(2) catia v5 assembly design

AIRBUS UK CATIA V5 Foundation Course

Foundation Course
Assembly Design
Compiled by: Kevin Burke Approved by: Authorised by:

Kevin Burke
Date: 16/Apr/2003 Date: Date:
AIRBUS UK Ltd. All rights reserved.

DMS42177 Page 1 of 71 Issue 1
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Contents

Session 5 – The Assembly Design Workbench ........................4
An Introduction to the Assembly Design Workbench .............................................. 5
Accessing the Assembly Design Workbench............................................................ 6
An overview of the different Specification Tree Nodes ........................................... 7
Different Display Modes when using CATProducts................................................. 8
Assembly Design Toolbars and Icons..................................................................... 11
Product Structure Tools Toolbar ............................................................................. 12
Add New Component.......................................................................................... 13
Add New Product (CATProduct)........................................................................ 13
Add a New Part (CATPart) ................................................................................. 14
Adding A Existing Component ........................................................................... 15
Replacing a Component ...................................................................................... 16
Graphic Tree Reordering..................................................................................... 18
Generate Numbering ........................................................................................... 18
Creating Multiple Instances of a Node................................................................ 19
Renaming a Node Name ..................................................................................... 20
Defining a Multi-Instantiation............................................................................. 22
Saving a Newly Creating CATProduct ................................................................... 24
Move Operations Toolbar ....................................................................................... 25
Manipulation ....................................................................................................... 25
Snap Operations .................................................................................................. 26
Explode Assembly............................................................................................... 27
Stopping Manipulation on Clash......................................................................... 27
Assembly Constraints.............................................................................................. 29
Assembly Constraints Toolbar ................................................................................ 29
Coincidence Constraint ....................................................................................... 29
Contact Constraint............................................................................................... 31
Offset Constraint ................................................................................................. 32
Angular Constraint .............................................................................................. 34
Fix Constraint...................................................................................................... 35
Fix Together Constraint ...................................................................................... 36
Quick Constraint ................................................................................................. 37
Flexible/Rigid Sub-Assembly ............................................................................. 37
Change Constraint ............................................................................................... 38
Reuse Pattern....................................................................................................... 38
Create a Scene ......................................................................................................... 38
Assembly Operations .............................................................................................. 42
Assembly Features .............................................................................................. 42
Create Symmetry................................................................................................. 45
An Overview of Contextual Links .......................................................................... 47
Session 6 - Analysis ..................................................................50
Accessing the Digital Mockup (DMU) Workbenches ............................................ 51
Proximity Queries ................................................................................................... 52
Clash Analysis......................................................................................................... 55
Sectioning................................................................................................................ 58

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Measuring Distances ............................................................................................... 65

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Session 5 – The Assembly Design
Workbench

On completion of this session the trainee will:

♦ Be able to access the Assembly Design Workbench.

♦ Understand the Assembly Design Toolbars and Icons.

♦ Be able to create Product Specification Tree.

♦ Be able to Position and Orientate Parts within the Product.

♦ Be able to apply Assembly Constraints.

♦ Be able to create a Scene.

♦ Have an understanding of Assembly Operations.

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An Introduction to the Assembly Design Workbench

The Assembly Design Workbench is used to bring together Parts (CATParts) into an
assembly, which is known as a CATProduct document and as such contains no
geometry but links to CATParts. CATProducts can also be made up of a mixture of
smaller CATProducts and CATParts to form larger complex assemblies.
CATProducts can be used in Kinematic simulation, Stress Analysis, Fitting
Simulation, etc.

The CATProduct structure is represented by the Specification Tree, which holds
details of all sub-assembles and their associated parts together with their relative
positions to each other. To maintain the position of the sub-assemblies and parts
within the CATProduct, Assembly Constraints are used which are attached to the
Specification Tree under a Constraints Node. Kinematic Mechanisms, Fitting
Simulations, etc. are also attached to the tree under an Applications Node.

Top level
Assembly Node Sub-Assemblies

Graphical
representation of
the Assembly

Sub-Assembly
Parts

Assembly
Constraints

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Accessing the Assembly Design Workbench
The Assembly Design Workbench can be accessed by either Selecting Start >
Mechanical Design > Assembly Design from the Start drop down menu.

If a CATProduct is not active you will be prompted to create a new product by the
appearance of the Part Name panel.

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An overview of the different Specification Tree Nodes
There are a variety of different node types displayed in the CATProduct Specification
Tree as well as the ones contain within a CATPart Specification Tree, below are the
three commonly used nodes: -

A Product – this node links to a CATProduct document and can be used to
position and orientate it within another CATProduct. Yon can attach other
nodes such as Product, Parts and Component to it.

A Part – contains a link to a CATPart document and used to position and
orientates the part within the CATProduct. You can not attach other nodes to a
Part node.

A Component – this node contains no links to external documents and can be
thought of as a dummy node. You can position/orientate this node and attach
other nodes to it such as Products and Parts.

Here is an example of a CATProduct with three Part nodes attached and a
Component node with a single Part node attached to it.
Product Node
Component Node

Part Nodes

Again the Specification Tree can be expanded or collapsed by selecting the ‘+’ or ‘-‘
symbol on the tree branch. You can also use the View>Tree Expansion drop down
menu.

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Different Display Modes when using CATProducts
There are two types of display modes available when viewing CATProducts: -

1. Visualisation Mode - This uses a Catia Graphical Representation or CGR format
to create a visualisation of the CATParts within the Product. Only the external
appearance of the component is visualised.

The main advantage of using this mode is that performance of the workstation is
improved by virtue of the fact that only a small amount of data is loaded into
memory on the Workstation compared to using Design Mode. This is especially
true on large Assemblies.

The main disadvantages when Parts are in Visualisation mode are that you can
not apply Assembly Constraints to them, modify any geometry or display the
Parts Specification Tree.

