM1 and O k a y to accept the direction for the Z-axis. 3. Click Plane Norm , select the FRONT datum and click Flip > O k a y to accept the direction for the X-axis.

Figure 8: Creating Normal Plane

4. Turn off the display of

.

5. Select the datum curve and click

> Modify .



NOTES

6. Select the 40.0 dimension, modify to [15.0], and Regenerate .

Figure 9: Regenerated Model

7. Notice the planes, points, axes, and csys have updated with the changes. 8. Modify the overall height dimension back to [40.0] and Regenerate .


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NOTES

EXERCISE 3: The Link Skeleton in an assembly Task 1.

Open and ‘flex’ an assembly with a skeleton.

1. Open LINK_SKEL.ASM, and turn off the display of datum features.

Figure 10: Link Assembly

2. Notice that the LINK_SKEL (from the last exercise) has been assembled as a skeleton in this assembly. The three solid models have been assembled to the skeleton. Task 2.

Make modifications to the skeleton.

1. Select the Link_Skeleton from the model tree, and click > Modify , then select the curve as shown in the following figure.

Figure 11: Selecting Curve to Modify



NOTES

2. Select the 40.0 dimension, modify to [15.0], and Regenerate > Automatic.

Figure 12: Model with Modified Dimensions

3. Notice that the components move with the skeleton. 4. Modify the overall height dimension to [48.0], and Regenerate > Automatic.

Figure 13: Model with Further Modified Dimensions

5. Save the model and click File > Close Window . 6. Click File > Erase > Not Displayed. Click OK .


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NOTES

OPTIONAL EXERCISE 4: The Vice Grip Task 1. Open a partially finished model consisting of datum features. Create additional features to complete the ‘skeleton’. 1. Open VICE_GRIP.PRT.


2.

Select the FRONT datum plane and click

.

3. Select the two default references and click Delete. 4. Display ONLY Axes and points. 5. Select axis A_1 and the two points for references as shown in the following figure.

Figure 15: Creating References



NOTES

Task 2.

Sketch the following curve.

Note: If you have difficulty creating the sketch, you may wish to open the completed vice-grip model.

Figure 16: Sketching a Model

1. After completing the sketch, click dimension.

and select the 45°

2. Increase the sensitivity slider to its maximum and scroll the thumbwheel approximately between 45° and 15°. Notice how the curves work together to form a ‘linkage’. The following figure has the angle modified to 18°.


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NOTES

Figure 17: Modified Angle

3. This ‘skeleton’ model now could be used to either design parts from as part of a top-down design process, or models could be directly assembled to simulate motion. 4. Complete the feature, save the model, and erase it from memory.



NOTES

MODULE SUMMARY In this module, you have learned that •

Additional Datum features are convenient and hassle-free features that aid model creation.

•

Datum features are mass-less and non-solid; therefore, they can be deployed frequently when creating solid geometry.

•

Datum Axes are created for all types of revolved features, holes, and extruded circles.

•

Datum Curves often aid in surface creation using sketcher functionality.

•

Datum Points are used as references for assembly constraints and to place holes on point when they are created.

•

Datum Coordinate Systems are used for orientations in manufacturing procedures.


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16 Layers and Suppression In this module you will learn how to use layers. Layers enable you to organize model components – features, datum planes, and parts – so that you can perform operations on those items collectively. Typical operations you might perform with layers include manipulating the model view by displaying or blanking, selecting, suppressing, and so on.


Create layers for a given model.

•

Associate items to a layer.

•

Manipulate layer display status.

•

Control data with the suppression function.

•

Re-work existing parent/child relationships.

•

Resume suppressed features.

Page 16-1

NOTES

DEFINING LAYERS Functionality •

Layers provide a means of organizing object items into related groups to avoid confusion

•

They allow you to perform certain collective operations on groups of items such as features in a part, components in an assembly, draft items on a drawing, even other layers.

•

Using layers, you can control the information that the system displays on the screen

•

Layers enable certain actions as deletion, plotting, and suppression for certain items.

Working With Layers •

If you use a default template, Pro/ENGINEER automatically associates the different features of a model to specific default layers. For example,



NOTES

Figure 1: Default Layers when Creating New Models from Template

•

You can create additional default layers using two methods. The first is through the Config file and the second is by using the def layers command from the Layer pull-down menu in the LAYERS dialog box.

•

A single item can be associated with multiple layers.

•

You can have as many layers as needed or none at all.

CREATING LAYERS Selecting the Object The active object is the model in which you actually create the layers and make changes. The principle is to associate those items to a layer that exist at the layer level. For example, if you select the top-level assembly as the active object, you can associate only items from the top-level assembly to a top-level assembly layer.

For University Use Only - Commercial Use Prohibited Layers and Suppression

P a g e 1 6- 3

NOTES

Note: In Drawing mode, you can select either the model or the drawing as the active model.

Creating Layers •

Pro/ENGINEER identifies layers by name only.

•

You can express the name in numeric or alphanumeric form, using a maximum of 31 characters.

•

After you have established the active model, you can define a new layer by clicking the

•

.

Once you have typed one layer name you can create multiple new layers by simply typing a new name and pressing .

Associating Items to a Layer Once you have created layers, you can associate items to them automatically as well as manually. For example in the following figure, you can associate axis to a new layer automatically by selecting from the Default Layer Types. Similarly other feature-types can also be associated either to the same layer or to another layer.

Figure 2: New Layer Dialog Box



NOTES

Using options in the LAYER dialog box, you can associate items to and remove them from selected layers manually as well. You can copy them or switch them from one layer to another. Table 1: Item Types Component

(Assembly mode only) Feature

Select component parts and/or assemblies. Click All Instances or Individual in the LAYER COMP menu.

•

Click the following feature options in the LAY FEAT menu:

•

Select

– Specifies the particular feature.

•

Range

– Specifies a range of features.

•

All of Type

•

Feat/Child

– Specifies a feature type from the ALL FEATURES menu. – Specifies a feature and all of its

children. Curve

Select a datum curve.

Quilt

Select a quilt.

2-D Items

Select detail items.

Text

Select nametags for datum planes, axes, points, and coordinate systems. When text tags are blanked, Click Sel By Menu, or select from the MODEL TREE

Point

Select a datum point.

Datum Plane

Select a datum plane.

Layer

Select a layer. Creates a layer hierarchy with sub-layers.

Solid Geometry

Select a feature. Blanks all solid features of the part.

Note: If you attempt to associate an item to a layer that does not exist in the active model, the system identifies the native model for the item. You can select or create a layer in the native model, or ignore the selection of that item.

Setting the Display Status of a Layer One of the main reasons that you would organize items using layers is to control the kind of information that the system displays on the screen for that particular object. You can perform the following procedures, as illustrated in the following figure:


P a g e 1 6- 5

NOTES

•

Show selected layers on the screen.

•

Blank selected layers from the screen by removing them.

•

Isolate selected layers by displaying them on the screen and removing all non-isolated layers from the screen.

•

Hide components associated to the selected layer by displaying them entirely as hidden lines when working in Hidden Line mode, or remove them from the screen when working in No Hidden mode (in Assembly mode only). The Hide display status has no effect when the environment setting is Wireframe .

Figure 3: Layer Display Dialog Box

Not all layer items are available for manipulation in every Pro/ENGINEER mode.



NOTES

Note: Pro/ENGINEER does not save the display status of a layer by default when it saves the object. The next time that you retrieve the object, the display status reverts back to Show for all layers. If you want to save the display status with the object, you must click Save Status from the LAYER DISPLAY dialog box.

Manipulating Layer Display Status In the following figure you create layers in Part mode and Assembly mode, associate items to them, and vary the display status of the items. In Part mode, you have a protrusion and three datum planes. •

Create the layers PROT, DATUM_A and DATUM_B.

•

Associate the protrusion to the PROT layer.

•

Associate datum plane A to the DATUM_A layer.

•

Associate datum plane B to the DATUM_B layer.

•

Do not associate datum plane C to any layers.

In Assembly mode, you have three components (A, B, and C) and two assembly datum planes. •

Create layers COMP_B, COMP_C and ADATUM_A.

•

Associate component B to the COMP_B layer.

•

Associate component C to the COMP_C layer.

•

Associate assembly datum plane A to the ADATUM_A layer.

•

Do not associate component A and assembly datum plane B to any layers.


P a g e 1 6- 7

NOTES

Part Mode

C

B

A

Assembly Mode

E

D

F

Figure 4: Illustration of Layer Display Status

•

A – All layers have a display status of S h o w n .

•

B – PROT: Blank ; DATUM_A: Shown; DATUM_B: Blank

•

C – PROT: Shown ; DATUM_A: Shown; DATUM_B: Isolate

•

D – All layers have a display status of Show .

•

E – COMP_B: Blank ; COMP_C: Show ; ADATUM_A: Blank

•

F – COMP_B: Isolate ; COMP_C: Show ; ADATUM_A: Show

SUPPRESSION FUNCTIONALITY •

Suppression temporarily removes a feature or component from the model

•

The system does not regenerate the item, and the model appears as if you had never created the item.

•

When you suppress items, you can resume them at a later date. Suppress differs from delete in that it is not permanent.

Using Suppression •

To simplify the model

•

To reduce regeneration time



NOTES

•

To reduce screen repaint time

•

To use design alternatives

Suppressing Parent/Child Relationships If you suppress a feature or a component that has children and do not select the children as well, Pro/ENGINEER requires you to do one of the following: •

Reroute the child references.

•

Change the dimensioning scheme of the child.

•

Suppress the child.

•

Suspend action on the child until you regenerate the model.

•

Freeze the component (in Assembly mode only).

Saving and Resuming Suppressed Features You can save a model with suppressed features and/or components. When you retrieve or regenerate it, Pro/ENGINEER informs you that it has suppressed items. When you resume or regenerate suppressed features, the system returns them to their original location in the feature list. You can resume them by selecting them from the MODEL TREE window or using one of the following options in the RESUME menu: •

All

•

Layer

•

Last Set

•

Feat ID

– Resumes all items that are currently suppressed. – Resumes items by layer. – Resumes the last group of suppressed items.

– Resumes items by specifying the feature ID of the item.


P a g e 1 6- 9

NOTES

LABORATORY PRACTICAL Goal The goal of this lab is to use layers for organizing items in a model. You will also use the suppression function to remove items from a model temporarily.

Method In Exercises 1 and 2, you learn to control the information that the system displays in a part model and an assembly model. You learn to use layers to control the display of the datum planes and axes of the part in Exercise 1, as opposed to turning their display off. In Exercise 3, you suppress a feature in a part. In Exercise 4, you experiment with suppressing a component in an assembly.

Tools Table 2: Layers Icons

Icons

Description Saved views list Create layers Add item to selected layer Layers blanked Show layers Select all Unselect all



NOTES

EXERCISE 1: Using Layers in Part Mode

Figure 5: Layer Crank Part

Task 1.

Retrieve the crank part; then shade and spin the model.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 16_layers_suppression. 3. Click

[File open] to open LAYER_CRANK.PRT.

4. Shade the model if it is not already so. Task 2.

Create two layers called DATUMS and AXES.

1. Click

[Saved views list]. There’s only one Default view here.

2. Click View > Layers and click

[Create layers].

3. Type [DATUMS], then click Add .


P a g e 1 6- 1 1

NOTES

4. Type [AXES], then click O K . Task 3.

Associate the default datum planes to the datum layer.

1. Select the Datums layer from the layers list. Make sure the A x e s layer is not highlighted. 2. Click the

[Add item to selected layer].

3. Click Datum Plane from the LAYER OBJ menu. 4. Select DTM1, DTM2, and DTM3 from the MODEL TREE, then click Done Sel > Done/Return Task 4.

Associate the axes of the part to the axes layer.

1. Unselect layer Datums and select layer A x e s. 2. Click the

icon and click Feature from the LAYER OBJ menu.

3. Click Query Sel . Select the A_1 boss protrusion. Accept the selection. 4. Now Select A_5 and the cross-hole protrusion. Accept the selection. 5. Click Query Sel . Select axis A_2 . Accept the selection. 6. Click Done Sel > Done Return > Done Return . Task 5. Use the LAYER dialog box to see the features you associated with layers. 1. Click Show > Layer Items. 2. Tree > Expand >All . Task 6.

Change the display status of the two layers you just created.

1. Click A x e s and Datums in the LAYERS dialog box 2. Click

and then click

.



NOTES

3. The system no longer displays the datum planes and axes on the screen, but they still exist. You can verify this by using the MODEL TREE. 4. Close the LAYERS dialog box. 5. Save the model and close the window Note: Pro/ENGINEER does not save the display status of the layers unless you click Save Status prior to exiting the LAYERS dialog box.

Figure 6: Layer Display Status Set to Blank


P a g e 1 6- 1 3

NOTES

EXERCISE 2: Using Layers in Assembly Mode

Figure 7: Layers Assembly

Task 1. Open an existing assembly and define two layers at the toplevel assembly called crank and gear. 1. Open the PINION.ASM. 2.

Click View > Layers and click

[Create layers].

3. Type [CRANK] and press . 4. Type [GEAR], then click O K . Task 2. Associate the crank part to the CRANK layer and the Gear part to the GEAR layer. 1. Unselect the GEAR layer and select the CRANK layer. 2. Click

.

3. Click Component from the LAYER OBJ menu.



NOTES

4. Click Individual from the LAYER COMP menu. 5. Click Sel By Menu , then select LAYER_CRANK.PRT. 6. Finish the association. Click Done Sel > Done/Return > Done/Return . 7. Repeat the steps above to associate the gear part to the gear layer Task 3.

Blank the crank and gear layers.

1. Select the crank and gear layers. 2. Click

[Blank layers].

3. Repaint the screen and turn off the datum planes and axes. 4. The system no longer displays the layer crank and layer gear components on the screen.

Figure 8: Layers Blanked from Display Task 4. 1.

Verify that the components still exist. Click Info > Feature List .

2. Click Top Level > Apply. 3. Read the information window and close the information window and the FEATURE LIST dialog box.


P a g e 1 6- 1 5

NOTES

Task 5.

Set the gear model to hidden line display.

1. Click

[Hidden line].

2. Click View > Layers. 3. Click G e a r in the LAYERS dialog box. 4. Click

from the LAYERS dialog box.

5. Repaint the screen. The system displays the component on the screen again. Task 6.

Determine the effect that other environment settings have on the setting for the layer.

Hidden Line

1. Click

.

Figure 9: Hidden Line Display Mode

2. Click

from the toolbar.



NOTES

Figure 10: No Hidden Display Mode

Note The icons next to the layer names in the dialog box indicate the current status of the layers. If [Show layers] next to the layer name is gray, then some of the layers of the same name in assembly sub-components have varying display statuses set

Task 7.

Determine the status of the datums layer.

1. In the LAYERS dialog box. 2. Click Show > Layer Items. 3. Expand the datums layer items. Click the + icon next to DATUMS. 4. Notice all the models have a layer called DATUMS, but only some of them are blanked.


P a g e 1 6- 1 7

NOTES

Task 8.

1.

Set both layers back to S h o w n.

