Copyright DASSAULT SYSTEMES 20021 Assembly Design Advanced CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-ASM-AF-V5R9. - презентация
Презентация была опубликована
3 года назад
Презентация на тему: " Copyright DASSAULT SYSTEMES 20021 Assembly Design Advanced CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-ASM-AF-V5R9." — Транскрипт:
Copyright DASSAULT SYSTEMES Assembly Design Advanced CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-ASM-AF-V5R9
Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will learn CATIA V5 advanced concepts concerning Assembly Design Workbench such as Bill of Material and Associativity. Targeted audience Advanced users Prerequisites Assembly Design Fundamentals 1 day
Copyright DASSAULT SYSTEMES Table of Contents (1/2) 1. Managing Scenes5 Introduction to Scenes6 Creating a Scene9 Editing Scenes14 Managing Components in Scenes20 Synchronizing Scenes to an Assembly26 Creating an Explode in a Scene32 Creating Drafting Views based on Scenes35 2.Distance, Sectioning, Clash … 39 Measuring Minimum Distance40 Introduction to Sectioning 43 Creating Section47 Positioning Main Section Plane 51 Using the Section Viewer57 Computing Clash61 3. Generating Reports and Numbering 68 Bill of Material Reports 69 Assembly Listing Reports 75 Product Structure Numbering Generating Annotation85 Weld Planner Annotations86 Text Annotations90 Flag Note93 Manipulating Annotations97
Copyright DASSAULT SYSTEMES Working with Large Assemblies 105 Hiding Components 106 Deactivating Representations 111 Deactivate a Component 119 Product Init 124 Using Visualization Mode 129 Summary of Modes Designing & Managing Contextual Parts 141 Creating Contextual Parts 142 Sketch and Design in Context 149 Knowledgeware and Design in Context 153 Editing Contextually-related Parts 161 Creating Assembly Features171 Analyzing Contextual Parts181 Isolating Contextual Parts 185 Saving Contextually-related Documents189 Deleting Contextually-related Components Creating and Using Published Geometry 199 Creating Published Geometry 200 Using Published Geometry Deleting Components211 Usefulness of Published Geometry 220 Table of Contents (2/2)
Copyright DASSAULT SYSTEMES Managing Scenes Introduction to Scenes Creating a Scene Editing Scenes Managing Components in Scenes Synchronizing Scenes to an Assembly Creating an Explode in a Scene Creating Drafting Views based on Scenes To Sum Up
Copyright DASSAULT SYSTEMES Introduction to Scenes
Copyright DASSAULT SYSTEMES What are Scenes ? Scenes can be used to set the working state by hiding, coloring, and positioning components. Scenes can control: Hide state of components Color of components Position of components Scenes control deactivation of representations Scenes can be used to create assembly drawings. Scenes are stored in an assemblys CATProduct file Scenes can be used to see the evolution of an assembly Use Scenes to try new positions and then apply positions to the main CATIA window product In Scenes, you can create reports. Check the DMU Basic Course Scenes enable capturing and restoring the state of components in an assembly in a saved viewpoint
Copyright DASSAULT SYSTEMES Scenes Workbench Presentation Exit Scenes Reset selected Components Search objects Explode Product A mini Scenes slide appears on the bottom of the screen for each scene created The name of the Scene is also identified in the specification tree Scene Window CATIA Window Scene Workbench DMU Navigator Workbench Save current viewpoint Publish report Snap
Copyright DASSAULT SYSTEMES About Scene creation You have only one way to create a first Scene: Using the Create Scene icon… To create a Scene with all components To create a Scene with selected components only But you can create the other scenes : Using the Create Scene icon Using the previous Scene as a reference
Copyright DASSAULT SYSTEMES Creating a Scene Specify a Scene name 3 Create a Scene 2 Manage your components 4 5 Exit the Scene Find the perfect viewpoint for your Scenes 1 Scenes capture the orientation of the session so be sure the orientation is correct before pressing the Create Scene icon. Move Components thanks to the compass, hide some or change color… On creation, all the Components are copying the state (Color, Position, Activation…) of the Main Assembly. The Main Assembly drives those states unless you modified it in the scene. !
Copyright DASSAULT SYSTEMES Creating a Scene with a Subset of the Assembly Specify a Scene name Select a component 31 Create Scene 2 Exit the Scene 4 The Scene includes only the selected component Keep in mind that Scenes capture the current color, position, and hide state of components in the assembly when you press the Create Scene icon. The components in a Scene can be limited to a component (and its children if the component is a sub-assembly).
