Catia Sheet Metal Design.pdf

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Sheet Metal Bend create Click Definition dialog box Select icon
Sheet Metal Design
 Preface
 What's New?
 Getting Started
 Basic Tasks
 Workbench
    Description
 Customizing
 Glossary
 Index
  
© Dassault Systèmes 1994-99. All rights reserved.
Preface
The V5 CATIA - Sheet Metal Design is a new generation product offering an
intuitive and flexible user interface. It provides an associative feature-based
modeling making it possible to design sheet metal parts in concurrent engineering
between the unfolded or folded part representation.
As a scalable product, CATIA Version 5 Sheet Metal Design can be used in
cooperation with other current or future companion products in the next CATIA
generation such as CATIA Version 5 Assembly Design and CATIA Version 5
Generative Drafting. The widest application portfolio in the industry is also
accessible through interoperability with CATIA Solutions Version 4 to enable
support of the full product development process from initial concept to product in
operation.
 
 
Highlights
V5R3 CATIA - Sheet Metal Design offers the following main functions:
Associative and dedicated Sheet Metal feature based modeling
Concurrent engineering between the unfolded or folded part representation
Access to company defined standards tables
Dedicated drawing capability including unfolded view and specific settings.
All sheetmetal specifications can be re-used by the CATIA - Knowledge Advisor to
capture corporate knowledge and increase the quality of designs.
Natively integrated, CATIA - Sheet Metal Design offers the same ease of use and user
interface consistency as all CATIA V5 applications.
 
 
 
Using This Product
This guide is intended for the user who needs to become quickly familiar with the
CATIA - Sheet Metal Design Version 5 product. The user should be familiar with
basic CATIA Version 5 concepts such as document windows, standard and view
toolbars.
To get the most out of this guide, we suggest you start reading and performing the
step-by-step tutorial "Getting Started".
The next sections deal with the handling of more detailed capabilities of the product.
 
 
Where to Find More Information
Prior to reading this book, we recommend that you read the CATIA - Infrastructure
User's Guide.
The CATIA - Part Design User's Guide Version 5, the CATIA - Assembly Design User's
Guide Version 5 and the CATIA - Generative Drafting User's Guide Version 5 may
prove useful.
 
 
What's New?
 
Enhanced
Defining the Sheet Metal Parameters
New
Creating Swept Walls
New
Creating Various Stamps
Enhanced
Recognize/Extrude
New
Bend Allowance from External Files
 
Getting Started
Before getting into the detailed instructions for using Version 5 CATIA - Sheet Metal
Design, the following tutorial provides a step-by-step scenario demonstrating how to
use key functionalities.
The main tasks proposed in this section are:
Tasks
All together, these tasks should take about 15 minutes to complete.
 
Accessing the Sheet Metal Workbench
The Sheet Metal Design functions are available when you are in the Part environment.
Several functions are integrated from Part Design workbench.
This task shows how to enter the workbench.
Choose the Sheet Metal Design item from the Start menu.
The Sheet Metal toolbar is displayed and ready to use.
You may add the Sheet Metal Design workbench to your Favorites, using the Tools -> Customize
item. For more information, refer to CATIA V5 - Infrastructure User's Guide.
 
 
 
 
 
 
 
Defining the Sheet Metal Parameters
This task shows you how to configure the sheet metal parameters.
1. Click the Parameters icon 
.
The Sheet Metal Parameters dialog box is displayed.
2. Enter 1mm in the Thickness field.
3. Enter 5mm in the Bend Radius field.
4. Select the Bend Extremities tab.
5. Select Tangent in the Bend Extremities combo list.
 An alternative is to select the bend type in the graphical combo list.
6. Click OK to validate the parameters and close the dialog box.
The Sheet Metal Parameters feature is added in the specification tree.
 