Click the

[Select all] icon from the LAYERS dialog box

2. Click

.

3. Repaint the screen. 4. All components and their datums should be visible again. If the datums and axes are not visible, check the environment icons in the toolbar, Task 9. You have the ability to effect the display of layers within all levels of the assembly, as well as associate items at any level. Change the display of all the part level datum planes. 1. Click

[Unselect all].

2. Select all the entries under Datums , except IN_LAYER_BASE.ASM. 3. Click

.

4. Repaint the screen. The system no longer displays the datum planes of the parts on the screen, but does display the assembly datums. Task 10. Add the layer called Datums at the top level and associate the default datums of the assembly.

1. Click

.

2. Type [asm_datums], then click OK 3. Select the datums layer and click

.

4. Select the three assembly level datum planes in the PINION.ASM. 5. Complete the association. Click Done Sel , then click Done/Return from the LAYER OBJ menu.



NOTES

Task 11. Save the display status of the datum planes for the next time that you retrieve the assembly, or any of the associated components, 1. Click Save Status from the LAYERS dialog box. 2. Click Close . 3. Save the assembly. 4. Erase the assembly from memory and all associated objects.

Figure 11: Top-Level Default Datum Planes


P a g e 1 6- 1 9

NOTES

EXERCISE 3: Suppressing in Part Mode In this exercise, you suppress a feature to make it easier to retrieve and regenerate the part. In the following figure, each hole has a cut that represents the threads; therefore, it requires a great deal of time to retrieve and regenerate it. For this design you only need the threads for mass property calculations, and not for other operations.

Figure 12: PLATE.PRT with Threaded Notes

Task 1. Modify the circular protrusion which comes before the helical threads in the regeneration list of the start model. 1. Open the part named PLATE.PRT, note the amount of time the system uses to retrieve the part. 2. Modify the height of the circular boss to 10mm. Click Modify and Select the boss protrusion. Select the 5 dimension and type[10]. 3. Regenerate the part. Note the amount of time that the system requires to update the geometry. Task 2.

Suppress the complex thread cuts.

1. Click Feature > Suppress from the menu manager. 2. Select the pattern of cuts from the MODEL TREE.



NOTES

3. Click Done Sel from the GET SELECT menu. Click Done from the SELECT FEAT menu. 4. Note that the cuts are no longer in the model. Verify this by checking in the MODEL TREE. Task 3. Once a feature is suppressed, Pro/ENGINEER does not consider it as existing in the model. Test the speed that the system regenerates the model without the threads in the model. 1. Click Done from the FEAT menu. 2. Change the height of the circular boss back to 5. Click Modify and Select the 10 dimension, then type [5]. 3. Regenerate the part. Note that the system updates the model much faster now. 4. Save the model and erase it from memory.

Figure 13: Thread Cuts Suppressed


P a g e 1 6- 2 1

NOTES

EXERCISE 4: Suppressing Components in Assembly Mode

Figure 14: Alternate Components

Task 1. Suppress the crank components in the assembly to see what the assembly will look like with a different crank part. 1. Open the SECOND_PINION.ASM, 2. Click Component from the ASSEMBLY menu. Click Suppress and Select the crank part. 3. Click Done Sel > Done . Note that the system no longer includes the component in the assembly.



NOTES

Task 2. You can assemble different components to test their compatibility with an assembly design. Assemble a model to replace the crank. 1. Click Component > Assemble and double-click HAND_CRANK.PRT

2. Click Align from the constraint drop-down list in the COMPONENT PLACEMENT dialog box. 3. Select axis A_1 of hand crank model. 4. Select axis A_1 of shaft model.

Figure 15: Axes Aligned

5. Select Align for the second constraint. 6. Select axis A_5 of hand crank model. 7. Select axis A_3 of shaft model. 8. Finish the placement. 9. Read the message in the message area, then click O K . 10. Close the COMPONENT PLACEMENT dialog box. Task 3.

Suppress the hand crank model.

1. Click Suppress . 2. Select the HAND_CRANK using the MODEL TREE.


P a g e 1 6- 2 3

NOTES

3. Click Done from the SELECT FEAT menu to complete the operation. Task 4.

Constrain the wheel crank to the end of the shaft.

1. Click Assemble . and double click the WHEEL_CRANK.PRT 2. Click Align from the CONSTRAINT TYPE drop-down list. 3. Align A_1 of wheel crank with axis A_1 of shaft model 4. Align axis A_5 of wheel crank model with axis A _ 3 of shaft model. 5. Finish the placement Task 5. With components suppressed you can easily switch between representations of the assembly to test which one is the most plausable. Suppress the third crank model and resume the original one 1. Suppress the wheel crank component. Click Suppress and Select the wheel crank part. Click Done from the SELECT FEAT menu. 2. List the suppressed components in the MODEL TREE. Click View > Model Tree Setup > Item Display

3. Select Suppressed Objects and click O K 4. Resume the original layer crank component. Right mouse click the LAYER_CRANK.PRT entry in the MODEL TREE, and select Resume from the pop-up menu. Task 6. Suppression temporarily removes a component from the assembly. A suppressed model is still associated to the assembly. Resume the suppressed components; then permanently delete them from the assembly. 1. In the MENU MANAGER, click Component > Resume > All > Done

2. Click Delete > Clip 3. Select only the hand crank part from the MODEL TREE. 4. Click Done Sel > Done .



NOTES

Tips & Techniques: You can use the MODEL TREE to delete suppressed features or components without resuming them first.

5. Save the model and click File > Close Window .. 6. Click File > Erase > Not Displayed. Click OK .


P a g e 1 6- 2 5

NOTES


The Layers feature is designed for greater flexibility of models and less clutter.

•

Items have to be deliberately associated to specific layers of a model.

•

Any number of layers can be created.

•

The display status of a layer can be set to Hidden

•

Suppression of features in a part and of components in a model leads to greater maneuverability in design.

•

Suppressed features can effect the parent/child relationship.

•

Suppressed features can be resumed.




Module

17 Creating Surfaces with Freeform Interactive Surface Design in Pro/ENGINEER (also referred to as “ISDX”) adds many new features to Pro/ENGINEER surface modeling. In this module you learn some of the ways to use ISDX, including an overview of the Style feature.


Describe the capabilities of ISDX.

•

Explain the use of the new hybrid modeling paradigm.

•

Describe how to use the tools and menus to create Style features.

•

Describe how to use the single- and quad-view window layouts.

•

Create 2-D and 3-D freeform curves.

•

Create freeform surfaces using boundary curves.

Page 17-1

NOTES

DESIGNING WITH INTERACTIVE SURFACES ISDX offers a spline-based freeform modeler that allows you to create 2-D and 3-D curves and freeform surfaces. You can use ISDX to create freeform surface models for: •

Conceptual design

•

Engineering design

•

Reverse styling

ISDX enables you to create STYLE features. Within the Style feature, you can create freeform curves and surfaces easily.

THE STYLE FEATURE A Style feature can contain several curves and surfaces or quilts. It appears in the MODEL TREE as Style.

Figure 1: The Style feature in the Model Tree



NOTES

Figure 2: A Style feature Containing Several Curves and Surfaces

The Style feature opens up a new modeling environment with a single or four-view window layout.

Figure 3: Four-View Window Layout

HYBRID MODELING Most products are a combination of geometric forms and freeform shapes. Style offers a unique situation where you can integrate the traditional feature based parametric modeling of Pro/ENGINEER with freeform unconstrained surfacing. You can create freeform curves and surfaces that can reference other geometric features.

For University Use Only - Commercial Use Prohibited Creating Surfaces with Freeform

P a g e 1 7- 3

NOTES

Any change in a parametric model regenerates the Style features allowing you to freely mix unconstrained freeform surfaces with geometrical parametric surfaces. This unique situation also allows you to carry out total product design in a single modeling environment.

CREATING SURFACES WITH ISDX You can use ISDX to create curves and freeform surfaces where geometry is either not defined or requires great flexibility. Also, you can use it when the design intent is dependent on visual or aesthetic criteria. Specifically, you can use ISDX to create: •

2-D and 3-D curves (referenced or unconstrained)

•

Curves On Surface (COS)

•

Styling design models

•

Blends and transition surfaces

•

Freeform surfaces along with parametric surfaces in engineering design models

•

Reverse styling surfaces

Creating 2-D and 3-D Curves You can use Style as a 2-D or 3-D sketcher to create unconstrained or referenced curves. These curves can be attached to features like points, curves, or edges and so on, and can be used to create Style or other Pro/ENGINEER features.



NOTES

Figure 4: Defining Curves in 3-D Space

Figure 5: A Blend Surface based on a Freeform 3-D Curve

Figure 6: Surfaces Created from 3-D Curves


P a g e 1 7- 5

NOTES

Using COS You can create Curve on Surface (COS) by sketching them directly on to the base surface or by using the Drop tool. Style allows easy manipulation or modification of the COS in order to capture the design intent. You can use COS to build further surfaces or to trim the surfaces.

Figure 7: Using COS for Trimming

Creating Styling Models You can use freeform, intuitive curves and surfaces to conceptualize products. Conceptualizing in ISDX allows you to access the inside engineering components directly in the same part or assembly while designing outer body shapes. You can also model using concept images that can be applied on to base surfaces as shown in the following figure.

(A)

(B)



NOTES

(C)

Figure 8: (A) Sketch (B) Sketch Applied on to the Base Surface (C) Model Developed Using the Sketch

Creating Freeform Surfaces with Parametric Controls While designing products you may need to impose dimensional controls on freeform surfaces. ISDX allows freeform curves and surfaces to reference with parametric curves or surfaces, enabling you to control the freeform surfaces using dimensions.

Figure 9: Dimensionally Controlling a Style Model


P a g e 1 7- 7

NOTES

Creating Blends and Transitions You can use Style to create quick and high quality spline blends to improve the aesthetics or smoothness of products.

Figure 10: Typical Transition Surfaces

Figure 11: Interactive Manipulation of Tangency

Applying Style Surfaces to Engineering Models You can combine Style surfaces with parametric surfaces while creating high curvature or transition surfaces.

Figure 12: High Curvature Transition Surfaces



NOTES

Reverse Styling You can conveniently refer to imported scan curves and faceted or surface data to build Style curves and surfaces.

Figure 13: Reverse Styling

CREATING STYLE SURFACES You can create Style surfaces using any four touching boundaries. For this purpose, Style curves, datum curves and edges as boundaries can be used as shown in the following figure

Figure 14: Style Surfaces from Four Touching Boundaries


P a g e 1 7- 9

NOTES

LABORATORY PRACTICAL Goal The goal of this lab is to use the Style interface and create simple style surfaces.

Method In Exercise 1, you redefine a Style feature created in a PDA model. You navigate through menus, shortcut menus and tool bars and also set different view orientations. In Exercise 2, you create surfaces for a flashlight part by connecting four style curve boundaries.

Tools Table 1: ISDX Icons

Icons

Description Set active datum plane Create and edit curves Display curvature plot Clear curvature plot Regenerate all Create surfaces from boundary curves



NOTES

EXERCISE 1: Interrogating the STYLE Interface Task 1.

Experiment with an existing Style feature.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 17_surfaces_freeform. 3. Open PALM.PRT.


Note: The ‘LCD screen’ is actually a *.jpg image applied on the model in Pro/E as a texture.

4. In the MODEL TREE, click STYLE id 89 and click Redefine .

>

5. Notice the Style working environment and particularly the new tools added to the interface as shown in the following figure.


P a g e 1 7- 1 1

NOTES

Figure 16: The Style Tool Bars

6. The grid displayed on the TOP plane indicates that TOP is set as the active plane. 7. Click View > Active Plane Orientation . The TOP is set parallel to the screen. 8. In the window, Task 2.

> Default Orientation.

Change the window layout.

1. Click View > Show All . 2. Click Styling > Set Active Plane . Select the Oblique plane from model tree.



NOTES

3. In the top left window, pop-up menu.

> Active Plane Orientation

from the

4. Rotate the model randomly in any window. 5. Click View > Default Orientation to reset all the windows. 6. Click anywhere in the window and then

> Show All .

7. Reset the active plane. Right-click S e t Active Plane and select the TOP plane. 8. Press + to get to the default orientation. Task 3.

Familiarize yourself with the Style preferences.

1. Click

and

.

2. Click Utilities > Styling Preferences. 3. Change the spacing of the grid. In the grid area of the dialog box, type [15] and press < ENTER> .

Figure 17: Changing Grid Spacing

4. In the Display area of the STYLING PREFERENCES dialog box, clear the Grid checkbox. 5. In the Surface Mesh area, move the quality slider to the right to make the mesh dense.


P a g e 1 7- 1 3

NOTES

6. Click

[Shading].

7. In surface mesh area, click On to display mesh on the shaded model.

Figure 18: Displaying Mesh on Shaded Model

8. Display the model without the curve and mesh display. Click View > Shade . 9. Close the STYLING PREFERENCES dialog box. 10. Click Task 4.

[Repaint].

Familiarize yourself with the selection procedure.

1. Click close to the cluster of curves as shown in the following figure.

Click here to select a curve

Figure 19: Selecting a Curve



NOTES

2. Click menu.

> Next from among the many commands in the pop-up

3. Choose entities from the selection bin. Right-click Show Sel Bin . In the SELECTION dialog box, click Style: (1) Curve:CF-116 . 4. Exit the Style feature, click 5. Close the window.


P a g e 1 7- 1 5

NOTES

EXERCISE 2: Creating a Handle on the Flashlight Task 1.

Add a Style feature to the flashlight body.

1. Open FLASHLIGHT.PRT.


Task 2.

Create the first handle curve.

1. Click Insert > Style . 2. Click

and select the FRONT datum from the model tree.

3. Click

> Front .

4. Click > New > Planar and create a curve with four points as shown in the following figure.

Figure 21: First Handle Curve

5. Click

[Display curvature plots]



NOTES

6. Click Edit and drag the curve points to form a shape similar to the one shown in the following figure.

Figure 22: Editing Curve

Task 3.

Create the second handle curve.

1. Click

[Clear curvature plot] to turn off the curvature plot.

2. Click N e w in the CURVE dialog box and create a curve with five points as shown in the following figure.

Figure 23: Creating Second Curve


P a g e 1 7- 1 7

NOTES

3. Click

[Display curvature plots]

4. Click Edit and drag the curve points to form a shape similar to the one shown in the following figure.

Figure 24: Editing Second Curve

5. Click Task 4.

[Clear curvature plot] to turn off the curvature plot.

Create third handle curve.

1. Click > New > Free and create the first cross section by clicking and snapping to the existing curves as shown in the following figure.



NOTES

Figure 25: Creating a Free Curve

2. Click Add > Midpoint and select a location as shown in the following figure.

Figure 26: Selecting a Midpoint Location

3. Click Edit and use the key to pull the point perpendicular from the FRONT plane. Shape the curve as shown in the following figure.

Figure 27: Shaping Curve


P a g e 1 7- 1 9

NOTES

Task 5. Using the same techniques, create another new curve and shape as shown in the following figure.

Figure 28: Creating and Shaping a Second Curve

1. Click OK to close the CURVE dialog box. 2. Click OK .

, select the four curves that form the handle, and click

3. Click

.