Copyright DASSAULT SYSTEMES Creating a New Scene from an Existing Scene 2 Copy Paste Right-click the Scene to be copied 4 1 Specify a new name 7 Right-click the new Scene 5 3 Right-click the Scenes branch Properties 6 Another way to copy a Scene is to select a Scene in the tree and press the Create Scene icon. Copy / paste is used to create a Scene from an existing Scene.
Copyright DASSAULT SYSTEMES About Editing Scene General Scene Management Calling a Scene Double click on the Scene to open Deleting Scenes Open Contextual menu and delete the Scene Replacing the Scene Viewpoint Modify the Viewpoint and click on the this icon Applying the Scene to the main CATIA Window, then apply the scenes scenario on the assembly Red means that nothing will be modified Green means that the modification(s) will be taken in account Grey means that nothing has been modified
Copyright DASSAULT SYSTEMES Calling a Scene Double-click the Scene 1
Copyright DASSAULT SYSTEMES Deleting a Scene Click with MB3 on the Scene 1 Select Delete 2 The Scene has been Deleted
Copyright DASSAULT SYSTEMES Modifying the Scenes Viewpoint When You create a Scene the viewpoint you used at the moment of the scene creation, is the one you open when accessing the scene. You will learn here how to modify it. Open the Scene 1 Modify the current viewpoint (by flying for example) 2 Click on 3 From now, whenever you are accessing this scene, the viewpoint will be this one. On opening you get the scene viewpoint
Copyright DASSAULT SYSTEMES Applying a Scene on the Assembly Right-click the Scene 1 Select the Scene name 2 Select Apply Scene on the Assembly The Apply Scene Window appears 3 Select the product attributes to apply on the Assembly 4 Click OK to apply the new positions 5 This function is very useful when you have stored different states of an assembly and want to re-apply them Red means that the scene attribute wont be applied on the assembly Green means that the it will be applied on the assembly Grey means that there is no difference between scene and assembly Lights indicate states of attributes that are different in the scene than in the assembly
Copyright DASSAULT SYSTEMES Managing Components in Scenes
Copyright DASSAULT SYSTEMES About Components Management in Scenes Show / No Show Components By default the scene is the copy of the Main window, or the selected scene. You may want to swap some objects to show or no show Modify Color Properties You can modify the color, without modifying it in the main window Move Components This is the main interest of the scenes. You can try new positions and then, apply them to the main assembly and check the result, by updating the different measures Deactivate Shape You can deactivate shapes, without modifying their state in the main window
Copyright DASSAULT SYSTEMES Hide Components in a Scene The position, color, and hide state of components can be set in a Scene. This does not effect the assembly. Access the Scene 1 3 Click on Show/No-Show button Select Components to No-Show 2 Hide these components
Copyright DASSAULT SYSTEMES Modify Color Properties in a Scene The position, color, and hide state of components can be set in a Scene. This does not effect the assembly. Access the Scene 1 5 Click OK to Confirm Select Components to modify color 2 3 Open the Contextual Menu Select Properties 4 Choose a Color in Graphic Tab
Copyright DASSAULT SYSTEMES Move components with the Compass in the Scene Drag and Drop the Compass on the object to be moved 1 3 Move Back the Compass to its original position after use Move the element according to the plane / axis 2 The elements can be moved in the same way than in the main window
Copyright DASSAULT SYSTEMES Reset Components position in the Scene The components in the main window are like this 1 2 Select the Yellow Part In the Scene they are like this The yellow part is not at the right position Click on The yellow part position has been modified according to the main CATIA window The elements can be reset, using the main window as reference You can reset more than one component at a time by selecting with the mouse while holding the [CTRL] key [CTRL] key
Copyright DASSAULT SYSTEMES Synchronizing Scenes to an Assembly You will learn how to Synchronize scenes with different kind of changes to an assembly
Copyright DASSAULT SYSTEMES What is Synchronizing Scenes ? New components are automatically added to Scenes, but they are inactivated In some cases Scenes are automatically synchronized with changes to an assembly. In other cases, manual intervention is required. Deleted components are automatically removed from Scenes Moved components are automatically moved in Scenes if they were not repositioned in the Scene Before After
Copyright DASSAULT SYSTEMES Synchronizing Scenes after Adding a Component Components that are added to an assembly will appear as inactivacted in Scenes. Activating the component in a Scene makes it visible. Double-click the Scene to open it Right-click the new component Activate Node The new component is inactivated 1 3 2
Copyright DASSAULT SYSTEMES Synchronizing Scenes after Deleting a Component The component is automatically deleted from all Scenes that exist in the assemblys CATProduct file Delete the component from the assembly Deleting a component from an assembly automatically removes it from all Scenes that exist in the CATProduct file. 1