 
 
 
 
 
 
Creating the First Wall
This task shows how to create the first wall of the Sheet Metal Part.
1. Click the Sketcher icon 
 then select the xy plane.
2. Select the Profile icon 
.
3. Sketch the contour as shown below:
4. Click the Exit Sketcher icon 
 to return to the 3D world.
5. Click the Wall icon 
.
The Wall Definition dialog box opens.
By default, the Material Side is set to the top.
6. Click OK.
The Wall.1 feature is added in the specification tree.
The first wall of the Sheet Metal Part is known as the Reference wall.
 
 
 
 
 
 
 
Creating the Side Walls
This task shows you how to add other walls to the Sheet Metal part.
1. Select the Wall on Edge
icon 
.
2. Select the left edge.
The Wall Definition
dialog box opens.
3. Enter 50mm in the Length field.
The application previews the wall.
By default, the Material Side is set to the outside and the Sketch Profile to the
top.
4. Reverse the Sketch Profile.
5. Click OK.
The wall is created.
CATIA displays this creation in the specification tree:
6. Select the Wall on Edge icon 
 again.
7. Select the right
edge.
The Wall Definition
dialog box opens with
the parameters
previously selected.
8. Press OK to validate.
9. Select the Wall on Edge icon 
 again.
10. Select the front edge.
The Wall Definition
dialog box opens with
the parameters
previously selected.
11. Enter 30 mm in the Length field.
12. Press OK to validate.
13. Relimit the last wall:
Select
Sketch.4
Place the
cursor and
right-click on
the top
edge: the
contextual
menu is
displayed.
Select
Mark.1
object ->
Isolate
Click the top
edge left
extremity
and drag it
10 mm to
the right
Click the top
edge right
extremity
and drag it
10 mm to
the left
14. Click the Exit Sketcher icon 
 to return to the 3D world.
Eventually, the final part looks like this:
 
 
 
 
 
 
 
Creating a Cutout
In this task, you will learn how to:
open a sketch on an existing face
define a contour in order to create a cutout.
1. Select the wall
on the right
(Wall.3) to define
the working plane.
2. Click the
Sketcher icon
.
3. Click the Oblong Profile icon 
 to create the contour.
To access to the
oblong profile,
click the black
triangle on the
Rectangle icon.
It displays a
secondary
toolbar.
4. Click to create the first point and drag the cursor.
5. Click to create the second point.
The first semi-axis of the profile is created.
6. Drag the cursor
and click to create
the third point.
The second
semi-axis is
created and
CATIA displays
the oblong profile.
7. Click the Exit Sketcher icon 
 to return to the 3D world.
8. Select the
Cutout icon 
.
 
The Pocket
Definition dialog
box is displayed
and CATIA
previews a cutout
with default
parameters.
 
9. Set the Type to
Up to last option
to define the limit
of your cutout.
This means that
the application will
limit the cutout
onto the last
possible face, that
is the opposite
wall.
 
10. Click OK.
This is your
cutout:
 
 
 
 
 
 
 
 
Creating the Bends Automatically
This task shows how to create the bends automatically.
Click the Automatic Bends icon 
.
The bends are created.
CATIA displays the bends creation in the
specification tree: Automatic Bends.1
The Sheet Metal part looks like this:
 
 
 
 
 
 
 
Unfolding the Sheet Metal Part
This task shows how to unfold the part.
1. Click the Unfold icon 
.
The part is unfolded according to the reference wall plane, as shown below.
2. Click this icon 
 again to refold the part for the next task.
 
 
 
 
 
 
 
 
Extracting Drawings
from the Sheet Metal Part
This task shows how to create the Sheet Metal Part views in the Drafting workbench.
The Sheet Metal part is displayed.
1. Click 
 or select File -> New...
2. Select the Drawing type and click OK.
The Drafting workbench is launched.
The New Drawing dialog box opens.
3. Keep the default parameters and click OK.
 
