T072 310-02 en-ed

PTC Global Services
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PPrroo//EENNGGIINNEEEERR
Release 2000i2
T072-310-02
- For University Use Only -
Commercial Use Prohibited

For University Use Only - Commercial Use Prohibited

Copyright
Introduction to Pro/ENGINEER
COPYRIGHT © 1989-2000 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.
Use of the software has been provided under a Software License Agreement.
Information described in this manual is furnished for information only, is subject to change without
notice, and should not be construed as a commitment by PTC. PTC assumes no responsibility or liability
for any errors or inaccuracies that may appear in this manual.
The software contains valuable trade secrets and proprietary information and is protected by United
States copyright laws and copyright laws of other countries. Unauthorized use of the software or its
documentation can result in civil damages and criminal prosecution.
Pro/ENGINEER and Pro/MECHANICA are registered trademarks, and all product names in the PTC
product family and the PTC logo are trademarks of Parametric Technology Corporation in the United
States and other countries. All other companies and products referenced herein have trademarks or
registered trademarks of their respective holders.
US GOVERNMENT RESTRICTED RIGHTS LEGEND
This Software and Documentation are provided with RESTRICTED RIGHTS. Use, duplication, or
disclosure by the Government is subject to restrictions as set forth in subparagraph (c)(1)(ii) of the
Rights in Technical Data and Computer Software-Restricted Rights at 48 CFR 52.227-19, as applicable.
Parametric Technology Corporation, 128 Technology Drive, Waltham, MA 02453
© 2000 Parametric Technology Corporation. Unpublished – all rights reserved under the copyright laws
of the United States.
PRINTING HISTORY
Document No. Date Description
T072-310-01 07/10/00 Initial Printing of Introduction to Pro/ENGINEER for Release 2000i2
T072-310-02 09/08/00 Revisions to Introduction to Pro/ENGINEER for Release 2000i2
Order Number DT-072-310-EN
Printed in U.S.A

Training Agenda
Day 1
The Pro/ENGINEER Interface
Pick-and-Place Features
The Sketcher Mode
Sketched Features
Day 2
Datum Planes
Parent/Child Relationships
Simple Sweeps and Blends
Relations
Day 3
Patterns and Copy
Drawing Creation and Views
Additional Detailing and Associativity
Creating Assemblies
Day 4
Layers and Suppression
Additional Datum Features
Additional Advanced Features
The Resolve Environment
Day 5
Information Tools
Configuring Pro/ENGINEER
Modeling Philosophy

PTC Telephone and Fax Numbers
The following is a list of telephone and fax numbers you may find useful:
Education Services Registration in North America
Tel: (888)-782-3773
Fax: (781) 398-5553
Technical Support (Monday - Friday)
Tel: (800) 477-6435 (U.S.)
(781) 894-5332 or (781) 894-5523 (outside U.S.)
Fax: (781) 398-5650
License Management
Tel: (800) 216-8945 (U.S.)
(781) 398-5559 (outside U.S.)
Fax: (781) 398-5795
Contracts
Tel: (800) 791-9966 (U.S.)
(781) 398-5700 (outside U.S.)
In addition, you can find the PTC home page on the World Wide Web at:
http://www.ptc.com. The Web site contains the latest training schedules,
course descriptions, registration information, directions to training facilities, as
well as information on PTC, the Pro/ENGINEER product line, Consulting
Services, Customer Support, and Pro/PARTNERS

Acknowledgments
The Pro/ENGINEER curriculum is a joint development effort between the courseware development
teams at PTC and RAND Worldwide.
Both companies strive to develop industry leading training material and in turn deliver it to you the
customer.
PTC
128 Technology Drive
Waltham, MA 02453
USA
1-781-398-5000
http://www.ptc.com
RAND Worldwide
5285 Solar Drive
Mississauga, ON
Canada
L4W 5B8
1-877-726-3243
http://www.rand.com

Table of Contents
INTRODUCTION TO PRO/ENGINEER 1-1
Pro/ENGINEER: A SOLID MODELER............................................................................1-2
Feature-Based .................................................................................................................... 1-3
Parametric .......................................................................................................................... 1-4
Associative......................................................................................................................... 1-5
THE PRO/ENGINEER INTERFACE 2-1
SCREEN LAYOUT............................................................................................................2-2
Main Window .................................................................................................................... 2-2
Pull-Down Menus .............................................................................................................. 2-2
Toolbar............................................................................................................................... 2-3
Display Area ...................................................................................................................... 2-3
Message Area..................................................................................................................... 2-4
WORKING WITH MODELS ............................................................................................2-4
Using Dialog Boxes ........................................................................................................... 2-5
Retrieving Models.............................................................................................................. 2-6
Retrieving Multiple Models............................................................................................... 2-8
Saving Changes.................................................................................................................. 2-9
Closing Windows............................................................................................................... 2-9
Deleting Files..................................................................................................................... 2-9
LABORATORY PRACTICAL........................................................................................2-11
EXERCISE 1: Using Pro/ENGINEER ............................................................................ 2-11
EXERCISE 2: Manipulating Model Size and Orientation............................................... 2-14
EXERCISE 3: Interrogating the Model Tree................................................................... 2-17
EXERCISE 4: Challenge Exercise................................................................................... 2-20
MODULE SUMMARY....................................................................................................2-24
PICK-AND-PLACE FEATURES 3-1
PICK AND PLACE FEATURES.......................................................................................3-2
Creating the Straight Hole Feature..................................................................................... 3-2
Creating the Simple Round................................................................................................ 3-5
Specifying Radius Values for a Simple Round.................................................................. 3-7

Creating an Edge Chamfer .................................................................................................3-7
LABORATORY PRACTICAL ......................................................................................... 3-9
EXERCISE 1: Creating an Edge Chamfer .........................................................................3-9
EXERCISE 2: Creating a Simple Edge Chain Round Feature.........................................3-14
EXERCISE 3: Exploring the Straight Hole Feature.........................................................3-20
Exercise 4: Challenge Exercise ........................................................................................3-29
MODULE SUMMARY................................................................................................... 3-32
SKETCHER BASICS 4-1
THE SKETCHER ENVIRONMENT ................................................................................ 4-2
The Sketcher Interface........................................................................................................4-2
Intent Manager ...................................................................................................................4-3
Pop-Up Menus....................................................................................................................4-4
SKETCHER MODE FUNCTIONALITY ......................................................................... 4-5
Sketcher Menus ..................................................................................................................4-5
Specifying References........................................................................................................4-6
Creating Geometry .............................................................................................................4-6
Dimensioning .....................................................................................................................4-8
Constraining .....................................................................................................................4-10
Additional Sketcher Tools................................................................................................4-11
SETTING SKETCHER PREFERENCES........................................................................4-14
SKETCHER PHILOSOPHY ........................................................................................... 4-17
Rules of Thumb................................................................................................................4-17
LABORATORY PRACTICAL ....................................................................................... 4-19
EXERCISE 1: Sketching Basics.......................................................................................4-19
EXERCISE 2: Sketching in Steps ....................................................................................4-25
EXERCISE 3: Sketching a Hexagon................................................................................4-30
MODULE SUMMARY................................................................................................... 4-33
SKETCHED FEATURES 5-1
TWO SKETCHED FEATURES........................................................................................ 5-2
Specifying Extruded and Revolved Forms.........................................................................5-2
SKETCHING AND REFERENCE PLANES.................................................................... 5-3
The Sketching Plane’s Default Orientation ........................................................................5-4
SKETCHER BASICS ........................................................................................................ 5-5
EXERCISE 1: Creating a Cut.............................................................................................5-9
EXERCISE 2: Creating a Protrusion................................................................................5-20
MODULE SUMMARY................................................................................................... 5-24