When you open an existing CATProduct you are automatically placed into
Visualisation mode, the CGR files are extracted from the CATPart documents
that are attached to the Product and placed in a Cache directory on the
Workstation.

Below is the Specification Tree for a Product when it is in Visualisation mode.
Note that that Assembly Constraints have yellow exclamation symbols attached to
them which indicate that the link to the relevant Features have been broken. This
is normal and the link should reconnect when you switch to Design Mode. In
Visualisation mode there is no means of expanding the Parts node to view the
Part Specification Tree.

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2. The other mode is called Design Mode which allows gain access to the Part
Specification Tree to edit Geometry, you can also apply constraints between
Features on different Parts.

As mention prevoiusly when you open an existing Product you are automatically
placed in Visualisation mode.

One way to enter Design mode is to select the
top or root Node of the CATProduct and then
use MB3 to access the contextual menu and
then select the Representations tab followed
by the Design Mode option. All the CATParts
attached to the Product Specification tree will
now be loaded into Design Mode. This also has
the effect of loading the CATPart documents
into the Workstations memory and on a large
Assembly there may be a time delay whilst this
task is performed.

Once in Design mode the CATPart
Specification Trees are accessible by selecting
the ‘+’ symbol next to the Part node. The
yellow exclamation symbol on the Constraints
should now have disappeared indicating that
they have successfully re-linked.

You also specify which Parts are loaded into Design mode by selecting them
individually on the Specification Tree and then use MB3 to load them. This may
be a more preferable method when large Assemblies are concerned.

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Another way to load a Product into Design mode is to select the Update All icon on
the button menu bar. When you first open an existing Product this icon will be yellow
if you are in Visualisation mode and by selecting it all the Parts on the Specification
will be loaded into Design mode and any links will be updated.

The Update All Icon

Update No Update
Required Required

To switch back to Visualisation mode by using MB3 > Representations
>Visualisation Mode.

Note: When you add a New Part to the Specification Tree it will be automatically
loaded in Design mode.

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Assembly Design Toolbars and Icons
There are five main toolbars
within the Assembly Design
Assembly Workbench Icon workbench: -
Features
1. Product Structure Tools –
Selection used to create the Specification
Tree.
Annotations Product Selection
2. Move Operations – used
for the positioning assembly
Products and Parts.

3. Assembly Features– used
to create assembly based
features within the Product.
Product 4. Annotations – attaches
Structure text annotation to assembly
Tools features.
Constraints
5. Constraints – creates
assembly constraints between
Products and Parts.

Move Operations

The Assembly
Create Scene Design Toolbars
are also accessible
via the Insert
Drop down menu

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Product Structure Tools Toolbar
The main purpose of this toolbar is to allow you to create a Specification Tree and
manipulate its order.
Insert New Component
Insert New Product
Insert New Part
Insert Existing Component
Replace Component
Reordered Tree
Generate Numbers
Load/Unloads Components
Manage Representations
Multi Instantiation Tools

You can also access the majority of these commands by the use of MB3 when you
pass over the currently selected node on the Specification Tree to display a contextual
menu and select Components to display a sub menu

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Add New Component
This allows you to add a new Component Node to the Specification Tree.

After selecting the icon a Part Number panel will appear in
which you must enter a name for the Node in the New Part
Number field and then click OK.

A new Component Node with the name you specified is added to the Specification
Tree attached to the currently active node that is highlighted in blue

Currently Active Node

New Component Node

Add New Product (CATProduct)
Selecting this icon will allow you to add a new CATProduct to the
Specification Tree.

Select the icon to display the Part Numder panel and enter a name for the
CATProduct. The name must conform to the relevant Airbus naming conventions and
procedures. After entering a valid name click OK to add the new CATProduct to the
Specification Tree. Again the new node is attached to the currently active node.
Currently Active Node

New CATProduct Node

Product/Part name Product/Part Instance name

Note: the Origin of the new CATProduct is same as the currently node. An
empty Product has no origin until a Part has been inserted. The Absolute Axis
system (origin) of the Product is defined by the first Part or Product inserted.

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Add a New Part (CATPart)
This icon allows you to add a new CATPart to the Specification Tree.

On selecting this icon the Part Number panel will appear and again you must enter a
valid part name. After you click OK the new CATPart will be attached to the
currently active node on the Specification Tree. As with adding a new CATProduct
the origin on the CATPart is the same as the current active node.

New CATPart Node

If you now add a second new CATPart to the Specification Tree, after entering a valid
part name in the Part Number panel and clicking OK. A New Part: Origin Point
panel will appear asking you to define the origin for the new part. If you select the
Yes button you will have to select either Point element from within an existing
CATPart on the Specification tree or an existing Node to specify the origin. If you
select the No button then the origin will be same as the currently active node.

Note: Using one of the Move Operations or Assembly Constraints can change the
position and orientation of a new CATPart.

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Adding A Existing Component
This command is not as the name implies to add an existing Component node
to the Specification, but in fact it is used to add existing CATProducts and
CATParts.

After selecting the icon an Insert an Existing Component panel will appear. Enter
the directory where you wish search for the required CATProducts or CATParts in the
Look in field and hit the Enter key. The standard directories to enter in this field are
/epd/parts, /epd/readparts or /epd/roa…..

The Name or the files and folders contained within the directory is now listed in the
main window of the panel together the file Type. You can limit your search to a
specific file type by selecting one of the options available in the Files of type field via
the down arrow. You can also enter partial file names together with * as a wildcard in
the File name field followed by hitting the Enter key to perform your search i.e.
L57P123* will list all files beginning with L57P123.

The Open as read-only check box limits access to read only although when you add
an existing file for the ROA it is already set to read only and can not be changed.

Once the required files are listed in the main window you can select them using MB1.
You can also multi select files using the Shift or Ctrl Key. The required file name(s)
will now appear in the File name field. Clicking Open will add them to the
Specification Tree and position them on the origin of the currently active node.

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Below is an example of an existing CATProduct containing a Component node and
seven Part nodes together with their associated Assembly Constraints.