For more information about this workbench, refer to CATIA -
Generative Drafting User's Guide.
4. The drawing sheet appears.
5. Tile the windows horizontally.
6. Select the Unfolded View icon 
 in the Drafting toolbar.
This icon is added to the Drafting toolbar providing the Sheet Metal workbench is present.
7. Choose the xy plane in the Sheet Metal specification tree.
The unfolded view is displayed with the bends axes.
Eventually, the Drafting sheet looks like this:
 
 
 
 
 
 
 
Basic Tasks
The Basic Tasks section explains how to create and modify various kinds of
features.
The table below lists the information you will find.
 
Theme
 
Managing the Default Parameters
This section explains and illustrates how to use or modify various kinds of
features.
The table below lists the information you will find.
Using Sheet Metal Design assumes that you are in a CATPart document.
 
 
 
 
 
 
Editing the Sheet and Tool
Parameters
This section explains how to change the different sheet metal parameters.
1. Click the Parameters icon 
.
The Sheet Metal Parameters dialog box is displayed.
2. Change the Thickness if need be.
3. Change the Bend Radius if need be.
Convention dictates that the inner angle between the two walls is used to
define the bend.
It can vary from 0° to 180° exclusive. This angle is constant and the bend
axis is rectilinear.
4. Press the Sheet Standards Files... button to access to the company
defined standards, if need be. For more information, refer to the Customizing
section.
5. Click OK to validate the Sheet Metal Parameters.
 
 
 
Modifying the Bend Extremities
This section explains how to change the bend extremities.
Click the Parameters icon 
.
The Sheet Metal Parameters dialog box is displayed.
The second tab concerns the bend extremities.
A combo box displays the six possible axial relimitations for the straight bend:
Minimum with no relief: the
bend corresponds to the
common area of the
supporting walls along the
bend axis.
Square relief: a square relief
is added to the bend
extremity. The L1 and L2
parameters can be modified
if need be.
Round relief: a round relief
is added to the bend
extremity. The L1 and L2
parameters can be modified
if need be.
Linear: the unfolded bend is
split by two planes going
through the corresponding
limit points (obtained by
projection of the bend axis
onto the edges of the
supporting walls).
Tangent: the edges of the
bend are tangent to the
edges of the supporting
walls.
Maximum: the bend is
calculated between the
furthest opposite edges of
the supporting walls.
These options can also be accessed through the pop-up button:
 
 
 
 
Defining the Bend Allowance
This section explains the calculations related to folding/unfolding operations.
When a bend is unfolded, the sheet metal deformation is represented by the
bend allowance V defined by the formula:
L = A + B + V
where:
L is the total unfolded length
A and B the dimensioning lengths as defined on the figures below:
bend < 90°
bend > 90°
Another way to compute the sheet metal deformation is the neutral fiber
definition (K Factor):
W = α * (R + k * T)
where:
W is the flat bend width
R the inner bend radius
T the sheet metal thickness
α the inner bend angle in radians.
If β is the opening bend angle in degrees:
α = π * (180 - β) / 180
Physically, the neutral fiber represents the limit between the material
compressed area inside the bend and the extended area outside the bend.
Ideally, it is represented by an arc located inside the thickness and centered
on the bend axis. Therefore the K Factor always has a value between 0 and
0.5.
When you define the sheet metal parameters, a literal feature defines the
default K Factor, according to the DIN standard:
K = (0.65 + log(R / T) / 2) / 2
This formula can be deactivated or modified using Knowledge Advisor
workbench.
When a bend is created, the bend K Factor and the bend allowance literals
are created.
Two cases may then occur:
If the Sheet Metal K Factor has an activated formula and uses the
default bend radius as input parameter, the same formula is activated
on the bend K Factor with the bend radius as input.
Else the bend K Factor is a formula equal to the Sheet Metal K Factor.
The bend allowance literal is equal to a formula representing the use of the
bend K Factor. This formula is fairly complex and it is strongly recommended
not to delete it.
V = α * (R + k * T) – 2 * (R + T) * tan ( min(π/2,α) / 2)
Though it is possible to deactivate the formula to enter a fixed value.
Finally, the bend flat width is computed from the bend allowance value.
 
