T869 310 03 En Ed

- For University Use Only -
Commercial Use Prohibited

PTC Global Services

Fundamentals of
Sheetmetal
Release 2000i2
T869-310-03


Copyright
Fundamentals of Sheetmetal

COPYRIGHT © 1989-2000 PARAMETRIC TECHNOLOGY CORPORATION. ALL RIGHTS
RESERVED.

This Fundamentals of Sheetmetal Training Guide may not be copied, reproduced, disclosed,
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© 2000 Parametric Technology Corporation. Unpublished – all rights reserved under the copyright laws
of the United States.

PRINTING HISTORY
Document No. Date Description
T869-310-03 09/22/00 Initial Printing of Fundamentals of Sheetmetal for Release 2000i2

Order Number DT-869-310-EN
Printed in U.S.A


Training Agenda
Day 1
8:30-8:45 Welcome and Introduction
8:45-9:15 Module 1 – Introduction to Sheetmetal Design
9:15-9:30 Module 2 – Primary Walls
9:30-10:00 Exercise
10:00-10:30 Module 3 – Secondary and Unattached Walls
10:30-10:45 Break
10:45-11:15 Exercise
11:15-11:30 Module 4 – Unbend, Bend Back, and Cuts
12:00-1:00 Lunch
1:00-1:30 Module 5 – Notches and Punches
1:30-2:00 Exercise
2:00-2:15 Break
2:15-2:45 Module 6 – Sheetmetal Forms
2:45-3:30 Exercise
3:30-4:00 Module 7 – Bend Features
4:00-4:30 Exercise
Day 2
8:30-9:00 Review
9:00-9:30 Module 8 – Unbending Sheetmetal Geometry
9:30-10:15 Exercise
10:15-10:30 Break
10:30-11:00 Module 9 – Converting Solid Parts
11:30-12:00 Module 10 – Sheetmetal Drawings with Flat States and Bend Order Tables
12:00-1:00 Lunch
1:00-1:45 Exercise
1:45-2:15 Module 11 – Additional Features
2:15-2:45 Exercise
2:45-3:00 Break
3:00-3:30 Module 12 – Setting Up for Design
3:30-4:00 Exercise
4:00-4:30 Module 13 – Interrogating the Sheetmetal Part
4:30-5:00 Exercise


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In addition, you can find the PTC home page on the World Wide Web at:
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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 RAND Worldwide
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Waltham, MA 02453 Mississauga, ON
USA Canada
1-781-398-5000 L4W 5B8
http://www.ptc.com 1-877-726-3243
http://www.rand.com


Table of Contents

INTRODUCTION TO SHEETMETAL DESIGN 1-1
THE SHEETMETAL DESIGN ENVIRONMENT............................................................1-3
SHEETMETAL PARTS.....................................................................................................1-3
Features .............................................................................................................................. 1-3
Sheetmetal Part Display ..................................................................................................... 1-4
Orienting the Sheetmetal Part ............................................................................................ 1-4
Developed Length .............................................................................................................. 1-5
DESIGN APPROACH .......................................................................................................1-5
MODULE SUMMARY......................................................................................................1-9

PRIMARY WALLS 2-1
WALL TYPES....................................................................................................................2-3
CREATING THE FIRST WALL .......................................................................................2-3
Wall Feature Options ......................................................................................................... 2-3
Sketching Technique.......................................................................................................... 2-5
LABORATORY PRACTICAL ..........................................................................................2-7
EXERCISE 1: Creating the Cable Box Base ..................................................................... 2-7
MODULE SUMMARY....................................................................................................2-13

SECONDARY AND UNATTACHED WALLS 3-1
TYPES OF SECONDARY WALLS ..................................................................................3-3
Resulting Geometry ........................................................................................................... 3-6
Creating Other Walls ......................................................................................................... 3-7
CREATING UNATTACHED WALLS .............................................................................3-9
Merging Unattached Walls .............................................................................................. 3-10
SECONDARY WALLS WITH RELIEF .........................................................................3-10
LABORATORY PRACTICAL ........................................................................................3-13
EXERCISE 1: Adding Walls to the Cable Box Base....................................................... 3-13
EXERCISE 2: Adding Walls to the Tuner Cover ............................................................ 3-17
EXERCISE 3: Creating the Box ...................................................................................... 3-26
EXERCISE 4: Creating an Unattached Wall ................................................................... 3-35
MODULE SUMMARY....................................................................................................3-41

UNBEND, BEND BACK, AND CUTS 4-1
THE UNBEND, REGULAR FEATURE........................................................................... 4-3
THE BEND BACK FEATURE ......................................................................................... 4-4
CREATING SHEETMETAL CUTS ................................................................................. 4-5
Dimensioning Scheme........................................................................................................4-6
LABORATORY PRACTICAL ......................................................................................... 4-7
EXERCISE 1: Unbend and Bend Back ..............................................................................4-7
MODULE SUMMARY ................................................................................................... 4-13

NOTCHES AND PUNCHES 5-1
INCREASING YOUR EFFICIENCY WITH SHEETMETAL NOTCHES AND
PUNCHES.......................................................................................................................... 5-3
Creating a Punch or Notch UDF.........................................................................................5-3
Placing a Punch or Notch Feature ......................................................................................5-5
EXERCISE 1: Creating Notches in the Flat State of the Model.........................................5-7
MODULE SUMMARY ................................................................................................... 5-15