Replacing a Component
By selecting this icon you can Replace a node on the Specification Tree with
another existing Product or Part node.

After selecting the icon you must select a Node on the Tree to be replaced. The Insert
an Existing Component panel will now appear. If required perform a search for the
replacement CATProduct or CATPart and select it using MB1 followed by clicking
theOpen button to continue.

Select Node to be
Replaced

Replacement
CATProduct

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A Replace Mode panel will appear asking you if you wish to replace all instances of
the selected node with the new one. If you select Yes then all occurrences of the
selected node in the Specification Tree will be replaced. If you select No then only the
selected node will be replaced.

The selected node will now be replaced at the same location.

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Graphic Tree Reordering
Allows you to Reorder the nodes on the Specification Tree.

After selecting the icon you must select a node on the tree that as other nodes attached
to it. A Graph tree reordering panel will now be displayed. Select the node name
from the list to be reordered and use one of the three buttons on the right side of the
panel to move the node up or down the tree: -

Increments the node up one position in
the tree.

Increments the node down one position
in the tree.

Moves the selected node next to a
second node you select from the list.

After you have moved the node to the desired position in the list click OK to
complete the reordering.
Generate Numbering
This icon can be used to generate numbers against all nodes in a selected
CATProduct that contains links to geometry.

Select the icon followed by the Product node with Parts
attached. A Generate Numbering panel will appear with the
option to either generate Integer or Letters. You can also select
whether Keep existing numbers or Replace them.

On clicking OK the number command is performed. Nothing
will have visibly changed but the numbers are added to the
Properties of the relevant node. This information can be
extracted and used to compile a Bill Of Materials for the
CATProduct which can then be imported into a CATDrawing.

This command allows you load document into memory. This is an advanced user
function and is not covered in the Foundation course.

This command allows different geometric representation of parts to be used. As with
the last command this is an advanced user function and is not covered in the
Foundation course.

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Creating Multiple Instances of a Node
It is possible to create multiple instances of a Component, Product and Part nodes
within the Specification Tree. The easiest way to perform this task is to select the
node to be instantiated then either use MB3 to access the contextual menu and select
Copy or use the Edit drop down menu and select Copy. The node is then copied
together with its position and orientation within the Tree.

Now select the node on the Tree where you want the new instance to be attached and
again use MB3 or the Edit drop down menu to Paste the new instance on to the Tree.
The new instance will appear on the tree and if there is a geometry associated (i.e.
CATPart) then this will be place in exactly the same position and orientation as the
original node. If you keep using Paste then more Instances will be added to the Tree
in the same position. You can then manipulate its position using the Compass, Snap or
Assembly Constraints.

If you copy a node that has other nodes attached to it then the attached nodes are
copied as well.

Unique Instance
Numbers

Instances
displayed after
repositioning

A unique instance number is added to the node name on the Specification Tree to
identify the new instances.

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Renaming a Node Name
There may be occasions when you will need to rename a Node name on the
Specification Tree. This can be done by selecting the node to be renamed using MB1
followed by MB3 to access the contextual menu and then select Properties.

Selected
Node

A Properties panel will appear which has four tabs enabling you to control the
following: -

1. The name of the Node.

2. The Graphic Properties.

3. The Mechanical Properties.

4. The Drafting Properties.

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The Product tab allows you to edit the
Node Part Number and Instance Name
together with various Attributes.

The important fields on this tab are: -

The Component instance name is the
name displayed in brackets on the
node. If you edit this name you should
ensure that it matches the name in the
Part Number field with the exception
of the instance number.

The Link to Reference lists the file to
which the node is linked and is not
editable.

The Part Number field allows you to
change the first portion of the node
name.

After editing the required fields click
OK to apply the change.

Note: Optegra or Primes do not currently use the Attributes.

The Graphic tab allows you to control the default colour and line font for displayed
geometry.

The Mechanical tab allows you to enter Mass Properties.

The Drafting tab allows you to control how the geometry is displayed in the
CATDrawing.

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Defining a Multi-Instantiation
Allows you create multiple instances of a part in a specified direction.

Fast Multi- Define Multi-
Instantiation Instantiation

Creates a Multi Instantiation of a part in a user-defined direction.

Select the icon to display the Multi Instantiation panel. The following options are
available: -

The Component to Instantiate field displays the part you have selected to
Instantiate.

By selecting the down arrow adjacent to the
Parameters field you will have three options
available to you: -

1. Instance(s) & Spacing equally spaces
the number of instances entered in the
New Instance(s) field using distance
value entered in the Spacing field to
define the Spacing or Step size.

2. Instance(s) & Length equally spaces the
number of instances entered in the New
Instance(s) field through the distance
value entered in the Length field.

3. Spacing & Length automatically derives
the instances by dividing the value
entered Length field by the value entered
in the Spacing field.

The Reference Direction portion of the panel allows you to define the direction of
the Instantiations. You can either use the Axis options to allow you to specify the
direction based on the X, Y or Z axis of the Compass or use a Selected Element i.e. a
Line, Planar face, etc. You can also Reverse the direction. The Result = fields display
the Vector values for the direction.

The Define As Default check box allows you set the current values as default.

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After selecting the part to be Instantiated, the Reference Direction and Instance
options, click OK to create the Instantiation. The Multiple Instances are created in the
Specification Tree.

In the following example a part is Instantiated with four New Instances with a
Spacing or step of 600mm along the X-Axis of the Compass.

Selected part to be
Instantiated

Preview of the
Instantiation

Resulting
Instantiations in the
Specification Tree

Resulting Instance Numbers
Instantiations in the Resulting
Specification Tree Instantiations

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This allows Fast Multi-Instantiations to be created using the Default setting of
the Multi Instantiation panel.

After selecting the part to be Instantiated select the icon to create the instances.

