catia v5 training airbus Foundation Course assembly design

To maintain the position of the sub-assemblies and partswithin the CATProduct, Assembly Constraints are used which are attached to the Specification Tree under a Constraints Node.. Produ

Compiled by: Kevin Burke

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

Measuring Distances 65

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

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 holdsdetails of all sub-assembles and their associated parts together with their relativepositions to each other To maintain the position of the sub-assemblies and partswithin 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 levelAssembly Node Sub-Assemblies

Sub-AssemblyParts

Graphicalrepresentation ofthe Assembly

AssemblyConstraints

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 theappearance of the Part Name panel

Product NodeComponent Node

Part Nodes

An overview of the different Specification Tree Nodes

There are a variety of different node types displayed in the CATProduct SpecificationTree as well as the ones contain within a CATPart Specification Tree, below are thethree 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 othernodes 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 attachother 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.

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

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 externalappearance of the component is visualised

The main advantage of using this mode is that performance of the workstation isimproved 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 theParts 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 theWorkstation

Below is the Specification Tree for a Product when it is in Visualisation mode.

Note that that Assembly Constraints have yellow exclamation symbols attached tothem 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

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 betweenFeatures 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 willnow be loaded into Design Mode This also hasthe effect of loading the CATPart documentsinto the Workstations memory and on a largeAssembly there may be a time delay whilst thistask is performed

Once in Design mode the CATPartSpecification Trees are accessible by selecting

the ‘+’ symbol next to the Part node The

yellow exclamation symbol on the Constraintsshould now have disappeared indicating thatthey 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

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

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.

UpdateRequired

No UpdateRequired

Create Scene

SelectionWorkbench Icon

Product Selection

Constraints

AssemblyFeatures

ProductStructureToolsAnnotations

Move Operations

Assembly Design Toolbars and Icons

There are five main toolbarswithin the Assembly Designworkbench: -

1 Product Structure Tools –

used to create the SpecificationTree

2 Move Operations – used

for the positioning assemblyProducts and Parts

3 Assembly Features– used

to create assembly basedfeatures within the Product

via the Insert

Drop down menu

Product Structure Tools Toolbar

The main purpose of this toolbar is to allow you to create a Specification Tree andmanipulate its order

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

Insert New Component

Multi Instantiation Tools

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

Add New Product (CATProduct)

Selecting this icon will allow you to add a new CATProduct to theSpecification 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

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.

Currently Active NodeNew Component Node

Currently Active Node

New CATProduct Node

Product/Part name Product/Part Instance name

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 CATProductthe origin on the CATPart is the same as the current active 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.

New CATPart Node

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 andCATParts

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

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 beReplaced

ReplacementCATProduct

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

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 thepanel to move the node up or down the tree: -

Increments the node up one position inthe tree

Increments the node down one position

in the tree

Moves the selected node next to asecond 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 selectedCATProduct 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 userfunction and is not covered in the Foundation course

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

Foundation course

Creating Multiple Instances of a Node

It is possible to create multiple instances of a Component, Product and Part nodeswithin 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 orAssembly Constraints

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

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

Unique InstanceNumbers

Instancesdisplayed afterrepositioning

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.

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

SelectedNode

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

Defining a Multi-Instantiation

Allows you create multiple instances of a part in a specified direction

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

Select the icon to display the Multi Instantiation panel The following options areavailable: -

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.

Fast Instantiation

Define Instantiation

Multi-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 beInstantiated

Preview of theInstantiation

ResultingInstantiations

ResultingInstantiations in theSpecification Tree

ResultingInstantiations in theSpecification Tree

Instance Numbers

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

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

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.

Move Operations Toolbar

Allows you to manipulate the position and orientation of Parts

Manipulation

Allows Freehand Manipulation to position and orientate a selected Part

Select the icon to display a Manipulation Parameters panel.

There are twelve options available, four allowing you to drag along an Axis, fourallowing 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 usingMB1 and then drag it in the required direction

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

Snap

Stop Manipulation

Explode AssemblyManipulation

Drag along the XY,

YZ or XZ Planes

Drag alongany Axis

button

Drag alongany Plane

Rotatearound anyAxis

Snap Operations

Positions parts using a snapping

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 aPlane, a Face, an Axis System, etc Now select an element within a second Part toindicate the new position

The following is an example of an existing Part that has been added to a CATProductand then positioned using its Axis System relevant to an Axis System in another Part

in this case a part containing Positioning Datum’s

Part to bemoved

Part containingPosition Datum’s(Axis Systems)

Axis System ofthe Part to bemoved

PositioningAxis System

Resultingmove

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 Thiscan be overcome by dropping the Compass onto the origin of the Axis System in thePart that is being moved Then rotation the reversed Axis through at least 180° andthen 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.

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.

X

√

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 toremove this panel and you are now in temporary Explode mode

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

Stopping Manipulation on Clash

Selecting this icon will cause the manipulation of parts when using theManipulation icon to be halted if the Part that is being moved Clashes with anadjacent Part

Note: The With respect to constraints check box on the Manipulation Panel must

be selected for this to function work.

SelectedCATProduct to

be Exploded

ResultingExplodedCATProduct

Assembly Constraints

Assembly constraints are used to position CATParts relative to each other with aCATProduct All assembly constraints are added to the Specification Tree and

attached to a Constraints Node.

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

Offset ConstraintAngle Constraint

FixFix Together

Reuse Pattern

Contact Constraint

Quick ConstraintFlexible/Rigid Assembly

Change Constraint

ConstraintsNode

AssemblyConstraints

Coincidence Constraint

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

highlighted on the screen and if you select it then the coincidence

is applied to the axis

In the following example the Hole feature on the bracket is made

coincident with the corresponding Hole feature on a frame

Axis of theHole displayedwhen you hoverover the feature

Hole Features to

be Constrained

Coincidence Constraint

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

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

CoincidentconstraintSymbol

Resultant up to dateCoincidence Constraint

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 Selectthe Update All icon to move the Parts to their constrained position The selectedfeatures 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 beConstrained

ContactConstraintSymbol

ContactConstraintattached to theSpecification Tree

Offset Constraint

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

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 eachother

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

OffsetConstraint

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

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 ofCylinder and Cones

Select the icon followed by the features to be constrained A Constraint Propertiespanel 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 beConstrained

Resulting 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 fromthe Specification Tree The constraint is added to the Specification Tree and displayedgraphically on the selected Part The Update command does not need to be used withfix as no positional changes are taking place

It is possible to Fix the Position of both Product and Component nodes by selecting

them on the Specification Tree

AngularConstraint

AngularConstraint

FixConstraint