SHEETMETAL FORMS 6-1
CREATING FORM FEATURES ...................................................................................... 6-3
CREATING FORM PARTS.............................................................................................. 6-3
Creating Rips in the Geometry ...........................................................................................6-5
Using Multiple Forms on a Single Die Model....................................................................6-5
Using Multiple Forms on a Single Punch Model ...............................................................6-6
PLACING FORM FEATURES ......................................................................................... 6-7
Placing By Reference .........................................................................................................6-7
Copying the Geometry .......................................................................................................6-8
RETURNING THE MODEL TO THE FLAT................................................................... 6-8
EXERCISE 1: Forms for the Cover ...................................................................................6-9
EXERCISE 2: Placing a Die Form...................................................................................6-18
MODULE SUMMARY ................................................................................................... 6-21

BEND FEATURES 7-1
BEND FEATURES............................................................................................................ 7-3
Angle ..................................................................................................................................7-3
Roll .....................................................................................................................................7-3
Regular ...............................................................................................................................7-4
W/Transit (With Transition)...............................................................................................7-4

Planar Bends ...................................................................................................................... 7-4
BEND LINES .....................................................................................................................7-5
Bend Line Adjustment ....................................................................................................... 7-7
EXERCISE 1: Creating a Model in the Flat ...................................................................... 7-9
MODULE SUMMARY....................................................................................................7-21

UNBENDING SHEETMETAL GEOMETRY 8-1
UNBENDING GEOMETRY AFTER DEFINING THE MODEL ....................................8-3
Unbending Ruled Geometry: the Regular Unbend ............................................................ 8-3
Unbending Nonruled Geometry: the Cross Section Driven Unbend ................................. 8-3
Adding Tears to the Geometry: Ripping ............................................................................ 8-4
DEFORMATION AREAS .................................................................................................8-6
EXERCISE 1: Creating a Regular Unbend Feature........................................................... 8-9
EXERCISE 2: Cross Sectional Unbend ........................................................................... 8-11
EXERCISE 3: Creating a Deformation Area ................................................................... 8-16
MODULE SUMMARY....................................................................................................8-21

CONVERTING SOLID PARTS 9-1
CREATING SHEETMETAL PARTS FROM SOLID PARTS .........................................9-3
CREATING A DEVELOPABLE PART............................................................................9-4
EXERCISE 1: Converting a Sheetmetal Part..................................................................... 9-7
EXERCISE 2: Using the Sheetmetal Conversion Feature ............................................... 9-10
MODULE SUMMARY....................................................................................................9-15

SHEETMETAL DRAWINGS WITH FLAT STATES AND BEND ORDER
TABLES 10-1
FLAT STATES.................................................................................................................10-3
Retrieving Instances......................................................................................................... 10-3
CREATING MULTI-MODEL DRAWINGS...................................................................10-4
DOCUMENTING THE BEND ORDER..........................................................................10-5
LABORATORY PRACTICAL ........................................................................................10-7
EXERCISE 1: Documenting the Model........................................................................... 10-7
MODULE SUMMARY..................................................................................................10-17

ADDITIONAL FEATURES 11-1
FLAT PATTERN .............................................................................................................11-3

SOLID FEATURES......................................................................................................... 11-3
EDGE TREATMENTS....................................................................................................11-3
Using Projected Datum Curves ........................................................................................ 11-4
LABORATORY PRACTICAL ....................................................................................... 11-7
EXERCISE 1: Using a Projected Datum Curve to Create a Cut ......................................11-7
MODULE SUMMARY ................................................................................................. 11-13

SETTING UP FOR DESIGN 12-1
CALCULATING DEVELOPED LENGTH .................................................................... 12-3
SETTING UP A DEFAULT RADIUS ............................................................................ 12-7
SETTING DEFAULT FIXED GEOMETRY .................................................................. 12-7
EXERCISE 1: Calculating the Length of a Sheetmetal Part ............................................12-9
EXERCISE 2: Setting Up for Sheetmetal ......................................................................12-12
MODULE SUMMARY ................................................................................................. 12-19

INTERROGATING THE SHEETMETAL MODEL 13-1
SHEETMETAL INFORMATION................................................................................... 13-3
Measurement ....................................................................................................................13-3
Surface Analysis...............................................................................................................13-3
Sheetmetal Bend Reports .................................................................................................13-4
Sheetmetal Radii Reports .................................................................................................13-5
DESIGN RULES.............................................................................................................. 13-6
Establishing a Design Rule Table.....................................................................................13-6
EXERCISE 1: Using Sheetmetal Information Tools........................................................13-9
MODULE SUMMARY ................................................................................................. 13-13

ADDITIONAL EXERCISES A-1
EXERCISE 1: Creating a Blended Primary Wall..............................................................A-3
EXERCISE 2: Creating a Flat Primary Wall.....................................................................A-6
EXERCISE 3: Creating a Swept Secondary Wall .............................................................A-8
EXERCISE 4: Creating a Twisted Secondary Wall ........................................................A-10
EXERCISE 5: Bend Line Adjustment.............................................................................A-13
EXERCISE 6: Creating an Edge Bend and a Rip............................................................A-18

SKETCHER BASICS B-1
THE SKETCHER ENVIRONMENT ............................................................................... B-2
The Sketcher Interface....................................................................................................... B-2

Intent Manager .................................................................................................................. B-3
Pop-Up Menus .................................................................................................................. B-4
SKETCHER MODE FUNCTIONALITY.........................................................................B-4
Sketcher Menus................................................................................................................. B-4
Specifying References....................................................................................................... B-5
Creating Geometry............................................................................................................ B-6
Dimensioning.................................................................................................................... B-7
Constraining.................................................................................................................... B-10
Additional Sketcher Tools .............................................................................................. B-11
SETTING SKETCHER PREFERENCES ...................................................................... B-14
SKETCHER PHILOSOPHY ...........................................................................................B-17
Rules of Thumb............................................................................................................... B-17
LABORATORY PRACTICAL .......................................................................................B-19
EXERCISE 1: Sketching Basics ..................................................................................... B-19
EXERCISE 2: Sketching in Steps................................................................................... B-25
EXERCISE 3: Sketching a Hexagon .............................................................................. B-30
MODULE SUMMARY...................................................................................................B-33