DATUM PLANES 6-1
USING BASE FEATURES AND DATUM PLANES ......................................................6-2
The Base Feature and Its Importance................................................................................. 6-2
What is a Datum Plane?..................................................................................................... 6-2
Using Default Datums as the Base Feature........................................................................ 6-3
CREATING ADDITIONAL DATUM PLANES...............................................................6-3
Defining a Datum Plane..................................................................................................... 6-3
Internal Datums.................................................................................................................. 6-4
LABORATORY PRACTICAL..........................................................................................6-5
EXERCISE 1: Creating a Base Feature ............................................................................. 6-5
EXERCISE 2: Using Default Datums as References to Other Features ............................ 6-9
EXERCISE 3: Creating an Additional Datum Plane ....................................................... 6-13
MODULE SUMMARY....................................................................................................6-16
PARENT/CHILD RELATIONSHIPS 7-1
PARENT/CHILD RELATIONSHIPS................................................................................7-2
Parent/Child Relationships with Pick-and-Place Features ................................................. 7-2
Parent/Child Relationships with a Sketched Feature ......................................................... 7-2
Changing the Parents of a Feature ..................................................................................... 7-3
ORDER OF FEATURE REGENERATION......................................................................7-5
Using Feature Insert Mode................................................................................................. 7-6
EXERCISE 1: Changing Design Intent ........................................................................... 7-10
MODULE SUMMARY....................................................................................................7-19
SWEEPS AND BLENDS 8-1
SWEPT FEATURES..........................................................................................................8-2
Defining a Sweep............................................................................................................... 8-2
Sweep Sections and Trajectories........................................................................................ 8-2
BLEND FEATURES..........................................................................................................8-3
Creating Parallel Blends..................................................................................................... 8-3
EXERCISE 1: Creating Parallel Blend Features................................................................ 8-6
EXERCISE 2: Creating a Simple Sweep Protrusion........................................................ 8-12
MODULE SUMMARY....................................................................................................8-16
RELATIONS 9-1
DEFINING PARAMETRIC RELATIONS........................................................................9-2
Types of Relations ............................................................................................................. 9-3

Representing Relations: Types and Symbols .....................................................................9-4
Using Relations ..................................................................................................................9-4
Relations: An Illustration ...................................................................................................9-5
Order of Relations ..............................................................................................................9-6
Design Changes..................................................................................................................9-8
EXERCISE 1: Creating Relations ......................................................................................9-9
EXERCISE 2: Creating Parameters for Feature-Control..................................................9-13
MODULE SUMMARY................................................................................................... 9-16
DUPLICATING FEATURES: PATTERNS AND COPY 10-1
CREATING A PATTERN............................................................................................... 10-2
Benefits of Patterning.......................................................................................................10-2
Types of Patterns..............................................................................................................10-2
Pattern Options.................................................................................................................10-3
THE COPY FEATURE ................................................................................................... 10-8
Specifying Location..........................................................................................................10-8
Choosing Features ............................................................................................................10-8
Establishing Dependence..................................................................................................10-8
LABORATORY PRACTICAL ..................................................................................... 10-10
EXERCISE 1: Creating a Dimension Pattern.................................................................10-10
EXERCISE 2: Creating a Reference Pattern..................................................................10-13
EXERCISE 3: Creating Rotational Patterns of Sketched Features.................................10-17
EXERCISE 4: Copying Features....................................................................................10-27
MODULE SUMMARY................................................................................................. 10-31
DRAWINGS AND VIEWS 11-1
DRAWING FUNDAMENTALS..................................................................................... 11-2
Creating a Drawing...........................................................................................................11-2
Adding Drawing Views....................................................................................................11-2
Types of Views.................................................................................................................11-2
Adding a Cross Section ....................................................................................................11-4
Manipulating Views .........................................................................................................11-5
EXERCISE 1: Creating a Drawing ..................................................................................11-7
MODULE SUMMARY................................................................................................. 11-14
ADDITIONAL DETAILING AND ASSOCIATIVITY 12-1
CAPTURING DESIGN INTENT.................................................................................... 12-2

Detailing the Drawing...................................................................................................... 12-2
Drawing and Solid Model: Need for Consistency............................................................ 12-2
Two Types of Dimensions ............................................................................................... 12-2
Manipulating Dimensions................................................................................................ 12-3
EXERCISE 1: Detailing the Gear Part Drawing.............................................................. 12-5
MODULE SUMMARY..................................................................................................12-10
CREATING ASSEMBLIES 13-1
ASSEMBLY CREATION................................................................................................13-2
The Surface Normal Vector ............................................................................................. 13-3
Constraint Options ........................................................................................................... 13-3
Packaging or Under-Constrained Components................................................................ 13-7
ASSEMBLY MODIFICATION.......................................................................................13-8
Changing Design Intent of the Assembly ........................................................................ 13-8
OTHER ASSEMBLY OPTIONS.....................................................................................13-9
Extracting a Bill of Materials........................................................................................... 13-9
Creating Exploded Views ................................................................................................ 13-9
LABORATORY PRACTICAL......................................................................................13-11
EXERCISE 1: Creating and Modifying an Assembly ................................................... 13-11
MODULE SUMMARY..................................................................................................13-22
LAYERS AND SUPPRESSION 14-1
DEFINING LAYERS.......................................................................................................14-2
Functionality .................................................................................................................... 14-2
Working Rules ................................................................................................................. 14-2
CREATING LAYERS......................................................................................................14-2
Selecting the Object ......................................................................................................... 14-2
Creating Layers................................................................................................................ 14-3
Associating Items to a Layer............................................................................................ 14-3
Setting the Display Status of a Layer............................................................................... 14-4
Manipulating Layer Display Status.................................................................................. 14-6
SUPPRESSION FUNCTIONALITY...............................................................................14-7
Using Suppression............................................................................................................ 14-8
Suppressing Parent/Child Relationships .......................................................................... 14-8
Saving and Resuming Suppressed Features..................................................................... 14-8
EXERCISE 1: Using Layers in Part Mode ...................................................................... 14-9
EXERCISE 2: Using Layers in Assembly Mode........................................................... 14-13
EXERCISE 3: Suppressing in Part Mode ...................................................................... 14-20

EXERCISE 4: Suppressing Components in Assembly Mode........................................14-22
MODULE SUMMARY................................................................................................. 14-25
ADDITIONAL DATUM FEATURES 15-1
ADDITIONAL DATUM FEATURES ............................................................................ 15-2
Datum Axes......................................................................................................................15-2
Datum Curves...................................................................................................................15-3
Datum Points....................................................................................................................15-3
Datum Coordinate Systems ..............................................................................................15-4
EXERCISE 1: Creating Additional Datum Features........................................................15-5
MODULE SUMMARY................................................................................................... 15-8
ADDITIONAL ADVANCED FEATURES 16-1
SURFACE DEFORMATION.......................................................................................... 16-2
Creating a Draft Feature ...................................................................................................16-2
OTHER FEATURES ....................................................................................................... 16-4
Creating a Rib...................................................................................................................16-4
Creating Standard Holes Based on Units..........................................................................16-5
Creating Counterbores and Countersunk Holes................................................................16-6
EXERCISE 1: Creating a Neutral Plane Draft Feature ....................................................16-8
EXERCISE 2: Creating a Rib.........................................................................................16-12
EXERCISE 3: Creating a Sketched Hole.......................................................................16-13
MODULE SUMMARY................................................................................................. 16-15
THE RESOLVE ENVIRONMENT 17-1
TYPES OF FAILURES ................................................................................................... 17-2
Entering the Resolve Environment...................................................................................17-2
Using the Resolve Environment Tools.............................................................................17-2
EXERCISE 1: Resolving a Failure...................................................................................17-6
MODULE SUMMARY................................................................................................. 17-10
INFORMATION TOOLS 18-1
MODEL DESIGN INFORMATION............................................................................... 18-2
Obtaining Information about a Specific Feature...............................................................18-2
Obtaining Regeneration Information................................................................................18-2
Accessing Information about Part Features......................................................................18-2

