Foundation Course Assembly Design

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Foundation Course Assembly Design

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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.

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  1. AIRBUS UK CATIA V5 Foundation Course Foundation Course Assembly Design Compiled by: Kevin Burke Approved by: Authorised by: Kevin Burke Date: 16/Apr/2003 Date: Date: AIRBUS UK Ltd. All rights reserved. DMS42177 Page 1 of 71 Issue 1 ANS-UG0300108
  2. AIRBUS UK CATIA V5 Foundation Course 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 Page 2 of 71 Issue 1 ANS-UG0300108
  3. AIRBUS UK CATIA V5 Foundation Course Measuring Distances ............................................................................................... 65 DMS42177 Page 3 of 71 Issue 1 ANS-UG0300108
  4. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 4 of 71 Issue 1 ANS-UG0300108
  5. AIRBUS UK CATIA V5 Foundation Course 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 DMS42177 Page 5 of 71 Issue 1 ANS-UG0300108
  6. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 6 of 71 Issue 1 ANS-UG0300108
  7. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 7 of 71 Issue 1 ANS-UG0300108
  8. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 8 of 71 Issue 1 ANS-UG0300108
  9. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 9 of 71 Issue 1 ANS-UG0300108
  10. AIRBUS UK CATIA V5 Foundation Course Another way to load a Product into Design mode is to select the Update All icon on the button menu bar. When you first open an existing Product this icon will be yellow if you are in Visualisation mode and by selecting it all the Parts on the Specification will be loaded into Design mode and any links will be updated. The Update All Icon Update No Update Required Required To switch back to Visualisation mode by using MB3 > Representations >Visualisation Mode. Note: When you add a New Part to the Specification Tree it will be automatically loaded in Design mode. DMS42177 Page 10 of 71 Issue 1 ANS-UG0300108
  11. AIRBUS UK CATIA V5 Foundation Course Assembly Design Toolbars and Icons There are five main toolbars within the Assembly Design Assembly Workbench Icon workbench: - Features 1. Product Structure Tools – Selection used to create the Specification Tree. Annotations Product Selection 2. Move Operations – used for the positioning assembly Products and Parts. 3. Assembly Features– used to create assembly based features within the Product. Product 4. Annotations – attaches Structure text annotation to assembly Tools features. Constraints 5. Constraints – creates assembly constraints between Products and Parts. Move Operations The Assembly Create Scene Design Toolbars are also accessible via the Insert Drop down menu DMS42177 Page 11 of 71 Issue 1 ANS-UG0300108
  12. AIRBUS UK CATIA V5 Foundation Course 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 DMS42177 Page 12 of 71 Issue 1 ANS-UG0300108
  13. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 13 of 71 Issue 1 ANS-UG0300108
  14. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 14 of 71 Issue 1 ANS-UG0300108
  15. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 15 of 71 Issue 1 ANS-UG0300108
  16. AIRBUS UK CATIA V5 Foundation Course Below is an example of an existing CATProduct containing a Component node and seven Part nodes together with their associated Assembly Constraints. Replacing a Component By selecting this icon you can Replace a node on the Specification Tree with another existing Product or Part node. After selecting the icon you must select a Node on the Tree to be replaced. The Insert an Existing Component panel will now appear. If required perform a search for the replacement CATProduct or CATPart and select it using MB1 followed by clicking theOpen button to continue. Select Node to be Replaced Replacement CATProduct DMS42177 Page 16 of 71 Issue 1 ANS-UG0300108
  17. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 17 of 71 Issue 1 ANS-UG0300108
  18. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 18 of 71 Issue 1 ANS-UG0300108
  19. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 19 of 71 Issue 1 ANS-UG0300108
  20. AIRBUS UK CATIA V5 Foundation Course 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. DMS42177 Page 20 of 71 Issue 1 ANS-UG0300108
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