 
 
Creating a Sheet Metal Part from an
Existing Solide
 
This section explains and illustrates how to create and use various kinds of features.
The table below lists the information you will find.
Using Sheet Metal Design assumes that you are in a CATPart document.
 
 
 
 
 
 
Recognizing Thin Part Shapes
This task illustrates how to create a Sheet Metal part using an existing solide.
Open the Scenario1.CATPart document from the \online\samples\sheetmetal directory.
The document contains a solide
created in the Part Design
workbench and it looks like this:
1. Click the Walls Recognition
icon 
.
2. Indicate a face to be the
reference wall.
The walls are generated from the
Part Design geometry.
The Walls Recognition.1 feature
is added in the tree view.
At the same time, the Sheet Metal parameters are created, deduced from the Part
geometry.
3. Select the icon 
 to edit the
Parameters:
the Thickness is equal to 1
mm
the Bend radius is twice
the thicknessvalue
the Bend Extremities field
is set to Square relief.
The solide is now a Sheet Metal part. All the features are displayed in the specification tree.
You can modify the parameters and add new features from the Sheet Metal workbench to
complete the design.
 
 
 
Generating Bends from Walls
This task explains two ways to generate the bends in the Sheet Metal part.
The Scenario1.CATPart document is still open from the previous task.
If not, open the Scenario1_2.CATPart document from the \online\samples\sheetmetal directory.
1. Select the Bend icon 
.
The Bend Definition dialog box
opens.
Note that the Radius field is in
gray because it is driven by a
formula: at that time, you cannot
modify the value.
2. Select Wall.1 and Wall.2 in the
specification tree.
The Bend Definition dialog box is
updated.
3. Right-click the Radius field: the
contextual menu appears.
 
4. Deactivate the formula: you can
now change the value.
5. Enter 4mm for the Radius and
click OK.
The Bend is created.
6. Select now the Automatic
Bends icon 
.
The bends are created and the
part looks like this:
 
It is also possible to create first all
the bends, using Automatic
Bends, then modify the
parameters for one or more
bends.
1. Select the Automatic Bends
icon 
.
The bends are created.
 
2. Select the bend of interest:
Bend.3
The Bend Definition dialog box
opens.
 
3. Right-click the Radius field: the
contextual menu appears.
4. Deactivate the formula:
you can now change the value.
 
5. Enter 4mm for the Radius and
click OK.
 
Bend.3 is modified.
 
 
 
Adding a Sheet Metal Feature
This task shows you how to complete the design by adding an oblong wall-cut across the bend area on the unfolded
view.
The Scenario1.CATPart document is still open from the previous task.
If not, open the Scenario1_3.CATPart document from the \online\samples\sheetmetal directory.
1. Unfold the part using this icon 
.
2. Select the Sketcher icon 
 and choose the xy plane.
3. Select the Oblong icon 
.
4. Sketch the following profile and quit the
Sketcher using the Exit icon 
.
5. Select the Cutout icon 
.
The Pocket Definition dialog box opens.
6. Enter 1mm in the Length field and click OK.
7. Fold the part again using this icon 
Eventually, the part looks like this:
 
 
 
Designing in Context
 
This section explains and illustrates how to create and use various kinds of
features.
The table below lists the information you will find.
 