Obtaining Information about the Assembly..................................................................... 18-2
MEASUREMENT, INTERFERENCE, AND MASS PROPERTIES..............................18-3
Calculating Mass Properties............................................................................................. 18-3
Calculating Clearance and Interference ........................................................................... 18-4
EXERCISE 1: Using Information Tools.......................................................................... 18-5
MODULE SUMMARY....................................................................................................18-8
CONFIGURING PRO/ENGINEER 19-1
CUSTOMIZING PRO/ENGINEER.................................................................................19-2
Configuration Files .......................................................................................................... 19-2
Creating Mapkeys ............................................................................................................ 19-4
CONFIGURING THE TOOLBAR ..................................................................................19-5
Adding Icons to Existing Toolbars .................................................................................. 19-5
Pull-down Menus and Mapkeys....................................................................................... 19-6
THE MODEL TREE ........................................................................................................19-7
LABORATORY PRACTICAL......................................................................................19-10
EXERCISE 1: Setting Up a Configuration File............................................................. 19-10
Exercise 2: Creating a Mapkey ...................................................................................... 19-15
EXERCISE 3: Configuring the Model Tree .................................................................. 19-18
MODULE SUMMARY..................................................................................................19-21
MODELING PHILOSOPHY 20-1
THE DESIGN INTENT....................................................................................................20-2
Recording Your Design Criteria ...................................................................................... 20-2
Using Pro/ENGINEER as a Parametric Tool................................................................... 20-2
Creating Parent/Child Relationships................................................................................ 20-2
Advantages of Pro/ENGINEER’s Associativity............................................................... 20-3
Changing Design Intent ................................................................................................... 20-4
MODULE SUMMARY....................................................................................................20-5
PROJECT LABORATORY A-1
INTRODUCTION .............................................................................................................A-2
PART CREATION............................................................................................................A-3
SECTION 1: Creating the Motor Part............................................................................... A-3
SECTION 2: Creating the Lower Housing Part................................................................ A-5
SECTION 3: Creating the Snap Ring Part........................................................................ A-9
SECTION 4: Creating the Upper Housing Part .............................................................. A-11
CREATING ASSEMBLIES AND DEVELOPING PART MODELS ...........................A-18

SECTION 1: Creating the Motor Assembly....................................................................A-18
SECTION 2: Concurrent Design of the Motor Housing .................................................A-22
SECTION 3: Creating the Blower Assembly..................................................................A-23
SECTION 4: Creating the Motor Part Drawing ..............................................................A-26
MODEL INTERROGATION......................................................................................... A-29
SECTION 1: Designing the Cover Part...........................................................................A-30
SECTION 2: Completing the Motor Part........................................................................A-33
SECTION: 3: Completing the Blower Assembly............................................................A-35
SECTION 4: Finishing the Motor Assembly ..................................................................A-39
......................................................................................................................................... A-41
FINISHING PARTS, ASSEMBLIES, AND DRAWINGS............................................ A-42
SECTION 1: Developing the Motor Part ........................................................................A-42
SECTION 2: Finishing the Lower Housing ....................................................................A-44
SECTION 3: Finishing the Drawing ...............................................................................A-46
USING PTC.HELP B-1
PTC HELP OVERVIEW .................................................................................................. B-2
PTC Help Features ............................................................................................................B-2
USING THE PRO/ENGINEER HELP SYSTEM ............................................................ B-2
To Get Help on Tasks in a Dialog Box..............................................................................B-2
GETTING HELP THROUGH THE PTC HELP SIDEBAR............................................ B-3
PTC HELP MODULE LIST............................................................................................. B-4
PTC GLOBAL SERVICES: TECHNICAL SUPPORT C-1
FINDING THE TECHNICAL SUPPORT PAGE............................................................ C-2
OPENING A TECHNICAL SUPPORT CALL................................................................ C-2
Opening a call via email....................................................................................................C-2
Opening a Call via Telephone ...........................................................................................C-3
Opening Calls on the PTC Web Site .................................................................................C-3
Sending Data to Technical Support...................................................................................C-3
CALL / SPR FLOW CHART AND PRIORITIES............................................................C-4
REGISTERING FOR ON-LINE SUPPORT .................................................................... C-5
ONLINE SERVICES ........................................................................................................ C-6
FINDING SOLUTIONS IN THE KNOWLEDGE BASE................................................ C-6
GETTING UP-TO-DATE INFORMATION.................................................................... C-8
CONTACT INFORMATION........................................................................................... C-8
Internet ..............................................................................................................................C-8
Telephone..........................................................................................................................C-9
ELECTRONIC SERVICES ............................................................................................ C-13

1
Module
Pro/ENGINEER is a powerful application. It is ideal for capturing
the design intent of your models because at its foundation is a
practical philosophy. In this lesson, you will learn the concepts that
drive this philosophy and the powerful functionality that it generates.
OBJECTIVES
After completing this module, you will be able to:
• Explain Pro/ENGINEER’s uses as a solid modeler
• Define the three pillars of Pro/ENGINEER’s practical philosophy,
its being feature-based, associative, and parametric

2 Introduction to Pro/ENGINEER
NOTES
Pro/ENGINEER: A SOLID MODELER
Pro/ENGINEER is a solid modeler—it develops models as solids,
allowing you to work in a three-dimensional environment. In
Pro/ENGINEER,
• The solid models have volumes and surface areas.
• You can calculate mass properties directly from the geometry you
create.
• While you can manipulate a solid model’s display on the screen, the
model itself remains a solid, as shown in Figure 1.
• As a solid modeling tool, Pro/ENGINEER is feature-based,
associative, and parametric.
Figure 1: Model Display

Introduction to Pro/ENGINEER Page 1-3
NOTES
Feature-Based
Pro/ENGINEER is feature-based. Geometry is composed of a series of
easy to understand features. A feature is the smallest building block in a
part model. Things to remember:
• Pro/ENGINEER allows building a model incrementally, adding
individual features one at a time.
• This means, as you construct your model feature by feature you choose
your building blocks as well as the order you create them in, thus
capturing your design intent.
• Design intent is the motive, the all-driving force, behind every feature
creation.
• Simple features make your individual parts as well as the overall
model flexible and reliable.
Figure 2: Building Models Feature by Feature
Base Feature Protrusion Added Blind Cut Added
Thru- All Cuts and Holes Added Chamfer Added Rounds Added

NOTES
Parametric
Pro/ENGINEER is parametric i.e. it is driven by parameters or variable
dimensions. This means:
• Geometry can be easily changed by modifying dimensions
• Features are interrelated.
• Modifications of a single feature propagate changes in other features
as well, thus preserving design intent.
• A relationship, known as a parent/child relationship, is developed
between features when one feature references another.
Figure 3: Protrusion and Hole Follow Side of Block
5 10

Introduction to Pro/ENGINEER Page 1-5
NOTES
Associative
Pro/ENGINEER models are often combinations of various parts,
assemblies, drawings, and other objects. Pro/ENGINEER makes all these
entities fully associative. That means if you make changes at a certain
level those changes propagate to all the levels. For example if you change
dimensions on a drawing the change will be reflected in the associated
part. Figure 4 shows associativity between a part and an assembly.
Figure 4: Associativity
Original shaft before
length modification
Shaft associated to assembly
Modification of shaft length
Assembly automatically updates
5
10

1
Module
The Pro/ENGINEER Interface
In this module, you examine the Pro/ENGINEER interface.
Proficiency in the interface enables you to take advantage of
Pro/ENGINEER’s powerful design functionality in subsequent
lessons.
Objectives
• Define the four elements of the main Pro/ENGINEER window and
describe their functionality.
• List the different Pro/ENGINEER model file types.
• Retrieve, save, erase, and delete various Pro/ENGINEER models.
• Describe the uses of the Model Tree and the Menu Manager.
• Prove the parametric, associative, and feature-based characteristics
of Pro/ENGINEER.