4. Click

to shade the model.

Figure 29: Creating Surface from Four Style Curves

5. Click Insert > Surface Operation > Merge . 6. Select the handle surface and then the body surface. 7. Toggle the mesh for the Quilt Sides as shown in the following figure.



NOTES

Figure 30: Quilting Sides

8. Click

.

9. Click Feature > Mirror Geom and select the FRONT plane.

Figure 31: Mirroring Geometry

10. Click Insert > Surface Operation > Merge , select the left and right halves of the flashlight body, and click . 11. Click Insert > Thin Protrusion > Use Quilt, and select the surface quilt. 12. Flip the Material Side arrow to add material to the INSIDE of the surface. 13. Enter a thickness value of [2 . 0] and click . (You may wish to add the Style curves to a layer and blank the layer)


P a g e 1 7- 2 1

NOTES

Figure 32: Finished Model

14. Save and click File > Close Window . 15. Click File > Erase > Not Displayed. Click OK



NOTES


ISDX integrates freeform surfacing and parametric modeling to enhance existing surfacing capabilities of Pro/ENGINEER, enabling you to create product forms that require flexible surfaces.

•

Style allows you to create geometry using a single-view layout or 4view layout.

•

While creating a Style feature, a new menu named Styling is added and many new commands are available.

•

A curve can be created as a free 3-D curve or as a planar curve.

•

To create a Style surface you need four touching boundary curves.

•

To change the shape of a surface, you need to manipulate the shape of the boundary curves.


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18 The Resolve Environment Pro/ENGINEER provides the Resolve Environment to help you fix regeneration failures. By learning how to use the Resolve Environment, you will be able to refine existing features and parameters. This is preferable and more efficient than recreating them.


Describe several regeneration failure types.

•

Start the Resolve Environment.

•

Diagnose feature regeneration problems.

•

Run the “quick fix” to resolve failed regenerations.

•

Describe some of the ways to change your model designs to resolve feature regeneration failures.

Page 18-1

NOTES

REGENERATION FAILURES Failures usually occur because a feature gets changed and the effected change conflicts with other features. These types of failures occur due to the following reasons: •

You create new features that are unattached and have one-sided edges.

•

You resume a feature that now conflicts with another (such as having an edge round and a chamfer on the same edge).

•

The feature intersection is no longer valid because dimensional changes have moved the intersecting surfaces.

•

An assembly you retrieve cannot open the required models that are included in the assembly.

•

The assembly constraints for a component are invalid.

•

You have violated a relation constraint.

Starting the Resolve Environment As soon as a regeneration failure occurs, Pro/ENGINEER automatically starts the Resolve Environment. When this happens: •

The F i l e pull-down menu is grayed out (unavailable) so you cannot save the model.

•

The failed feature and all subsequent features remain un-regenerated.

•

The current model displays only the features that have regenerated up to the point of failure.

•

Pro/ENGINEER displays an explanation of the problem in the Message Area.

•

Pro/ENGINEER displays the RESOLVE menu options in the MENU MANAGER and a diagnostics window.

Resolving Regeneration Failures Once you have entered the Resolve Environment, you can address the failure problem using any of the following methods: •

Undo all of the changes that you have made since the last successful regeneration.

•

Diagnose the cause of the model failure using the current (failed) model or the backup model.



NOTES

•

Attempt a quick fix of the problem using shortcuts for performing standard operations on the failed feature only.

•

Change the failed model or a backup model using standard part or assembly functionality.

Specifying a Model When you diagnose the problem or change the model, you can work on the current failed model or a backup model. If you use a backup model, Pro/ENGINEER shows all features in their pre-regenerated state, so that you can modify or restore dimensions of the features that are not displayed in the current model. If you select the Regen Backup option from the ENVIRONMENT dialog box, the system saves a copy of the current model to disk with the name REGEN_BACKUP_MODEL####.PRT prior to each regeneration, and removes the file when you exit the Resolve Environment. Otherwise, it uses the last version of the current model saved on disk prior to the failure.

Undoing Changes Rather than attempt to resolve the problem, you can simply undo the step that brought you into the Resolve Environment. However, this may not be the best choice in some cases. For example, if the feature fails because of the change that you have made, even if you undo the change, the model itself still remains problematic. The Undo approach is most appropriate in those cases in which you either did not intend to make the change or you want to fix the problem in the model without using the Resolve Environment tools.

Note: Keep in mind that the Resolve Environment tools are designed to resolve failures in order to allow you to build more robust models.

Diagnosing the Problem When you use the Resolve Environment, it is always good practice to interrogate the model to determine what has caused the model failure. The system gives you many diagnostic tools to perform an investigation. To interrogate the model, you can use the FAILURE DIAGNOSTICS window to display the following information:

For University Use Only - Commercial Use Prohibited The Resolve Environment

P a g e 1 8- 3

NOTES

•

A description of the current model and backup models.

•

Information concerning the failed feature.

•

Hints on resolving the problem.

Figure 1: FAILURE DIAGNOSTICS Window

If you need to investigate the problem further, you can use the Investigate option to obtain the following information about the current model or the backup model, if it exists: •

Modified dimensions.

•

All modifications and changes.

•

All references for the failed feature in the model.

•

Invalid geometry of the failed feature.

You can then choose to roll the model back to one of the following: the failed feature (for the backup model only), the feature just before the failed feature, the state at the end of the last successful feature regeneration, or a specified feature.

Performing a Quick Fix on the Failed Feature Using the QUICK FIX menu, you can perform the following operations on the failed feature only: •

Redefine it.

•

Reroute it.

•

Suppress the failed feature along with its children.

•

Delete it with its children.



NOTES

Note: When you make changes in the Resolve Environment, they can affect the failed feature or another specified feature. If you suppress features using the QUICK FIX menu, you should investigate the cause of the failure before continuing with the part design. If you do not make any corrections, you may not be able to resume the feature later in the design.

Changing the Model Using the FIX MODEL menu, you can change any feature or component to solve the regeneration problem. As you change a model in the Resolve Environment, however, consider any parent/child relationships that exist between features and components to avoid changing the intent of the model itself. Specifically, you can use any of the following approaches: •

Use the FEAT menu to perform feature operations on the model.

•

Modify dimensions using the standard MODIFY menu.

•

Regenerate the model again.

•

Restore dimensions, parameters, relations, or all of these to their values prior to the failure.

•

Add, delete, or modify relations, as necessary, to regenerate the model.

•

Display the PART SETUP menu to perform additional part set up procedures.


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NOTES

LABORATORY PRACTICAL Goal The goal of this lab is resolve regeneration failures by using the resolve environment.

Method In this exercise, you add features to a part, which causes other features to fail. You then investigate and resolve the problem in the Resolve Environment.

EXERCISE 1: Resolving a Regeneration Failure Task 1. Use the Feature List and Model Player options to determine how the chamfer part was built. 1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 18_resolve. 3. Retrieve CHAMFERS.PRT. 4. Open the feature list. Click Info > Feature List . Review the Information Window and close it. 5. Regenerate the model in steps. Click Utilities > Model Player. 6. First click feature. 7. Click

to rewind the model player to begin at the first

to regenerate feature by feature.

Note: The system regenerates the two chamfers after the two protrusions. You will not see datum planes if you have them off.



NOTES

Task 2. Insert an edge round on the bottom edge of the model. Add the rounds after the second (triangular) protrusion. 1. Click Feature > Insert Mode > Activate from the MENU MANAGER. 2. Insert after the second protrusion. Select the second protrusion feature of the model. Note that the system no longer displays the chamfers, as shown in the following figure. Round these four edges.

Insert after this protrusion

Figure 2: The Resolve Model

3. Click Insert > Round . 4. Leave Simple as the default. Then click Done from the ROUND TYPE menu. 5. Leave Constant and Edge Chain the defaults; and click Done from the RND SET ATTR menu. 6. Click Surf Chain from the CHAIN menu. 7. Query Sel the hidden bottom surface and click Accept . 8. Select all the highlighted edges to round. Click Select All from the CHAIN OPT menu; then click Done from the CHAIN menu. 9. Enter a radius value. Type [2.0] followed by . 10. Complete the round feature. Click O K . 11. Click Feature List from the INFO pull-down menu.


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NOTES

Note: The system created the round feature after the second protrusion. Also, note the regeneration status of the two chamfers.

12. Click Close to exit the INFORMATION window. 13. Click Feature > Insert Mode > Cancel to exit insert mode. When the system asks you if you want to resume the features that it suppressed when activating insert mode, type [yes]. Task 3. Pro/ENGINEER places you in the Resolve Environment because it cannot regenerate the chamfer feature. The references for the chamfer feature no longer exist because the system replaced them with the round feature that you created in insert mode. Diagnose the model’s problem. 1. Review all of the information provided in the FAILURE DIAGNOSTICS window. 2. Click Overview and review the Resolve Feature Overview. Close the window. 3. Click Feature Info and review the Failed Feature Info. Close the window. 4. Click Resolve Hints and review Pro/ENGINEER’s suggestions for resolving the problem. Close the window. 5. Click Investigate from the RESOLVE FEAT menu. Accept the default Current Modl , and click Show Ref from the INVESTIGATE menu. 6. Navigate through the window of the missing chamfer by clicking on each item and showing references. When you have finished showing the missing references, click Close . Note: The edge references for the chamfer appear on the screen, but they are no longer part of the model. The round feature that you created removed these edges. Because it regenerated prior to the chamfer, it regenerated successfully and the chamfer failed.



NOTES

Task 4. Resolve the failed feature by removing the failed chamfer feature from the part model. Recall that the quick fix option for resolve only works on the failed feature. 1. Click Quick Fix from the RESOLVE FEAT menu; then click Delete from the QUICK FIX menu. Read the prompt. Click Delete All > Yes from the YES/NO menu to exit the Resolve Environment. 2. Again review the feature list. Click Info > Feature List . Note that the chamfer feature is no longer part of the model. 3. Save the model and erase it from memory.


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NOTES


It is not uncommon for models to fail due to problems in design.

•

Pro/ENGINEER provides a Resolve Environment to rectify failed features.

•

Failures usually occur due to design changes in certain parts after an extensive model has been built up.

•

The Failure Diagnostics window in the Resolve Environment displays accurate and specific information regarding particular failures.

•

Rerouting, redefining, suppressing, and deleting a feature along with its children are some of the quick fixes that can be performed on a failed feature.

•

A failed model can more permanently fixed by using the FIX MODEL menu.




Module

19 Information Tools In this module you learn how to obtain many kinds of information from your models and assemblies. You will learn how to query your designs to obtain regeneration information, clearance and interference characteristics, and more.


Obtain information about features, parts, and assemblies.

•

Obtain regeneration information.

•

Calculate mass properties.

•

Calculate clearance and interference between parts.

Page 19-1

NOTES

MODEL INFORMATION It is good design practice to determine the way a model was built before making any modifications and additions. For this, Pro/ENGINEER provides useful tools to extract information about individual features, regeneration, assembly components, and entire models.

Obtaining Information about a Specific Feature Using the Info Feature option, you can obtain information about a particular feature in PART, ASSEMBLY, and DRAWING modes.

Obtaining Regeneration Information Using Utilities > Model Player, you can step successively through the regeneration of the part—starting from a specified feature or from the beginning—in the current order of creation.

Figure 1: The Model Player Dialog Box

The model player option is particularly useful because it allows you to observe the design of a part, and assists you in determining if poor design practices were used to create it.

Accessing Information about Part Features Using the Model option, you can access information about every feature on a part. The system lists regenerated and suppressed features, all



NOTES

coordinate systems, cross-sections, and reference dimensions in an INFORMATION WINDOW. Using Feature List , you can list all features in the model in their regeneration order and obtain the feature number, feature ID, name, type, suppression order, and regeneration status for each.

Obtaining Information about Assemblies Using the Component option in ASSEMBLY mode, you can obtain information about how a component was assembled, how its parent/child relationships and parameters were formed. You can also use the Model option to access information about selected assembly components. In the INFORMATION WINDOW, the system displays the names of the components in a hierarchical structure to show how they were assembled.

Tips & Techniques: The system lists only the names of the objects in the Information Window. However, if you set the configuration file option DISPLAY_FULL_OBJECT_PATH to yes, it displays the full pathnames of the objects, along with their object-types and version-number suffixes.

MEASUREMENT, INTERFERENCE, AND MASS PROPERTIES With Pro/ENGINEER’s ANALYSIS pull-down menu you can: •

Add engineering information to a model.

•

Analyze the model through measurement.

•

Check interference.

•

Calculate mass properties.

Calculating Mass Properties Using the Model Analysis option, you can compute mass properties for parts, assemblies, and cross-sections.

For University Use Only - Commercial Use Prohibited Information Tools

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NOTES

In a mass properties calculation, the system does not include the mass of suppressed features or suppressed components in any assembly.

Note By default, mass properties do not automatically update when you make changes to the model. You must recalculate the mass properties to Using the Model Analysis option, you can:

•

Calculate volume or interference between pairs of any combination of subassemblies, parts, surfaces, cables, and entities.

•

Perform a global clearance check to find all pairs of parts or subassemblies with clearances less than a specified clearance distance.

•

Perform a global interference check to find all interfering pairs of parts or subassemblies.



NOTES

LABORATORY PRACTICAL Goal In this laboratory you learn to extract information to determine how a part was created.

Method In Exercise 1, you learn to use information tools to calculate measurements.

EXERCISE 1: Using Information Tools Task 1.

Interrogate the regeneration cycle of a gear part .

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 19_info_tools. 3. Open GEAR_COUNTERWEIGHT.PRT. 4. Click Utilities > Model Player. 5. Click

to rewind the model player.

6. Click

to step through the model.

7. Click Show Dims. 8. Click Feat Info to obtain information about the feature to see how it was created. 9. Click Close in INFORMATION WINDOW. 10. Click to continue to step through the regeneration of the part, feature by feature. 11. Complete the regeneration and close the MODEL PLAYER dialog box. 12. Click Info > Model .


P a g e 1 9- 5

NOTES

13. Scroll through the feature list in the INFORMATION WINDOW dialog box, then close. Task 2.

Determine mass properties for the model.

1. Click Analysis > Model Analysis. 2. Click Compute , accepting all the default options in the MODEL ANALYSIS dialog box. 3. Click Info in the MODEL ANALYSIS dialog box. Information on the mass properties gets displayed. 4. Scroll down the INFORMATION WINDOW and close it when you are done. 5. Close the MASS PROPERTIES dialog box. Task 3.

Measure the model.

1. Click Analysis > Measure 2. In the MEASURE dialog box, click Area from the TYPE drop-down list. 3. Select the front cylindrical surface. select this edge to measure the length.

First select this surface to calculate the surface area.

Figure 2: Measuring Surface Area and Curve Length



NOTES

Task 4.

Measure the length of the gear edge feature.

1. Click Curve Length in the TYPE drop-down list. 2. Select the gear edge as shown in the preceding figure. 3. The length of the edge appears in the message area of your screen and also in the RESULTS area of the dialog box. Task 5.