 
 
 
 
 
Designing...
This tasks explains how to create a Sheet Metal part in an Assembly context.
Open the Scenario2.CATProduct document from the \online\samples\sheetmetal directory.
You are in Assembly Design workbench.
The document contains two parts.
1. Right-click Product1 in the file tree and
select New Part...
A dialog box is displayed:
 
2. Enter Part3 in the New part Number
field and click OK.
A New Part dialog box proposes two
locations to define the origin point.
For more information, refer to Inserting a 
New Part.
3. Click No to locate the part origin
according to the Product1 origin point.
Make sure you are in Design Mode:
Select Product1
Choose Edit -> Design Mode
 
4. Switch to Sheet Metal Design
workbench.
5. Activate Part3.
6. Select the Parameters icon 
 to
create the Sheet Metal characteristics for
the part:
1mm for the Thickness,
3mm for the Bend radius,
Linear for the Bend extremities,
and click OK.
7. Click the Sketcher icon 
 and select
the zx plane.
8. Select the Profile icon 
.
9. Sketch the contour and set the contraints as shown below:
5mm between the Sheet Metal
vertical walls and each pad
0mm between the Sheet Metal
horizontal walls and each pad top
0mm between the last point of the
Sheet Metal sketch and the right
pad side.
10. Click the Exit icon 
 to return to the 3D world.
11. Select the Extrusion icon 
.
12. Select the Sheet Metal profile.
The Extrusion Definition dialog box
appears.
13. Enter 50mm for Length1 then click
OK.
The Material Side should be set to the
outside.
14. Select the Automatic Bends icon 
.
The bends are created.
The new features are shown in the
specification tree:
Extrusion.1 with five walls
Automatic Bends.1 with four
bends.
Eventually, the Sheet Metal part looks
like this:
 
 
 
Modifying the Design
In this task, you are going to modify the height and the sketch of Pad.1.
The Scenario2.CATProduct document is open from the previous task.
if not, open the Scenario2_2.CATProduct document from the
\online\samples\sheetmetal directory.
1. Double-click Part1\Pad.1 in the
specification tree.
The dialog box is displayed.
2. Enter 40mm for the Length and click OK.
The pad is updated.
3. Select the Product and Update the Sheet Metal part.
4. Select Part1\Pad.1\Sketch.1.
5. Modify the sketch:
6. Click the Exit icon 
 to return to
the 3D world.
The constraints are respected.
After the Product update, the document looks like this:
 
 
 
 Creating Swept Walls
This section explains and illustrates how to create and use various kinds of
features.
The table below lists the information you will find.
 
 
 
 
 
 
 
 Creating a Flange
This task explains how to generate a flange from a spine and a profile.
Open the SweptWall01.CATPart document from the \online\samples\sheetmetal directory.
1. Select the Flange icon
.
 
The Flange Definition
dialog box opens.
2.Select the edge as
shown in red.
3. Enter 2 mm in the
Radius field,
10 mm in the Length field
and 120° for the Angle.
4. Click OK to create the
flange.
The feature is added to the specification tree.
 
 
 
 
 Creating a Hem
This task explains how to generate a hem from a spine and a profile.
The SweptWall01.CATPart document is still open from the previous task.
If not, open the SweptWall02.CATPart document from the \online\samples\sheetmetal directory.
1. Select the Hem icon
.
The Hem Definition
dialog box opens.
2.Select the edges as
shown in red.
3. Enter 2 mm in the
Radius field, and 3 mm
in the Length field.
4. Click OK to create the
hem.
The feature is added to the specification tree.
 
 
 
 
 Creating a Tear Drop
This task explains how to generate a tear drop from a spine and a profile.
The SweptWall01.CATPart document is still open from the previous task.
If not, open the SweptWall03.CATPart document from the \online\samples\sheetmetal directory.
1. Select the Tear Drop
icon 
.
The Tear Drop
Definition dialog box
opens.
2.Select the edge as
shown in red.
3. Enter 3 mm in the
Radius field, and 8 mm
in the Length field.
4. Click OK to create the
tear drop.
The feature is added to the specification tree.
 