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Saving a Newly Creating CATProduct
The first time you save a newly created CATProduct the Save As panel will appear.
You can then specify the directory where CATProduct to be saved by entering the
path in the Save in field. The correct path for storing such data is /epd/parts. You can
also change the name of the CATProduct by entering a new name in the File name
field.

When you click OK if your CATProduct contains new CATParts that have not been
saved then a Save panel will appear asking you if you wish to proceed.

If you click OK then the CATProduct will be saved into the directory defined in the
Save in field under the specified name together with any new CATParts attached to it.

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Move Operations Toolbar
Allows you to manipulate the position and orientation of Parts.

Manipulation
Snap
Explode Assembly
Stop Manipulation

Manipulation
Allows Freehand Manipulation to position and orientate a selected Part.

Select the icon to display a Manipulation Parameters panel.

Display the
currently selected
button Drag along
any Axis
Drag along the
X, Y or Z-Axis Drag along
any Plane
Drag along the XY,
YZ or XZ Planes Rotate
around any
Axis
Rotate around
the X, Y or Z-
Axis

There are twelve options available, four allowing you to drag along an Axis, four
allowing dragging along Planes, and four allowing you to rotate about an Axis.

After selecting the required button you must select the part to be manipulated using
MB1 and then drag it in the required direction.

This command will stay active until click on the OK or Cancel Button.

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Snap Operations
Positions parts using a snapping.

Snap Smart Move

Snaps one Part to another by selecting elements.

Select the icon and then select an element contained within the Part to be moved i.e. a
Plane, a Face, an Axis System, etc. Now select an element within a second Part to
indicate the new position.

The following is an example of an existing Part that has been added to a CATProduct
and then positioned using its Axis System relevant to an Axis System in another Part
in this case a part containing Positioning Datum’s.

Part containing
Position Datum’s
(Axis Systems)
Part to be
moved
Positioning
Axis System

Axis System of
the Part to be
moved
Resulting
move

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When you snap two Axis Systems together the orientation of the X, Y and Z-Axis is
automatically aligned although is some cases the Axis direction may be reversed. This
can be overcome by dropping the Compass onto the origin of the Axis System in the
Part that is being moved. Then rotation the reversed Axis through at least 180° and
then re-apply the Snap command.

Note: You can only use the Snap command if the currently Active node on the
Specification Tree is the Parent of both Parts being snapped.

√ X
This command is similar to the Snap command. It allows you to Snap one Part
to another and it also allows you to create Assembly Constraints.

After selecting the icon a Smart Move panel will appear and then click on the More
button to display the Quick Constraint options. If you select the Automatic
constraint creation, when you select the elements to snap together and click OK the
parts are snapped together and a Constraint is generated. The use of Assembly
Constraints is explained later in this session.

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Explode Assembly
Allows you to Explode selected CATProducts.

Select the icon to display the Explode panel and select the CATProduct(s) to be
exploded.

You have the following options: -

The Depth field allows you to control how
many levels of the selected CATProduct(s)
are exploded. The choices are limited to
First Level or All Levels.

The Type field allows you to specify the
direction of the Explode to be controlled in
3D, 2D or inline with Constraints.

The Selection field lists the CATProduct(s) you have selected to explode.

The Fixed product field lists CATProduct(s) that you have select to be Fixed and will
not be affected by the Explode.

The Scroll Explode bar allows you to simulate the movement of the Explode.

If you now click OK the CATProduct will be Exploded and Scroll bar will appear in
the Scroll Explode portion of the panel. A Warning message will be displayed
informing you that you are about to modify product positions. If you click Yes then
the Explode will permanently move the Parts together with any Sub-Products and the
command will end. If you click No then the Explode is temporary, which is probably
the safer option and the Explode panel will stay on the screen.

If you select the Apply then again the CATProduct will be Exploded and the Scroll
bar will appear in the Scroll Explode portion of the panel. An Information box
appears informing you than you can use the Compass to move Products. Click OK to
remove this panel and you are now in temporary Explode mode.

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You can use the Scroll bar in the Scroll explode portion of the panel to increment
through the movement of the Parts on the screen from Exploded to assembled.

When you have finished click Cancel to exit Explode mode and this will also reset
the Parts back to their assembly positions.

Below is an example of an exploded CATProduct.

Selected
CATProduct to
be Exploded

Resulting
Exploded
CATProduct

Stopping Manipulation on Clash
Selecting this icon will cause the manipulation of parts when using the
Manipulation icon to be halted if the Part that is being moved Clashes with an
adjacent Part.

Note: The With respect to constraints check box on the Manipulation Panel must
be selected for this to function work.

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Assembly Constraints
Assembly constraints are used to position CATParts relative to each other with a
CATProduct. All assembly constraints are added to the Specification Tree and
attached to a Constraints Node.

Constraints
Node

Assembly
Constraints

When you select one of the Constraint icons an
Assistant panel appears. If you wish, click on the
Do not prompt in the future check box and
Click OK to remove the panel.

Assembly Constraints Toolbar
Coincidence Constraint
Contact Constraint
Offset Constraint
Angle Constraint
Fix
Fix Together

Quick Constraint
Flexible/Rigid Assembly
Change Constraint
Reuse Pattern

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Applies a Coincidence Constraint between two Parts. This is ideally used to
constrain the axis of two Cylindrical features together although you can apply
it to a Points, Edges, Faces, etc.

Select the icon followed by the two elements/features on two different Parts that are to
be constrained. The constraint is attached to the Specification and temporarily
displayed on the screen. If you now click on the Update All button the two Parts that
have features selected will move to align the elements so that they are coincident with
each other.

As you hover over a Cylindrical features the axis of the feature is Axis of the
highlighted on the screen and if you select it then the coincidence Hole displayed
is applied to the axis. when you hover
over the feature

In the following example the Hole feature on the bracket is made
coincident with the corresponding Hole feature on a frame.

Hole Features to
be Constrained

attached to the Specification
Tree prior to the Update All
button being selected

Update symbol
indicating that the
new Constraint is
not up to date
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The resulting constrained Parts after the Update All button has been selected. The
Axis of the Holes is aligned but the two Parts do not necessarily contact each other.

