AIRBUS UK                  CATIA V5 Foundation Course       Foundation Course       Assembly DesignCompiled by: Kevin Burk...
AIRBUS UK                              CATIA V5 Foundation CourseContentsSession 5 – The Assembly Design Workbench ..........
AIRBUS UK                           CATIA V5 Foundation Course Measuring Distances ..........................................
AIRBUS UK                   CATIA V5 Foundation Course        Session 5 – The Assembly Design                   WorkbenchO...
AIRBUS UK                   CATIA V5 Foundation Course      An Introduction to the Assembly Design WorkbenchThe Assembly D...
AIRBUS UK                  CATIA V5 Foundation Course            Accessing the Assembly Design WorkbenchThe Assembly Desig...
AIRBUS UK                  CATIA V5 Foundation Course     An overview of the different Specification Tree NodesThere are a...
AIRBUS UK                 CATIA V5 Foundation Course      Different Display Modes when using CATProductsThere are two type...
AIRBUS UK                  CATIA V5 Foundation Course2. The other mode is called Design Mode which allows gain access to t...
AIRBUS UK                   CATIA V5 Foundation CourseAnother way to load a Product into Design mode is to select the Upda...
AIRBUS UK           CATIA V5 Foundation Course                 Assembly Design Toolbars and Icons                         ...
AIRBUS UK                   CATIA V5 Foundation Course                    Product Structure Tools ToolbarThe main purpose ...
AIRBUS UK                  CATIA V5 Foundation CourseAdd New Component      This allows you to add a new Component Node to...
AIRBUS UK                  CATIA V5 Foundation CourseAdd a New Part (CATPart)       This icon allows you to add a new CATP...
AIRBUS UK                    CATIA V5 Foundation CourseAdding A Existing Component    This command is not as the name impl...
AIRBUS UK                  CATIA V5 Foundation CourseBelow is an example of an existing CATProduct containing a Component ...
AIRBUS UK                   CATIA V5 Foundation CourseA Replace Mode panel will appear asking you if you wish to replace a...
AIRBUS UK                   CATIA V5 Foundation CourseGraphic Tree Reordering       Allows you to Reorder the nodes on the...
AIRBUS UK                   CATIA V5 Foundation CourseCreating Multiple Instances of a NodeIt is possible to create multip...
AIRBUS UK                    CATIA V5 Foundation CourseRenaming a Node NameThere may be occasions when you will need to re...
AIRBUS UK                    CATIA V5 Foundation CourseThe Product tab allows you to edit theNode Part Number and Instance...
AIRBUS UK                   CATIA V5 Foundation CourseDefining a Multi-InstantiationAllows you create multiple instances o...
AIRBUS UK                   CATIA V5 Foundation CourseAfter selecting the part to be Instantiated, the Reference Direction...
AIRBUS UK                    CATIA V5 Foundation Course       This allows Fast Multi-Instantiations to be created using th...
AIRBUS UK                   CATIA V5 Foundation Course                Saving a Newly Creating CATProductThe first time you...
AIRBUS UK                   CATIA V5 Foundation Course                         Move Operations ToolbarAllows you to manipu...
AIRBUS UK                    CATIA V5 Foundation CourseSnap OperationsPositions parts using a snapping.                   ...
AIRBUS UK                  CATIA V5 Foundation CourseWhen you snap two Axis Systems together the orientation of the X, Y a...
AIRBUS UK                   CATIA V5 Foundation CourseExplode Assembly       Allows you to Explode selected CATProducts.Se...
AIRBUS UK                  CATIA V5 Foundation CourseYou can use the Scroll bar in the Scroll explode portion of the panel...
AIRBUS UK                  CATIA V5 Foundation Course                           Assembly ConstraintsAssembly constraints a...
AIRBUS UK                   CATIA V5 Foundation CourseCoincidence Constraint        Applies a Coincidence Constraint betwe...
AIRBUS UK                   CATIA V5 Foundation CourseThe resulting constrained Parts after the Update All button has been...
AIRBUS UK                   CATIA V5 Foundation CourseContact Constraint       Allows you to create a Contact Constraint b...
AIRBUS UK                  CATIA V5 Foundation CourseOffset Constraint      Applies an Offset Constraint between selected ...
AIRBUS UK                  CATIA V5 Foundation CourseAfter clicking OK the resulting Constraint is added to the Specificat...
AIRBUS UK                   CATIA V5 Foundation CourseAngular Constraint       Creates an Angular Constraint between two f...
AIRBUS UK                  CATIA V5 Foundation CourseResulting Angular Constraint.                                        ...
AIRBUS UK                    CATIA V5 Foundation CourseFix Together Constraint      This constraint allows you fix togethe...
AIRBUS UK                    CATIA V5 Foundation CourseBy using the Manipulation command and selecting the With respect to...
AIRBUS UK                   CATIA V5 Foundation CourseChange Constraint      With this command you can change one constrai...
AIRBUS UK                    CATIA V5 Foundation Course                                 Create a SceneScenes can be used t...
AIRBUS UK                   CATIA V5 Foundation Course      After selecting the required node on the specification tree se...
AIRBUS UK                   CATIA V5 Foundation CourseWhen you enter the Scene the background colour of the graphic displa...
AIRBUS UK                   CATIA V5 Foundation Course                             Assembly OperationsAssemblies Operation...
AIRBUS UK                    CATIA V5 Foundation CourseAfter clicking OK on the Assembly Features Definition panel a Selec...
AIRBUS UK                   CATIA V5 Foundation CourseThe selected Parts are now split and anAssembly Split node is added ...
AIRBUS UK                  CATIA V5 Foundation CourseThe following commands are not covered in the Foundation Course      ...
AIRBUS UK                  CATIA V5 Foundation CourseA preview of the symmetry will be display together with an Assembly S...