Copyright DASSAULT SYSTEMES Synchronizing Scenes after Moving a Component Move components in the assembly There are two possible behaviors for components in Scenes: Components are moved automatically in the Scene (to be in the same position as in the assembly) if the Scene does not define an alternate position If the Scene defines an alternate position, there is no synchronization, the component keeps its position defined in the scene These two components are moved in the assembly This component is moved in the Scene There are two possible effects from moving a component in an assembly. To define an alternate position in the scene, a component must have been moved or reset in the scene 1
Copyright DASSAULT SYSTEMES Listing Components that are in an Alternate Position Components that have been moved in a Scene must be manually synchronized with the assembly. Inquiring about these components is the start. Double-click the Scene Check PositioningComponents in an alternate position are highlighted 1 2
Copyright DASSAULT SYSTEMES Creating an Explode in a Scene The Scene workbench offers Explode capabilities thanks to the Explode Function whose result can be modified manually
Copyright DASSAULT SYSTEMES Using the Explode Dialog Box Selected Products to be exploded Select in Depth : One Level only the first level components of the product(s) will be exploded All Level all the components of the product(s) will be exploded Select type of Explode: 3D Product(s) are exploded in the space Projection Products are exploded and placed in the same plane, parallel to the screen* Constrained Products are exploded according to assembly constraints (Not working in Scenes) 3DProjection Cursor representing level of Depth in exploded Products. Example : To navigate through levels of Explode Level 3Level 2Level 1Level 0 2x click 3x click Select fixed Product
Copyright DASSAULT SYSTEMES Exploding in a Scene Create a Scene 1 Click on 23 Click on the Apply Button 4 Click OK to Confirm 6 Move the Components 5 Use the Compass to move components in scenes Fill the Explode Dialog Box
Copyright DASSAULT SYSTEMES Creating Drafting Views based on Scenes You will learn how to create a drafting view based on a Scene
Copyright DASSAULT SYSTEMES What are Drafting Views based on Scenes ? Without Scenes it would be difficult to create a drafting sheet that shows the assembly in two different states (as shown below). Scenes make it possible to have drafting views where components are in different states than the assembly. Scenes also avoid the need to reconstruct manually views as components are added, deleted, replaced, and moved in an assembly. Scenes also avoid the need to reconstruct views (such as the exploded view shown below) when components are added, deleted, replaced, and moved in the assembly.
Copyright DASSAULT SYSTEMES Creating a Drafting View based on a Scene Creating a drafting view based on a Scene follows nearly the same steps as normally done when creating views. Double-click the Scene 1 Switch to the Drafting Workbench and select a view creation icon 2 Select the node that is below the Scene name 3 Select a reference plane 4 Click the drafting sheet to accept the view (as normally done when creating a view) 5 You can expand the tree and select a different node. Only selected node and its components will appear in the view.
Copyright DASSAULT SYSTEMES To Sum Up... You have seen how to Create and Utilize Scenes: How to create Scenes How to Apply Scenes to an Assembly How to create drafting views based on Scenes How to synchronize Scenes with changes of an assembly How to delete Scenes
Copyright DASSAULT SYSTEMES Distance, Sectioning, Clash … New Toolbar available in Assembly Design Clash Sectioning Distance
Copyright DASSAULT SYSTEMES Measuring Minimum Distance You will learn how to measure minimum distances
Copyright DASSAULT SYSTEMES About Measuring Minimum Distances Measuring Minimum Distance This tool will help you to measure minimum distance between two selections or analyse minimum distance between one component to all others
Copyright DASSAULT SYSTEMES Measuring Minimum Distance 2 Select the computation type Inside one selection : Each selected components are tested against all others in the same selection Between two selections : Each component in the first selection are tested against all components in the second selection Selection against all : Each product in the defined selection against all other products in the document Select the products according to computation type 3 Measure minimum Click on Distance icon The Edit Distance Window appears 1 4 Click apply to compute the distance The Preview window displays selected products and the minimum distance It is no possible to keep results on the Specification Tree
Copyright DASSAULT SYSTEMES Introduction to Sectioning Create Sections and Cuts
Copyright DASSAULT SYSTEMES About Sections Check Distances See what is inside Components using 3D Cuts Check if your components are empty or not Identify Conflicts You can Create Sections in the Clash Window
Copyright DASSAULT SYSTEMES General Process From product Position and resize the Section on the component to section Open and Manipulate the Section result 3 2 create the section 1