Coincident
constraint
Symbol

Resultant up to date

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Contact Constraint
Allows you to create a Contact Constraint between two Features on different
Parts. This Constraint is generally used between Planes and Planar Faces,
Lines and Points.

Select the icon and the two features on different Parts that require constraining. Select
the Update All icon to move the Parts to their constrained position. The selected
features will be aligned to each other but they may not touch.

In the following example the bottom face of the bracket is constrained to the side face
of the frame

Features to be
Constrained

Contact
Constraint Contact
attached to the Constraint
Specification Tree Symbol

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Offset Constraint
Applies an Offset Constraint between selected feature on two different Parts.
This constraint can be applied to between Points, Lines ,Planes and Planar
Faces.

Select the icon followed by the two features to display Constraint Properties panel
will appear with the following options: -

The Name field contains the name of the Constraint, which you may change.

The Supporting Elements field lists the selected features and the Status displays
whether they are connected or not.

The Orientation allows you to control how the selected features are orientated to
each other with the following option available by clicking on the down arrow: -

1. Undefined applies a constraint
with no controlling orientation.

2. Same ensures the selected feature
are facing the same direction

3. Opposite orientates the features
to face opposite direction to each
other.

You can use the Green arrows to
switch direction.

The Offset field allows you to enter a
value for the offset distance between
the selected features

Offset
Constraint

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After clicking OK the resulting Constraint is added to the Specification Tree you then
have to Update the constraint to move the selected features to the correct position.
The features will be aligned but may not contact each other.

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Angular Constraint
Creates an Angular Constraint between two features on different Parts. This
constraint can be applied between Lines, Planes, Planar Faces and the Axis of
Cylinder and Cones.

Select the icon followed by the features to be constrained. A Constraint Properties
panel appears with the following options: -

The Name field allows you to specify a
name for the constraint.

There are four check boxes on the left of
the panel allow you to specify the
constraint type: Perpendicularly,
Parallelism, Angle (default) and Planar
angle.

The Supporting Elements lists the
features that you have selected to
constraint. Again the Status filed indicates
whether they are connected or not.

The Sector menu allows you to select
which sector of a 360° circle is used to
define the angle.

The Angle field specifies the angle value for the constraint.
After you click OK the Angle constraint is added to the Specification Tree and you
must select the Update All icon to position the features.

Feature to be
Constrained

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Resulting Angular Constraint.

Angular
Constraint

Angular
Constraint

Fix Constraint
Allows you to Fix the position of Parts.

Select the icon followed by selecting the Part to be fixed either graphically or from
the Specification Tree. The constraint is added to the Specification Tree and displayed
graphically on the selected Part. The Update command does not need to be used with
fix as no positional changes are taking place.

Fix
Constraint

It is possible to Fix the Position of both Product and Component nodes by selecting
them on the Specification Tree.

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Fix Together Constraint
This constraint allows you fix together multiple Parts so that when one of the
Parts is repositioned the others will move with it.

Select the Fix Together icon and select the Parts to be fixed together. A Fix Together
panel will appear listing the parts you have selected to fix together. If you make a
mistake re-select the incorrect part(s) to remove them from the list.

Name of the
Constraint
displayed in the
Specification Tree

List of Parts to be
Fixed Together

When you click OK the fix together constraint is applied to the selected Parts and
added to the specification Tree.

Selected Part to
be Fixed

Fix Together
Constraint

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By using the Manipulation command and selecting the With respect to constraints
check box, when you select one of the Parts that is fixed together and move it, then all
other Parts constrained to it using the Fix Together constraint will be moved as well.

Quick Constraint
Selecting this icon allows you to quickly apply constraint between features on
different Parts.

After selecting the icon select the two features on different parts to be constrained.
Catia automatically applies a constraint of a type that best suits the features selected.
The resulting Constraint is added to the Specification Tree.

Flexible/Rigid Sub-Assembly
This command allows assembly constraint within a Sub-Assembly to be
overridden temporarily thus allowing parts to be repositioned.

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Change Constraint
With this command you can change one constraint type to another.

After selecting the icon select the Constraint to be changed. A ChangeType panel
will appear listing the alternative constraints that are available for the selected
features.
Replacement
Constraint

Selected
constraint to be
changed

After selecting the alternative constraint from the list click OK and the Update All
icon to complete the change.

Result of changing
the Constraint from
an Offset to a
Coincidence

New
constraint

Reuse Pattern
This command allows you to select a Pattern from within an existing Part and
use it to position multiple instances of a Part in the Product.

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Create a Scene
Scenes can be used to develop an existing Product assembly in a separate window
without affecting the original (i.e. create an Exploded version). You can create
multiple Scenes within a Product that show various iterations of the design Assembly.

The following attributes contained either in scenes or in the assembly can be changed
without the modifications being replicated in the other: -

1. The viewpoint or state.

2. The graphical attributes of the components

3. The Hide/Show state of the components

4. Whether a Part in active or not.

If a Parts position is changed in the Assembly then it is replicated in the Scenes as
long as the assembly and the scenes are synchronised. On the other hand if the Parts
position is modified in a Scene then is not replicated in the assembly and the Scene
and Assembly are said to be of de-synchronised

Scenes are identified by name in the Specification Tree and by a graphic symbol in
the graphic window

When creating a Scene the Parts and Sub-Product that make up the Scene are
determined by the current selection in the Specification Tree: -

1. If no element is selected in the Specification Tree or if top or Root Product node is
selected, then the created Scene will include all the components of the entire
Product.

2. If a Sub-Product of the assembly is selected in the Specification Tree, then the
created Scene will include only the components of the selected Sub-Product.

3. If an existing Scene is selected in the Specification Tree, then a copy of the
selected Scene is created.

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After selecting the required node on the specification tree select the Scene
icon. An Edit Scene panel appears where you can enter a name for the Scene
in the Name field. When you click OK the Scene is added the Specification
Tree under the Applications node and you are entered into the Scene Workbench.