Measure the distance between two vertices:

1. Click Distance from the TYPE drop-down list. 2. Click Vertex from the FROM drop-down list. 3. Select the vertex as shown in the following figure. 4. Select Vertex from the TO drop-down list 5. Select the second vertex as shown. 6. The system measures the distance between vertices and displays it in the message area and in the RESULTS area of the dialog box. 7. Click Close .

Select this vertex first.

Select this vertex second

Figure 3: Measuring Distance

8. Save the model.


P a g e 1 9- 7

NOTES




NOTES


With Pro/ENGINEER you not only provide information to the system while building models but you can also retrieve information for analysis or manufacturing purposes.

•

In any model you can obtain information about any specific feature.

•

You can access information about any specific part to learn how it was built feature by feature using the Regen Info option

•

You can calculate mass properties for parts, assemblies, and sections using the Model Analysis option.

•

In a part you can measure, among other things, distances between vertices, length of curve edge, and surface areas.

•

You can calculate interference between pairs of any combination of subassemblies, parts, surfaces, cables, and entities to reduce the amount of calculation time needed to perform a global interference check among all components.


P a g e 1 9- 9



20 Configuring Pro/ENGINEER In this module you learn how to modify your Pro/ENGINEER working environment. You learn how to configure Pro/ENGINEER either to create a company-wide standard or to suit your own individual needs.


Locate network-based Pro/ENGINEER configuration files.

•

Create customized Pro/ENGINEER work sessions.

•

Automate processes with map keys.

•

Configure your toolbar and model tree

Page 20-1

NOTES

CUSTOMIZING PRO/ENGINEER You use configuration files to customize your Pro/ENGINEER work environment. These files can include your preferences for tolerance, display formats, calculation accuracy, the number of digits used in Sketcher, and so on. The default name for the Pro/ENGINEER configuration file is CONFIG.PRO. You can edit configuration files to set company standards in several areas, including: •

Storing drawing formats.

•

Submitting project objects.

•

Setting default measurement units for new parts (such as millimeters instead of inches).

•

Setting library file locations.

Defining Configuration Files Pro/ENGINEER can read configuration files from several areas, as shown in the following figure. However, if a particular option is present in more than one configuration file, uses the last value read will be used. When starting, Pro/ENGINEER first reads a protected configuration file called CONFIG.SUP (the “.sup” extension stands for “Supervisor’s configuration file”) from the directory /TEXT (the directory from which you install Pro/ENGINEER). These options override the same options that may be set in other configuration files. This file can be used to establish customized company standards for all of your Pro/ENGINEER users. Every entry in the CONFIG.SUP file locks out any duplicate entries in your local CONFIG.PRO configuration files.


Configuring Pro/ENGINEER

NOTES

Figure 1: Possible Locations of Configuration Files on a Network

Pro/ENGINEER reads in configuration files from the following directories in this order: •

The CONFIG.PRO file in the LOADPOINT directory.

•

The CONFIG.PRO file in your home directory.

•

The CONFIG.PRO file in your start-up directory.

•

Default values built into the software. Note For a complete listing of configuration file options and defaults, refer to the Introduction to Pro/ENGINEER User’s Guide.

Editing Configuration Files You can edit configuration files during your working session. Do this by using the Options option in the UTILITIES menu. The following figure shows the OPTIONS dialog box.

For University Use Only - Commercial Use Prohibited Configuring Pro/ENGINEER

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NOTES

Figure 2: Preferences Dialog Box

Note Configuration files are not automatically loaded after editing. They have to be loaded by clicking the Apply button.

CreatingMapkeys A Mapkey is a keyboard macro that you can create using the Mapkeys option in the UTILITIES pull-down menu. It performs a series of selections when you type only one or two keystrokes. The MAPKEYS dialog box lists each mapkey that is in session and provides a description of its function. The RECORD MAPKEY dialog box allows you to create, modify, run, delete, and save mapkeys to a configuration file. Both are displayed in the following figures.



NOTES

Figure 3: Mapkeys and Record Mapkey Dialog Boxes

CUSTOMIZING YOUR TOOLBAR Adding Icons to Existing Toolbars All pull-down menu options can be associated with easy-to-use toolbar icons. To do this, you can create new icons and add them to existing toolbars The CUSTOMIZE dialog box includes a list of existing pull-down menu options on the left with corresponding icons on the right. This is illustrated in the following figure. As you go down the menu options on the left, you can simply drag the associated icon of your choice onto the toolbar.


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NOTES

Figure 4: Setting Toolbar Icons

Saving the Settings You save your changes to toolbars by using the Automatically Save To option in the CUSTOMIZE dialog box. This option creates a file called CONFIG.WIN in the same directory that the file resides in. This file automatically loads when Pro/ENGINEER is started the next time.

Creating Pull-down Menus You can create a separate pull-down menu for newly defined Mapkeys. This allows the use of the mouse to select your mapkey definitions. Quick keys, such as F1 , are also valid for the mapkey.



NOTES

Tips & Techniques: Name keystrokes so that you can easily remember what they refer to. An example is sd for Cosmetic Shade."

Associating New Icons for Mapkeys Mapkeys have a default icon associated with them but you have the option to change the icon. With the CUSTOMIZE dialog box open, you can modify the displayed icon. The modifying options include the ability to: •

Delete the icon.

•

Copy the icon image.

•

Paste a copied icon image.

•

Edit the icon image with an icon editor.

•

Choose a button image from a predefined list.

•

Show the text associated to the icon.

THE MODEL TREE The MODEL TREE is a powerful tool to organize and manipulate active objects. Most importantly, the MODEL TREE is an information tool as well as an interactive operations tool, complete with a configurable interface and search engine.


P a g e 2 0- 7

NOTES

Figure 5: MODEL TREE Display

In addition to using the MODEL TREE tool to display features, you can also configure it to maintain predefined and customized columns that correspond to items in the tree. Some commonly used columns are: •

Info –

provides information regarding:

Status (regenerated, unregenerated, failed, frozen, or suppressed) Feature number Feature ID (as shown in the preceding figure.) Feature type •

Feature name Layers – Provides the status of layers.

•

Model Params –

Displays new model parameters affecting the entire

model. •

Feat Params –

Displays new parameters affecting a feature.



NOTES

Figure 6: MODEL TREE COLUMNS Dialog Box

The MODEL TREE COLUMNS dialog box is available with the VIEW menu Model Tree Setup option.


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NOTES

LABORATORY PRACTICAL Goal In this laboratory you learn to configure the default Pro/ENGINEER interface to suit your working environment.

Method In Exercise 1, you develop a configuration file and a toolbar to customize the Pro/ENGINEER working environment. In Exercise 2, you create a mapkey to help increase efficiency.


Icons

Description Save as Mapkey icon you create



NOTES

EXERCISE 1: Setting Up a Configuration File Task 1.

Create a new configuration file in the local directory and edit it.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 20_config_proe. 3. Open BUSHING.PRT. 4. Click Utilities > Options.

Figure 7: Editing the Configuration File

Task 2. Alter default values to tailor the working environment to suit your preferences. 1. In the SHOWING dropdown menu, select Current Session . 2. Clear the Show only options loaded from file check box. 3. In the SORT drop-down box, select By Category . Now, set it back to Alphabetical . 4. Scroll down the list and select spin_center_display.


P a g e 2 0- 1 1

NOTES

5. The default Value is YES , which means the spin center will always be displayed when Pro/ENGINEER is launched. 6. In the VALUE drop-down list, select No , then click Add/Change .

Figure 8: Selecting a Configuration File Option.

7. Check the Show only options loaded from file box. Only the options you have changed from the default settings will be listed. 8. In the OPTION box, type [spin_with_part_entities], then press . 9. In the VALUE drop-down list, select YES and click Add/Change . This option is added to the list of changed settings for this session of Pro/ENGINEER.



NOTES

Figure 9: Second Option Added

Task 3. Add additional options using a Keyword Search. Look for an option that will prompt you to save any "unsaved" data when you exit Pro/ENGINEER. 1. In the OPTIONS dialog box, click Find . 2. In the TYPE KEYWORD box, type [exit]. 3. Click Find Now . One option is found. Read the description and select it. 4. Set the default value to YES in the SET VALUE dialog box. Click Add/Change . Task 4. Add an option that includes more lines to the message area of Pro/ENGINEER. 1. In the TYPE KEYWORD box, type [message]. 2. Click Find Now .


P a g e 2 0- 1 3

NOTES

3. Select visible_message_lines.

4. Select visible_message_lines in the CHOOSE OPTIONS dialog box. Type [5] in the SET VALUE box. 5. Click Add/Change > Close . 6. Click Apply in the OPTIONS dialog box. Task 5. Save the changes to the settings such that they are effective every time Pro/ENGINEER is launched.

1. Click

.

2. Leave the default [config.pro] as the name. 3. Click OK > Close . 4. Click File > Exit to save the file and exit the editor.



NOTES

Task 6. Verify that the changed settings are currently in effect. Some settings will require a software restart to be active 1. Click File > Exit. 2. Start a new session of Pro/ENGINEER and open BUSHING.PRT. 3. Spin the part using the mouse. Notice that the datum planes remain displayed during spinning. This is a result of the change to the spin_with_part_entities option. 4. Modify a feature. Click Modify . Select the center hole of the bushing. Select the 19.12 dimension, type [10.00]. 5. Click Regenerate to update the geometry. Notice that the message window has been expanded to list five lines. 6. Click File > Exit > Yes. Since you modified the bushing but did not save it, you are presented with the option to save the model. 7. Press to save the part. 8. Restart Pro/ENGINEER.


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NOTES

EXERCISE 2: Creating a Mapkey Task 1.

Create a mapkey that will rename a feature.

1. Click File > Set Working Directory . 2. Set the working directory to \ intro_proe_320 \ 20_config_proe. 3. Open CRANK.PRT. 4. Click Utilities > Mapkeys. 5. Click N e w in the MAPKEYS dialog box. Task 2.

Define a mapkey to develop .

1. Type [fn] as the KEY SEQUENCE. 2. Type [Feature Name] as the NAME. 3. Type [Name a feature for easy identification] for DESCRIPTION . 4. Select Pause for keyboard input . 5. Click Record . Task 3.

Record the mapkey.

1. Click Setup > Name . 2. Select on the hole feature in the model. 3. Type [Shaft_bore] and press 4. Click Done . 5. Click Stop in the RECORD MAPKEYS dialog box. 6. Click OK . 7. Click Save leaving the default name CURRENT_SESSION.PRO. 8. Close the RECORD MAPKEY dialog box



NOTES

Task 4.

Test your new mapkey.

1. Type [fn]. 2. Select on the boss and type [boss] as the new name. 3. Click Info > Feature List . You will notice the new names you have given to the model features. Task 5.

Learn to include an icon onto your toolbar.

1. Click Utilities > Customize Screen. 2. Select the third icon from the right; then click Description . 3. Read the description, then click . 4. Drag the icon next to the OPEN icon on the SAVE toolbar, as shown below:

Figure 10 Inserting Erase Icon into the Standard Toolbar

Task 6. Customize your toolbar to include an icon for the [fn] mapkey you created. 1. In the CUSTOMIZE dialog box, select Mapkeys in CATEGORIES to highlight it. 2. In the MAPKEYS area of the dialog box, click the smile face . 3. Click Modify Selection > Choose Button Image . 4. In the SELECT MAPKEY ICON dialog box, click 5. Now drag it from the dialog box onto your toolbar. Note The system will automatically save the changes the CONFIG.WIN file to your working directory. You can change the directory that the file is saved to.


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NOTES

Task 7.

Finish the definition of the toolbars.

1. Notice the entry at the bottom of the dialog box. Leave the option to automatically save the file and click OK . 2. A part of your customized toolbar could look like this:

Feature name mapkey icon

Figure 11:Customized Toolbar

3. Erase the current testing model from memory. Click the newly added Erase Current icon from the toolbar, then click Yes.



NOTES


The Pro/ENGINEER environment is customizable.

•

You should first load the CONFIG.PRO file in order to configure your environment.

•

You can create mapkeys, or macros, of frequently used series of steps in the design process.

•

New toolbars and toolbar icons can be created to associate with the mapkeys you create.

•

New pull-down menus can be created.

•

The MODEL TREE can be used as an effective information tool with many customizable columns.


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Module

21 Modeling Philosophy Design intent is the concept that connects the various techniques for creating parts, assemblies, and drawings. Capturing design intent by various methods is the core of Pro/ENGINEER's modeling philosophy.


Describe how to incorporate your design intent into new models.

•

Describe the benefits of using parent/child relationships in your designs.

•

Describe how to use relations.

•

Describe the importance of associativity in Pro/ENGINEER.

•

Describe how to change design intent in your models.

Page 21-1

NOTES

DESIGN INTENT Before you start designing parts and assemblies in Pro/ENGINEER, it is important that you first define the intention of your design. At this preliminary stage, the high-level design intent is usually already understood. Before starting a new design in Pro/ENGINEER, you should be able to answer following questions: •

What is the purpose of the product? How will it satisfy this purpose?

•

What are the major subsystems necessary to satisfy this function?

•

How will these individual subsystems be incorporated into the overall product?

•

What design changes are likely to occur as the product is being developed?

•

Is this a new design or is it based on an existing product?

•

What are the relevant design constraints? (size, weight, cost, and so on)

•

How will this product interact with its environment?

Answers to many of these questions may already exist in the form of product specifications, product quotes, and proposals. Also, any conceptual design work that has already been completed should provide information on how the product will look and how each of its subsystems will interact with one another. This information can be managed using Pro/INTRALINK and Pro/ENGINEER. Existing documents that are not Pro/ENGINEER files can be managed by Pro/INTRALINK. Dependencies between the nonPro/ENGINEER files and the assemblies and parts with which they are associated can be created, so that this information is available to the designer working on the detailed components. In addition, conceptual design results and ideas can be captured in Pro/NOTEBOOK. Pro/NOTEBOOK (also known as Layout Mode) is an optional module within Pro/ENGINEER that provides tools to create twodimensional layouts. Two-dimensional sketches and pictures of an assembly design can be documented with critical design dimensions, notes and parameters. These parameters can be shared globally among all components of the assembly and can be used to drive design parts, assemblies and skeletons.



NOTES

Recording Your Design Criteria Before you start creating a model, you should record the design criteria for the model that would include: •

Order of features

•

Feature form

•

Base feature

•

Feature type

•

Feature duplication

•

Depth

Using Pro/ENGINEER as a Parametric Tool •

One of the major facets of the parametric nature of Pro/ENGINEER is the ability to generate parent/child relationships.

•

You can also use Pro/ENGINEER to interrelate feature dimensions by creating relations without creating parent/child relationships.

Creating Parent/Child Relationships Methods The following are some of the ways in which you can create parent/child relationships among features: •

Specifying the sketching/placement plane.

•

Orienting the reference plane.

•

Dimensioning and specifying Sketcher references and constraints.

•

Defining feature depth /depth references.

•

Edge references (Rounds/Chamfers)

•

Component Assembly constraints.

Using Relations Relations allow you to create a relationship between features or components in an assembly without creating a parent/child relationship in which child features control their parents.