AIRBUS UK                  CATIA V5 Foundation CourseThe resulting Specification Tree as the Symmetrical Part(s)/Product(s...
AIRBUS UK                   CATIA V5 Foundation Course                   An Overview of Contextual LinksIt is possible wit...
AIRBUS UK                   CATIA V5 Foundation CourseBelow is the resulting Specification Tree for the CATProduct with Ex...
AIRBUS UK                    CATIA V5 Foundation CourseDue to the fact that the links have been create between the two Par...
AIRBUS UK                   CATIA V5 Foundation CourseA Links to Element panel appears that list all the External Referenc...
AIRBUS UK                   CATIA V5 Foundation Course                      Session 6 - AnalysisThis session covers the us...
AIRBUS UK               CATIA V5 Foundation Course     Accessing the Digital Mockup (DMU) WorkbenchesThe DMU Workbenches c...
AIRBUS UK                  CATIA V5 Foundation Course                              Proximity QueriesThe Proximity Query an...
AIRBUS UK                  CATIA V5 Foundation CourseOnce you have selected the Product(s) and set the Clearance and Accur...
AIRBUS UK                  CATIA V5 Foundation CourseYou can now use the Select button together with the Group icon, which...
AIRBUS UK                   CATIA V5 Foundation Course                                  Clash AnalysisThe Clash Analysis t...
AIRBUS UK                  CATIA V5 Foundation CourseIn the following example the active product is selected by default to...
AIRBUS UK                  CATIA V5 Foundation CourseIf you select one of the results from the table (in this case row 5) ...
AIRBUS UK                  CATIA V5 Foundation CourseIf you now click OK the Clash is attached to the Speciication Tree un...
AIRBUS UK                   CATIA V5 Foundation Course                                      SectioningThis command allows ...
AIRBUS UK                  CATIA V5 Foundation CourseThe Section Plane Type has three options available by selecting the s...
AIRBUS UK                   CATIA V5 Foundation CourseThe Position and Dimensioning portion of the panel allows you to spe...
AIRBUS UK                   CATIA V5 Foundation CourseThe Align Plane with geometry button when selected allows you to pos...
AIRBUS UK                  CATIA V5 Foundation CourseThe following are examples of different Section Cuts Available.      ...
AIRBUS UK                 CATIA V5 Foundation Course                                               Two               First...
AIRBUS UK                 CATIA V5 Foundation Course                                                       Section        ...
AIRBUS UK                   CATIA V5 Foundation Course                             Measuring DistancesTo measure geometry ...
AIRBUS UK                  CATIA V5 Foundation CourseIf you select Keep Measure then the distance between the selected ele...
AIRBUS UK                CATIA V5 Foundation CourseThe following is an example of use measure between using Any Geometry a...
AIRBUS UK                 CATIA V5 Foundation CourseIn the following example the Distance and Angle to measured and displa...
AIRBUS UK                   CATIA V5 Foundation CourseThe second measure option is to measure in Chain mode.After selectin...
AIRBUS UK                   CATIA V5 Foundation CourseThe third option is to create measurements in a Fan or Stacked form....
AIRBUS UK                 CATIA V5 Foundation CourseThe final measure option is Measure Item which also accessible from th...
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Transcript of "(2) catia v5 assembly design"

  1. 1. AIRBUS UK CATIA V5 Foundation Course Foundation Course Assembly DesignCompiled by: Kevin Burke Approved by: Authorised by:Kevin BurkeDate: 16/Apr/2003 Date: Date: AIRBUS UK Ltd. All rights reserved.DMS42177 Page 1 of 71 Issue 1ANS-UG0300108
  2. 2. AIRBUS UK CATIA V5 Foundation CourseContentsSession 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 .......................................................................... 47Session 6 - Analysis ..................................................................50 Accessing the Digital Mockup (DMU) Workbenches ............................................ 51 Proximity Queries ................................................................................................... 52 Clash Analysis......................................................................................................... 55 Sectioning................................................................................................................ 58DMS42177 Page 2 of 71 Issue 1ANS-UG0300108
  3. 3. AIRBUS UK CATIA V5 Foundation Course Measuring Distances ............................................................................................... 65DMS42177 Page 3 of 71 Issue 1ANS-UG0300108
  4. 4. AIRBUS UK CATIA V5 Foundation Course Session 5 – The Assembly Design WorkbenchOn 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 1ANS-UG0300108
  5. 5. AIRBUS UK CATIA V5 Foundation Course An Introduction to the Assembly Design WorkbenchThe Assembly Design Workbench is used to bring together Parts (CATParts) into anassembly, which is known as a CATProduct document and as such contains nogeometry but links to CATParts. CATProducts can also be made up of a mixture ofsmaller CATProducts and CATParts to form larger complex assemblies.CATProducts can be used in Kinematic simulation, Stress Analysis, FittingSimulation, 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 theSpecification Tree under a Constraints Node. Kinematic Mechanisms, FittingSimulations, 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 ConstraintsDMS42177 Page 5 of 71 Issue 1ANS-UG0300108
  6. 6. AIRBUS UK CATIA V5 Foundation Course Accessing the Assembly Design WorkbenchThe 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.DMS42177 Page 6 of 71 Issue 1ANS-UG0300108
  7. 7. AIRBUS UK CATIA V5 Foundation Course An overview of the different Specification Tree NodesThere 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 aPart 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 aComponent node with a single Part node attached to it. Product Node Component Node Part NodesAgain 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 downmenu.DMS42177 Page 7 of 71 Issue 1ANS-UG0300108
  8. 8. AIRBUS UK CATIA V5 Foundation Course Different Display Modes when using CATProductsThere 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 1ANS-UG0300108
  9. 9. AIRBUS UK CATIA V5 Foundation Course2. 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 1ANS-UG0300108