The Scene Workbench Toolbars

Workbench Selection

Selection
Exit Workbench
Reset the selected products
Save Viewpoint

Snap

Search
Explode
Start Publish

The Reset the selected products icon allows you to reset representation of
selected Products within the Scene back to their original status.

Select the icon followed by the Products on the Specification Tree to perform the
reset.

The Save Viewpoint icon allows you to save the current view in the Scene.

Select the icon to save the current View State.

The Snap icon allows you position Parts by snapping without affecting the Part
positions within the Product

Search allows you to perform search for data held in the Product.

The Explode icon allows you to Explode the Scene Assembly without
affecting the Product.

The Start Publish allows you to Publish the Scene.

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When you enter the Scene the background colour of the graphic display changes to
indicate that you are no longer in standard Assembly mode. When you have
completed the desired Scene use the Exit Workbench icon to return to the Assembly
Product

In the following example the Exploded GA Scene is created from a product with the
use of the Explode command.

The Assembly
Product unaffected
by the Explode
command used in
the Scene

Exploded
Scene attached Scene
to the
Specification
Tree

Scene
displayed in
the Graphics
Window

The created Scene can then be used to create an Exploded view in a CATDrawing

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Assembly Operations
Assemblies Operations can be used to create Assembly Features and Symmetrical
Parts within the Product.

Assembly
Features
Create
Symmetry

Assembly Features
This toolbar allows you to create Assembly Based Features within the Product i.e. a
hole that passes through multiple Parts.
Hole Add

Split Remove

Pocket

This command allows you to Split a group of selected Parts within a Product
using a Plane Or Surface.

Select the icon followed by the Splitting element to
display an Assembly Features Definition panel.

The Name field contains the name of the split
command, which will be displayed on the
Specification Tree.

The Parts possibly affected lists all the Parts in the
tree that can be split. Either select the double down
arrow to move the all the listed Parts into the
Affected parts field or select the required Parts
from the list using MB1 followed by the single
down arrow. If you make a mistake you can use the
double and single Up Arrows to remove Parts from
the Affected parts list. To highlight the selected
parts click on the Highlight affected parts check
box.

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After clicking OK on the Assembly Features Definition panel a Selection in
Context panel appears asking if you would like to keep the link with the selected
Object i.e. the splitting element. If you select Yes then a Contextual link is
established between the Part containing the Splitting element and the Part(s) being
Split. If No is selected then the Parts are Split with no link to the splitting element i.e.
the splitting element is Isolated in the Part being Split.

After selecting Yes or No the Assembly Features Definition panel reappears
together with a Split Definition panel. The Assembly Features Definition panel
contains the list of the Parts affected by the Split and the Split Definition panel lists
the splitting element. If required use the Orange Arrow to select the portion of the
Parts to be kept.

Click OK on the Split Definition panel to complete the operation.

Splitting
Element

Arrow indicating
the portion of the
solid to be kept

Parts to
be Split

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The selected Parts are now split and an
Assembly Split node is added to the
Specification Tree attached to an Assembly
Features node. The Assembly Split node
contains nodes that define the Split operation
on each of the affected Parts.

If you selected Yes to keep a Contextual link
between the splitting element and the Part(s)
being split then an External Reference is
created in the part Specification Tree. Therefore
if the splitting element changes then the Resulting
resulting split will update. The Part node on the Split Parts
Specification Tree indicates that there is an
External Reference contained within it by the
appearance of a Green chain link Symbol on the
node.

Green Chain
Link Symbol

External
Reference

Link to the Surface held
within the
Assembly MASTERSURF1 Part,
Features node which is attached to the
ENV Component node

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The following commands are not covered in the Foundation Course

This command allows you to create a Hole feature through series of selected
Parts in a Product using a similar method to the Assembly Split command.

This command allows you to create a Pocket feature through series of selected
Parts in a Product again using a similar method to the Assembly Split
command.

You can use the Add command to add a Partbody from the Specification Tree
of one Part in the Product into the Specification Tree of other Part(s).

This command allows you Remove a Partbody in an existing Part from
Specification Tree other Parts in the Product.

Create Symmetry
Create Symmetry Part(s) of existing Part(s) within the Product.

After selecting the icon a Symmetry panel will appear. First you have to select a
Plane that is to be used as the Mirror or Symmetry Plane followed by the Part(s) and
/or Products to be mirrored from the Specification.

Note: You can not select the top or Root node of the Product

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A preview of the symmetry will be display together with an Assembly Symmetry
Wizard and by clicking Finish on this panel Catia will proceed to create the required
symmetrical Part(s)/Product(s) and attached Symmetry nodes to the Specification
Tree.

When the command is completed an Assembly Symmetry Result panel will appear
detailing the number New Components, Instances and Products that have been
affected by the Symmetry. Select the Close button to remove the panel.

Resulting
Symmetry

The Update All icon must now be selected to synchronise the Product.

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The resulting Specification Tree as the Symmetrical Part(s)/Product(s) attached to it
together with an Assembly Features node containing an Assembly Symmetry node.

Note: When using this command be aware that the larger the assembly being
mirrored the longer the task will take.

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An Overview of Contextual Links
It is possible within Catia to link elements contained within one CATPart to elements
in another. Typical this can be done by Splitting a Solid contained in one CATPart
using a Surface containing in another or by copying a element/Feature from one Part
and Pasting it with a Link into another Part. In both cases an external Reference can
be created in the CATPart.

In the following example a CATProduct which as two CATParts attached to it. One of
the Parts (MASTERSURF1) has two surfaces contained within it that are used to
Split a PartBody in CATIAV5RIBPART.

Resulting Split
PartBody contained Surfaces contained
within within
CATIAV5RIBPART MASTERSURF1
CATPart

During the Split operation a panel will appear asking if want to keep the link with
the selected Object.

