Catia v5 Assembly Design

AIRBUS UK

CATIA V5 Foundation Course

Foundation Course Assembly Design Compiled by: Kevin Burke

Approved by:

Authorised by:

Date:

Date:

Kevin Burke Date: 16/Apr/2003

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 DMS42177 ANS-UG0300108

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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 Required

No Update 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

Assembly Features

There are five main toolbars within the Assembly Design workbench: -

Workbench Icon

1. Product Structure Tools – used to create the Specification Tree.

Selection 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.

Constraints

Product Structure Tools

4. Annotations – attaches text annotation to assembly features. 5. Constraints – creates assembly constraints between Products and Parts.

Move Operations

Create Scene

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The Assembly 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

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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.

Define MultiInstantiation

Fast MultiInstantiation

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. DMS42177 ANS-UG0300108

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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

Instance Numbers Resulting Instantiations in the Specification Tree DMS42177 ANS-UG0300108

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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 ZAxis

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.

Smart Move

Snap

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 DMS42177 ANS-UG0300108

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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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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.

Axis of the Hole displayed 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

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 DMS42177 ANS-UG0300108

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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 Coincidence Constraint

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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 attached to the Specification Tree

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Contact Constraint 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. DMS42177 ANS-UG0300108

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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. DMS42177 ANS-UG0300108

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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

Scene attached 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

Remove

Split 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. DMS42177 ANS-UG0300108

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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 DMS42177 ANS-UG0300108

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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 split will update. The Part node on the Specification Tree indicates that there is an External Reference contained within it by the appearance of a Green chain link Symbol on the node.

Resulting Split Parts

Green Chain Link Symbol

External Reference

Assembly Features node

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Link to the Surface held within the MASTERSURF1 Part, 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. DMS42177 ANS-UG0300108

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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 within CATIAV5RIBPART

Surfaces contained within 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. DMS42177 ANS-UG0300108

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

Extrude.1 is Linked to Surface.3

Extrude.2 is Linked to 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. DMS42177 ANS-UG0300108

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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 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 Toggle

Clash Detection Automatic Update Toggle

Section Plane Type Volume Cut

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Export File 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.

Reset the Section Plane

Edit Plane Position and Dimensions Align the Section with geometry

Invert the Section 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 Value

Rotation Increment value Translation Increment buttons

Translation Increment 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 Section Planes

First Plane

Plane Manipulator visible when you place the mouse pointer over the plane. Use MB1 to drag the plane to a new position

Second Plane

Plane Compass controls both section Planes

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

Second 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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