  10. 10. AIRBUS UK CATIA V5 Foundation CourseAnother way to load a Product into Design mode is to select the Update All icon onthe button menu bar. When you first open an existing Product this icon will be yellowif you are in Visualisation mode and by selecting it all the Parts on the Specificationwill be loaded into Design mode and any links will be updated.The Update All Icon Update No Update Required RequiredTo 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 automaticallyloaded in Design mode.DMS42177 Page 10 of 71 Issue 1ANS-UG0300108
  11. 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. 12. AIRBUS UK CATIA V5 Foundation Course Product Structure Tools ToolbarThe main purpose of this toolbar is to allow you to create a Specification Tree andmanipulate 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 ToolsYou can also access the majority of these commands by the use of MB3 when youpass over the currently selected node on the Specification Tree to display a contextualmenu and select Components to display a sub menuDMS42177 Page 12 of 71 Issue 1ANS-UG0300108
  13. 13. AIRBUS UK CATIA V5 Foundation CourseAdd 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 inwhich you must enter a name for the Node in the New PartNumber field and then click OK.A new Component Node with the name you specified is added to the SpecificationTree attached to the currently active node that is highlighted in blue Currently Active Node New Component NodeAdd 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 theCATProduct. The name must conform to the relevant Airbus naming conventions andprocedures. After entering a valid name click OK to add the new CATProduct to theSpecification Tree. Again the new node is attached to the currently active node. Currently Active Node New CATProduct Node Product/Part name Product/Part Instance nameNote: the Origin of the new CATProduct is same as the currently node. Anempty Product has no origin until a Part has been inserted. The Absolute Axissystem (origin) of the Product is defined by the first Part or Product inserted.DMS42177 Page 13 of 71 Issue 1ANS-UG0300108
  14. 14. AIRBUS UK CATIA V5 Foundation CourseAdd 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 avalid part name. After you click OK the new CATPart will be attached to thecurrently active node on the Specification Tree. As with adding a new CATProductthe origin on the CATPart is the same as the current active node. New CATPart NodeIf you now add a second new CATPart to the Specification Tree, after entering a validpart name in the Part Number panel and clicking OK. A New Part: Origin Pointpanel will appear asking you to define the origin for the new part. If you select theYes button you will have to select either Point element from within an existingCATPart on the Specification tree or an existing Node to specify the origin. If youselect 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 theposition and orientation of a new CATPart.DMS42177 Page 14 of 71 Issue 1ANS-UG0300108
  15. 15. AIRBUS UK CATIA V5 Foundation CourseAdding 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. Enterthe directory where you wish search for the required CATProducts or CATParts in theLook 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 themain window of the panel together the file Type. You can limit your search to aspecific file type by selecting one of the options available in the Files of type field viathe down arrow. You can also enter partial file names together with * as a wildcard inthe 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 addan 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 theSpecification Tree and position them on the origin of the currently active node.DMS42177 Page 15 of 71 Issue 1ANS-UG0300108
  16. 16. AIRBUS UK CATIA V5 Foundation CourseBelow is an example of an existing CATProduct containing a Component node andseven 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 Insertan Existing Component panel will now appear. If required perform a search for thereplacement CATProduct or CATPart and select it using MB1 followed by clickingtheOpen button to continue. Select Node to be Replaced Replacement CATProductDMS42177 Page 16 of 71 Issue 1ANS-UG0300108
  17. 17. AIRBUS UK CATIA V5 Foundation CourseA Replace Mode panel will appear asking you if you wish to replace all instances ofthe selected node with the new one. If you select Yes then all occurrences of theselected node in the Specification Tree will be replaced. If you select No then only theselected node will be replaced.The selected node will now be replaced at the same location.DMS42177 Page 17 of 71 Issue 1ANS-UG0300108
  18. 18. AIRBUS UK CATIA V5 Foundation CourseGraphic 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 attachedto it. A Graph tree reordering panel will now be displayed. Select the node namefrom 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 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 tocomplete 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 Partsattached. A Generate Numbering panel will appear with theoption to either generate Integer or Letters. You can also selectwhether Keep existing numbers or Replace them.On clicking OK the number command is performed. Nothingwill have visibly changed but the numbers are added to theProperties of the relevant node. This information can beextracted and used to compile a Bill Of Materials for theCATProduct 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 theFoundation course.DMS42177 Page 18 of 71 Issue 1ANS-UG0300108
  19. 19. AIRBUS UK CATIA V5 Foundation CourseCreating Multiple Instances of a NodeIt 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 thenode to be instantiated then either use MB3 to access the contextual menu and selectCopy or use the Edit drop down menu and select Copy. The node is then copiedtogether with its position and orientation within the Tree.Now select the node on the Tree where you want the new instance to be attached andagain 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 theoriginal node. If you keep using Paste then more Instances will be added to the Treein 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. Unique Instance Numbers Instances displayed after repositioningA unique instance number is added to the node name on the Specification Tree toidentify the new instances.DMS42177 Page 19 of 71 Issue 1ANS-UG0300108
  20. 20. AIRBUS UK CATIA V5 Foundation CourseRenaming a Node NameThere may be occasions when you will need to rename a Node name on theSpecification Tree. This can be done by selecting the node to be renamed using MB1followed by MB3 to access the contextual menu and then select Properties. Selected NodeA Properties panel will appear which has four tabs enabling you to control thefollowing: -1. The name of the Node.2. The Graphic Properties.3. The Mechanical Properties.4. The Drafting Properties.DMS42177 Page 20 of 71 Issue 1ANS-UG0300108