If you select Yes then the Surface is copied into the Part being Split and is created in
the Specification Tree which embeds a Link to the Part containing the Surface thus
allowing any changes in the original Surface to be Updated in the Part being Split. If
you select No then the Surface is copied into the Part being Split and it is Isolated,
therefore if the original Surface is changed then copy will not Update.

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Below is the resulting Specification Tree for the CATProduct with External
References linking MASTERSURF1 and CATIAV5RIBPART.

Extrude.1 Extrude.2
is Linked to is Linked to
Surface.3 Surface.4

As with using the Assembly Split Operation
the node of the Part being Split as a small
Link Symbol attached to it to indicate that it
has External References to another Part
within the current Product.

The two Surfaces attached to the External
Reference node within the Part being Split
also have Green Diamond Symbol to indicate
that they linked and are up to date.

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Due to the fact that the links have been create between the two Parts within the
CATProduct (CATIAV5TRAIN12) the External references are said to be created
‘In Context’ with the Product. This means that if the CATPart containing the
External Reference is opened in its own right or it is added to another CATProduct
then the links will not be found and they will temporarily be broken. This is signified
by a red ‘?’ symbol being displayed on the Surface nodes attached to the External
References within the Part and a red zigzag symbol is displayed on the Part instance
node when the CATPart is attached to another CATProduct.

It is possible to check to see if a CATPart as links present by either selecting the Part
node within the CATProduct or opening the CATPart in its own right and then select
Links from the Edit drop down menu.

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A Links to Element panel appears that list all the External References and the
Context link together with their Status i.e. OK or Not Found.

You can also use this panel to Isolate the linked element or Replace them. If a link is
broken or as been Isolated then a red zigzag symbol is displayed on the node.

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Session 6 - Analysis
This session covers the use of some of the Digital Mockup (DMU) analysis tools
available within Catia.

On completion of this session the trainee will:

♦ Be able to access the DMU Workbenches.

♦ Be able to perform Proximity Queries.

♦ Be able to perform Clash Analysis

♦ Be able take Sections through Assemblies.

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Accessing the Digital Mockup (DMU) Workbenches
The DMU Workbenches can be entered by Selecting Start > Digital Mockup and
then select the required Workbench.

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Proximity Queries
The Proximity Query analysis tool can be found in the DMU Navigator Workbench
on the DMU Data Navigation Toolbar and is called Spatial Query. This allows you
to check the clearance between selected Products and surround geometry. This
command can be used to allow you to limit the number of Products, Sub-Products
and Parts displayed when working on large complex Assemblies or just the portion of
the assembly you are interested in. Catia uses a representation of the selected Parts,
which is made of series of cubes to perform the query. The size of the cube is
controlled by the Accuracy value.

Spatial Query

Select the icon to display a Spatial Query panel. The main options to consider when
using this panel are: -

The Selection Field lists the Product(s) you
have selected to perform the query.

The Clearance field allows you to specify
the distance to check between selected
Product(s) and the surrounding Geometry.

The Accuracy field is used to specify the
accuracy of the check.

Note: The smaller the Accuracy value the
longer the query will take.

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Once you have selected the Product(s) and set the Clearance and Accuracy you must
select the Search button to perform the Query. Catia will now perform the query
during which a Computation in progress panel will appear detailing the operation
progress.

Upon completion the Parts whose distance from the selected Product(s) is less than
the Clearance value are displayed in the Results portion of the panel and are
highlighted graphically.

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You can now use the Select button together with the Group icon, which can be found
on the DMU Navigator Tools Toolbar to group the highlighted items together.

Group

A Group node is added to the Specification Tree under the Applications Node. The
Group node contains all the groups that you have created

On selecting the Group icon an Edit Group and Preview panels appear. The Edit
Group panel allows you to edit the name of the group and also lists the associated
Products and Parts. The Preview panel shows a graphic display of the Group.

Once the group has been created you can use Hide/Show to display the group only.

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Clash Analysis
The Clash Analysis tool is accessible through both the Assembly Design and DMU
Space Analysis Workbenches and is located on the Space Analysis Toolbar.

Clash

Select the icon to display a Check Clash panel.

The Name field allows you to
enter a name for the analysis.
This is displayed as a node on
the Specification Tree under
the Applications >
Interference.

The Type field allows you
specify the type check to be
performed: -

Contact + Clash. Performs a
check for both Contact and Clash

Clearance + Contact + Clash. This will allow you to enter a distance value for the
Clearance check in the right hand field.

Authorised penetration. Allows you to check for clash over a specified interference
distance which is entered in the right hand field

Clash rule. Allows you to specify a rule using Knowledgeware.

The field under the Type field allows you to select whether you want to run the
analysis against all components, only inside the selected Product, all components
against the selected Product and between two selections.

By default if you do not select a Product then Catia will perform the clash against the
currently active Product.

When you click Apply the analysis is performed and the Clash Check panel will
expand to display the results. A Computing panel may be seen briefly during the
check.

Note: The larger the assembly that is checked then the longer the process will
take.
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In the following example the active product is selected by default to which a Contact
and Clash analysis is performed against all components.

After clicking Apply the check is performed and the Check Clash panel expands to
display the results.

The number of
Interference’s found

Results

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If you select one of the results from the table (in this case row 5) a Preview window
appears displaying the components involved in the check. The value of the clash, if
any, is displayed in the Value field and the Status value changes.

Any clash is
hightlighted in
a window
which you can
Zoom and Pan
using the
mouse.

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If you now click OK the Clash is attached to the Speciication Tree under the name
specified in the Name field. To view the results again double click on the Results

Clash node

Results
Node
node.

You can also save the results as XML file, a plain Text file or a Catia Version 4
.model by selecting the Export button. There is also the option to toggle the Preview
results to the main graphics window by select the Results Window button.