 
 
 
 Creating a Swept Flange
This task explains how to generate a swept from a spine and a user-defined profile.
The SweptWall01.CATPart document is still open from the previous task.
If not, open the SweptWall04.CATPart document from the \online\samples\sheetmetal directory.
1. Using the Sketcher 
, define a profile as shown below:
Then quit the Sketcher, using the Exit icon 
2. Select the Swept Flange icon 
.
The User Defined Flange Definition
dialog box opens.
3. Select the edge and the profile, as
shown in red.
The dialog box looks like this:
4. Click OK to create the swept flange.
The feature is added in the specification tree.
 
 
 
 
 Stamping
This section explains and illustrates how to create and use various kinds of
stamps.
The table below lists the information you will find.
 
 
 
 
 
 
 
 Creating a Point Stamp
This task shows you how to create a point stamp by specifying the punch geometrical parameters.
Open the Stamping.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Point Stamp icon
.
2. Select a point on the top
face.
The Point Stamp Definition
dialog box opens, providing
default values.
3. Change the value in the
different fields, if need be:
Height H,
Radius R1,
Radius R2,
Angle A,
Diameter D.
4. Click OK to validate.
The specification tree indicates
the point stamp has been
created.
 
 
 
 
 
 
 Extruded Hole
This task shows you how to create an extruded hole by specifying the punch geometrical parameters.
The Stamping.CATPart document is still open from the previous task.
If not, open the Stamping2.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Extruded Hole icon 
.
2. Select a point on the top face
where you want to place the hole.
The Extruded Hole Definition dialog
box opens, providing default values.
3. Change the value in the different
fields, if need be:
Height H,
Radius R,
Angle A,
Diameter D.
4. Click OK to validate.
 
The specification tree indicates that
the extruded hole has been created.
 
 
 
 
 
 
 Curve Stamp
This task shows you how to create a curve stamp by specifying the punch geometrical parameters.
The Stamping.CATPart document is still open from the previous task.
If not, open the Stamping3.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Curve Stamp icon
.
2. Select Sketch.4, the curve
previously defined.
The Curve Stamp Definition
dialog box opens, providing
default values.
 
3. Change the value in the
different fields, if need be:
Height H,
Radius R1,
Radius R2,
Angle A,
Length L.
4. Click OK to validate.
The specification tree indicates
that the curve stamp has been
created.
 
 
 
 
 
 
 Surface Stamp
This task shows you how to create a surface stamp by specifying the punch geometrical parameters.
The Stamping.CATPart document is still open from the previous task.
If not, open the Stamping4.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Surface Stamp icon 
.
2. Select Sketch.5, the profile
previously defined.
The Surface Stamp Definition dialog
box opens, providing default values.
 
3. Change the value in the different
fields, if need be:
Height H,
Radius R1,
Radius R2,
Angle A.
4. Click OK to validate.
 
The specification tree indicates that the
surface stamp has been created.
 
 
 
 
 
 
 Bridge
This task shows you how to create a bridge by specifying the punch geometrical parameters.
The Stamping.CATPart document is still open from the previous task.
If not, open the Stamping5.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Bridge icon 
.
The Bridge Definition dialog
box opens, providing default
values.
2. Change the value in the
different fields, if need be:
Height H,
Radius R1,
Radius R2,
Angle A,
Length L1,
Length L2.
3. Select a point on the top
face where you want to place
the bridge.
4. Select an edge to give the
direction of the bridge.
5. Click OK to validate.
 
 
The specification tree
indicates that the bridge has
been created.
 
 
 
 
 
 
 Creating a Louver
This task shows you how to create a louver by specifying the punch geometrical parameters.
The Stamping.CATPart document is still open from the previous task.
If not, open the Stamping6.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Louver icon 
.
2. Select Sketch.8, the profile
previously defined on Wall.2.
The Louver Definition dialog box
opens, providing default values.
3. Change the value in the different
fields, if need be:
Height H,
Radius R1,
Radius R2,
Angle A1,
Angle A2.
4. Click OK to validate.
 
 
The specification tree indicates that
the louver has been created.
 