USING PTC.HELP C-1
PTC HELP OVERVIEW...................................................................................................C-2
PTC HELP FEATURES....................................................................................................C-2
USING THE PRO/ENGINEER HELP SYSTEM .............................................................C-2
Getting Help While Performing a Task..............................................................................C-2
GETTING HELP THROUGH THE PTC HELP SIDEBAR.............................................C-3
PTC HELP MODULE LIST..............................................................................................C-4

PTC GLOBAL SERVICES: TECHNICAL SUPPORT D-1
FINDING THE TECHNICAL SUPPORT PAGE.............................................................D-2
OPENING A TECHNICAL SUPPORT CALL ................................................................D-2
Opening a call via email: .................................................................................................. D-2
Opening a Call via Telephone:.......................................................................................... D-3
Opening calls on the PTC Web Site:................................................................................. D-3
Sending Data To Technical Support ................................................................................. D-3
CALL / SPR FLOW CHART AND PRIORITIES............................................................D-4
REGISTERING FOR ON-LINE SUPPORT.....................................................................D-5
ONLINE SERVICES.........................................................................................................D-6
FINDING SOLUTIONS IN THE KNOWLEDGE BASE ................................................D-6
GETTING UP-TO-DATE INFORMATION ....................................................................D-8
CONTACT INFORMATION............................................................................................D-8
Internet .............................................................................................................................. D-8

Telephone ..........................................................................................................................D-9
ELECTRONIC SERVICES ............................................................................................ D-13


For University Use Only - Commercial Use Prohibited

Module

Introduction to Sheetmetal Design
Using the functionality available with the Pro/SHEETMETAL
module, you can capture your design intent by bending flat material
into its final formed shape, as well as create a flat form for
manufacturers to use to develop the actual model.

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

• List benefits of designing sheetmetal components using
Pro/SHEETMETAL
• List specialized sheetmetal feature types
• Describe the display of a sheetmetal part
• Describe how to orient a sheetmetal part
• Describe the design approach for a sheetmetal part

Page 1-1

NOTES

THE SHEETMETAL DESIGN ENVIRONMENT
Using Pro/SHEETMETAL to generate sheetmetal components enables
you to do the following:

• Design a sheetmetal part that defines the supporting structures in an
assembly
• Add sheetmetal-specific features such as walls, bends, cuts, punches,
notches, and forms to a model in either the formed or flat condition
• Control the developed length of the bends when creating a flat instance
of the model
• Create flat patterns and flat states of the model geometry to reflect the
manufacturing and design models
• Create bend order tables that define the bend order, bend radius, and
bend angle used in the manufacturing process
• Document the design by generating production drawings of the flat
model and design model, as well as bend order tables

SHEETMETAL PARTS
Features
Sheetmetal parts are created in Sheetmetal mode, Assembly mode as
sheetmetal components, or from a regular Pro/ENGINEER part. When you
create a new file, you can use a default template or choose one from a list
of standard or user customizable templates. When you use a template that
contains designated parameters, you are able to enter parameter values as
you create the model. Templates also include default datum planes and a
coordinate system, saved views, and default layers.

Pro/ENGINEER offers specialized feature types for the sheetmetal design
environment. They include the following:

• sheetmetal cuts
• notches
• punches
• bends
• unbends

Introducti on to Sh eetm etal D esig n Pag e 1- 3

NOTES

• bend backs
• forms
• walls

Note:
Create features in an order that captures your design intent, not
in the order in which you would manufacture the geometry.

Sheetmetal Part Display
A sheetmetal part appears with green and white surfaces with side surfaces
in between to define depth. This enables you to visualize the part and
geometry selection, since sheetmetal parts tend to be comparatively thin.
Sheetmetal parts always have a constant thickness. Pro/ENGINEER
creates the white surface by offsetting it from the green surface by the
amount of the material thickness. The side (depth) surfaces do not appear
until the part has been successfully regenerated.

Orienting the Sheetmetal Part
When orienting a sheetmetal part, the first selection must be a planar
surface or a datum plane and the second selection may be an edge. (This
way of viewing is available in all modes of Pro/ENGINEER.) You may
also use the thin edge surfaces of the sheetmetal part for orienting. Using
Query Select is the suggested method of selecting these thin surfaces.

Figure 1: Orienting a Sheetmetal Part

Pag e 1- 4 Fundament als of Sh e etme t al

NOTES

Developed Length
Pro/ENGINEER automatically compensates for stretching that occurs in
the area of a bend by taking into account the thickness of the sheetmetal,
the radius of the bend, the bend angle, and other material properties. This
enables you to capture your design intent through the creation of the
formed sheetmetal model, but also enables you to create a flat form of the
model for manufacturers to use to develop the actual model.

Figure 2: The Developed Length

DESIGN APPROACH
You can generate sheetmetal models at either the sheetmetal level or the
assembly level, but the assembly level enables you to use the top-down
design approach.

The following is a typical design approach for creating sheetmetal parts at
the assembly level:

1. Create the assembly by assembling all major components relative
to each other. You can include simple supporting structures, or
sheetmetal parts that are not completely defined at this time.


NOTES

Figure 3: Assembly of Sheetmetal Components

2. Create or modify sheetmetal parts in Assembly mode using the
internal components as references. This process will aid in creating
support walls, form features for stiffening panels, and punches and
notches for fastening the components.


NOTES

Cover created in Additional
assembly features added to
referencing complete cover
internal in Sheetmetal
components mode

Figure 4: Modify Sheetmetal Parts in Assembly Mode

3. After the cabinet and supporting structures are defined relative to
the internal components and each other, add any remaining
components or features.