  21. 21. AIRBUS UK CATIA V5 Foundation CourseThe Product tab allows you to edit theNode Part Number and Instance Nametogether with various Attributes.The important fields on this tab are: -The Component instance name is thename displayed in brackets on thenode. If you edit this name you shouldensure that it matches the name in thePart Number field with the exceptionof the instance number.The Link to Reference lists the file towhich the node is linked and is noteditable.The Part Number field allows you tochange the first portion of the nodename.After editing the required fields clickOK 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 displayedgeometry.The Mechanical tab allows you to enter Mass Properties.The Drafting tab allows you to control how the geometry is displayed in theCATDrawing.DMS42177 Page 21 of 71 Issue 1ANS-UG0300108
  22. 22. AIRBUS UK CATIA V5 Foundation CourseDefining a Multi-InstantiationAllows you create multiple instances of a part in a specified direction. Fast Multi- Define Multi- Instantiation Instantiation Creates a Multi Instantiation of a part in a user-defined direction.Select the icon to display the Multi Instantiation panel. The following options areavailable: -The Component to Instantiate field displays the part you have selected toInstantiate.By selecting the down arrow adjacent to theParameters field you will have three optionsavailable 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 ofthe Instantiations. You can either use the Axis options to allow you to specify thedirection based on the X, Y or Z axis of the Compass or use a Selected Element i.e. aLine, Planar face, etc. You can also Reverse the direction. The Result = fields displaythe Vector values for the direction.The Define As Default check box allows you set the current values as default.DMS42177 Page 22 of 71 Issue 1ANS-UG0300108
  23. 23. AIRBUS UK CATIA V5 Foundation CourseAfter selecting the part to be Instantiated, the Reference Direction and Instanceoptions, click OK to create the Instantiation. The Multiple Instances are created in theSpecification Tree.In the following example a part is Instantiated with four New Instances with aSpacing or step of 600mm along the X-Axis of the Compass. Selected part to be Instantiated Preview of the Instantiation Resulting Instantiations in the Specification Tree Resulting Instance Numbers Instantiations in the Resulting Specification Tree InstantiationsDMS42177 Page 23 of 71 Issue 1ANS-UG0300108
  24. 24. AIRBUS UK CATIA V5 Foundation Course 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.DMS42177 Page 24 of 71 Issue 1ANS-UG0300108
  25. 25. AIRBUS UK CATIA V5 Foundation Course Saving a Newly Creating CATProductThe 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 thepath in the Save in field. The correct path for storing such data is /epd/parts. You canalso change the name of the CATProduct by entering a new name in the File namefield.When you click OK if your CATProduct contains new CATParts that have not beensaved 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 theSave in field under the specified name together with any new CATParts attached to it.DMS42177 Page 25 of 71 Issue 1ANS-UG0300108
  26. 26. AIRBUS UK CATIA V5 Foundation Course Move Operations ToolbarAllows you to manipulate the position and orientation of Parts. Manipulation Snap Explode Assembly Stop ManipulationManipulation Allows Freehand Manipulation to position and orientate a selected Part.Select the icon to display a Manipulation Parameters panel. Display the currently selected button Drag along any Axis Drag along the X, Y or Z-Axis Drag along any Plane Drag along the XY, YZ or XZ Planes Rotate around any Axis Rotate around the X, Y or Z- AxisThere 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.DMS42177 Page 26 of 71 Issue 1ANS-UG0300108
  27. 27. AIRBUS UK CATIA V5 Foundation CourseSnap OperationsPositions parts using a snapping. Snap Smart Move Snaps one Part to another by selecting elements.Select the icon and then select an element contained within the Part to be moved i.e. 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 Partin 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 moveDMS42177 Page 27 of 71 Issue 1ANS-UG0300108
  28. 28. AIRBUS UK CATIA V5 Foundation CourseWhen you snap two Axis Systems together the orientation of the X, Y and Z-Axis isautomatically 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 theSpecification 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 Morebutton to display the Quick Constraint options. If you select the Automaticconstraint creation, when you select the elements to snap together and click OK theparts are snapped together and a Constraint is generated. The use of AssemblyConstraints is explained later in this session.DMS42177 Page 28 of 71 Issue 1ANS-UG0300108
  29. 29. AIRBUS UK CATIA V5 Foundation CourseExplode Assembly Allows you to Explode selected CATProducts.Select the icon to display the Explode panel and select the CATProduct(s) to beexploded.You have the following options: -The Depth field allows you to control howmany levels of the selected CATProduct(s)are exploded. The choices are limited toFirst Level or All Levels.The Type field allows you to specify thedirection of the Explode to be controlled in3D, 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 willnot 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 inthe Scroll Explode portion of the panel. A Warning message will be displayedinforming you that you are about to modify product positions. If you click Yes thenthe Explode will permanently move the Parts together with any Sub-Products and thecommand will end. If you click No then the Explode is temporary, which is probablythe 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 Scrollbar will appear in the Scroll Explode portion of the panel. An Information boxappears informing you than you can use the Compass to move Products. Click OK toremove this panel and you are now in temporary Explode mode.DMS42177 Page 29 of 71 Issue 1ANS-UG0300108
  30. 30. AIRBUS UK CATIA V5 Foundation CourseYou can use the Scroll bar in the Scroll explode portion of the panel to incrementthrough 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 resetthe Parts back to their assembly positions.Below is an example of an exploded CATProduct. Selected CATProduct to be Exploded Resulting Exploded CATProductStopping 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 anadjacent Part.Note: The With respect to constraints check box on the Manipulation Panel mustbe selected for this to function work.DMS42177 Page 30 of 71 Issue 1ANS-UG0300108