 
 
 
 
 
 Stiffening Rib
This task shows you how to create a stiffness rib by specifying the punch geometrical parameters.
The Stamping.CATPart document is still open from the previous task.
If not, open the Stamping7.CATPart document from the \online\samples\sheetmetal directory.
1. Click the Stiffness Rib icon 
.
2. Select Bend.1, where you want to
place a stiffener.
Note that the stiffener will always be
centered on the bend radius,
wherever the point may be along the
curve.
The Stiffening Rib Definition dialog
box opens, providing default  values.
3. Change the value in the different
fields, if need be:
Radius R1,
Radius R2,
Angle A,
Length L.
4. Click OK to validate.
 
The specification tree indicates the
stiffness rib has been created.
 
 
 
 
 
 
Patterning
In this task, you are going to create cutouts according to a pattern.
CATIA allows you to define two types of patterns: rectangular and circular
patterns.
These features make the creation process easier.
Open the Scenario3.CATPart
document from the Samples/sheet
metal directory.
The Sheet Metal part looks like this:
1. Select the cutout you want to
duplicate, that is the rectangular one.
2. Click the Rectangular Pattern icon
.
The Rectangular Pattern Definition
dialog box is displayed. Each tab is
dedicated to a direction to define the
location of the duplicated feature.
Set the specification for the First
Direction:
3. Select the Edge.1, as shown, to
specify the first direction of creation.
An arrow is displayed on the wall.
4. Click the Reverse button or select
the arrow to modify the direction.
5. Keep the Instances & Spacing
options to define the parameters.
Choosing these parameters types
dims the Length field because the
application no longer needs this
specification to space the instances.
6. Enter 2 as the number of instances
you wish to obtain in the first direction.
7. Define the spacing along the grid:
enter 30mm.
Defining the spacing along the grid
and the length of your choice, would
make the application compute the
number of possible instances and
space them at equal distances.
8.  Now, click the Second Direction tab
to define the other parameters.
Note that defining a second direction
is not compulsory. Creating a
rectangular pattern defining only one
direction is possible.
9. Select the Edge.2, as shown, to
define the second direction.
10. Keep the Instances & Spacing
option: enter 8 and 10 mm in the
appropriate fields.
Additional cutouts have been aligned
along this second direction.
12. Click OK to repeat the cutouts.
After the update, the Sheet Metal part
looks like this:
13. Select this icon 
 to unfold the
part:
The pattern is updated on the
unfolded view.
Using a similar scenario, you can define a circular pattern.
To know more about patterns, refer to CATIA - Part Design User's Guide.
 
 
 
 
 
 
Interoperability
In a CATPart document, you may have Part Design features and Sheet Metal features
according to the following rules:
Part Design features can be created before Sheet Metal features.
a Part Design feature can also be created after Sheet Metal features as long as
the part is in folded view.
in the unfolded view, the Part Design feature will not be displayed.
it is no longer possible to create Sheet Metal features after this last Part Design
feature in folded view.
1. Create
two walls
with an
Automatic
Bend.
2.Switch to
Part
Design
workbench.
3. Launch
the
Sketcher
and draw
an oblique
line in the
yz plane.
4. Click the
icon 
 to
create a
Stiffener.
5. Switch to the Sheet Metal workbench.
6. Click the Unfold icon 
.
The stiffener is not displayed on the unfolded view.
To add a new Sheet Metal feature, select the Bend for example and right-click the
Define In Work Object item.
The new Sheet Metal feature will be added after the Bend but before the Stiffener.
 
 
 
 
 
 
Workbench Description
 
The CATIA - Sheet Metal Design Version 5 application window looks like this:
Click the hotspots to display the related documentation.
 
Menu Bar
Toolbars
Menu Bar
The Menu Bar and items which are available in CATIA - Sheet Metal Design
workbench are the standard ones.
The tools and commands are described in the V5 CATIA - Infrastructure User's
Guide.
Refer to the CATIA Menu Bar section.
 