Note You can document the modeling intent by commenting the relation and changing the symbolic name.

For University Use Only - Commercial Use Prohibited Modeling Philosophy

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NOTES

Optimizing Designs with Relations

If you have developed good parent/child relationships along with a welldefined parametric behavior of the model, relations can elevate as well as optimize certain design criteria. Optimizing Designs with Behavioral Modeler

With Behavioral Modeler you have the ability to perform an iterative analysis of your design by developing a Design Study. A multitude of objectives can be met this way. You can: •

Determine the dependency between a design specification and a model parameter or dimension using a Sensitivity Analysis.

•

Find a set of values of specified model parameters that satisfy a set of design specific criteria using a Feasibility study.

•

Find a set of values of specified parameters that optimize the design based on some criteria while satisfying a set of design specifications using an Optimization study.

Advantages of Pro/ENGINEER Associativity Creating Assemblies Associativity among drawings, parts, features leads to easy regeneration while reducing the effort needed in designing complex machines.

Creating Skeleton Parts You can also create parts at the assembly level, referred to as skeletons, to capture the intent of the interrelationship between components in an assembly. You can also use these parts to define motion in an assembly.



NOTES

Figure 1: Skeleton Example

Using Engineering Notebooks Pro/ENGINEER allows you to generate a centralized location to capture, document, and control the design intent of a product model. Layouts and parametric relations can be stored and retrieved as necessary

Changing Design Intent •

Redefine

•

Reroute – Changes

•

Insert Mode – Changes

•

Reorder – Changes

•

Interchange Mode – Changes

– Changes any of the originally defined elements in features or defined constraints in an assembly. the external references that features and components have in a model. the regeneration cycle by allowing you to insert features or components into the regeneration cycle. the order of the regeneration of existing features in a part or components in the assembly. the design intent of an assembly by swapping one functionally equivalent model with another.


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NOTES

LABORATORY PRACTICAL Goal The goal of this lab is to review in a classroom question-answer format the main points about capturing design intent with Pro/ENGINEER.

Methods In Part 1, capturing Part Level Design Intent is discussed. In Part 2, capturing Assembly Level Design Intent is discussed.

Part I: Part Level Design Intent In the following part model the goal is to build the model as efficiently as possible, while maintaining Design Intent. Since the only source of design intent available is the drawing on the following page, it must be strictly followed. The entire model must be built using only those dimensions shown: no more, no less. For example if a particular feature uses a certain dimension, no other feature may use the same dimension.

Figure 2: Building a Model with Specific Design Intent



NOTES

Decision Process Questionnaire 1.

What should the base feature be?

ANS:

2. What feature types are possible for the base feature? ANS:

3. Which of the possible feature types will best fit out Design Intent? ANS:

4. What type of feature(s) can create next feature? ANS:

5. Which of the possible feature types will best fit out Design Intent? ANS:

6. What order should the features be created in? ANS:

7. How should the small hole be created twice? ANS:


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NOTES

8. When should the rounds be created? ANS:



NOTES

Figure 3: Drawing of Part Model


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NOTES

Part II: Assembly level Design Intent For the next discussion, consider the following views and drawing of the VALVE assembly. Overall, determine courses of action to create the assembly. The part models may or may not have already been created in Pro/ENGINEER.

Figure 4: Assembling Parts

Decision Process Questionnaire 1. What technique could be used to help relate the components together for assembly and motion analysis purposes? ANS:



NOTES

2. What types of features could exist in a skeleton? What might it look like? ANS:

3. Which component should be assembled first? Second? How is this affected when using a skeleton? ANS:

4. What implications could arise from deleting the center shaft? Suppressing? Blanking on a Layer? Replacing? How could some of these issues be handled? ANS:

5. How should the assembly be structured with subassemblies? ANS:

6. We wish to be able to change the angular constraint on the center shaft from 0° to 90°. How does this affect our decisions? ANS:

7. What effect would changing the center shaft diameter have on the other components? ANS:


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NOTES

8. How would interactions with other components affect the process? ANS:

Figure 5: Assembly Drawing



NOTES


Pro/ENGINEER's modeling philosophy is driven by considerations of effectively capturing design intent.

•

Pro/ENGINEER's feature-based, parametric, and associative nature has many advantages in achieving the desired intent.

•

The capacity to introduce parametric relations while creating models is a special feature of the software that furthers the cause of design intent capture.

•

Parent/Child Relationships in Assemblies and methods of specifying and altering them enables changes in intent.

•

Information tool, drawings, engineering notebooks, the behavioral modeler, the ability to customize Pro/ENGINEER environment, the Resolve Environment to solve regeneration problems—all in their own respective ways help in the overarching goal of capturing design intent and thus are essential components of Pro/ENGINEER's modeling philosophy.


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Appendix

A Review Questions This module contains review questions intended for an interactive daily discussion in class. It is divided into five sections corresponding to the five days of instructor-led training.


Review the important concepts and principles that are covered during each training day.

•

Participate in discussion of related topics.

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NOTES

DAY 1: REVIEW QUESTIONS 1. What is design intent?

2. List three pick and place features.

3. List two types of sketched features.

4. What are the advantages of a solid model?

5. List three types of holes. What are the placement options for each?

For University Use Only - Commercial Use Prohibited P a g e A- 2


NOTES

6. How does the sketching plane capture design intent? The Reference Plane?

7. List two ways to create an edge chain round.

8. What is the difference between a hole and a cut?

9. Must the reference plane always be perpendicular to the sketching plane?

10. What is the Pro/ENGINEER convention for orienting the view of the sketching plane when creating a feature that adds material? Removes material?

For University Use Only - Commercial Use Prohibited Review Questions

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NOTES

11. What does feature-based modeling mean?

12. What does parametric mean?

13. List two functions that References provide in Sketcher.

14. What is the most important thing to ‘build’ into your sketch before exiting Sketcher?

15. What is the difference between the options for ONE SIDE compared to BOTH SIDES for a protrusion or cut?

16. List the nine Sketcher constraint options. Which of these options are multi-purpose?



NOTES

17. Can you over-dimension or under-dimension a section in Intent Manager?

18. With what features can Dynamic Modify be used? How is it activated?

19. Why does Intent Manager create “weak” dimensions? How can you remove them?

20. What is the easiest procedure for deleting or redefining features?


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NOTES

DAY 2: REVIEW QUESTIONS 1. What is a model template? What does it contain?

2. When should you use a start template? Can it be customized?

3. What is the importance of the first solid ‘base’ feature?

4. Do the sketching plane and reference plane always become parents to a sketched feature?

5. When orienting the sketching plane using a horizontal reference, if you click Top from the menu and select Datum TOP , which side of Datum TOP will face the top of the computer screen?



NOTES

6. What is a parent/child relationship in Pro/ENGINEER, and why is it so important?

7. Do Sketcher references establish parent/child relationships? List six ways a Sketcher reference can be established.

8. Why would you want to set up a parameter in Pro/ENGINEER?

9. What is required in the sketch of a revolved feature? What is the case with more that one of this entity type?

10. What are the two sections required for a swept feature?

11. How would you create a 3-Dimensional (3-D) sweep?


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NOTES

12. What is the minimum number of sections required for a blended feature?

13. What are the requirements for each section of a blend?

14. Is it possible to create a swept or blended cut?

15. For what purpose do you use relations? Give an example.

16. How do you know if your relation is working correctly?

17. What are the three types of blends? What are the two options for each?



NOTES


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NOTES

DAY 3: REVIEW QUESTIONS 1. What is a Datum Analysis feature and how is it used? List three types.

2. What does BMX stand for?

3. Sensitivity and Optimization/ Feasibility studies are major components of Behavioral Modeler. Briefly define each.

4. What is the difference between an Analysis and an Analysis Feature? An Optimization and an Optimization Feature?

5. What is a drawing template? List at least three functions that a template can be setup to perform.

For University Use Only - Commercial Use Prohibited P a g e A- 1 0


NOTES

6. How can you make multiple instances of a single feature? A single instance of multiple features?

7. Why is it important to use default datum planes when orienting a general view in a drawing?

8. What is unique about a general view?

9. What is the difference between a Projection view and an Auxiliary view? A Detail view and a Partial View?

10. How can you create a rotational dimension in a sketched feature that you are going to pattern?

11. How do you include a dimension and/or parameter in a drawing note?


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NOTES

12. How should you start every assembly?

13. What is the importance of the base component in an assembly?

14. Are parent/child relationships relevant in Assembly mode?

15. A drawing is created from bracket.prt, and modifications are then made to the bracket. The drawing views will then have to reprojected. True or False? What about the assembly using the bracket? What is this ability called?

16. How can you change a component’s placement references without having to delete the component and reassemble it? How can this be accomplished with no menu interaction?



NOTES

17. What does and the three mouse buttons do when assembling a component?

18. List five of the constraint types for assembling a component.

19. What is the importance of subassemblies, and how can you create them in Pro/ENGINEER?

20. What are the differences among Mod Dim, Mod Assem, Mod Subasm, and Mod Part?

21. List the various options for Copying features.

22. List and compare the three Pattern types. How many directions are available for each?


P a g e A- 1 3

NOTES

DAY 4: REVIEW QUESTIONS 1. For what purpose can you use layers in Part mode? Assembly mode? Drawing mode?

2. What are three reasons why you might want to suppress a Pro/ENGINEER feature?

3. Layers do not affect parent/child relationships, while Suppression does. True or False?

4. List four types of additional datum features.

5. What are some uses for datum curves?

6. Describe the major concepts of Top Down Design



NOTES

7. What are six steps or phases of Top Down Design?

8. What is a skeleton and how can it be used?

9. Can a skeleton be used for part design as well as assembly design? If so, How?

10. What is a surface? What types of models benefit from surfacing?

11. What does ISDX stand for?


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NOTES

12. Is ISDX the only way to create surfaces in Pro/ENGINEER?

13. What can be accomplished with the STYLE feature?

14. How many features (curves, surfaces) can be contained in a style feature?

15. What is required to generate a surface using ISDX?



NOTES

DAY 5: REVIEW QUESTIONS 1. What is a parent/child relationship in Pro/ENGINEER?

2. List seven ways to establish a parent/child relationship in Pro/ENGINEER.

3. What is design intent?

4. What does associativity mean?

5. What is a configuration file in Pro/ENGINEER, and why should you use these files?

6. What is a mapkey?

7. When does Pro/ENGINEER activate the Resolve Environment?


P a g e A- 1 7

NOTES

8. Will Pro/ENGINEER allow you to save a model that has a failed feature?

9. What is the difference between the Quick Fix and Fix Model options in the RESOLVE menu?

10. Why should you generally try to fix failed features instead of using the Undo Changes option in the Resolve Environment?

11. What is the difference between Redefine and Reorder?

12. What are some advantages of feature-based modeling?



NOTES

13. Name four ways to capture design intent in a part model.

14. Name three ways to capture design intent in an assembly.

15. What options are avialable under Analysis> Measure ? In Analysis > Model Analysis?

16. What is the model player and how can it be used?

17. What is your next step in the process of attaining mastery with Pro/ENGINEER?


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Appendix

B Project Laboratory This module contains an advanced self-paced project that you can work on after finishing the standard module exercises. The purpose of this project is to provide you with an opportunity to practice the skills you learned in the class without relying on step-by-step instructions.


Apply the skills you learned in the course to real-world design projects.

Page B-1

NOTES

INTRODUCTION Throughout the next few days you will design several assembly components. It is suggested that you use the project components that you create during this course as part of this project lab. However, you may choose to skip portions of the project and instead use the supplied models to complete sections of the project laboratories. As shown in the next figure, you will create a motor part, lower housing part, snap ring part, and upper housing part. These components will be used to build a blower and motor assembly. Throughout the project, you will be working in the directory named project. All measurement units are in metric.

Snap rings

Motor housing Cover

Motor shaft Upper housing Lower housing Blower

Figure 1: Exploded View of Completed Project

For University Use Only - Commercial Use Prohibited P a g e B-2


NOTES

PART CREATION SECTION 1: Creating the Motor Part To follow the design intent of the motor part, you must build it using only those dimensions shown in the following figure. You create the part using extruded sketched features, along with holes. In addition, you also use relations to constrain the electronics support foundation (rectangular shaped protrusion) a constant distance from the back surface of the base feature.

Figure 2: Dimensions for Motor Part

1. Create a part named motor.prt. 2. Create the first solid feature. You may want to extrude a 70.00diameter circle to a blind depth of 90.00. 3. Add a feature to represent the electronics support foundation. This foundation must be rectangular, measuring 82.5 X 60.0, as shown in the following figure (with the height measuring 60.00 from the center of the motor).

For University Use Only - Commercial Use Prohibited Appendix B

P a g e B-3

NOTES

Figure 3: Electronics Support Foundation

4. To follow the design intent, place the electronics support foundation a distance of 7.5 away from the surface of the cylindrical base feature. Write a relation to cause the size of the electronics support (base feature) to change when the base feature depth changes. Regenerate the part and test the relation by modifying the depth dimension of the base feature. Remember to change the dimension back to the original depth value of 90. 5. Add the 100.0-diameter front protrusion feature to the model. You will use that for a bolt flange. 6. Add a cut feature to the model so that you can remove material to receive an armature. Assign it a 60.00-diameter and leave a 5.0wall thickness at the back of the motor, as shown in Section A-A. Tips & Techniques: You should pay careful attention to your selection or creation of a datum plane for the section, as well as what type of feature you create. The 5.0 wall thickness is the key to these selections.

7. Add a 15.0-diameter hole feature to the back of the motor to use for the motor shaft. 8. Save the model and clear the window by erasing the part.



NOTES

SECTION 2: Creating the Lower Housing Part According to the design intent of the lower housing part, the revolved cut must remain a specific distance from the side surfaces of the base feature so that the model maintains a specific wall thickness. In addition, if the diameter dimensions of the base support changes, the support feature and flange feature should change as well.

Figure 4: Lower Housing Part

1. Create a part named lower_housing.prt. 2. Create the first solid feature. You may want to extrude a 120diameter semicircle to a blind depth of 80. 3. Create a flange to bolt this part to another component in an assembly. As shown in the following figure, give the flange feature dimensions of 15 x 4.1 (Hint: Using the power of feature-based modeling, create the feature with an open section.)


P a g e B-5

NOTES

Figure 5: Lower Housing Flange

4. Add the base support feature to the model. Sketch the feature on the central datum plane and extrude the feature in both directions, as shown in the two following figures.

Figure 6: Lower Housing Base Support



NOTES

Figure 7: Lower Housing Base Support Section

Note: In this figure, the sketched centerline is aligned to the silhouette edge of the cylindrical surface of the base feature.

5. Add a revolved cut feature to the model as shown in the following figure. Regardless of how the base feature changes in depth, the wall thickness should remain 2.5.

Figure 8: Lower Housing Revolved Cut


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NOTES

6. Cut away part of the front housing, as shown in the following figure.

Figure 9: Lower Housing Cut

7. Add a 30-diameter hole feature at the rear of the housing as shown in the Lower Housing dimensions at the beginning of this section. After you have finished, save the model and erase the part from memory.