NOTES
SCREEN LAYOUT
Figure 1 Sample Model in Pro/E Main Window
Main Window
When you start Pro/ENGINEER, the main window opens on your desktop.
You create your designs in this window. The four distinct elements of the
window are:
• Pull-down menu
• Toolbar
• Display area
• Message area
Pull-Down Menus
The Pro/ENGINEER pull-down menus are valid in all modes of the
system.

The Pro/ENGINEER Interface Page 2-3
NOTES
• File – Contains commands for manipulating files
• Edit – Contains action commands
• View – Contains commands for controlling model display and display
performance.
• Datum – Creates datum features
• Analysis – Provides access to options for model, surface, curve and
motion analysis, as well as sensitivity and optimization studies.
• Info – Contains commands for performing queries and generating
reports.
• Applications – Provides access to various Pro/ENGINEER modules.
• Utilities – Contains commands for customizing your working
environment.
• Windows – Contains commands for managing various
Pro/ENGINEER windows.
• Help – Contains commands for accessing online documentation.
Toolbar
The Pro/ENGINEER toolbar contains icons for frequently used options
from the pull-down menus. The toolbar can also be customized.
Figure 2: Standard Pro/ENGINEER Toolbar
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.

NOTES
Message Area
The message area between the toolbar and the display area performs
multiple functions by:
• Providing status information for every operation performed.
• Providing queries/hints for additional information to complete a
command/task.
• Prompting you for additional information by sounding a bell.
• Displaying icons in the message area, which represent different forms
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
Pro/ENGINEER has file extensions associated with different models such
as drawings, parts, and assemblies.
• .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 two-
dimensional sketches that are parametric.

NOTES
Using 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.
General Dialog Box
A general dialog box performs general functions such as saving, viewing,
and interrogating. The graphic in Figure 3 represents some of the common
elements in a general dialog box.
Figure 3: Example of a Dialog Box
Model Dialog Box
A model dialog box creates and modifies model geometry by requesting
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 are not necessary for completing the feature.
The following figure illustrates a model dialog box that defines a round
feature.
Tabs
Drop-down
arrow
Title
Check box
Text box
Command button

NOTES
Figure 4: A Model Dialog Box
Buttons in the above dialog box are described below:
• Define – Allows you to define and/or change selected elements in the
dialog box.
• Refs – Displays the external references of the current selected
element.
• Info – Generates a listing of the properties of the feature that you are
creating.
• OK – Completes the definition of the elements, creating the feature or
model entity.
• Cancel – Cancels the current feature or model entity.
• Preview – Allows you to check geometry before completing the
feature definition. It is not available until you have defined all required
elements.
In addition, Resolve rectifies failures in defined elements by allowing
changes to these elements.
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.
Using the Model Tree
The MODEL TREE presents the model structure feature by feature. You
can choose features from the MODEL TREE for modification and deletion.
MODEL TREE icons denote the corresponding item type and its current
status.

NOTES
Figure 5: Model Tree with Added Parameters
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.
Help with Menus
Holding your mouse over any menu option provides one-line help
displayed on the bottom of the current active window. If you need
additional help, choose the menu option with the right mouse button and
click Get Help from the pop-up menu.
Note:
The system administrator must install and set up the online
documentation for you to be able to access this functionality.

NOTES
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 allows you to work only
on one active window at a time. 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.
Figure 6: A New Window over the Main Window

NOTES
Saving Changes
Save changes at any time by clicking File > Save. It is a good practice to
save often. When saving a model, Pro/ENGINEER creates a new version
by increasing the version number, thereby creating two existing versions.
To retrieve an old version, you must specify the version number in the
retrieval name. To display the version numbers in the FILE OPEN dialog
box, use the All Versions option.
Figure 7: Opening a Version of a Model
Closing Windows
To close a window use Window > Close or File > Close Window.
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, erase it from memory by clicking File >
Erase > Current. To erase all models that are in session but not displayed
in windows, click File > Erase > Not Displayed.
Deleting Files
Click File > Delete to remove old versions of a model. When you click
File > Delete > All Versions, the system deletes all versions of the model
from the system memory as well as from the hard drive.

NOTES
LABORATORY PRACTICAL
Goal
To prove that Pro/ENGINEER is a parametric, associative, and feature-
based solid modeler.
Method
The first two exercises of this lab deal with the user interface and how to
manipulate the size and orientation of a model. The final exercise
demonstrates that Pro/ENGINEER is a parametric, associative, and
feature-based solid modeler.
EXERCISE 1: Using Pro/ENGINEER
Task 1. Open the master assembly.
1. Click File > Open.
2. In the OPEN dialog box, click the Type drop-down arrow and click
Assembly. Only assembly files become visible.
3. Open master.asm.
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.
3. Click Apply. Do not close the dialog box.
4. At the bottom of the dialog box, click Hidden Line from the
DISPLAY STYLE drop-down list.
5. Click Apply.
Task 3. Change the orientation of the assembly.
1. From the DEFAULT ORIENT drop-down list, click Isometric.

NOTES
2. Click Apply.
3. Change the orientation back to Trimetric.
4. Click OK to close the dialog box.
Figure 8: Hidden Line Display of Assembly
Task 4. Use the toolbar to manipulate the model.
1. Click on the Datum Planes icon in the toolbar. Datum planes
reappear.
Figure 9: Datum Display Section of Toolbar
2. Shade the model. Click the Shade icon from the toolbar.
Display datum
planes
Display axes Display datum
points
Display coordinate
systems

NOTES
Figure 10: Changing the Model Display
3. Once again, revert back to hidden line display.
4. You may also use the pull-down menu to cosmetically shade the
model. Click View > Shade.
Note:
Hidden Line remains selected on the toolbar because we
have only cosmetically shaded the model and have not
switched to a shaded display mode.
5. Repaint the screen. Click View > Repaint.
Wireframe
display
Hidden Line
display
No Hidden Line
display
Shade display

NOTES
EXERCISE 2: Manipulating Model Size and
Orientation
Task 1. Change the size and orientation of the model using the toolbar.
1. Click the Zoom In icon.
Figure 11: Model Orientation Options
2. Pick a location on the model with the left mouse button and pick a
second location to create a zoom box.
3. The model zooms in.
4. Now click the Zoom Out icon.
5. Click the Refit icon to resize the model.
Task 2. Orient the model so that the bracket faces front.
1. Click .
2. A dialog box opens with the Orient by Reference type already
selected.
3. In Options, Reference 1 refers to what is to be parallel to the screen
and Reference 2 what orients that parallel reference.
4. Leave the default FRONT from the REFERENCE 1 drop-down list.
5. Pick the front surface of the bracket part as shown in Figure 12.
Refit
Repaint
Zoom In
Orient the model
Saved Views

NOTES
Figure 12: Surface Selection for Orientation
6. Now pick the other surface of the bracket part as Reference 2, as
shown above.
7. The model changes its orientation.
8. Click OK in the ORIENTATION dialog box.
Figure 13: Model after Orientation
Pick this
surface to face
front for
Reference 1.
Pick this surface
as the top for
Reference 2.

NOTES
Task 3. Change the model back to the default orientation.
1. Click View > Default.
Tips & Techniques:
You can also manipulate the model orientation by using the
mouse buttons and <Ctrl> key. The left mouse button zooms
the model, the middle spins it, and the right pans it.

NOTES
EXERCISE 3: Interrogating the Model Tree
Task 1. Modify dimensions of model using the MODEL TREE.
1. Click View > Model Tree, if the Model Tree is not on.
2. Modify offset of the master shaft part. Right-click and hold on
MASTER_SHAFT.PRT.
3. Click Modify from pop-up menu.
4. Pick the 76 dimension that appears.
5. In the text box in the message area, type [90] and press <ENTER>.
6. Click Done in the MODIFY menu of the MENU MANAGER.
7. Click Done/Return in the ASSEM MOD menu.
Task 2. Regenerate the assembly.
1. In ASSEMBLY menu, click Regenerate.
2. In PRT TO REGEN menu, click Automatic.
3. The shaft moves to its new location.
4. Note that 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. Open MASTER_SHAFT.PRT.
2. Click Modify in MENU MANAGER.
3. Pick the shaft as shown in Figure 14.