4. Create or select a bend table to provide material allowances when
unbending the part. The bend table data will be used to ensure
accurate flat pattern geometry of the sheetmetal part.

5. In Sheetmetal mode, create a bend order table to define the
bending sequences for each part.

6. Add a Flat Pattern feature. This will create the flat pattern for
manufacturing. Another option is to create a Flat State.

7. Create a family table for each sheetmetal part that includes at least
two instances: the unbent flat pattern instance and the “as


NOTES

designed” instance. These instances are automatically created
using the Flat State option.

8. Document the parts by creating drawings. You can include both
instances (that is, with a multi-model drawing). Show the
dimensions for the “as designed” part and show/create dimensions
for the flat pattern part. Add the bend order table as a note.

Figure 5: Drawing of Sheetmetal Part


NOTES

MODULE SUMMARY
In this module, you have learned about:

• The benefits of using Sheetmetal mode to design sheetmetal parts
• Display and orientation characteristics specific to sheetmetal parts
• A design approach for creating sheetmetal parts at the assembly level



Module

Primary Walls
In this module, you will learn how to create primary walls. The first
sheetmetal feature must be a wall.

Objectives

• Create the primary wall in a sheetmetal model
• Use sketching techniques to create the section for a primary wall

Page 2-1

NOTES

WALL TYPES
Pro/SHEETMETAL gives you the ability to create two types of walls:
primary and secondary. Primary walls do not need another wall in order to
exist. They can stand alone. A secondary wall, however, must be attached
to another wall because it cannot exist independently; thus, it is always a
child of another wall.

CREATING THE FIRST WALL
Wall Feature Options
To create any model in Pro/ENGINEER, you should start with three
default datum planes. If you use one of the sheetmetal templates, the part
will automatically include these. When creating sheetmetal geometry, you
must add a wall as the next feature.

The following options are available for creating walls:

• Extrude – Sketches the side section of the wall and extrudes it to a
specified depth, as shown in Figure 1.

Figure 1: Extruding to a Specified Depth

• Revolve – Sketches the side section of the wall and revolves it about a
centerline, as shown in Figure 2.

P rim a ry Wa lls Pag e 2- 3

NOTES

Figure 2: Revolving about a Centerline

• Blend – Uses parallel, rotational, or general blend feature forms to
create a wall, as shown in Figure 3. For more information on blends,
see “Creating a Blend” in PTC Help.

Figure 3: Using Blend Feature Forms

• Flat– Sketches the boundaries of the wall in the Sketcher plane, as
shown in Figure 4.

Figure 4: Sketching in a Plane


NOTES

• Offset – Offsets from an existing surface, as shown in Figure 5. For
more information on offset surfaces, see “Creating Surfaces by
Offsetting” in PTC Help.

Figure 5: Offsetting from an Existing Surface

• Advanced – Creates a wall by using datum curves, multiple
trajectories, and so on.

Sketching Technique
When creating an extruded wall, you can insert bends to represent inside
and outside radii. Usually, you dimension all bends in sheetmetal parts to
the inside. To do this, you may need to use the Thicken option to thicken
the material and dimension the offset edges, as shown in Figure 6.


NOTES

Figure 6: Thickening the Material

It is common practice to dimension sheetmetal walls to the mold line (the
intersection of the flat wall extensions). To create this dimensioning
scheme, you must add Sketcher centerlines and points while creating the
wall section. You can then dimension to the Sketcher points, instead of the
tangent points on the arc, as shown in Figure 7.

Figure 7: Defining a Mold Line


NOTES

LABORATORY PRACTICAL
Goal
The goal of this exercise is to create the primary wall of a sheetmetal part
as an extruded wall.

Method
In this exercise, you begin developing the lower housing of a cable box.
The section of the extruded wall will be thickened and the inside radii
dimensioned.

EXERCISE 1: Creating the Cable Box Base

Figure 8: First Wall of Cable Box

Task 1. Start the definition of a sheetmetal model.

1. Create a new part file and select Sheetmetal as the sub-type in the
NEW dialog box, as shown in Figure 9. The Use default template
option is selected so that the part uses the default sheetmetal
template.

2. Type [CABLE_BOX_BASE] as the name and click OK .


NOTES

Sub-type
selection

Figure 9: NEW Dialog Box

Task 2. Create an extruded wall on both sides of the FRONT datum
plane.

1. Click Feature > Create > Wall > Extruded > Done > Both Sides
> Done .

2. Select datum plane FRONT as the sketching plane and datum plane
TOP as the top reference.

3. Sketch the section as shown in Figure 10.


NOTES

Figure 10: The Dimensioning Scheme

Task 3. Change the dimensioning scheme so that the system dimensions
the inside radius by thickening the geometry.

1. Click Sketch > Feature Tools > Thicken .

2. Click Flip or Okay to add material inside the sketched section.

3. Type [0.08] as the thickness.

4. Delete the existing radius dimension.

5. Add a radius dimension to the thicken line, as shown in Figure 11.
This results in an inside radius.

Tips:
Make sure that you pick the thicken arc, not the solid arc. Use
Query Sel to make it easier.


NOTES

Dimension
the thicken
arc

Figure 11: Dimensioning the Thicken Line

6. Modify the radius dimension to [.13] and exit from Sketcher.

7. Extrude to a blind depth of [12]. The completed wall feature
appears as shown in Figure 12.


NOTES

Figure 12: The Finished Base

8. Save the model and erase it from memory.


NOTES

MODULE SUMMARY
In this module, you have learned that:

• The first sheetmetal feature must be a wall.
• The section of a wall can be thickened so that inside radii are
dimensioned.
• Centerlines can be used in the section of a wall to dimension to the
mold line.