NOTES

SECTION 3: Creating the Snap Ring Part The snap ring part is purchased directly from a supplier, so it does not need a flexible design. You can create it with only two features.

Figure 10: Snap Ring Dimensions

1. Create a part named snap_ring.prt. 2. Create a solid feature by extruding the outline of the snap ring, as shown in the following figure. The part has a thickness of 1.5mm

Figure 11: Snap Ring Section


P a g e B-9

NOTES

3. Add a 2-radius simple edge round as indicated. After you have finished, save and erase the model.

Round these edges.

Figure 12: Snap Ring Rounds

For University Use Only - Commercial Use Prohibited P a g e B-1 0


NOTES

SECTION 4: Creating the Upper Housing Part According to the design intent of the upper housing part, the diameter of the base feature relates to all the other features. You place the discharge on the model symmetrically back-to-front. You use a swept feature to create a portion of the model geometry that represents the housing, centering the sweep about the base feature. By extruding the base feature on both sides of the sketching plane, you can avoid having to create an additional datum plane later. To complete the housing discharge geometry, you create a blend feature to incorporate the widening characteristic of the discharge housing.

Figure 13: Upper Housing Dimensions

1. Create a part named upper_housing.prt. 2. Extrude a 120-diameter semicircle to a depth of 80. Extrude on both sides of the sketching plane so that you can use the same sketching plane for the trajectory of the discharge housing. 3. Use a swept protrusion with the Free Ends attribute to create a portion of the housing discharge as shown in the first following figure. Make the trajectory of the sweep a line and arc, giving it a


P a g e B-1 1

NOTES

distance of 81.5 from the end of the line to the center of the housing, and assigning a radius of 100 to the arc. Ensure that the sweep remains attached to the base feature at this location, regardless of the diameter of the base feature, by aligning the endpoint of the arc to both the cylindrical and planar surfaces of the base feature (see the second following figure). Locate the start point of the trajectory at the end of the line (notice the centerlines in the third following figure). Create the cross-section as a rectangle. Trajectory

Section

Figure 14: Completed Sweep

Start point

Trajectory

Figure 15: Sweep Trajectory Section



NOTES

Centerlines (provided by system)

Figure 16: Sweep Section

4. Create a straight parallel blend to complete the discharge of the housing. Use only two sections with a depth of 57.5 for Section 2. Create Section 1 of the blend using the edge of the sweep. (Hint: Use a centerline to denote symmetry in Sketcher).


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NOTES

Figure 17: Blend Sections

5. Your part should look like the following figure.

Figure 18: Blend Complete

6. Create a simple, edge chain round with a radius of 15. Your part should look as shown in the following figure.



NOTES

Pick this edge for the tangent chain of the 40 radius

Pick this edge for the 5 radius

Figure 19: Upper Housing Rounds

7. To improve airflow, create a simple edge round with a radius value of 40. 8. Create another simple edge round with a radius of 5. As references, pick the edges where the swept protrusion intersects the first solid feature, as shown in the previous figure.

Remove two hidden surfaces for the shell feature.

Figure 20: Shell References

9. Create a shell feature. Remove these two surfaces as references: the end surface of the discharge diffuser (planar surface of the blended feature), and the bottom flat surface of the first solid feature. Specify a value of 2.5 for the shell thickness. 10. Add a 04.1-thick bolting flange, as shown in the following figure. Make this feature similar to the flange on the motor part.


P a g e B-1 5

NOTES

11. Make a 97.5-diameter cut in the front of the housing, as shown in the following figure.

Flange

Hole Detail

Figure 21: Upper Housing Flange and Cut

12. Make a 30-diameter hole in the back of the housing. If an axis exists in the model, create a coaxial hole. If the model does not have an axis, create a datum axis. Note: To create a datum axis choose Insert , Datum , A x i s, Thru Cylinder and select the cylindrical surface of the base protrusion. You will learn more about datum axis in a later chapter.



NOTES

Figure 22: Upper Housing

13. Add a straight hole, as shown in Detail A of the Upper Housing dimensions at the beginning of this section. After you have finished, save the model and erase it from memory.


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NOTES

CREATING ASSEMBLIES To complete the parts for these assemblies, you modify the parts, create new features, and add relations in both Part and Assembly modes. Although the models are not complete, you also start creating production drawings and assemblies. As you complete this project, you can observe the associativity between the part, assembly, and drawing files. Note: You should attempt to use the models that you completed from the previous project lab. When creating these assemblies and production drawings, you can either use the models that you created previously or the models that are stored in a library which reflect the model at the end of the previous project. The stored models are indicated in parenthesis ( ).

SECTION 1: Creating the Motor Assembly In keeping with the design intent of the motor assembly, you must fully constrain all part models into the assembly. The motor part must be placed as the first component. In this portion of the project, you only change the motor part in Part mode.

Figure 23: Exploded View of Completed Motor Assembly

1. Create an assembly named motor.asm.



NOTES

2. Assemble the motor part you created in the previous project lab (or beta_motor.prt) to the default assembly datum planes. After placing it in the assembly, turn off the datum planes to make it easier to place the remaining component. 3. Assemble the motor shaft part (beta_shaft.prt) into the assembly (see the following two figures).

Figure 24: Motor Shaft Assembled into Motor

Align inside surface of revolved cut of motor shaft with back surface of motor.

Figure 25: Alignment References for Motor Shaft

4. Create another snap ring groove in the shaft so that it does not slide into the motor. Retrieve the motor shaft part (beta_shaft.prt) in a separate window. 5. Pattern the first snap ring groove to create a second one 141.8 from the leader, as shown in the following figure.


P a g e B-1 9

NOTES

Figure 26: Patterning the Groove

6. Save and close the shaft part model. 7. Open the motor assembly. Note that the snap ring groove now appears in the shaft. 8. Assemble snap_ring.prt (beta_ring.prt) into the shaft groove (revolved cut) of motor shaft. 9. Assemble the motor cover (beta_cover.prt) to the motor part. Only create parent child references between the motor part and the cover. 10. Create an assembly pattern to assemble the second snap ring into the assembly using “ref pattern.” 11. Turn the datum planes back on.



NOTES

Figure 27: Motor Assembly

12. Note that the patterned snap ring groove is positioned too far down on the shaft. Modify the offset of the patterned grove in the motor shaft part (beta_shaft.prt). Change the distance to 127.5 and Regenerate. 13. Save the assembly.


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NOTES

SECTION 2: Concurrent Design of the Motor Housing At this point in the design process the motor housing and most other assembly components have not been completed. You can work concurrently between assemblies and parts in Pro/ENGINEER. To prepare the motor for mounting holes, create a set of holes in the motor to match the ones that you are going to create in the cover. 1. Open the motor part (beta_motor.prt). Add a hole at an angle using radial placement. When prompted for the dimensioning scheme, use a radial dimension. 2. Create a radial pattern using three instances. When you have finished, save the model and close the window. Create this hole first

Figure 28: Radial Pattern of Holes in the Motor



NOTES

SECTION 3: Creating the Blower Assembly According to the design intent of this assembly, you use the lower housing as the base component and assemble everything to it. As you place components into the assembly, you will find that several features are missing. Create these features using the Modify in Assembly mode. 1. Create an assembly named blower.asm. 2. Assemble lower_housing.prt (beta_lower.prt) to the three default assembly datum planes. 3. The lower housing was created without any holes in the mounting flange. Modifying the part at assembly level, create the hole in lower housing and pattern it in Assembly mode. Create a straight hole on the flange with the dimensioning scheme shown in the following figure. Note: Do not exit the FEATURE menu after creating the hole. In the next task, you use Pattern from the same menu.

Figure 29: Hole Dimension


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NOTES

4. Pattern the hole for a total of four (4) instances including the original. If you exited the FEATURE menu, choose Modify , Mod Part . Select the lower housing; then choose Feature . Note: Do not exit the FEATURE menu after creating the pattern. In the next task, you use Copy from the same menu.

5. According to the design intent, you should mirror the flange along with the pattern of holes to the other side of the model (as shown in the following figure). Offset from this surface for the blower . Mirror plane

Mirror protrusion and holes

Figure 30: Mirror References 6. Assemble the blower that part you completed in the “Patterns and Feature Copying” lesson. (If you did not finish the model, use the part called beta_blower in the current directory.) Use a mate offset command with an offset value of 1 to place it with respect to the back of the lower housing. Exit the part modification menus. 7. View the obvious interference between lower housing and blower by shading the model. Change the dimension for the blower fins from 73.5 to 65.0 and regenerate the part. 8. Assemble the upper housing part (beta_upper.prt) to the lower housing. Fully constrain the component by mating the flange surfaces, aligning the central axis, and aligning the front faces on both components.



NOTES

9. The upper housing does not have a pattern of mounting holes on the flange. Open the part so that you can make the changes in Part mode in its own window. 10. Create the four holes by patterning them with an increment of 20. 11. Use Copy , Mirror to create the bolt flange and holes on the other side of the base feature.

Mirror protrusion and holes.

Figure 31: Upper Housing Copy Command

12. Save the part file and close the window. Activate the assembly window. Note that the assembly now reflects the changes that you made in Part mode. Save the assembly and erase the window.


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NOTES

SECTION 4: Creating the Motor Part Drawing Although you have not completely finished the motor part, you now begin creating the production drawings. In the drawing, the views and dimensions update with changes to the part model regardless of whether you made the changes in Part, Assembly, or Drawing mode. In this portion of the project, you set up the drawing views only; you do the detailing later. 1. Create a drawing named motor.drw. 2. Use a C-size sheet and associate motor.prt (beta_motor.prt) with the drawing.

FOURTH VIEW FIFTH VIEW

SECOND VIEW

SIXTH VIEW

FIRST VIEW

THIRD VIEW

Figure 32: Placement of Views for Motor Drawing

3. Add the first general view. Orient it to a side view of the motor model using the default datum planes. Use No Scale to allow Pro/ENGINEER to determine the scale of the drawing. 4. Add the front projected view, labeled as the second view in the previous figure. 5. Add the back projected view, labeled as the third view in the previous figure.



NOTES

6. Add the top projected view, labeled as the fourth view in the previous figure. 7. Add the cross-section view, labeled as the fifth view in the previous figure. 8. Add sixth view as a general view with a scale of 0.75. 9. Change the display mode of the views. For the first, third, and fifth views, change the display mode to Hidden line , Tan Phantom . 10. Change the display mode of the remaining views to No Hidden, No Disp Tan. Note: Once you set a view using Display Mode , it remains at that setting even if you change the Environment setting.

11. Save the drawing. 12. Create a drawing named motor_asm.drw. 13. Use a C-size sheet and associate the MOTOR.ASM model to the drawing using the dialog box.

FOURTH VIEW

SECOND VIEW

THIRD VIEW

FIRST VIEW

Figure 33: Placement of Views for the Motor Assembly Drawing

14. Place the first general view. Choose No Scale .


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NOTES

15. Place the second projection view. 16. Place the third projection view. 17. Place the fourth projection view. 18. Change the display mode of all of the views to No Hidden, No Disp Tan. When you have finished, save the model and erase all.



NOTES

INTERROGATING YOUR MODELS For this project, you continue developing the models according to the original design intent. You do this by adding features, analyzing mass properties for individual parts and whole assemblies, and investigating interference between components. You also write relations to prevent interference between components. After completing these tasks, you place the blower subassembly into the motor assembly. The cover part is incomplete. According to the design intent, you must create tabs to mount the cover to the motor part, and add cooling slots to the top of the cover, as shown in the following figure.

Figure 34: Cover Modifications


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NOTES

SECTION 1: Designing the Cover Part 1. Open the cover part.

Figure 35: Cover Part

2. To make it easier to create the slotted cuts representing cooling slots, suppress the protrusion, hole, and round on top of the base feature. 3. Add the first slot, as shown in Detail C of the cover modifications. 4. Pattern the slot for a total of seven (7) instances, including the original. 5. Resume the suppressed features. 6. Note in the following figure, the system removed the underside of the small cylindrical boss when you added the cooling fins. The second protrusion was originally sketched on the inside of the base feature. Reorder the cut and pattern after the first protrusion, and note the difference on the model.



NOTES

Material is removed due to feature order.

Figure 36: X-Section of Cover Before Reorder

Reorder leaves material in place.

Figure 37: X-Section of Cover after Reorder

7. Add a protrusion that you can pattern rotationally. For the horizontal or vertical reference plane, use an internal datum at an angle. You can then use the associated angle to pattern later. Sketch the open section shown in the following figure. Extrude to a depth of 5.0.


P a g e B-3 1

NOTES

Open section

Figure 38: Sketching open section

Angle from Make Datum

Cylindrical surface for axis

Figure 39: Rotational Pattern

8. Pattern the leader tab, incrementing the angle by 120 degrees. Make a total of three instances, including the original. 9. Create a datum axis through the cylindrical surface of the leader tab. 10. Reference pattern the datum axis. 11. Create a co-axial straight hole on the leader tab. Make the diameter 7.5.



NOTES

Figure 40: Cover Before Reference Pattern of Holes

12. Reference pattern the straight hole. When you have finished, save the model.


P a g e B-3 3

NOTES

SECTION 2: Completing the Motor Part You have now determined the final design of the base support for the motor part. In this section of the project, you create a support foundation on the cylindrical base feature.

Figure 41: Changes to the Motor Part

1. Open the motor part (gamma_motor.prt). 2. Suppress all features, except for the first solid protrusion and the default datum planes. 3. Add a feature for the motor foundation, as shown in the following figure (Hint: Use a section that will not fill the central hole when it is resumed. An open section will also work).



NOTES

Figure 42: Motor Foundation

4. Resume all suppressed features. 5. Create a cut on the side of the electronics foundation, as shown in Detail A of the changes to be made to the motor part. Pattern the cut to include four (4) instances, including the original.

Figure 43: Side Cut

6. Mirror the patterned cut features that are on the side of the electronics foundation to the other side. After you have finished, save the model and erase all.


P a g e B-3 5

NOTES

SECTION: 3: Completing the Blower Assembly To finish the assembly, you measure interference and create an assembly relation to prevent the blower part from interfering with the other components. In addition, you also create a Bill of Materials (BOM) and calculate the mass properties of the components in the assembly. 1. Open blower.asm (gamma_blower.asm). 2. Change the height of the blower parts (gamma_blower.prt) blade from 65 depth to 73.5. Regenerate the assembly. 3. Measure the interference between the members of the blower assembly. Use the Model Analysis… option in the Analysis pulldown menu. Select Global Interference from the Type drop-down list in the dialog box. Choose the defaults shown in the following figure. Toggle the results of the models by clicking on the arrows in the dialog box.

Toggle between

Figure 44: Modal Analysis Dialog Box



NOTES

4. Explode the assembly model so that you can see inside the model. Click Modify , Mod Explode to change the position of the blower using a normal plane, as shown in the following figure.