Results Window Export file
button button

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Sectioning
This command allows you to take 3D section cuts through selected Products. As with
Clash, this icon can be found on the Space Analysis Toolbar in both Assembly
Design and DMU Space Analysis Workbenches.

Sectioning

Select the icon to display a Sectioning Definition panel a Preview window.

The following options are available on this panel: -

The Name field allows you to specify a name for the
resulting Section which is displayed on the Specification
Tree under the Application > Sections nodes.

The Selection field allows you to select which Product is
used in the section. Default is the currently active
Product.

There are seven buttons below the selection field that allow the following options: -

Results Window Clash
Toggle Detection

Section Automatic
Plane Type Update Toggle

Volume Export File
Cut Section Fill

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The Section Plane Type has three options available by selecting the small arrow on
the button: -

2D Section - Takes a section using a single Plane.

Section Slice – Creates two sections superimpossed on each other using two
parallel Planes.

Section Box – creates superimpossed sections using planes defining using a
rectangular box.

The Volume Cut toggle allows you to limit the display of the Solid geometry on the
screen to the positive side of the section plane.

The Results Window toggle switches the Preview window into a full window.
The Section Fill toggle allows you to specify a fill for the section.

The Clash Detection toggle switches on the Clash Detection in a second window.

The Export File button allows you to save the result in one of the following formats:

♦ CATPart
♦ CATDrawing
♦ dxf
♦ dwg
♦ igs
♦ model
♦ stp
♦ wrl

The Automatic Update button has two options available by selecting the small arrow
on the button: -

Allows automatically updates the section.

Freezes the section.

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The Position and Dimensioning portion of the panel allows you to specify the position
and orientation of the section plane.

The X, Y and Z check box orientation the plane with the x, y, z plane of the Product.

Edit Plane Reset the
Position and Section
Dimensions Plane
Align the Invert the
Section with Section
geometry direction

If you select the Edit Plane button then the following panel appears that allows you to
position and orientate the Section plane.

Plane origin
relative to the
Product origin Section
Plane size

Translation
Increment Rotation
Value Increment
value

Translation Translation
Increment Increment
buttons buttons

Undo/Redo
option
The Translation and Rotation Increment values allow you move the section a set
distance or angle by using the increment buttons.

You can also position and orientate the Section plane by dragging the plane compass
with MB1.

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The Align Plane with geometry button when selected allows you to position the
Section plane on a selected element. Once you select the element the section plane is
positioned normal to the element at the position you indicate.

The Invert button reverse the positive direction of the plane.

The Reset button resets the Section plane to original start position.

Once you have selected your desired settings for the Section Cut click OK to create
the Section node on the Specification Tree. The created Section can be editted by
double clicking on the node.

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The following are examples of different Section Cuts Available.

Single
Section
Plane

Section
Plane
Compass

Single Section Plane
through a Spoiler Bracket
and Spar

Preview window displaying the
resulting section. In this case
clearly showing a Clash

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Two
First Plane Section
Planes
Plane Manipulator visible
when you place the mouse
pointer over the plane. Use
Second MB1 to drag the plane to a
Plane new position

Plane Compass
controls both
section Planes

A Section Cut which
superimposes to
sections in the same
Preview window

Second Section Plane
Cut

First Section Plane
Cut
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Section
Box

Wireframe
intersection
geometry

A composite
Section using
the Section Box
option

Section
Compass

Composite
Section

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Measuring Distances
To measure geometry within Catia you can use the following icons on the Measure
Toolbar, which is available in the majority of the Workbenches on the bottom toolbar.

Measure
Between
Measure
Item

By selecting the Measure Between icon a Measure Between panel is displayed.
There are four measuring options available, which can be selected by using the four
buttons at the top of the panel.

The first option is to Measure Between
two selected elements.

The Selection 1 and 2 mode allows you
to specify what type selection method is
to be used.

The Other Axis checkbox allows you
to specify an axis from which to base
the measure on. By default Catia will use the Product or Part Axis.

The Calculation mode allows you select whether the measurement is Exact or
Approximate. If you measure in a Product that is in Visualisation mode then the
result will be approximate until you switch to Design mode.

The results are displayed in the Result portion of the panel.

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If you select Keep Measure then the distance between the selected elements is
displayed on the screen permanently and a MeasureBetween node is added to the
Specification Tree.

You can customise the measure result by selecting the Customize button.

You have the option to display the
Distance and Angle between the selected
elements both in the measure panel and
graphically.

Components displays in the Measure
panel only the delta X, Y and Z cordinate
values between the measure points on the
selected elements.

Point 1 and 2 displays the X, Y and Z
values in the Measure panel from the
Product or Part Axis to the measure point
on the selected element.

Once you have customised your display either click Apply to temporarily apply the
display or OK to set the customised displayed.

Clicking OK on the main Measure Between panel completes the command.

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The following is an example of use measure between using Any Geometry and Any
Geometry, Infinite between the same features.

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In the following example the Distance and Angle to measured and displayed between
the two Spoiler Brackets.

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The second measure option is to measure in Chain mode.

After selecting this button you have to select the first element to measure followed by
the second. The desired distance/angle is then displayed. If you now select a third
element then a distance/angle is displayed between the second and third elements. All
other options are the same as Measure Between.

Measuring
in Chain
mode

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The third option is to create measurements in a Fan or Stacked form.

After selecting this button you have to select the first element to measure followed by
the second. The desired distance/angle is then displayed. If you now select a third
element then a distance/angle is displayed between the first and third elements. Again
all other options are the same as Measure Between.

Fan or
Stack mode
Measuring

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The final measure option is Measure Item which also accessible from the Measure
Toolbar. When you select this button a Measure Item panel appears. The option
allows you to measure individual elements i.e. Feature Edges, Faces, etc. after
selecting your desired options and the element to be measured the results are
displayed both graphically and in the Results portion of the panel.

Click OK to complete the command. If the Keep Measure checkbox is selected then
the measure result is permanently displayed and added to the Specification Tree.

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(2) catia v5 assembly design

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