Module

Secondary and Unattached Walls
After you create the base wall for a sheetmetal model, you can attach
secondary walls to its edges. You can also create unattached walls
and later merge the geometry.

Objectives

• Create an attached secondary wall along the complete length of the
primary wall edge
• Create an attached secondary wall partially along the primary wall
edge
• Create relief for secondary walls
• Create unattached walls and merge the geometry

Page 3-1

NOTES

TYPES OF SECONDARY WALLS
You can create several different types of secondary walls by sketching the
bend in the wall or automatically creating a bend along the attachment
edge. Using the No Radius and Use Radius options, you can create flat,
extruded, partial, and swept secondary walls.

• Flat, No Radius – Sketch the boundaries of the wall attached to the
selected edge. The new wall is automatically created parallel to the
adjacent wall, as shown in Figure 1 and Figure 2.

Figure 1: Flat, No Radius

Figure 2: A Wall Partially Along the Edge

• Extruded, No Radius – Sketch the side section of the wall that will be
extruded along the attachment edge. You determine if the bend is
created when sketching the section, as shown in Figure 3.

Figure 3: Extruded, No Radius

Se conda ry and Un atta ched Wall s Pag e 3- 3

NOTES

If you sketch an arc to define the bend, you must sketch it tangent to the
attachment edge and adjacent to the green or white surface, as shown in
Figure 4.

Figure 4: Ensuring Tangency

You can also partially extrude the wall along the selected edge using the
blind depth option and by defining a sketching plane partially along the
edge.

• Swept, No Radius – You can attach the wall to a nonlinear edge, but
the edge must consist of all tangent entities, as shown in Figure 5. The
green or white surfaces of the attachment edge do not necessarily have
to be planar. For more information on sweeps, see “Creating a Sweep”
in PTC Help.

Figure 5: Swept, No Radius

• Flat, Use Radius – You can define the sketching plane at a specific
angle through a selected attachment edge and then define a radius for
the desired bend at the attachment edge, as shown in Figure 6.


NOTES

Figure 6: Flat, Use Radius

• Extruded, Use Radius – You can sketch the side profile of the wall
with a specified angle and then define the radius of the bend, as shown
in Figure 7. This bend deforms a portion of the existing attachment
wall.

Figure 7: Extruded, Use Radius

You can also partially extrude a wall along an edge using a blind depth
and relief, as shown in Figure 8.

Figure 8: Using Make Datum and Depth Option Blind


NOTES

• Swept, Use Radius – You can sketch the section for the wall, and
then specify the radius, as shown in Figure 9. With the Use Radius
option, you cannot enter a wall angle that is greater than 180° to the
adjacent green or white surface of the attachment edge.

Figure 9: Swept, Use Radius

Resulting Geometry
The Use Radius option produces different results, depending on the
attachment edge that you select, as shown in Figure 10 and Figure 11. If
you attach the geometry to an edge that is going to be the outside edge of
the wall, the length of the original wall does not change. However, if you
attach it to the inside edge, the wall extends a distance beyond the length
of the original wall that is equal to the thickness of the geometry.

Attached to inside edge

Attached to outside edge

Figure 10: Extruded Walls


NOTES

Figure 11: Flat Walls

When creating a flat wall, Pro/ENGINEER also enables you to
automatically miter a corner by sketching outside the attachment edge and
aligning to an existing wall, as shown in Figure 12. You must add rip
relief at the attachment edge.

Aligned to
inside edge

Figure 12: Mitered Corner

Part and Feature Bend Tables
When creating a wall with the Use Radius option, you must specify
whether you want to use a part bend table or a feature bend table. Bend
tables control the developed length of the bends. Using the Part Bend Tbl
option, you can use a single table to control all of the bends on the entire
model.

Creating Other Walls
A twist takes the form of an extension to a straight edge on an existing
planar wall. It can be rectangular or trapezoidal. It has an axis running
through it center, perpendicular to the attach edge and it can be twisted
around the axis by a specified amount, as shown in Figure 13. You cannot
use a radius with the twist wall type. You can unbend a twisted wall using


NOTES

the Unbend and Regular options. You can also add more walls to the end
of the wall.

To generate the twisted geometry, you must specify the following values:

• Point of attachment
• Width at the start
• Width at the end
• Length
• Twist angle
• Developed length

Figure 13: Twisted Wall

To create an extended wall, you can extend the existing green surface of a
wall up to an existing planar surface or to a specified distance. Using this
technique, you can close gaps between walls in the geometry by extending
up to the inside or outside surfaces of the wall, as shown in Figure 14. You
cannot use a radius with the extended wall type.


NOTES

Open corner

Extended to
the inside Extended to
surface outside surface

Figure 14: Closing Gaps between Walls by Extending

CREATING UNATTACHED WALLS
After you add the first wall of the model, you can create additional
unattached walls using the same methods. Figure 15 shows a primary wall
with an unattached wall. The Unattached option enables you to capture
the intent of the model with greater flexibility by enabling you to
concentrate in more than one area on the model. Once you have created
the walls, you can use an unattached or secondary wall to “bridge the gap”
and then merge the geometry.

Figure 15: Unattached Wall


NOTES

Merging Unattached Walls
To successfully merge an unattached wall with an unattached or secondary
wall, the wall geometry must be tangent to the wall with which you are
merging it.

Also, the corresponding green side of the unattached wall must be adjacent
to the green side of the adjacent wall. You can change this, if necessary,
by using the Swap Side element, as shown in Figure 16.

Figure 16: Matching the Side

SECONDARY WALLS WITH RELIEF
When creating walls or bends that require relief, the system provides an
automatic relief function. The choices are as follows:

• No Relief – Attach the wall without reliefs.
• StrtchRelief – Use material stretching to provide bend relief at the
wall attachment points, as shown in Figure 17. The system prompts for
the width and angle of the stretch relief.