  31. 31. AIRBUS UK CATIA V5 Foundation Course Assembly ConstraintsAssembly constraints are used to position CATParts relative to each other with aCATProduct. All assembly constraints are added to the Specification Tree andattached to a Constraints Node. Constraints Node Assembly ConstraintsWhen you select one of the Constraint icons anAssistant panel appears. If you wish, click on theDo not prompt in the future check box andClick 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 PatternDMS42177 Page 31 of 71 Issue 1ANS-UG0300108
  32. 32. AIRBUS UK CATIA V5 Foundation CourseCoincidence Constraint Applies a Coincidence Constraint between two Parts. This is ideally used to constrain the axis of two Cylindrical features together although you can applyit to a Points, Edges, Faces, etc.Select the icon followed by the two elements/features on two different Parts that are tobe constrained. The constraint is attached to the Specification and temporarilydisplayed on the screen. If you now click on the Update All button the two Parts thathave features selected will move to align the elements so that they are coincident witheach other.As you hover over a Cylindrical features the axis of the feature is Axis of thehighlighted on the screen and if you select it then the coincidence Hole displayedis applied to the axis. when you hover over the featureIn the following example the Hole feature on the bracket is madecoincident 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 dateDMS42177 Page 32 of 71 Issue 1ANS-UG0300108
  33. 33. AIRBUS UK CATIA V5 Foundation CourseThe resulting constrained Parts after the Update All button has been selected. TheAxis of the Holes is aligned but the two Parts do not necessarily contact each other. Coincident constraint Symbol Resultant up to date Coincidence ConstraintDMS42177 Page 33 of 71 Issue 1ANS-UG0300108
  34. 34. AIRBUS UK CATIA V5 Foundation CourseContact 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 faceof the frame Features to be Constrained Contact Constraint Contact attached to the Constraint Specification Tree SymbolDMS42177 Page 34 of 71 Issue 1ANS-UG0300108
  35. 35. AIRBUS UK CATIA V5 Foundation CourseOffset 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 panelwill 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 displayswhether they are connected or not.The Orientation allows you to control how the selected features are orientated toeach 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 direction3. Opposite orientates the features to face opposite direction to each other.You can use the Green arrows toswitch direction.The Offset field allows you to enter avalue for the offset distance betweenthe selected features Offset ConstraintDMS42177 Page 35 of 71 Issue 1ANS-UG0300108
  36. 36. AIRBUS UK CATIA V5 Foundation CourseAfter clicking OK the resulting Constraint is added to the Specification Tree you thenhave to Update the constraint to move the selected features to the correct position.The features will be aligned but may not contact each other.DMS42177 Page 36 of 71 Issue 1ANS-UG0300108
  37. 37. AIRBUS UK CATIA V5 Foundation CourseAngular 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 Propertiespanel appears with the following options: -The Name field allows you to specify aname for the constraint.There are four check boxes on the left ofthe panel allow you to specify theconstraint type: Perpendicularly,Parallelism, Angle (default) and Planarangle.The Supporting Elements lists thefeatures that you have selected toconstraint. Again the Status filed indicateswhether they are connected or not.The Sector menu allows you to selectwhich sector of a 360° circle is used todefine 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 youmust select the Update All icon to position the features. Feature to be ConstrainedDMS42177 Page 37 of 71 Issue 1ANS-UG0300108
  38. 38. AIRBUS UK CATIA V5 Foundation CourseResulting Angular Constraint. Angular Constraint Angular ConstraintFix 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. Fix ConstraintIt is possible to Fix the Position of both Product and Component nodes by selectingthem on the Specification Tree.DMS42177 Page 38 of 71 Issue 1ANS-UG0300108
  39. 39. AIRBUS UK CATIA V5 Foundation CourseFix 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 Togetherpanel will appear listing the parts you have selected to fix together. If you make amistake 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 TogetherWhen you click OK the fix together constraint is applied to the selected Parts andadded to the specification Tree. Selected Part to be Fixed Fix Together ConstraintDMS42177 Page 39 of 71 Issue 1ANS-UG0300108
  40. 40. AIRBUS UK CATIA V5 Foundation CourseBy using the Manipulation command and selecting the With respect to constraintscheck box, when you select one of the Parts that is fixed together and move it, then allother 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.DMS42177 Page 40 of 71 Issue 1ANS-UG0300108
  41. 41. AIRBUS UK CATIA V5 Foundation CourseChange Constraint With this command you can change one constraint type to another.After selecting the icon select the Constraint to be changed. A ChangeType panelwill appear listing the alternative constraints that are available for the selectedfeatures. Replacement Constraint Selected constraint to be changedAfter selecting the alternative constraint from the list click OK and the Update Allicon to complete the change. Result of changing the Constraint from an Offset to a Coincidence New constraintReuse 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 Page 41 of 71 Issue 1ANS-UG0300108
  42. 42. AIRBUS UK CATIA V5 Foundation Course Create a SceneScenes can be used to develop an existing Product assembly in a separate windowwithout affecting the original (i.e. create an Exploded version). You can createmultiple 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 changedwithout the modifications being replicated in the other: -1. The viewpoint or state.2. The graphical attributes of the components3. The Hide/Show state of the components4. Whether a Part in active or not.If a Parts position is changed in the Assembly then it is replicated in the Scenes aslong as the assembly and the scenes are synchronised. On the other hand if the Partsposition is modified in a Scene then is not replicated in the assembly and the Sceneand Assembly are said to be of de-synchronisedScenes are identified by name in the Specification Tree and by a graphic symbol inthe graphic windowWhen creating a Scene the Parts and Sub-Product that make up the Scene aredetermined 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.DMS42177 Page 42 of 71 Issue 1ANS-UG0300108
  43. 43. AIRBUS UK CATIA V5 Foundation Course 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 SpecificationTree 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 thereset. 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.DMS42177 Page 43 of 71 Issue 1ANS-UG0300108