NOTES
Figure 14: Modifying the Shaft
4. Pick the 152 dimension.
5. Type [250] and press <ENTER>.
6. Click Regenerate in the MENU MANAGER.
7. Save the shaft model by clicking .
8. Accept the default name of MASTER_SHAFT.PRT.
Task 4. Check for associativity between the shaft and the assembly
1. Close the SHAFT window by clicking Window > Close Window.
2. Make the assembly window active. Click Window > Activate.
3. Regenerate the assembly. From Menu Manager, click Regenerate
> Automatic.
4. The regenerated assembly appears with modified shaft dimensions,
as shown below.
Pick this dimension
to modify.
Pick the shaft
here

NOTES
Figure 15: 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. Now, investigate the associativity between one assembly
component and an incomplete drawing.
1. Open the drawing DRAW_CRANK2. DRW.
2. Click Modify in the DETAIL menu.
3. Pick the dimension to be modified 60.50.
4. Enter 90.5 as the new dimension.
Figure 16: Crank2 Drawing
5. Click Drawing > Regenerate > Model to see the changes.
6. Save the drawing model.
7. Close the drawing window. Click File > Close Window.
8. Activate the assembly window. Notice that the crank is updated in
the assembly.
Modify this
dimension

NOTES
Task 2. Check for interference between the solid models of the
assembly.
1. Start the interference calculation. Click Analysis > Model
Analysis. The MODEL ANALYSIS dialog box appears. The default
type is set to Assembly Mass Properties.
2. Change the analysis type to check for global interference. Select
Global Interference from the TYPE drop-down list.
3. Start the calculation. Accept the defaults and click Compute.
Figure 17: Analyzing Global Interference
4. Investigate the results. In the RESULTS window, the system
indicates that two parts are interfering. Use the arrow to toggle to
the different models. Note that the volume of interference
highlights on the screen.
5. Close the dialog box.
6. Save the assembly model. Click File > Save and accept default
name.
TYPE drop-
down list

NOTES
Task 3. Determine the results of closing the master assembly window.
1. Click Window > Close Window from the pull-down menu. Notice
the base Pro/ENGINEER window cannot be removed as indicated
in the message area.
2. Open the CRANK2 part that is still in memory. In the FILE OPEN
dialog box, click the In Session icon.
Figure 18: Using the IN SESSION Option
3. Select CRANK2. PRT. Click Open. 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 the selected models that are in session.
Click OK from the dialog box to complete the operation.
In Session
icon

NOTES
Task 5. Retrieve in session models again to determine which ones
remain in session.
1. Open the OPEN dialog box again. Click File >Open. Click In
Session. Note that the CRANK2.PRT is the only model that is
listed because it was displayed in a window when you erased the
other models.
2. Close the operation. Click Cancel in the dialog box.
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, toolbar, display area, and 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.
• You can work with multiple windows. Pro/ENGINEER automatically
opens a new main window each time you open an additional model.
• Erasing models that are not in use frees up system memory.

1
Module
Pick-and-Place Features
Certain Pro/ENGINEER features need not be (Keep it simple) built.
They are freely provided and can simply be utilized whenever
needed. These features are called Pick-and-Place features.
Objectives
• Identify and define the three 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.

NOTES
PICK AND PLACE FEATURES
The three Pick-and-Place features are:
• straight hole
• edge round
• edge chamfer
To create any of these 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 pick on a surface, a dialog box
appears with various reference 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.
• Linear – Places the hole on a plane. Dimensions the center of the hole
from two surfaces or edges using linear dimensions.

Pick-and-Place Features Page 3-3
NOTES
Figure 1: Linear Hole
• Radial – 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.
Figure 2: Radial Holes on a Plane
• Coaxial – Places the hole coaxially using an existing axis. Does not
create placement dimensions, only a diameter dimension for the hole
itself.
Figure 3: Coaxial Hole

NOTES
• On Point – Places the center of the hole directly on an on surface
datum point. The axis of the hole is normal to the placement surface.
Figure 4: 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 5: Side Options
The system determines how deep to create the hole based on your depth
specification. Figure 6 illustrates the various depth options listed in the
HOLE dialog box.

NOTES
Figure 6: Hole Depth Options
Creating the Simple Round
Round features create a rounded smooth transition between two adjacent
surfaces. An edge round smoothes the hard edges between adjacent
surfaces.
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 a Simple Edge Chain Round
• Constant – Assigns the same radius value to every selected edge.
• Variable – Specifies radii at every selected edge at the endpoints and,
optionally, at intermediate vertices along the edge being rounded.
Figure 7: Constant and Variable Radius Rounds
• Full Round – Creates a round that completely removes a model
surface.
Thru Next
Thru Until
Thru All
Variable
To Reference

NOTES
Figure 8: Full Round
Note:
Do not dimension other features to the edges or tangent edges
of round features. Round features make unstable parents.
Tip:
You should create round features on your model as late in the
design process as possible.
Figure 9: Cut Feature Dimensioned to the Edge Round
Full Round

NOTES
Specifying Radius Values for a Simple Round
• Enter – (default) Specifies a new radius value that does not appear in
the menu. Use the <ESC> key to select other radius type options.
• Pick On Surf – Specifies a point on the adjacent surface that
determines the radius value (Figure 10).
• Thru Pnt/Vtx – Specifies a datum point, vertex, curve, or edge end
through which the radius of the round should pass (Figure 11).
• Default Values – Specifies a radius value as the system default value
or a previously entered radius value in the SEL VALUE menu.
Figure 10: Using the Pick On Surf Option
Figure 11: Using the Thru Pnt/Vtx Option
Creating an Edge Chamfer
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 Figure 12.
Original model
Picked a point on
this surface. Round created
tangent
Picked this vertex.
Original Model

NOTES
Figure 12: 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.

NOTES
Goal
By the end of this lab, you will have command over the important Pick-
and-Place features of Pro/ENGINEER: the Straight Hole, the Simple
Edge Chain Round and the Edge Chamfer.
Method
This lab is structured to present the Pick-and-Place features in their order
of complexity.
EXERCISE 1: Creating an Edge Chamfer
In this exercise, you add two edge chamfers to an existing model using
two different dimensioning methods: 45 x d and d1x d2.
Figure 13: The Starting Model
Task 1. Adding the 45 x d edge chamfer to a cylinder.
1. Retrieve the CHAMFERS.PRT from the INTRO_PROE_310
directory.

NOTES
2. From MENU MANAGER, click Feature > Create > Solid >
Chamfer.
3. Click Edge > 45 x d. Type [1.0] as the value for the chamfer
dimension.
4. Pick the two circular edges on either end of the cylindrical
protrusion.
5. After the edges have been selected, click Done Sel > Done Refs.
Figure 14: Selecting the Circular Edges
6. Click OK to complete the chamfer.
Pick these
two edges

NOTES
Figure 15: Completed Chamfer
Task 2. Add the D1 X D2 chamfer to the four edges at the bottom of the
model.
1. Click Create > Solid > Chamfer > Edge.
2. Select D1 X D2 from the SCHEME menu. Type [1.0] as the value
for D1 and [2.0] as the value for the D2 dimension.
3. Switch to a Hidden Line view. Click Query Sel, then pick the
hidden bottom surface as the reference surface for the D1
dimension.
Figure 16: Picking the Bottom Surface
Pick the bottom
surface.