Figure 17: Stretch Relief


NOTES

• Rip relief– At the wall attachment points, rip the existing material
normal to the edge and back to the tangent line as shown in Figure 18.

Figure 18: Rip Relief

• RecRelief – At the wall attachment points, apply a rectangular cut by
defining its width and depth, as shown in Figure 19.

Figure 19: Rectangular Relief

• ObrndRelief - At the wall attachment points, apply an obround cut by
defining its width and depth, as shown in Figure 20.

Figure 20: Obround Relief


NOTES

Goal
The goal of this exercise is to create secondary walls with relief, when
necessary and create unattached walls that are eventually merged with
existing geometry.

Method
In the first exercise, you will create secondary walls using different types
of automatic relief. In the second exercise, you will create secondary walls
and create additional extruded and extended walls to close gaps in the
geometry. In the third exercise, you will create a new part using several
different techniques to construct the walls. In the fourth exercise, you will
create two unattached walls in a part and merge them to complete the
geometry.

EXERCISE 1: Adding Walls to the Cable Box Base

Figure 21: Cable Box Base

Task 1. Create a Flat, Use Radius wall with obround relief on one end
of the cable box base.

1. Open CABLE_BOX_BASE.PRT. If you did not complete the base of
the cable box, open SECONDARY_CABLE_BASE.PRT.

2. Click Feature > Create > Wall > Flat > Use Radius > Done .


NOTES

3. Click Part Bend Tbl > Done/Return > Inside Rad >
Done/Return .

4. Pick the lower green edge to attach the wall as shown in Figure 22.

Attach to the green
lower edge

Figure 22: Attaching the Wall to the Lower Edge

5. Click Done to use the default bend angle of 90 degrees.

6. Click Okay to accept the viewing direction.

7. Sketch the section as an open section consisting of three lines as
shown in Figure 23.

Align the endpoint
to the edge

Figure 23: Sketching an Open Section

8. Exit Sketcher when the section is complete and orient to the
default view.

9. Click w/Relief > Done . A point on the attachment edge highlights
at the end of the new wall.

10. Click ObrndRelief > Done for the first end of the wall.


NOTES

11. Click Enter Value and type [0.20] for the relief’s width.

12. Click Tan To Bend .

13. Define the same relief for the other end of the wall.

14. Type [0.13] for the bend radius value. Click OK in the dialog
box. The part should appear as shown in Figure 24.

Figure 24: Flat Wall with Obround Relief

Task 2. Create another wall on the other end of the part.

1. Create a similar flat wall on the opposite end of the cable box. Use
obround relief on both ends of the wall. Make this wall reference
the first flat wall (that is, no dimensions are required for the second
flat wall). The part should appear as shown in Figure 25.


NOTES

Figure 25: Completed Cable Box Base

2. Save the model and erase it from memory.


NOTES

EXERCISE 2: Adding Walls to the Tuner Cover

Figure 26: Secondary Walls Added to Tuner Cover

Task 1. Create a flat wall on one end of the part that does not extend
past the existing wall.

1. Open TUNER_COVER.PRT.

2. Click Feature > Create > Wall > Flat > Use Radius > Done .

Done/Return .

4. Pick the edge indicated in Figure 27.

Pick the upper
white edge

Figure 27: Attachment Edge for Flat Wall


NOTES

5. Click 90.000 > Done .

6. Click Okay for the direction of viewing the sketching plane.

7. Sketch an open section in which the endpoints pass through the
Sketcher points provided by the system. Align the horizontal edge
to the lower surface of the existing side wall, as shown in Figure
28.
Section sketched
to Sketcher points

Align to bottom
surface of wall

Figure 28: Open Section for Flat Wall

8. When finished sketching, exit from Sketcher.

9. Use rip relief at both ends of the wall.

10. Type [.05] as the bending radius value.

11. Click OK . The model should appear as shown in Figure 29.

Task 2. Create an extruded wall on the other end of the model.

1. Click Create > Wall > Extruded > Use Radius > Done .

Done/Return .

3. Click One Side > Done .

4. Pick the edge to attach the wall, as shown in Figure 29.


NOTES

Pick here on
the white edge

Figure 29: Selection Edge for Extruded Wall

5. Click Default > Flip to define the sketching plane and viewing
direction.

6. Sketch the section as shown in Figure 30. Make sure that the
endpoint passes through the Sketcher point provided by the system.
Align the other end to the edge of the existing wall.

Align endpoint to
edge

Sketched line

Figure 30: Section for Extruded Wall


NOTES

7. Finish the wall definition using rip relief on both ends and type
[.05] as the bending radius value. The part should appear as
shown in Figure 31. The walls that you just created look identical.

Figure 31: Flat and Extruded Walls

Task 3. Extend the flat wall to the outside of the side walls.

1. Click Create > Wall > Extend > Done .

2. Pick the edge shown in Figure 32 as the edge to extend.

3. Click Query Sel to pick the hidden inside surface of the side wall
to define the extension distance.


NOTES

Pick hidden
inside surface
Pick this
edge

Figure 32: Defining the Geometry to Extend

4. Click OK . The part should appear as shown in Figure 33.

Figure 33: Completed Extension

5. Create another wall extension on the other end of the flat wall
using the references shown in Figure 34.


NOTES

Extend the
wall to this
surface

Pick this
edge

Figure 34: Defining the Second Wall Extension

Task 4. Use Extruded walls to create tabs on the back wall of the model
to close the gap.