  44. 44. AIRBUS UK CATIA V5 Foundation CourseWhen you enter the Scene the background colour of the graphic display changes toindicate that you are no longer in standard Assembly mode. When you havecompleted the desired Scene use the Exit Workbench icon to return to the AssemblyProductIn the following example the Exploded GA Scene is created from a product with theuse of the Explode command. The Assembly Product unaffected by the Explode command used in the Scene Exploded Scene attached Scene to the Specification Tree Scene displayed in the Graphics WindowThe created Scene can then be used to create an Exploded view in a CATDrawingDMS42177 Page 44 of 71 Issue 1ANS-UG0300108
  45. 45. AIRBUS UK CATIA V5 Foundation Course Assembly OperationsAssemblies Operations can be used to create Assembly Features and SymmetricalParts within the Product. Assembly Features Create SymmetryAssembly FeaturesThis toolbar allows you to create Assembly Based Features within the Product i.e. ahole that passes through multiple Parts. Hole Add Split Remove Pocket This command allows you to Split a group of selected Parts within a Product using a Plane Or Surface.Select the icon followed by the Splitting element todisplay an Assembly Features Definition panel.The Name field contains the name of the splitcommand, which will be displayed on theSpecification Tree.The Parts possibly affected lists all the Parts in thetree that can be split. Either select the double downarrow to move the all the listed Parts into theAffected parts field or select the required Partsfrom the list using MB1 followed by the singledown arrow. If you make a mistake you can use thedouble and single Up Arrows to remove Parts fromthe Affected parts list. To highlight the selectedparts click on the Highlight affected parts checkbox.DMS42177 Page 45 of 71 Issue 1ANS-UG0300108
  46. 46. AIRBUS UK CATIA V5 Foundation CourseAfter clicking OK on the Assembly Features Definition panel a Selection inContext panel appears asking if you would like to keep the link with the selectedObject i.e. the splitting element. If you select Yes then a Contextual link isestablished between the Part containing the Splitting element and the Part(s) beingSplit. 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 reappearstogether with a Split Definition panel. The Assembly Features Definition panelcontains the list of the Parts affected by the Split and the Split Definition panel liststhe splitting element. If required use the Orange Arrow to select the portion of theParts 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 SplitDMS42177 Page 46 of 71 Issue 1ANS-UG0300108
  47. 47. AIRBUS UK CATIA V5 Foundation CourseThe selected Parts are now split and anAssembly Split node is added to theSpecification Tree attached to an AssemblyFeatures node. The Assembly Split nodecontains nodes that define the Split operationon each of the affected Parts.If you selected Yes to keep a Contextual linkbetween the splitting element and the Part(s)being split then an External Reference iscreated in the part Specification Tree. Thereforeif the splitting element changes then the Resultingresulting split will update. The Part node on the Split PartsSpecification Tree indicates that there is anExternal Reference contained within it by theappearance of a Green chain link Symbol on thenode. Green Chain Link Symbol External Reference Link to the Surface held within the Assembly MASTERSURF1 Part, Features node which is attached to the ENV Component nodeDMS42177 Page 47 of 71 Issue 1ANS-UG0300108
  48. 48. AIRBUS UK CATIA V5 Foundation CourseThe 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 Splitcommand. 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 aPlane 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 ProductDMS42177 Page 48 of 71 Issue 1ANS-UG0300108
  49. 49. AIRBUS UK CATIA V5 Foundation CourseA preview of the symmetry will be display together with an Assembly SymmetryWizard and by clicking Finish on this panel Catia will proceed to create the requiredsymmetrical Part(s)/Product(s) and attached Symmetry nodes to the SpecificationTree.When the command is completed an Assembly Symmetry Result panel will appeardetailing the number New Components, Instances and Products that have beenaffected by the Symmetry. Select the Close button to remove the panel. Resulting SymmetryThe Update All icon must now be selected to synchronise the Product.DMS42177 Page 49 of 71 Issue 1ANS-UG0300108
  50. 50. AIRBUS UK CATIA V5 Foundation CourseThe resulting Specification Tree as the Symmetrical Part(s)/Product(s) attached to ittogether with an Assembly Features node containing an Assembly Symmetry node.Note: When using this command be aware that the larger the assembly beingmirrored the longer the task will take.DMS42177 Page 50 of 71 Issue 1ANS-UG0300108
  51. 51. AIRBUS UK CATIA V5 Foundation Course An Overview of Contextual LinksIt is possible within Catia to link elements contained within one CATPart to elementsin another. Typical this can be done by Splitting a Solid contained in one CATPartusing a Surface containing in another or by copying a element/Feature from one Partand Pasting it with a Link into another Part. In both cases an external Reference canbe created in the CATPart.In the following example a CATProduct which as two CATParts attached to it. One ofthe Parts (MASTERSURF1) has two surfaces contained within it that are used toSplit a PartBody in CATIAV5RIBPART. Resulting Split PartBody contained Surfaces contained within within CATIAV5RIBPART MASTERSURF1 CATPartDuring the Split operation a panel will appear asking if want to keep the link withthe selected Object.If you select Yes then the Surface is copied into the Part being Split and is created inthe Specification Tree which embeds a Link to the Part containing the Surface thusallowing any changes in the original Surface to be Updated in the Part being Split. Ifyou 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 Page 51 of 71 Issue 1ANS-UG0300108
  52. 52. AIRBUS UK CATIA V5 Foundation CourseBelow is the resulting Specification Tree for the CATProduct with ExternalReferences linking MASTERSURF1 and CATIAV5RIBPART. Extrude.1 Extrude.2 is Linked to is Linked to Surface.3 Surface.4As with using the Assembly Split Operationthe node of the Part being Split as a smallLink Symbol attached to it to indicate that ithas External References to another Partwithin the current Product.The two Surfaces attached to the ExternalReference node within the Part being Splitalso have Green Diamond Symbol to indicatethat they linked and are up to date.DMS42177 Page 52 of 71 Issue 1ANS-UG0300108