Select this surface to define the normal direction

Select these two surfaces

Figure 45: Exploding the Assembly

5. Determine the distance that can be used for the blower. Measure the distance from the back inside surface of the blower to the front inside surface of the blower using Analysis, Measure , Distance and selecting the surfaces shown in the previous figure. Remember the distance value. 6. Modify the blade height again on the blower so it will fit within the lower housing of the model. Change the blade length to be the distance you just measured minus the thickness of the top and base of the blower and a clearance. At the current values the distance is equal to 75 – (5 + 2.5 + 5) or 62.5. 7. Develop a relation that drives the blower to always be centered within the lower housing by driving the offset value. Use the parameters shown in the next figure.


P a g e B-3 7

NOTES

BLOWER PART

LOWER_HOUSING PART

Figure 46: Symbolic Dimensions for Assembly Relations

8. Note that the lower housing part does not have any dimensions that control the inside dimension of the interior opening. According to the design intent, you must control the wall thickness. This intent was captured by driving the revolved cut off the dimension of 2.5 (shown as d8:0, d10:0, and d9:0 in the previous figure) from all the edges of the surface of the model. 9. Create a number parameter in the lower housing part. Open the lower housing (or the gamma_lower.prt) part in a sub-window. Choose Relations and pick the revolved cut and base protrusion to show their symbolic dimensions. 10. Write a relation that is equal to the length of the cut (cut_length = d1 – (d8+ d10)). Remember to use symbolic dimensions. Enter the parameter name in the relation to automatically create a number parameter in the model.



NOTES

11. Save lower_housing.prt (or the gamma_lower.prt) and close the window. Activate the assembly window again. 12. Create another parameter in the blower model that represents the overall height of the blower including the base, blade and top. Open the blower part (or gamma_blower.prt) in another window. Add the following relation, height = d1+d9+d18, to automatically create the parameter height. 13. Save the blower and close the window. 14. Drive the offset of the blower model within the lower housing so that they are equally offset. Enter a relation similar to d0:1 = (cut_length:0 - height:2)/2. 15. Regenerate the model. Check the message area to see if the system displayed a warning; you may have to regenerate twice, depending on the order in which you added the relations. (Hint: Use Sort R e l s.) 16. Click Analysis > Model Analysis to calculate the mass properties of the assembly. Add the density values of your choice to the components. (example 7.63e-9 tonne/mm3 for steel) 17. Use the Info menu to create a BOM. When you have finished, save the model.


P a g e B-3 9

NOTES

SECTION 4: Completing the Motor Assembly In this portion of the project, you complete the motor assembly by constraining the blower assembly into the motor assembly. You also examine the difference between blanking layers in an assembly and suppressing components using the Model Tree tool. While suppressing components, the system places you into the Resolve Environment because component references are missing. 1. Open motor.asm (gamma_motor.asm). 2. Redefine the component constraints of the cover so that the mount holes align with the motor holes. Add an alignment constraint. Pick the axis on the first hole of the tabs on the cover, and the appropriate axis on the motor. 3. Assemble blower.asm (gamma_blower.asm) into motor.asm (or gamma_motor.asm). Use your own discretion when choosing the constraints. 4. Change the column display of the Model Tree to show Status and FeatID. List suppressed components by choosing View , Model Tree Setup , and Item Display.

Figure 47: Model Tree for Motor Assembly

5. Create a layer at the top-level assembly called “base_comp.”



NOTES

6. Set all of the components (not the sub-assemblies) of the motor part to the BASE_COMP layer. 7. Blank the BASE_COMP layer, as shown in the following figure.

Figure 48: Set Display Dialog Box

Note: Note that the motor part is no longer visible in the working window, but it is still listed in the Model Tree with the status of Regenerated.

8. Unblank the BASE_COMP layer. 9. Suppress the motor component. Note: Pro/ENGINEER prompts you to select an option for the child components. However, you cannot reroute or redefine them because they all reference the base component of the assembly.

10. Suspend all child components.


P a g e B-4 1

NOTES

Note: Suspend is a temporary action; it only suspends components in place until the next regeneration, which in this situation occurs as soon as you choose Done/Return. This action causes the assembly to fail.

11. The system places you into the Resolve Environment because the child components have missing references. To exit the Resolve Environment, select Quick Fix and Freeze for all of the components. As soon as the system freezes one component, another component causes you to remain in the Resolve Environment because it is also missing references. 12. Once you have exited the Resolve Environment, review the suppressed, frozen, and regenerated components listed in the Status column of the Model Tree. 13. Resume the motor part. Note that all frozen components automatically update in the Model Tree. Save the model and erase all components.



NOTES

COMPLETING THE PROJECT You are now ready to complete the project by finishing the parts, assemblies, and drawings. After documenting the motor part and motor assembly in production drawings, you review the associativity between all three modes of Pro/ENGINEER.

Front flange

Figure 49: Changes to Motor Part

SECTION 1: Developing the Motor Part According to the design intent, you increase the width of the front flange of the motor part and change the holes in the flange. You make these changes in Part mode. 1. Open motor.prt (delta_motor.prt). 2. Change the thickness of the front flange to 15. 3. Delete the three holes on the front flange. 4. Create three sketched holes using a radial placement. The sketched section is detailed in the next figure.


P a g e B-4 3

NOTES

Figure 50: Sketched Hole Section

Figure 51: The Completed Holes

5. Save the model and close the window.



NOTES

SECTION 2: Finishing the Lower Housing According to the design intent, you strengthen the cylindrical wall of the base feature by creating some ribs with draft features attached to them. 1. Open lower_housing.prt (delta_lower.prt). Build a rib between the cylindrical base feature and the foundation base. See the figure below for dimensions, and use Make Datum to create an offset datum as the sketching plane taking care of the offset direction.

Single sketched line

Datum offset dimension

Figure 52: Rib Dimensions

2. Extract the body of the part from a mold. Create a draft feature on the two parallel sides of the rib. Accept the default attributes of Neutral Plane , No Split, and Constant . Create a neutral plane through the top edge of the rib, parallel to the base surfaces. Use the neutral plane as the reference plane. Enter [ -10] as the draft angle.


P a g e B-4 5

NOTES

Draft surfaces

Figure 53: References for Draft Feature (surfaces meshed for clarity)

3. Copy the rib and draft features to create two supports. Use Move and select the attribute of Dependent . Translate the features with reference to the front of the model by a distance of 3.00 4. Mirror the ribs and draft features to the other side of the part. If the mirroring operation fails because you cannot construct the geometry, redefine the draft angle to -10 degrees. After you have finished this task, save the model.

Mirror plane

Copy these ribs with the draft.

Figure 54: References for Copy of Rib and Draft Features



NOTES

SECTION 3: Completing the Drawing To complete the motor assembly and part drawings, you must detail them. In the part drawing all of the dimensions are feature dimensions. In the assembly drawing, most of the dimensions exist at the component level; the only assembly dimensions are those that you use for offset constraints. Because the assembly dimensions assist in describing the part, they were created in Drawing mode. After detailing the motor drawing, you modify the feature dimensions to show the full associativity of all of the models. 1. Open motorasm.drw (delta_motor_asm.drw). 2. The system automatically places you into the Resolve Environment. Read the prompt in the resolve window. The system cannot place the cover because you deleted the holes from the motor part earlier. 3. Use the Quick Fix option to redefine the placement constraints. Change the missing reference for the assembly to the axis of the sketched hole that you created earlier. 4. Detail the drawing as shown in the following figure, and add the ISO view in the corner. Keep in mind that most of the dimensions were created in Drawing mode. After you have finished the task, save the drawing and close the window.

Figure 55: Assembly Drawing.

5. Open motor.drw (delta_motordrw.drw if you did not complete the motor part or drawing from the previous project lab). Notice how


P a g e B-4 7

NOTES

the features you added to the motor part have automatically been added to the drawing.

Figure 56: The Original Motor Drawing

6. Add additional views, change the default scale to 0.7, and move the additional views to an added sheet on the drawing. Detail the drawing according to the next two figures. When you have finished, save the model.

Figure 57: Sheet 1 of the Motor Drawing



NOTES

Figure 58: Sheet 2 of the Motor Drawing

7. Notice that the axis circle does not appear around the patterned holes on the flange. Change the setup file in the drawing so that radial_pattern_axis_circle is set to YES . Then show the axis of the patterned holes.

Figure 59: Pattern Axis Circle


P a g e B-4 9

NOTES

8. Modify the dimensions of the motor part (delta_motor.prt) foundation in the drawing so that its depth is 7.5. Regenerate the model. Retrieve the motor part into session and examine the changes to the part.

Copy this protrusion translated from this surface

Figure 60: The Modified Base

9. Create a dependant copy of the base using the move option translated 60 units from the surface, as shown in the preceding figure. Add another protrusion to cap of the base with the dimensions shown in the following figure.

Figure 61: The Completed Base



NOTES

10. Open the motor assembly (delta_motor.asm) and examine the changes to the assembly. Finally, retrieve motor drawing and notice how the changes are reflected. Save the drawing, assembly, and parts by saving the assembly drawing. 11. Erase the models from memory and close Pro/ENGINEER. 12. Congratulations!


P a g e B-5 1



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Appendix

D


Using PTC Help You can use PTC Help to quickly search for Pro/ENGINEER information. PTC Help includes quick references and detailed information on selected topics.


Start PTC Help.

•

Search for specific information about Pro/ENGINEER.

•

Obtain context-sensitive help while performing a task.

Page D-1

NOTES

PTC HELP OVERVIEW PTC Help is a fully functional help system that is integrated into Pro/ENGINEER.

PTC Help Features PTC Help offers: •

A new help system with a table of contents, an index, and searching capability

•

Context-sensitive help, allowing access to PTC Help with a click of the mouse

•

Online Tutorials focussed on teaching different aspects of the software

•

Expanded help topics available as special dialog boxes

Please visit the PTC Technical Support Online Knowledge Database , which features thousands of Suggested Techniques. For more information, see the Technical Support Appendix.

USING Pro/ENGINEER HELP Launching Help: Four Methods There are four procedures for launching the help system.

1. Main Menu This is the standard way of accessing the full-blown help system complete with contents, index, and search capabilities. Depending on your system speed, it may take a few seconds to launch the entire help system. Click Help > Contents and Index from the main menu as shown in the following figure.

For University Use Only - Commercial Use Prohibited P a g e D-2


NOTES

Figure 1 Starting PTC Help The Pro/ENGINEER Online Help homepage appears in your web browser window.

Figure 2: Contents and Index in PTC Help

In the left frame of the window, you see a list of topics arranged in a tree structure. By clicking on each higher level topic, you can access subtopics, and by clicking the sub-topics you can access detailed instructions, explanations, and tips.

For University Use Only - Commercial Use Prohibited Using PTC Help

P a g e D-3

NOTES

2. Context-Sensitive Help 1. Click

on the right end of the main toolbar.

2. Click on any icon or any part of the Pro/ENGINEER main window about which you want an explanation. 3. A browser window opens that explains the topic. 4. In the following example, clicking on the model tree icon in the toolbar launched a browser window that explained the icon functionality.

Figure 3: Context-Sensitive Help

5. In addition, you will also notice at the lower left there is a “See Also” link which on clicking provides a list of related topics that may be of immediate interest.



NOTES

6. You may click on any topic you want to read additionally.

Figure 4: The ‘See Also’ List of Topics

3. Pro/ENGINEER Menu Manager 1. Click

on the right end of the main Pro/ENGINEER toolbar.

2. Click any menu command from the menu manager. 3. A TOPIC ROUTER browser window opens with a list of topic links that explain the menu command. 4. Click the topic you want to read. 5. In the following example, clicking on X-Section in the menu manager launched the TOPIC ROUTER browser window with a list of two useful topics.


P a g e D-5

NOTES

Figure 5: Launching Help through Menu Manager

4. Vertical Menu Commands 1. Right-click and hold on a menu command until the GETHELP window appears.

Figure 6: Right-Clicking in Menu Manager



NOTES

PTC HELP MODULES There are four main branches in the PTC Help table of contents: Welcome, Pro/ENGINEER Foundation, Using Foundation Modules, and Using Additional Modules.

Figure 7: Four Main Branches in Help System

Refer to the following list to find a particular module in the table of contents:

Figure 8: Foundation and Additional Modules in Help


P a g e D-7


Appendix For University Use Only - Commercial Use Prohibited -

E

PTC Global Services: Technical Support PTC Global Services is committed to providing top quality assistance to our customers. In addition to our Technical Support Hotline, we also offer Web-based assistance to fit your individual needs by providing 24 hour / 7 day availability. PTC Global Services is committed to continually improving customer service. Through our Quality Monitoring Program we have demonstrated our commitment to service by achieving Global ISO 9000 Certification for our Technical Support offerings.

Objectives After completing this module you will be able to: •

Open a Technical Support Call.

•

Register for on-line Technical Support.

•

Navigate the PTC Products Knowledge Base.

•

Find telephone numbers for technical support and services.

Page E-1

NOTES

FINDING THE TECHNICAL SUPPORT WEB PAGE Choose Support from the PTC Home Page www.ptc.com or go directly to www.ptc.com/support/support.htm.

OPENING TECHNICAL SUPPORT CALLS Opening Technical Support Calls via E-mail Send email to [email protected] with copen as the e-mail subject. Please use the following format (or download the template from www.ptc.com/cs/doc/copen.htm): FNAME:

First Name

LNAME:

Last Name

CALLCENTER: Tokyo PHONE:

U.S., Germany, France, U.K., Singapore, or

NNN NNN-NNNN x-NNNN

CONFIG_ID:

NNNNNN

PRODUCT:

X

MODULE:

XX

PRIORITY:

X

DESC_BEGIN: description starts description continues description ends DESC_END

For University Use Only - Commercial Use Prohibited P a g e E- 2


NOTES

Opening Technical Support Calls via Telephone Call us directly by telephone (refer to the Contact Information page for your Local Technical Support Center). The Technical Support Engineer will ask you for the following information when logging a call: •

Your PTC software Configuration ID

•

Your name and telephone number

•

The PTC product (module) name

•

Priority of the issue

Opening Technical Support Calls via the Web You can use the PTC Web site www.ptc.com/support to open Technical Support calls 24 hours a day, 7 days a week, by using the Pro/CALL LOGGER

Sending Data Files to PTC Technical Support To send data files to PTC Technical Support, please follow the instructions at: www.ptc.com/support/cs_guide/additional.htm. When the call is resolved your data will be deleted by the Technical Support Engineer. Your data will not be divulged to any third party vendors under any circumstances. You may also request a Non-Disclosure Agreement from the Technical Support Engineer.

For University Use Only - Commercial Use Prohibited Customer Support Information

P a g e E- 3

NOTES

Routing Your Technical Support Calls

Call Customer question

Telephone Call

Web Call

Tech SupportEngineer creates a call in the database

Investigation

Call is automatically created in the database

Call Back and Investigation

Support Engineer solves issue or reports it to Development (SPR)

SPR Software Performance Report SPR fixed from Development

Software Performance Report (SPR) SPR Verification through Tech. Support Engineer

Update CD to customer



NOTES

Technical Support Call Priorities •

Extremely Critical

•

Critical

•

Urgent

•

Not Critical

•

General Information

– Work stopped

– Work severely impacted – Work impacted

Software Performance Report Priorities •

Top Priority

– Highly critical software issue that is causing a work

stoppage. •

High

•

Medium

– Critical software issue that affects immediate work and a practical alternative technique is not available. – Software issue that does not affect immediate work or a practical alternative technique is available.