1. Click Create > Wall > Extruded > No Radius > Done .

2. Use a part bend table to drive the bend geometry and extrude one
side of the sketching plane.

3. Pick the attachment edge as shown in Figure 35.

Pick this
hidden edge
for
attachment
(inside edge)

Figure 35: Specifying the Attachment Edge


NOTES

4. Click Default > Okay to define the sketching plane and viewing
direction.

5. Sketch a section consisting of a line and a tangent arc, as shown in
Figure 36. Use the dimensioning scheme shown.

Tangent arc
Line

Figure 36: Section for Extruded Wall

6. Finish the definition of the wall. It should appear as shown in
Figure 37 (as viewed from the underside of the part).

Figure 37: Tab Created as an Extruded Wall


NOTES

7. Add another extruded No Radius wall to the other side of the wall
to fully close up the cover. The completed part should appear as
shown in Figure 38.

Figure 38: Completed Part

Task 5. Determine if any of the walls that you created overlap in the
unbent state of the model.

1. Click Create > Unbend > Regular > Done and pick the top
surface of the cover to remain fixed.

2. Click Unbend All > Done .

3. Click OK to complete the feature. The unbent state of the model
should appear as shown in Figure 39. If any of the walls overlap,
they are highlighted in red.


NOTES

Surface to
remain fixed

Figure 39: Unbent State

4. Save the part and erase it from memory.


NOTES

EXERCISE 3: Creating the Box

Figure 40: Completed Model

Task 1. Create a new sheetmetal part.

1. Create a new sheetmetal part called BOX.

2. For the first sheetmetal feature, create an extruded wall using the
section shown in Figure 41, sketched on the TOP datum plane.


NOTES

Figure 41: Section for Base Wall

3. Click Thicken on the pop-up menu to thicken the sketch. Type
[0.12] as the inside wall value to maintain the proper
dimensioning scheme. Make sure that the 0.35 dimension belongs
to the inside (thickened) portion.

4. Extrude the wall to a blind depth of [10.00].

Task 2. Create three flat secondary walls attached to the base wall.

1. Create a flat wall using the Use Radius , Part Bend Tbl , and
Inside Rad options.

2. Pick the green edge indicated in Figure 42 to attach the wall.


NOTES

Attach wall to
the green edge

Figure 42: Attaching the Wall

3. Use the default bend angle of 90 degrees.

4. Sketch the wall as shown in Figure 43. After finishing the sketch,
click No Relief and type [0.10] as the bend radius.

Figure 43: First Secondary Wall


NOTES

5. Create another flat wall so that it closes off the end of the box and
Pro/ENGINEER miters the corner automatically. Use the Use
Radius , Part Bend Tbl , and Inside Rad options. Use the default
bend angle of 90 degrees. Pick the edge shown in Figure 44.

Attachment edge
(white edge)

Figure 44: Creating Another Flat Wall

6. Sketch the section for the wall, as shown in Figure 45. You do not
need to add dimensions, but add the appropriate references. Notice
that the side of the sketch crossing the bend is beyond the Sketcher
point. Pro/ENGINEER, therefore, miters both walls at this corner.


NOTES

Right vertex
of edge

Figure 45: Sketching Second Wall to Create a Miter

7. After finishing the sketch, click W/Relief and use the Rip relief
option for the right vertex, as shown in Figure 45. Type [0.35] as
a bend radius.

8. Create another flat wall for the other end of BOX.PRT. Use the
default bend angle of 90 degrees. Pick the white edge indicated in
Figure 46.

Attachment edge
(white edge)

Figure 46: Creating a Flat Wall for the Other End of BOX.PRT


NOTES

9. Sketch the wall using the section shown in Figure 47. After
finishing the sketch, click No Relief and type [0.10] as the bend
radius.

Figure 47: Sketching the Flat Wall

Task 3. Create a secondary wall that is partially extruded along the base
wall.

1. Create an extruded wall using the Use Radius , Part Bend Tbl ,
and Inside Rad options.

2. Click One Side > Done .

3. Pick the green edge as shown in Figure 48.


NOTES

Pick this green
edge to attach
wall

Offset the datum
plane from datum
plane RIGHT

Figure 48: Offsetting Datum Point

4. Click Make Datum and create a datum plane Offset from datum
plane RIGHT by [2.0].

5. Flip the viewing direction. Keep in mind that the direction of
viewing for the wall is also the direction of feature creation.

6. Click Default on the SKET VIEW menu to define the orientation.

7. Sketch the section as shown in Figure 49.


NOTES

Figure 49: Sketching the Partial Wall

8. After completing the sketch, click W/Relief and use the Rip Relief
option on each end of the wall.

9. Type [0.10] as the bend radius value. Do not click OK yet.

10. Click the optional Depth element in the dialog box, then click
Define .

11. Type a Blind depth of [1.5].

12. Click OK to complete the feature. The wall should appear as shown
in Figure 50.


NOTES

Figure 50: Partial Wall Feature with Rip Relief

Task 4. Redefine the wall to change the relief from rip to stretch.

1. Redefine the last wall and click Relief in the dialog box.

2. Click w/Relief > Done > StrtchRelief > Done .

3. Type [0.25] as a stretch relief value and [45] as an angle for
both ends. Notice the changes that occur where the partial wall
meets the base feature wall, as shown in Figure 51.

Figure 51: Partial Wall Feature with a Stretch Relief



NOTES

EXERCISE 4: Creating an Unattached Wall

Figure 52: Custom Shield

Task 1. Open the part and use the surface geometry to create two walls.