NOTES
4. Pick the front edge and right side edge as edge references.
5. Click Query Sel, then pick the two hidden bottom edges.
Figure 17: Picking the Hidden Edges
Note:
When Pro/ENGINEER prompts for you to pick an edge or
surface, the system can determine the difference between the
two, thus filtering out everything but the prompted reference
type.
6. Click Done Sel > Done Refs.
7. Click OK to complete the chamfer.
8. Click the Shade icon to display a shaded model.
Pick these two
hidden bottom
edges.
Pick front
and right
side edges

NOTES
Figure 18: Completed Chamfers Model
9. Save the model. Accept the default name when saving the part.
10. Close the current working window.

NOTES
EXERCISE 2: Creating a Simple Edge Chain Round
Feature
In this exercise, you add four different simple edge chain round features to
the model.
Figure 19: Simple Edge Chain Round Feature
Task 1. Open the model and add some rounds.
1. Open ROUNDS.PRT.
2. Create the first round feature as a corner break on the front end of
the cylinder. Click Feature > Create > Solid > Round > Simple >
Done.
3. Give the round a constant radius value. Click Constant > Edge
Chain > Done.
4. Leave the default tangent chain and pick the first edge of the
cylinder to round, as shown in Figure 20. Click Done.

NOTES
Figure 20: Selection of the Edge
5. Type [.5] as the value for the radius dimension and click OK.
Task 2. Create a second edge round, similar to the first, at the other end
of the cylinder.
1. Click Feature > Create > Solid > Round > Simple > Done.
2. Click Constant > Edge Chain > Done.
3. Pick the back edge of the cylinder, as shown in Figure 21, then
choose Done.
Pick this edge

NOTES
Figure 21: Second Edge Reference
4. Type [.75] as the radius value. Click OK.
Task 3. Create a simple round with a variable radial attribute. Look at
the final graphic of this section for an idea of what you want to achieve.
1. Start defining the edge round. Click Feature > Create > Solid >
Round > Simple > Done.
2. Click Variable > Edge Chain > Done.
3. Switch to the Hidden Line display.
4. Define the single edge references. Click One By One.
5. Pick the three visible vertical edges of the base as shown in Figure
22.
6. Click Query Sel. Pick the hidden vertical edge.
7. Click Done.
Pick this
circular edge

NOTES
Figure 22: Selecting the Variable Rounds References
8. Do not add any intermediate points. Click Done.
Task 4. Pro/ENGINEER highlights geometry when querying for
information. Define the radius values, keeping track of the vertices that
Pro/ENGINEER highlights.
1. As the system highlights each end of every edge, type [0] as a
value for the top of the edge; type [2] as a value for the bottom of
the edge.
2. Complete the round feature. Click OK.
Task 5. Use the surface chain attribute to round the base edges of the
part.
1. Click Create > Solid > Round.
2. Click Simple > Done > Constant > Edge Chain > Done.
Pick the fourth
(hidden) edge here.
Pick these
three edges

NOTES
3. From the MENU MANAGER, click Surf Chain over the default
tangent chain. Read the message window.
4. Click Query Sel, then pick the bottom surface as the selection
reference.
Figure 23: Selecting the Surface Reference
5. Click Select All > Done.
Task 6. Define a radius value by selecting on the surface of the model
(without entering a numerical value as usually done).
1. To activate the RADIUS TYPE menu, press <ESC>.
2. Click Pick on Surf.
3. Pick the front edge of the base first.
4. Now pick above the edge on the adjacent angled surface, as shown
in figure below.
5. Click OK to create the feature.
Pick the
bottom
surface.

NOTES
Figure 24 Defining Radius by Picking on Surface
6. The completed model will look as in the figure below.
Figure 25: The Completed Model
7. Save the part and erase it from memory.
Pickt this point
on the surface to
define radius
Pick this edge
first

NOTES
EXERCISE 3: Exploring the Straight Hole Feature
Figure 26: Straight Hole Feature
Task 1. Create a linear placed hole with a variable depth of 30 on the
top of the base feature of the model, as shown in Figure 26.
1. Open STRAIGHT_HOLES.PRT.
2. Click Feature > Create > Solid > Hole. The HOLE dialog box
appears, as shown in Figure 27.
Base feature
270-degree
flange
Fluid pipe
Four cooling fins

NOTES
Figure 27 Hole Dialog Box
3. Leave the default hole type as Straight.
4. Type [7.5] as the diameter value. Press <ENTER>.
5. Leave the depth one default as Variable and depth two as None.
6. Type [30] as the depth value. Press <ENTER>.
7. Through the Primary Reference you define the location of the hole.
8. First click on the arrow next to the primary reference. Choose the
placement plane by picking on the top surface of the base feature
as shown in Figure 28.

NOTES
Figure 28: Creating a Linear Placed Hole
9. For the first linear reference, click > Query Sel to pick the
hidden side of the base feature. Type [10] as the distance for this
reference. Press <ENTER>.
10. For the second linear reference again click > Query Sel to
pick the visible front surface. Type [15] for the distance from this
reference. Press <ENTER>.
11. Click .
Second dimension
reference
First dimension
reference (hidden
side surface)
Placement plane

NOTES
Figure 29: The First Completed Hole
Task 2. Add a linear hole that runs through the cooling fins. Reference
it to the back and right side surfaces of the fins, so that if the fins get
longer or wider the hole will move with them.
1. Start the definition of the hole feature. Click Feature > Create >
Solid > Hole.
2. In the HOLE dialog box, leave the default hole type as Straight.
3. Type [12.5] for the hole diameter. Press <ENTER>.
4. Click Thru All as the depth option.
5. Define the placement location. Pick the top surface of the first
cooling fin near the right back corner, as shown in Figure 30.
Figure 30: Creating the Second Straight Hole Feature
First dimension reference
(hidden back surface)
Second dimension
reference (visible
thin surface of fin)
Placement plane

NOTES
6. For the first linear reference, click Query Sel, then pick the hidden
back side surface of the base feature. Type [10] as the distance for
this reference. Then press <ENTER>.
7. For the second reference, click Query Sel, then pick the side
surface (not the edge) of the topcooling fin. Type [10] for the
distance. Then press <ENTER>.
Note:
If you are creating another hole after creating a hole, use the
repeat button .
8. You may preview the hole feature but do not close the HOLE
dialog box.
Figure 31: 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 <ENTER>.
2. Click To Reference in the Depth One option dropdown menu.

NOTES
3. Click Query Sel, then pick 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.
Figure 32: Creating the Third Hole
4. For the Primary Reference, pick the top surface of the first fin as
shown in figure.
5. For the first Linear Reference, pick the front part of the base
feature and type [10] for the distance. Press <Enter>.
6. For the second Linear Reference, pick the visible side surface of
the cooling fin. Define the second distance as 10 units as well.
7. Complete the hole feature.
Pick this surface
as the placement
plane
First
Dimensional
reference
Second
dimensional
reference

NOTES
Figure 33: The Up to Surface Hole
Task 4. Create a coaxial hole to the cylindrical feature.
1. Define the hole. Click Feature > Create > Solid > Hole
2. In the HOLE dialog box, leave the default hole type as Straight.
3. Type [5] as a value for the hole diameter.
4. Let the Depth One dimension be a To Reference. Click Query
Sel, then pick the visible front surface of the base feature as the
depth reference.
5. In the HOLE PLACEMENT box, select the front surface of the
cylindrical protrusion as the primary reference.
6. Select Coaxial from the PLACEMENT TYPE drop-down list.
7. Pick the A_3 axis of the cylindrical protrusion as the axial
reference. If you cannot see the axis, turn it on in the toolbar.
Select the hidden
underside
surface

NOTES
8. Click checkmark to complete the coaxial hole feature.
Figure 34: Creating a Coaxial Straight Hole
Axis line (A_3)
Depth surface to
extrude up to
Pick here for
the placement
plane

NOTES
Exercise 4: Challenge Exercise
Task 1. Create a straight hole radially placed on a planar surface.
Figure 35: The Completed Model
1. Set the hole specifications.
½ Diameter = 15mm
½ Depth One = To Reference
½ Depth Two = None
½ Depth Reference = Invisible surface of the circular flange.
2. Set the hole placement.
½ Primary Reference = Visible front surface of the circular flange
½ Placement Type = Radial
½ Axial Reference = A_3 of the fluid pipe
½ Distance = 25 mm

NOTES
½ Angular Reference = Front face of the flange near the angled
cut.
½ Angle = 25.
Figure 36: Creating a Radial Mounting Hole
Figure 37: Selection of the Reference
3. Complete the hole.
4. Optional: Change the diameter of the flange from 47 to 60 and
regenerate to see the change in the model.
Pick this surface
as the placement
location
Small angled surface
Pick this axis

NOTES
5. Save the part and erase it from memory.