 
Toolbars
This section describes the various icons available in the Sheet Metal Design
workbench.
The toolbars are located in the application window border.
The last icon is available whenever you are in the Drafting workbench.
 
 
See Managing Default Parameters
See Sketching...
See Creating the First Wall
See Creating Side Walls
See Designing in Context
See Creating Swept Walls
See Generating Bends from Walls
See Recognizing Thin Part Shapes
See Creating Automatic Bends
See Unfolding the Part
See Creating a Cutout
See Stamping
See Patterning
 
 
See Setting Constraints
See Setting Constraints
 
Sheet Metal in Drafting
 
See Extracting Drawings...
 
 
 
Customizing
This section describes how to customize settings.
The task described here deals with permanent setting customizing.
 
Using Sheet Metal Standards Files
This task explains how to access company standards files.
Open a new document.
1. Click the Sheet Metal Parameters icon 
.
The Sheet Metal Parameters dialog box opens.
2. Select the
Sheet Standards
Files... button.
The Sheet Metal
Part Samples
window is
displayed.
3. Indicate the
path to the
Sheet Metal
tables.
These files are available under .xls or.txt format.
4. Click Open.
In the Sheet
Metal
Parameters
dialog box, the
Design Table
icon 
appears
opposite the
Thickness and
Bend radius
fields.
The parameters
are now in gray,
indicating that
you can no
longer modify
the values.
5. Click the Thickness Design Table icon 
 and select  line 1.
6. Click OK.
The parameter values are updated in the Sheet Metal Parameters dialog box.
7. Click the
Bend Radius
Design Table
icon 
.
8. Select line 2
and click OK.
The parameter
values are
updated in the
Sheet Metal
Parameters
dialog box.
9. Create a
bend.
The Bend
Definition dialog
box displays a
design table for
the Bend
Radius.
The default
mode, it's to say
the formula:
Bend Radius =
Part Radius is
deactivated.
 
Let's see the Bend Radius Table, using this icon 
It shows the Bend Radius and the corresponding Bend Table.
10. Click OK.
If the Angle value is contained in the Bend Table, the Bend Allowance uses the
corresponding value.
If not, the Bend Allowance is computed according to the KFactor.
An alternative if you use the V5R2 Sheet Metal Tables: for example BNDTABL2.
the steps 1 to 4 are identical.
5. Click the Design Table icon 
 and select a line.
6. Click OK.
The parameter values are updated in the Sheet Metal Parameters dialog box.
At that time, the parameters Thickness and Bend radius are driven by the design
table.
They are now in gray, indicating that you can no longer modify the values.
Note that if you create a bend, there is no design table: it's the formula which is used.
To disable the access to design tables:
Select the Tools -> Options -> Part -> Display items and check
Relations:
the Design Table icon 
 is displayed in the specification tree.
Right-click this icon: the contextual menu appears.
Select BNDTABL2.txt object -> Deactivate
The relation is no longer used but still exists.
It can be activated at any time.
 
 
Glossary
B
bend
a feature joining two walls
bend extremity
axial relimitation for a straight bend
C
cutout
a feature corresponding to an opening through a feature
the shape of the opening corresponds to the extrusion of a profile.
E
extrusion
a feature created by extruding a profile and adding thickness
F
flange
a feature created by sweeping a profile along a spine
the different flanges available are:
simple and swept flange, hem and tear drop
P
pattern
a set of similar features repeated in the same feature or part
profile
an opened or closed shape including arcs and lines created by the profile command in the
Sketcher workbench
R
reference wall
the first created wall; when unfolding the part, it is the fixed wall.
S
stamp
a feature created by embossing sheet metal
the different stamps available are:
point, extruded hole, curve, surface, bridge, louver and stiffening rib.
W
wall
a feature created by adding thickness to a profile