1. Open CUSTOM_SHIELD.PRT.

2. Click Feature > Create > Sheet Metal > Wall > Offset > Done .

3. Pick the surface on the right-hand side, as shown in Figure 53.
Pick this surface
from which to
offset

Figure 53: Pick Right-Hand Surface

4. Type [0] as the offset value.

5. If necessary, flip the arrow outward (to the right), as shown in
Figure 54. Click Okay.


NOTES

Figure 54: Offset Direction

6. Type [.05] as the thickness and click OK .

7. Create an unattached offset wall on the other side. Notice that the
Unattached option is automatically selected when you click
Offset . Type [0] as the offset value and add the thickness to the
outside (to the left), as shown in Figure 55.

Figure 55: Direction of Offset

8. Blank the SURFACES layer.

Task 2. Create an unattached flat wall that spans the gap between the
two offset walls.

1. Click Create > Wall > Flat > Unattached > Done .

2. Pick the FRONT datum plane as the sketching reference. Flip the
arrow outward as shown in Figure 56.

3. Pick the TOP datum plane as the top reference.


NOTES

Figure 56: Sketch Viewing Direction

Note:
Keep in mind that the direction of viewing is also the direction
in which Pro/ENGINEER adds the material thickness.

4. Pick the top datum planes and the two vertical surfaces as
references for the section, as shown in Figure 57.

Pick these
surfaces as
references

Figure 57: Section References

5. Sketch a horizontal centerline along the TOP datum plane.

6. Sketch a rectangle, symmetric about the centerline, where the
vertical edges lie on the referenced surfaces, as shown in Figure
58. Complete the feature when finished sketching.


NOTES

Figure 58: Section for Flat Wall

Task 3. Merge the three walls.

1. Click Create > Wall > Merge > Done .

2. Pick the bend surface on the first wall and click Done Sel > Done
Refs .

3. Pick the front flat surface and click Done Sel > Done Refs again.

4. Click OK in the dialog box.

Pick these surfaces to
merge

Figure 59: Merging the Flat Wall with the First Offset Wall

5. Create another merge feature for the other offset wall on the left
side (Figure 60).


NOTES

Figure 60: Finished Model



NOTES

MODULE SUMMARY
In this module, you have learned that:

• When creating some secondary wall types, you have the option of
having the system automatically apply a radius at the attachment edge.
• The Use Radius option produces different results depending on the
attachment edge selection.
• You can extrude secondary walls partially along an attachment edge
by using the optional Depth element.
• Unattached walls enable you to concentrate on more than one area of
the model.
• Automatic relief can be added to walls when necessary.



Module

Unbend, Bend Back, and Cuts
It is easier to create sheetmetal parts in a completely bent condition;
however, some features must be created in a flat state. Combinations
of unbend and bend back features enable these features to be created
effectively.

Objectives

• Create unbend features
• Create bend back features
• Create sheetmetal cut features

Page 4-1

NOTES

THE UNBEND, REGULAR FEATURE
The unbend, regular feature will unbend the curved surfaces of the part
created by walls and bend features. If all bends are selected, a flat pattern
of the part is automatically generated. You are prompted to pick a plane or
edge to remain fixed while the part is being unbent. It is good practice to
always pick the same plane or edge each time an unbend or bend back
feature is created. This will keep the part in a consistent orientation.

Original model Unbend selected

Unbend all

Figure 1: Unbend Sheetmetal Geometry

Unbend , Bend B ack , and Cu ts Pag e 4- 3

NOTES

THE BEND BACK FEATURE
The bend back feature may be used to return an unbent feature to its
original condition. When you create a bend back feature, you can specify
contours to remain fixed (that is, unbent) by picking on the edge of that
contour.

Figure 2: The Bend Back Feature

Notes:
When a sheetmetal wall overlaps and intersects in the unbent
position, the system highlights it and issues a warning.


NOTES

CREATING SHEETMETAL CUTS
A sheetmetal cut feature enables you to create Thru All and Thru Next
cuts. The techniques for creating the cuts are the same as in Part mode.
Unlike the solid cut, the sheetmetal cut always removes material normal to
the green or white side of the model in order to emulate most sheetmetal
manufacturing processes. The solid cut removes material normal to the
sketching plane.

Solid cut

Sheetmetal cut projected on the white side

Sheetmetal cut projected on green side

Figure 3: Removing Material Using a Sheetmetal Cut


NOTES

Dimensioning Scheme
Features may be added to the sheetmetal part while the part is in any
design condition (that is, completely bent, completely unbent in its flat
condition, or at any stage in-between). It is easiest to design sheetmetal
parts in the completely bent condition. When creating features in the
unbent stages, care must be taken when picking sketcher references. See
the example in Figure 4.

Cut created before bend Cut created after bend
and unbend features

When bend is created,
new surfaces result. Cut
section stays in old
surface location. When bent back, cut section
stays with cut feature. The
cut could have been created
in the bent state.

Figure 4: Creating a Cut in the Flat Condition


NOTES

Goal
The goal of this lab is to create sheetmetal cuts across bent geometry that
result in flat contours.

Method
In this exercise, you create a wall with two bends. An unbend feature is
created followed by two sheetmetal cuts. A bend back feature is then
created, but with two contours remaining flat.

Figure 5: Sheetmetal Cuts with Flat Contours

EXERCISE 1: Unbend and Bend Back
Task 1. Create a new sheetmetal part.

1. Create a new part called BEND_BACK using the default template.

2. Create an extruded wall using the dimension scheme shown in
Figure 6 (use an equal length constraint for the horizontal
segments). Create the wall on both sides of the datum plane. Type
a blind depth of [6.0].


NOTES

Figure 6: Extruded Wall

Task 2. Create an unbend feature.

1. Click Feature > Create > Sheet Metal > Unbend > Regular >
Done .

2. Pick the surface shown in Figure 7 as the one to remain fixed while
unbending.

Pick this surface to
remain fixed

Figure 7: Surface to Remain Fixed during Unbend

3. Click Unbend All > Done and click OK in the dialog box.


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