NOTES
MODULE SUMMARY
In this module, you have learned that:
• Hole, Round, and Chamfer form the three important Pick-and-Place
features in Pro/ENGINEER.
• The Hole feature can be placed linearly, radially, coaxially, and on
point and has many depth options.
• The Round and Chamfer features are best created towards the end of
the design process because they are not good references. Also, they
can complicate design intent with unwanted parent-child relationships.
• Rounds can be created with varying radius options: Constant,
Variable, and Fully Rounded.
• Chamfers can be placed not only on planes and perpendicular surfaces
but also on circular edges.

1
Module
Sketcher Basics
Previously, you have learned that “Pick and Place” features allow
for very fast creation of features such as holes and rounds whose
geometry is easily understood as part of standard engineering
operations. For any geometry that involves the definition of more
complex, individual shapes, you will actually sketch them.
To enable this, Pro/ENGINEER provides a Sketcher mode and
includes a built-in Intent Manager to help you capture design intent.
This module starts with the basics of the Sketcher mode.
Objectives
• Describe the functions and tools in the Sketcher mode.
• Explain how the Sketcher dimensioning scheme allows you to
capture design intent.
• Create geometry including lines, centerlines, arcs, circles,
rectangles, and sketched points.
• Apply geometrical constraints to sketched entities, such as the
“equal lengths” constraint and the “perpendicular” constraint.
• Employ Sketcher Tools to change section sketches.

NOTES
THE SKETCHER ENVIRONMENT
The Sketcher Interface
The Sketcher interface consists of:
• A menu bar with the usual Pro/ENGINEER pull-down menus and two
additional Sketcher-specific menus—EDIT and SKETCH.
• A standard Pro/ENGINEER toolbar.
• An additional Sketcher toolbar with specific Sketcher functionality
such as Undo, Dimensions On/Off, and Grid On/Off.
• 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

Sketcher Basics Page 4-3
NOTES
• The color red is used to highlight and select entities. This provides
accurate and easily identifiable entities selections.
• Using the mouse, you can select individual or multiple-specific
sketched entities, or all entities that fall within a swept box.
Intent Manager
• The Intent Manager with fly-out icons appears automatically on the
right side of the screen when you enter the Sketcher mode.
• These icons are logically grouped together, based on capability.
Figure 2 Intent Manager’s Fly-Out Icons
• With fly-out icons, you can access the most frequently used sketching
tools with a single click without having to go to pull-down menus.
Default cursor to
pick entities
To create dimensions
To trim Entities
To modify dimensions
To impose constraints
Icons to create
different kinds of
geometry

NOTES
Pop-Up Menus
• Additional pop-up menus can be accessed by holding the right-mouse
button in the Sketcher mode display area.
• These pop-up menus aid ease-of-use.
• They offer short-cut methods for sketching, modifying, dimensioning,
deleting, and undoing steps.
Figure 3 A Typical Sketcher Pop-Up Menu

NOTES
SKETCHER MODE FUNCTIONALITY
Sketcher Menus
• EDIT and SKETCH are two top-level menus specific to the Sketcher
mode.
• They contain all the commands needed in the sketching environment.
They are shown below.
Figure 4 Edit and Sketch Menus
• In addition, all Intent Manager commands are available through these
menus.
• You can insert Text into the Sketching area using the Text option in
the SKETCH menu.
• With the new EDIT menu, you can manipulate your sketched geometry
with the Modify, Move, Trim, Toggle Construction, and Toggle
Lock commands.

NOTES
Specifying References
One of the first things you will be prompted for after beginning a sketch in
the Sketcher mode will be to specify references of the section you are
about to sketch.
You will need to provide references when you:
• Create a new feature.
• Redefine a feature with missing or insufficient references.
• Provide insufficient 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.
Creating Geometry
Sketcher mode enables the creation of a variety of geometrical shapes and
entities. The basic ones—lines, arcs, and circles—are discussed below.
Lines
Figure 5 Lines Fly-Out Icons
Using the Line fly-out icons in the Intent Manager, you can create two
types of sketched lines—straight lines from point to point or centerlines
for referencing or constraining entities.
Arcs
Figure 6 Arcs Fly-Out Icons

NOTES
Using the Arcs fly-out icons in the Intent Manager, you can create four
types of arcs. You can create:
• An arc by 3 points or tangent to an entity at its endpoint.
• A concentric arc.
• An arc by picking its center and endpoints.
• A conic arc.
Circles
Figure 7 Circle Fly-Out Icons
Using the Circle fly-out icons in the Intent Manager, you can create three
types of circles. You can create:
• A circle by picking the center and a point on the circle.
• A concentric circle.
• A full ellipse.
Figure 8 Sketching a Concentric Circle to an Edge
Sketched circle
Concentric to this
edge

NOTES
Dimensioning
After completing a sketch, you must dimension it. To place dimensions in
Sketcher, pick the entity with the left mouse button and place the
dimension with the middle-mouse button.
The following figure illustrates the simple dimensioning of a rectangle.
Figure 9 Creating Dimensions for a Rectangle
• You can grab a dimension and place it at a more convenient position in
the Sketcher at any point during or after sketching.
• An orderly arrangement of dimensions helps visual clarity, particularly
when the sketch gets complex.
Figure 10 Grabbing and Moving Dimensions

NOTES
Modifying Dimensions
• Sketcher makes it easy to modify dimensions of geometric entities at
any time.
• With the MODIFY DIMENSIONS dialog box, shown below, you can
change the dimension values of multiple entities with just a click of the
mouse.
Figure 11 Modify Dimensions Dialog Box
• In addition, you can now double-click on an individual dimension to
change its value.
• The SENSITIVITY scrollbar at the bottom right of the dialog box allows
you to adjust the sensitivity of the control wheels for changing
dimensions dynamically.
• You also have the options to dynamically Regenerate and Lock
Scale the sketch.

NOTES
Constraining
• Sketcher assumes certain constraints for the geometrical entities you
create.
• You are free to impose your own constraints overriding the system’s
default constraints to capture your design intent.
• This can be done easily by accessing the CONSTRAINTS dialog box
shown below.
Figure 12 Sketcher Constraints Dialog Box
You can use 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.

NOTES
Additional Sketcher Tools
EDGE
The Edge tool has two instances represented by its two fly-out icons in the
Intent Manager, as shown below:
Figure 13 Edge Fly-Out Icons
• Use Edge – Uses an existing model edge to create sketched entities.
Automatically selects that edge as a specified reference.
Figure 14: Using Existing Model Edge to Create Sketched Entities

NOTES
• Offset Edge – Uses existing model edge to create sketched entities at
an offset distance.
Figure 15: Creating Sketched Entities at an Offset Distance
Note:
The Use Edge and Offset Edge options create parent/child
relationships with the referenced feature.
Copy
Copies 2-D draft/imported entities from a drawing. You can dynamically
move and scale a section, making legacy data easier to manipulate. This
functionality can be accessed by clicking Edit > Copy from the pull-down
menus.
Mirror
This tool mirrors sketched entities from one side of a centerline to the
other. This can be accessed by Edit > Mirror.
Move
• Repositions sketched entities. The MOVE ENTITY menu displays the
following options:
• Drag Item – Moves an entity or its vertex to a new location.
½ Drag Many – Translates picked entities within a sketch.