  53. 53. AIRBUS UK CATIA V5 Foundation CourseDue to the fact that the links have been create between the two Parts within theCATProduct (CATIAV5TRAIN12) the External references are said to be created‘In Context’ with the Product. This means that if the CATPart containing theExternal Reference is opened in its own right or it is added to another CATProductthen the links will not be found and they will temporarily be broken. This is signifiedby a red ‘?’ symbol being displayed on the Surface nodes attached to the ExternalReferences within the Part and a red zigzag symbol is displayed on the Part instancenode 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 Partnode within the CATProduct or opening the CATPart in its own right and then selectLinks from the Edit drop down menu.DMS42177 Page 53 of 71 Issue 1ANS-UG0300108
  54. 54. AIRBUS UK CATIA V5 Foundation CourseA Links to Element panel appears that list all the External References and theContext 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 isbroken or as been Isolated then a red zigzag symbol is displayed on the node.DMS42177 Page 54 of 71 Issue 1ANS-UG0300108
  55. 55. AIRBUS UK CATIA V5 Foundation Course Session 6 - AnalysisThis session covers the use of some of the Digital Mockup (DMU) analysis toolsavailable 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.DMS42177 Page 55 of 71 Issue 1ANS-UG0300108
  56. 56. AIRBUS UK CATIA V5 Foundation Course Accessing the Digital Mockup (DMU) WorkbenchesThe DMU Workbenches can be entered by Selecting Start > Digital Mockup andthen select the required Workbench.DMS42177 Page 56 of 71 Issue 1ANS-UG0300108
  57. 57. AIRBUS UK CATIA V5 Foundation Course Proximity QueriesThe Proximity Query analysis tool can be found in the DMU Navigator Workbenchon the DMU Data Navigation Toolbar and is called Spatial Query. This allows youto check the clearance between selected Products and surround geometry. Thiscommand can be used to allow you to limit the number of Products, Sub-Productsand Parts displayed when working on large complex Assemblies or just the portion ofthe 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 iscontrolled by the Accuracy value. Spatial QuerySelect the icon to display a Spatial Query panel. The main options to consider whenusing this panel are: -The Selection Field lists the Product(s) youhave selected to perform the query.The Clearance field allows you to specifythe distance to check between selectedProduct(s) and the surrounding Geometry.The Accuracy field is used to specify theaccuracy of the check.Note: The smaller the Accuracy value thelonger the query will take.DMS42177 Page 57 of 71 Issue 1ANS-UG0300108
  58. 58. AIRBUS UK CATIA V5 Foundation CourseOnce you have selected the Product(s) and set the Clearance and Accuracy you mustselect the Search button to perform the Query. Catia will now perform the queryduring which a Computation in progress panel will appear detailing the operationprogress.Upon completion the Parts whose distance from the selected Product(s) is less thanthe Clearance value are displayed in the Results portion of the panel and arehighlighted graphically.DMS42177 Page 58 of 71 Issue 1ANS-UG0300108
  59. 59. AIRBUS UK CATIA V5 Foundation CourseYou can now use the Select button together with the Group icon, which can be foundon the DMU Navigator Tools Toolbar to group the highlighted items together. GroupA Group node is added to the Specification Tree under the Applications Node. TheGroup node contains all the groups that you have createdOn selecting the Group icon an Edit Group and Preview panels appear. The EditGroup panel allows you to edit the name of the group and also lists the associatedProducts 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.DMS42177 Page 59 of 71 Issue 1ANS-UG0300108
  60. 60. AIRBUS UK CATIA V5 Foundation Course Clash AnalysisThe Clash Analysis tool is accessible through both the Assembly Design and DMUSpace Analysis Workbenches and is located on the Space Analysis Toolbar. ClashSelect the icon to display a Check Clash panel.The Name field allows you toenter a name for the analysis.This is displayed as a node onthe Specification Tree underthe Applications >Interference.The Type field allows youspecify the type check to beperformed: -Contact + Clash. Performs acheck for both Contact and ClashClearance + Contact + Clash. This will allow you to enter a distance value for theClearance check in the right hand field.Authorised penetration. Allows you to check for clash over a specified interferencedistance which is entered in the right hand fieldClash rule. Allows you to specify a rule using Knowledgeware.The field under the Type field allows you to select whether you want to run theanalysis against all components, only inside the selected Product, all componentsagainst the selected Product and between two selections.By default if you do not select a Product then Catia will perform the clash against thecurrently active Product.When you click Apply the analysis is performed and the Clash Check panel willexpand to display the results. A Computing panel may be seen briefly during thecheck.Note: The larger the assembly that is checked then the longer the process willtake.DMS42177 Page 60 of 71 Issue 1ANS-UG0300108
  61. 61. AIRBUS UK CATIA V5 Foundation CourseIn the following example the active product is selected by default to which a Contactand Clash analysis is performed against all components.After clicking Apply the check is performed and the Check Clash panel expands todisplay the results. The number of Interference’s found ResultsDMS42177 Page 61 of 71 Issue 1ANS-UG0300108
  62. 62. AIRBUS UK CATIA V5 Foundation CourseIf you select one of the results from the table (in this case row 5) a Preview windowappears displaying the components involved in the check. The value of the clash, ifany, 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.DMS42177 Page 62 of 71 Issue 1ANS-UG0300108
  63. 63. AIRBUS UK CATIA V5 Foundation CourseIf you now click OK the Clash is attached to the Speciication Tree under the namespecified in the Name field. To view the results again double click on the Results Clash node Results Nodenode.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 Previewresults to the main graphics window by select the Results Window button. Results Window Export file button buttonDMS42177 Page 63 of 71 Issue 1ANS-UG0300108
  64. 64. AIRBUS UK CATIA V5 Foundation Course SectioningThis command allows you to take 3D section cuts through selected Products. As withClash, this icon can be found on the Space Analysis Toolbar in both AssemblyDesign and DMU Space Analysis Workbenches. SectioningSelect 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 theresulting Section which is displayed on the SpecificationTree under the Application > Sections nodes.The Selection field allows you to select which Product isused in the section. Default is the currently activeProduct.There are seven buttons below the selection field that allow the following options: - Results Window Clash Toggle Detection Section Automatic Plane Type Update Toggle Volume Export File Cut Section FillDMS42177 Page 64 of 71 Issue 1ANS-UG0300108
