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- 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.
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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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