NOTES
½ Rotate90 – Rotates sketched entities about a specified point by
multiples of 90 degrees.
½ Dimension – Repositions a dimension within a sketch.
Trim
This can be accessed by clicking Edit > Trim. Trim shortens (or extends)
an entity in three different ways corresponding to the three fly-out icons
shown below:
Figure 16 Trim Fly-Out Icons
½ The first dynamically trims section entities
½ The second cuts or extends entities to other entities or
geometry.
½ 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
To obtain information about a particular section within Sketcher, click
Analysis > Section Analysis. This option provides you with information
about
• intersection and tangency points
• angles and distances
• dimensioning references
• entity curvature display
Sketcher Points
½ They force coincidence among sketched entities.
½ Allow slanted dimensions between sketched entity end-points.

NOTES
Figure 17: Midpoint Definition Using Sketcher Point
Figure 18 Defining Theoretical Sharps Using Sketcher Points
SETTING SKETCHER PREFERENCES
You can now modify the Sketcher environment in the new SKETCHER
PREFERENCES dialog box in the UTILITIES menu.

NOTES
Figure 19 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-D
When you select the Use2D Sketcher option from the ENVIRONMENT
dialog box. Sketcher starts in 2-D orientation (that is, with the sketching
plane parallel to the computer screen).

NOTES
Figure 20 The Environment Dialog Box
When you do not select this option, Sketcher starts in 3-D orientation. You
may change the view orientation at any time and sketch in 3-D. Using
View > Sketch View, you can re-orient a Sketcher section into the 2-D
view while in Sketcher mode.

NOTES
SKETCHER PHILOSOPHY
Rules of Thumb
Certain rules of thumb must be rigorously adhered to gain maximum
advantage from the power of the Sketcher mode’s diverse capabilities,
1. Keep sketches simple.
½ This makes the final model flexible and helps regeneration.
2. Use the Undo option
½ The Undo option restores a sketched section to its prior state.
½ This is extremely useful when sketching features
incrementally.
3. Do not sketch to scale.
½ Firstly, concentrate on getting your geometry straight by
sketching large.
½ Secondly, resolve the sketch by modifying dimensions.
½ This rule is particularly helpful when the sketched entities are
small.
4. Use the grid as an aid.
½ Create lines equal, parallel, or perpendicular.
½ Align sketched entities.
½ Align centers horizontally and vertically.
5. Do not extend the sketch outside of the part.
½ 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 accuracy.
½ The range for the accuracy is 1.0 e-9 through 1.0 (default).
½ 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.
½ When sketching an open section, you cannot have more than
one open section per feature.

NOTES
½ If you use an open section, you must explicitly align its open
ends to the part.
½ 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.
Figure 21: Open and Closed Sections
Protrusion A
Protrusion B
Cut

NOTES
Goal
By the end of this lab, you will be conversant with basic sketching skills
such as entering sketcher mode, creating straight lines, creating arcs,
applying constraints, dimensioning, and generating solid models.
Method
In Exercise 1, you learn sketching basics.
In Exercise 2, you create a snap ring by sketching in steps.
In Exercise 3, you create a hex section using construction entities.
EXERCISE 1: Sketching Basics
Figure 22 Completed Sketch after Exercise 1
Task 1. Create a new sketch named ROUND_RECTANGLE.
1. Click File > New.
2. In the NEW dialog box, select Sketch.
3. Type [ROUND_RECTANGLE].
4. Sketcher mode activates.

NOTES
Task 2. Sketch four lines as shown, the bottom line being horizontal.
Figure 23 Sketching a Quadrilateral
Task 3. Apply the constraint to make the lines perpendicular.
1. Click > , then pick two lines to make them perpendicular.
2. Similarly, once again pick the other two lines to make them
perpendicular.

NOTES
Figure 24 Applying the Perpendicular Constraint
3. Close the CONSTRAINTS dialog box.
Task 4. Delete the two vertical lines.
1. With the pointer icon pick the left vertical line.
2. Hold shift and pick 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 .
2. Pick the top left vertex and drag the mouse out of the left quadrant
of the circle to get a tangent end arc.
3. Pick the end point to be the bottom left end point, as shown below.

NOTES
Figure 25 Sketching a Tangent End Arc
Task 6. Repeat the process on the right side of the section.
Figure 26 Sketching Tangent End Arcs on Both Sides
Task 7. Add the proper dimensions.
1. Click .
2. Pick each arc with the left mouse button, then place the dimension
where you would like it to appear with the middle button.
3. Select Tangent and Horizontal for type and orientation.

NOTES
Figure 27 Dimensioning the Arcs
Task 8. Create a diameter dimension on the left arc.
1. Click .
2. Pick the left arc twice with the left mouse button and place it with
the middle.
Figure 28 Dimensioning the Left Arc

NOTES
Task 9. Modify both dimensions.
1. Pick both the horizontal dimension and the diameter dimension
using the <SHIFT> key and click icon.
Figure 29 Modify Dimensions Dialog Box
2. Modify the diameter to [2] and the linear dim to [4].
3. Save and close the MODIFY DIMENSIONS dialog box.
Figure 30 Sketch with Modified Dimensions
4.

NOTES
EXERCISE 2: Sketching in Steps
Figure 31 Completed Snap Ring after Exercise 2
Task 1. Create a new sketch called SNAP_RING.
1. Click File > New.
2. Select Sketch.
3. Type [SNAP_RING] as the name of the sketch.
Task 2. Create two offset circles aligned horizontally.
1. Click and draw two circles as shown in the next figure.

NOTES
Figure 32 Two Offset Circles Aligned Horizontally
Task 3. Create a rectangle that snaps to the inside circle on both upper
vertices.
Figure 33 Sketching Rectangle Inside Circles
1. For the rectangle, click . Just click once to start and then click
again to end sketching.
2. Then use the dynamic trim to create intersections. Click , Put
your cursor below the bottom horizontal line and drag it to above
the top horizontal line.
Start dynamic
trim here
Stop cursor here
Delete

NOTES
3. Make sure that each item becomes highlighted. If all the crossed
items are not highlighted continue to hold the mouse button and
drag over the lines until they do highlight.
4. The result is shown in the figure below.
Figure 34 Using Dynamic Trim
Task 4. Sketch another rectangle.
1. This time snapping to the outside circle and the bottom of the two
vertical lines as shown below.
2. Make sure not to snap through any of the arc’s vertices.

NOTES
Figure 35 Sketching a Second Rectangle
Task 5. Use the dynamic trim to remove the final lines and arc.
1. Click to trim the unwanted entities.
2. The result is shown below.
Figure 36 Capturing Intent with Dynamic Trim

NOTES
Task 6. Dimension the entities.
1. Click to create the dimensions.
2. Pick each entity with the left mouse button and place the
dimension with the middle mouse button.
3. Click to modify the six dimension values.
Figure 37 Modifying Dimensions
4. Save and close

NOTES
EXERCISE 3: Sketching a Hexagon
Task 1. Create a new sketch called HEX.
1. Click File > New. Select Sketch and type [HEX] as the name.
Task 2. 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 on the centerline button in the line fly-out icons.
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 below.
Figure 38 Modifying Angles between Centerlines

NOTES
Task 5. Create a circle centered on the point.
1. Left-click on the circle to highlight it in red.
2. Right-click and hold on the circle for a pop-up menu.
3. Click Toggle Construction to convert it to a construction circle
Figure 39 Creating a Construction Circle
Task 6. Create a hexagon by sketching 6 lines from the intersection
points of the circle and the centerlines.
Figure 40 Creating a Hexagonal Sketch

NOTES
1. Add a diameter dimension to the construction circle and modify it’s
value to [1.0]
2. Save and close.

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