REGISTERING FOR ON-LINE SUPPORT Go to www.ptc.com/support and click Sign-up Online , to open the registration form and enter your Configuration ID. To find your Pro/ENGINEER Configuration ID, click Help > About Pro/ENGINEER .

Complete the information needed to identify yourself as a user with your personal data. Please write down your username and password for future reference.


P a g e E- 5

NOTES

ONLINE SERVICES After you have registered, you will have full access to all Online Tools.

You can search our Knowledge Base using a Search-Engine. Our Online Support Applications controls the status of calls (Call Tracker) and SPRs (SPR Tracker) and adds comments to these. If you add a comment, the Technical Support Engineer assigned to your call will be notified automatically. Additionally, contact information such as the customer feedback line and electronic order of software and manuals are available. The Software Update Tool allows you to request the latest software updates for any PTC product.

FINDING ANSWERS IN THE KNOWLEDGE BASE The Technical Support Knowledge Base contains over 18,000 documents. Technical Application Notes (TANs), Technical Point of Interest (TPIs), Frequently Asked Questions (FAQs), and Suggested Techniques offer upto-date information about all relevant software areas. All FAQs and Suggested Techniques are available in English, French, and German.



NOTES

Terminology used by Technical Support – Technical Application Note provides information about SPRs that may affect more than just the customer originally reporting an issue. TANs also may provide alternative techniques to allow a user to continue working. TAN

– Technical Point of Interest provides additional technical information about a software product. TPIs are created by Technical Support to document the resolution of common issues reported in actual customer calls. TPIs are similar to TANs, but do not reference an SPR. TPI

– Provides step-by-step instructions including screen snapshots, on how to use PTC software to complete common tasks. Suggested Techniques

– Frequently Asked Questions provides answers to many of the most commonly asked questions compiled from the PTC Technical Support database. FAQ


P a g e E- 7

NOTES

GETTING UP-TO-DATE INFORMATION To subscribe to our Knowledge Base Monitor e-mail service, go to www.ptc.com/support. 1. Click Technical Support > Online Support Applications > Knowledge Base Monitor . 2. Select the PTC Product or Module for which you want to get information. 3. You will receive daily e-mail with update information; this can help you by upgrading to a new PTC product or to a new release.

Figure 1: Knowledge Base Monitor Sign Up



NOTES

CONTACT INFORMATION PTC Technical Support Worldwide Electronic Services. These services are available seven days a week, 24 hours a day. Web:

•

www.ptc.com/support/index.htm (Support)

•

www.ptc.com/company/contacts/edserv.htm (Education)

E-mail:

•

[email protected] (for opening calls and sending data)

•

[email protected] (for comments or suggestions about the Customer Service Web site)

FTP (for transferring files to PTC Technical Support):

•

ftp.ptc.com

Technical Support Customer Feedback Line The Customer Feedback Line is intended for general customer service concerns that are not technical product issues. E-mail:

•

[email protected]

Telephone:

•

www.ptc.com/cs/doc/feedback_nums.htm


P a g e E- 9

NOTES

Telephone For assistance with technical issues, contact the Electronic Services noted in the previous section, or the Technical Support line as listed in the Phone and Fax Information sections below. PTC has nine integrated Technical Support Call Centers in North America, Europe, and Asia. Our worldwide coverage ensures telephone access to Technical Support for customers in all time zones and in local languages.

North America Phone Information Customer Services (including Technical Support, License Management, and Documentation Requests): Within the United States and Canada:

•

800-477-6435

Outside the United States and Canada:

•

781-370-5332

•

781-370-5513

Maintenance:

•

888-782-3774

Education:

•

888-782-3773

For University Use Only - Commercial Use Prohibited P a g e E- 1 0


NOTES

Europe Phone Information Technical Support Phone Numbers: Austria

0800 29 7542

Belgium

0800-15-241 (French) 0800-72567 (Dutch)

Denmark

8001-5593

Finland

0800-117092

France

0800-14-19-52

Germany

0180-2245132 49-89-32106-111 (for Pro/MECHANICA® outside of Germany)

Ireland

1-800-409-1622

Israel

1-800-945-42-95 (All languages including Hebrew) 177-150-21-34 (English only)

Italy

800-79-05-33

Luxembourg

0800-23-50

Netherlands

0800022-4519

Norway

8001-1872

Portugal

05-05-33-73-69

South Africa

0800-991068

Spain

900-95-33-39

Sweden

020-791484

Switzerland

0800-55-38-33 (French) 0800-83-75-58 (Italian) 0800-552428 (German)

United Kingdom

0800-318677

License Management Phone Numbers: Belgium

0800-75376

Denmark

8001-5593

Finland

0800-117-092

Eastern Europe

44 1252 817 078


P a g e E- 1 1

NOTES

France

0800-14-19-52

Germany

49 (0) 89-32106-0

Ireland

1-800-409-1622

Italy

39 (0) 39-65651

Netherlands

0800-022-0543

Norway

8001-1872

Portugal

05-05-33-73-69

Russia

44 1252 817 078

Spain

900-95-33-39

Sweden

020-791484

Switzerland

41 (0) 1-8-24-34-44

United Kingdom

0800-31-8677

Education Services Phone Numbers: Benelux

31-73-644-2705

France

33-1-69-33-65-50

Germany

49 (0) 89-32106-325

Italy

39-039-65-65- 652 39-039-6565-1

Spain/Portugal

34-91-452-01-00

Sweden

46-8-590-956-00 (Malmo) 46-8-590-956-46 (Upplands Vasby)

Switzerland

41 (0) 1-820-00-80

United Kingdom

44-0800-212-565 (toll free within UK) 44-1252-817-140

Asia and Pacific Rim Phone Information Technical Support Phone Numbers: Australia

1800-553-565

China*

10800-650-8185 (international toll free) 108-657 (manual toll free)

Hong Kong

800-933309

India*

000-6517



NOTES

Indonesia

001-803-65-7250 7-2-48-55-00-35

Japan

120-20-9023

Malaysia

1-800-80-1026

New Zealand

0800-44-4376

Philippines

1800-1-651-0176

Singapore

65-830-9899

South Korea

00798-65-1-7078 (international toll free) 080-3469-001 (domestic toll free)

Taiwan

0080-65-1256 (international toll free) 080-013069 (domestic toll free)

Thailand

001-800-65-6213

*Note: Callers dialing from India or China must provide the operator with the respective string: China

MTF8309729

India

MTF8309752

The operator will then connect you to the Singapore Technical Support Center. License Management Phone Numbers Japan

81 (0) 3-3346-8280

Hong Kong

(852) 2802-8982

Education Services Phone Numbers Australia

61 2 9955 2833 (Sydney) 61 3 9561 4111 (Melbourne)

China

86-20-87554426 (GuangZhou) 86-21-62785080 (Shanghai) 86-10-65908699 (Beijing)

Hong Kong

852-28028982

India

91-80-2267272 Ext.#306 (Bangalore) 91-11-6474701 (New Delhi) 91-226513152 (Mumbai)


P a g e E- 1 3

NOTES

Japan

81-3-3346- 8268

Malaysia

03-754 8198

Singapore

65-8309866

South Korea

82-2-3469-1080

Taiwan

886-2-758-8600 (Taipei) 886-4-3103311 (Taichung) 886-7-3323211 (Kaohsiung)

ELECTRONIC SERVICES Up-to-Date + Information

Worldwide ISO 9000 Certification Quality Control System

= Maximum Productivity with PTC Products




INDEX Assemblies Constraining Components, 13-3 Design Intent, 13-8 Modifying, 13-7 Options, 13-8 BOM, 13-8 Exploded Views, 13-9 Overview, 13-2 Placing Components, 13-6 Surface Normal Vector, 13-2 Under-Constrained Components, 13-7 Associativity, 1-5 Behavioral Modeler Achieving Desired Results, 10-6 Analyzing Effects of Parameter Changes, 10-6 Components Analysis Features, 10-8 Feasibility Studies, 10-11 Field Points, 10-8 Optimization, 10-12 Sensitivity Analysis, 10-10 User-defined Analysis, 10-9 Creating Datum Geometry, 10-5 Creating Feature Parameters, 10-4 Creating New Measurement Systems, 10-5 Graph Matching, 10-7 Interaction with Data Analysis Tools, 10-6 Motion Analysis, 10-8 Behavioral Modeling Applications, 10-4 Definition, 10-2 Features, 10-2 Objective-Driven Design, 10-4 Smart Models, 10-3 Config.PRO File, 20-2 Configuration Files Config.PRO, 20-2 Editing, 20-3 Mapkeys, 20-4 Order of Precedence, 20-3 Constraints Sketcher Mode, 4-9 Copy Choosing Features, 12-10 Dependency Options, 12-11 Methods, 12-8 Customizing Pro/ENGINEER, 20-2 Deleting Files, 2-10

Design Intent, 21-2 Assemblies, 13-8 Associativity, 21-4 Changing, 21-5 Design Criteria, 21-3 Parent/Child Relationships, 21-3 Pro/NOTEBOOK, 21-2 Dialog Boxes, 2-5 General, 2-5 Models, 2-6 Option Buttons, 2-6 Dimensions Angular, 5-9 Diameter, 5-7 Linear, 5-6 Modifying in Sketcher, 4-8 Radial, 5-8 Sections, 5-5 Display Area, 2-3 Drawings Adding New Views, 11-2 Creating, 11-2 Cross Sections, 11-4 Detailing, 11-7 Dimensions Drawing Notes, 11-9 Driven, 11-8 Features, 11-8 Manipulating, 11-8 Parametric Notes, 11-9 Manipulating Views, 11-5 Templates, 11-6 Applications, 11-6 Customizing, 11-7 View Type Menu, 11-3 Broken View, 11-3 Full View, 11-3 Half View, 11-3 Partial View, 11-3 Views Auxiliary, 11-2 Detailed, 11-3 General, 11-3 Projection, 11-2 Revolved, 11-3 Edge, 4-9 Extruded Forms, 5-2 Feature-Based Models, 1-3 Features

For University Use Only - Commercial Use Prohibited INDEX

P a g e -1

Copy To Locations, 12-8 Copying, 12-8 File Commands Closing Windows, 2-10 Deleting Files, 2-10 Saving Your Work, 2-9 File Types, 2-4 Assemblies, 2-4 Drawings, 2-4 Parts, 2-4 Sketches, 2-4 Freeform Surfaces Applying to Engineering Models, 17-8 Blends and Transitions, 17-8 Parametric Controls, 17-7 Geometry Creating in Sketcher Mode, 4-6 Help, 2-8 Hybrid Modeling, 17-3 Information About Features, 19-2 Model Info, 19-2 Regeneration Info, 19-2 Intent Manager, 4-3 Interference, 19-3 ISDX, 17-2 2-D Curves, 17-4 3-D Curves, 17-4 Creating Surfaces, 17-4 Curves On Surface (COS), 17-6 Style Models, 17-6 Layout Mode, 21-2 Macros Mapkeys, 20-4 Mapkeys, 20-4 Mass Properties, 19-3 Calculating, 19-3 Measurement, 19-3 Menu Manager, 2-8 Menus, 2-2 Adding Mapkeys, 20-7 Customizing, 20-6 Message Area, 2-4 Viewing Information, 2-4 Model Tree, 2-7, 20-7 General Usage, 20-8 Models Multiple Models, 2-8 Retrieving (Opening), 2-6 Sub-windows, 2-8 Offset Edge, 4-10 Parallel Blends Creating, 8-3

Straight and Smooth Attributes, 8-5 Tools, 8-4 Parameters Symbols Used to Describe, 9-4 Parametric Features, 1-4 Parametric Relations, 9-2 Assembly, 9-2 Design Changes, 9-8 Design Intent, 9-4 Examples, 9-5 Feature, 9-3 Order of Operations, 9-6 Part, 9-2 Pattern, 9-3 Parent Features Modifying, 7-3 Redefining, 7-4 Rerouting, 7-3 Parent/Child Relationships Definitions, 7-2 Pick-and-Place Features, 7-2 Sketched Features, 7-2 Patterns Benefits of Using, 12-2 Creating, 12-2 Options, 12-3 Rotational, 12-5 Types, 12-2 Dimensions, 12-2 Reference, 12-2 Preferences Sketcher, 4-13 Pro/ENGINEER Customizing, 20-2 Pro/NOTEBOOK, 21-2 Problems Diagnosing Regeneration Problems, 18-3 Reference Planes, 5-3 Default, 5-3 Regeneration Model Info, 19-2 Regeneration Failures, 18-2 Resolve Environment, 18-2 Regeneration Problems Feature Reorder, 7-6 Insert Mode, 7-6 Parent/Child Features, 7-5 Resolving, 7-5 Resolve Environment Diagnosing Problems, 18-3 Resolving, 18-2 Specifying a Model, 18-3 Starting, 18-2

For University Use Only - Commercial Use Prohibited P a g e -2

INDEX

Undoing Changes, 18-3 Resolve Environment:, 18-4 Reverse Styling, 17-9 Revolved Forms, 5-2 Saving Your Work, 2-9 Sketched Features Cuts, 5-2 Defining, 5-2 Extruded and Revolved Forms, 5-2 Protrusions, 5-2 Sketcher 3-D Sketching, 4-13 Arcs, 4-6 Best Practices, 4-14 Circles, 4-6 Constraints, 4-9 Copying, 4-10 Creating Geometry, 4-6 Customizing, 4-13 Dimensioning, 4-7 Intent Manager, 4-3 Interface Features, 4-2 Lines, 4-6 Menus, 4-4 Mirroring, 4-11 Moving, 4-11 Points, 4-12 Pop-Up Menus, 4-3 References, 4-5 Replacing, 4-11 Section Analysis, 4-11 Selecting Sketched Entities, 4-3 Sketcher Mode, 4-4 Tools, 4-9, 5-5 Trimming, 4-11 Sketching Planes, 5-3 Solid Modeling

Associativity, 1-5 Core Concepts, 1-2 Feature-Based Models, 1-3 Parametric Features, 1-4 Style Creating Style Surfaces, 17-9 Features, 17-2 Introduction, 17-2 Sweeps and Trajectories Creating, 8-2 Templates Drawing Templates:, 11-6 Toolbar Customizing, 20-5 Toolbars, 2-3 Top-Down Design, 14-2 Approach, 14-2 Benefits, 14-4 Characteristics, 14-3 Comparison with Traditional Approaches, 14-3 Pro/ENGINEER Tools, 14-7 Process, 14-4 Stages, 14-2 Use Edge, 4-10 User Interface, 2-2 Dialog Boxes, 2-5 Display Area, 2-3 Menus, 2-2 Message Area, 2-4 Pro/ENGINEER, 2-2 Toolbars, 2-3 Windows Closing, 2-10

For University Use Only - Commercial Use Prohibited INDEX

P a g e -3

For University Use Only - Commercial Use Prohibited P a g e -2

INDEX

Intro Proe 320

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