  65. 65. AIRBUS UK CATIA V5 Foundation CourseThe Section Plane Type has three options available by selecting the small arrow onthe 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 thescreen 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♦ wrlThe Automatic Update button has two options available by selecting the small arrowon the button: - Allows automatically updates the section. Freezes the section.DMS42177 Page 65 of 71 Issue 1ANS-UG0300108
  66. 66. AIRBUS UK CATIA V5 Foundation CourseThe Position and Dimensioning portion of the panel allows you to specify the positionand orientation of the section plane.The X, Y and Z check box orientation the plane with the x, y, z plane of the Product. Edit Plane Reset the Position and Section Dimensions Plane Align the Invert the Section with Section geometry directionIf you select the Edit Plane button then the following panel appears that allows you toposition and orientate the Section plane. Plane origin relative to the Product origin Section Plane size Translation Increment Rotation Value Increment value Translation Translation Increment Increment buttons buttons Undo/Redo optionThe Translation and Rotation Increment values allow you move the section a setdistance or angle by using the increment buttons.You can also position and orientate the Section plane by dragging the plane compasswith MB1.DMS42177 Page 66 of 71 Issue 1ANS-UG0300108
  67. 67. AIRBUS UK CATIA V5 Foundation CourseThe Align Plane with geometry button when selected allows you to position theSection plane on a selected element. Once you select the element the section plane ispositioned 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 createthe Section node on the Specification Tree. The created Section can be editted bydouble clicking on the node.DMS42177 Page 67 of 71 Issue 1ANS-UG0300108
  68. 68. AIRBUS UK CATIA V5 Foundation CourseThe 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 ClashDMS42177 Page 68 of 71 Issue 1ANS-UG0300108
  69. 69. AIRBUS UK CATIA V5 Foundation Course Two First Plane Section Planes Plane Manipulator visible when you place the mouse pointer over the plane. UseSecond MB1 to drag the plane to a Plane new position Plane Compass controls both section Planes A Section Cut which superimposes to sections in the same Preview window Second Section Plane Cut First Section Plane Cut DMS42177 Page 69 of 71 Issue 1 ANS-UG0300108
  70. 70. AIRBUS UK CATIA V5 Foundation Course Section Box Wireframe intersection geometry A composite Section using the Section Box option Section Compass Composite SectionDMS42177 Page 70 of 71 Issue 1ANS-UG0300108
  71. 71. AIRBUS UK CATIA V5 Foundation Course Measuring DistancesTo measure geometry within Catia you can use the following icons on the MeasureToolbar, which is available in the majority of the Workbenches on the bottom toolbar. Measure Between Measure ItemBy selecting the Measure Between icon a Measure Between panel is displayed.There are four measuring options available, which can be selected by using the fourbuttons at the top of the panel.The first option is to Measure Betweentwo selected elements.The Selection 1 and 2 mode allows youto specify what type selection method isto be used.The Other Axis checkbox allows youto specify an axis from which to basethe measure on. By default Catia will use the Product or Part Axis.The Calculation mode allows you select whether the measurement is Exact orApproximate. If you measure in a Product that is in Visualisation mode then theresult will be approximate until you switch to Design mode.The results are displayed in the Result portion of the panel.DMS42177 Page 71 of 71 Issue 1ANS-UG0300108
  72. 72. AIRBUS UK CATIA V5 Foundation CourseIf you select Keep Measure then the distance between the selected elements isdisplayed on the screen permanently and a MeasureBetween node is added to theSpecification Tree.You can customise the measure result by selecting the Customize button.You have the option to display theDistance and Angle between the selectedelements both in the measure panel andgraphically.Components displays in the Measurepanel only the delta X, Y and Z cordinatevalues between the measure points on theselected elements.Point 1 and 2 displays the X, Y and Zvalues in the Measure panel from theProduct or Part Axis to the measure pointon the selected element.Once you have customised your display either click Apply to temporarily apply thedisplay or OK to set the customised displayed.Clicking OK on the main Measure Between panel completes the command.DMS42177 Page 72 of 71 Issue 1ANS-UG0300108
  73. 73. AIRBUS UK CATIA V5 Foundation CourseThe following is an example of use measure between using Any Geometry and AnyGeometry, Infinite between the same features.DMS42177 Page 73 of 71 Issue 1ANS-UG0300108
  74. 74. AIRBUS UK CATIA V5 Foundation CourseIn the following example the Distance and Angle to measured and displayed betweenthe two Spoiler Brackets.DMS42177 Page 74 of 71 Issue 1ANS-UG0300108
  75. 75. AIRBUS UK CATIA V5 Foundation CourseThe second measure option is to measure in Chain mode.After selecting this button you have to select the first element to measure followed bythe second. The desired distance/angle is then displayed. If you now select a thirdelement then a distance/angle is displayed between the second and third elements. Allother options are the same as Measure Between. Measuring in Chain modeDMS42177 Page 75 of 71 Issue 1ANS-UG0300108
  76. 76. AIRBUS UK CATIA V5 Foundation CourseThe 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 bythe second. The desired distance/angle is then displayed. If you now select a thirdelement then a distance/angle is displayed between the first and third elements. Againall other options are the same as Measure Between. Fan or Stack mode MeasuringDMS42177 Page 76 of 71 Issue 1ANS-UG0300108
  77. 77. AIRBUS UK CATIA V5 Foundation CourseThe final measure option is Measure Item which also accessible from the MeasureToolbar. When you select this button a Measure Item panel appears. The optionallows you to measure individual elements i.e. Feature Edges, Faces, etc. afterselecting your desired options and the element to be measured the results aredisplayed both graphically and in the Results portion of the panel.Click OK to complete the command. If the Keep Measure checkbox is selected thenthe measure result is permanently displayed and added to the Specification Tree.DMS42177 Page 77 of 71 Issue 1ANS-UG0300108

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