Copyright DASSAULT SYSTEMES How to Use Section Tools? When section is created, the Sectioning Definition dialog box appears Contextual Menu available in the Section Results Window Transform Section into 3D CutEdit Plane Window (Precise positioning)Place your Section plane on a Geometric Target Invert Normal direction Cancel Move Open and Maximize Section Viewer Clash detection in the Section Viewer Export Section View Fill sections. Activate and deactivate Grid Modify Grid Properties Section Mode: section plane section slice section box Automatic Update/Freeze Section Automatic Update Freeze Section
Copyright DASSAULT SYSTEMES Creating Section You will learn the different ways to Create Section, and will see how to activate 6 cutting plane simultaneously
Copyright DASSAULT SYSTEMES How to Create a Section Create the section plane Position plane(s) Resize plane(s)
Copyright DASSAULT SYSTEMES Creating a Section Plane Click on The plane created will section all components 1 Manipulate your Section Plane 2 Create dynamically a section using a cutting plane
Copyright DASSAULT SYSTEMES Creating 3D Section Cut Edit the desired section plane, slice or box by double clicking Click on Volume Cut icon Cutting away the material above the plane, beyond the slice or outside the box to expose the cavity within the product 1 2
Copyright DASSAULT SYSTEMES Positioning Main Section Plane You will learn how to position plane using edge as support and how to dimension main section plane
Copyright DASSAULT SYSTEMES About Section Manipulation By default, the section plane is : centered on the surrounding box center of the pre selected elements, oriented by the XY plane square shaped dimensioned according to the longest dimension between center of inertia and the furthest element Most of the time the section plane is not at the right position or size. You will have to: re – center it translate and rotate it re dimension it
Copyright DASSAULT SYSTEMES How to manipulate a Section Move the plane using: Direct Manipulation Geometrical target Edit Position Command Re dimension the plane using Direct Manipulation Edit Position Command
Copyright DASSAULT SYSTEMES Manipulating a Section Plane Reset Position icon : Restore the plane to its original position Edit the desired section plane by double clicking it 1 Re-dimension the section plane clicking and dragging plane edges 3a 3b Move the section plane along its normal vector clicking over the plane and drag Move the cursor over the section plane, section plane edge or local axis system Translate the plane by pressing MB1, then MB2 and dragging Rotate the section plane clicking over the desired plane axis system and dragging 3c 3d 2 The appearance will change and arrows appear to help you to move your section plane Re-dimension, move and rotate section planes
Copyright DASSAULT SYSTEMES Positioning Plane with respect to a Geometrical Target Reset Position icon : Restore the plane to its original position Edit the desired section plane by double clicking on it Click on Geometrical Target icon Point to the target of interest : Simply Click an Edge or an Axis to position the section plane normal to the desired edge Simply Click a Surface to position the section plane on the tangent to a surface Simply Click on a Cylindrical Surface to position the Section Plane normal to the Axis The Rectangle is a representation of the section plane, to assist you in positioning it
Copyright DASSAULT SYSTEMES Positioning Plane Using the Edit Position Command Edit the desired section plane by double clicking it Click on to Edit Position Change the current position : Click X, Y or Z to position the normal vector (z-axis) of the plane perpendicular to the selected absolute axis system Change the center of the plane coordinates : Values in Origin X, Y and Z boxes (absolute system coordinates) Move the section plane : Enter translation step, then click +Tx, -Tx, +Ty … to move the plane along the selected axis by the defined step (local plane axis system) Rotate the section plane : Same as for the translation use, to rotate the plane around the selected axis by the defined step 1 2 Fill Edit Position Dialog Box 3 Click close to exit and save last plane position 4 Undo / Redo section plane move Change the plane / slice / box dimensions Enter the width of the main section plane Enter thickness of the box or the slice (Distance between the 2 parrallel cuting planes) Position the section plane more precisely
Copyright DASSAULT SYSTEMES Using the Section Viewer
Copyright DASSAULT SYSTEMES About Section Viewer Display the result of the section, in a particular interface Special tools are available in this interface, in order to: Display Grid Modify Grid options Rotate section Lock 2D Viewer contextual menu
Copyright DASSAULT SYSTEMES How to use Viewer Tools? Lock 2D Visualization Rotate 90° Edit Grid Properties Swap to symmetrical position Show / No Show Grid Horizontal and Vertical Grid step Reset Grid steps to defaults Use Absolute Axis or section plane center as origin Choose style of Grid Fill / No Fill Section Contextual Menu in the Viewer
Copyright DASSAULT SYSTEMES Viewing Section Edit the desired section plane Click on Results Window icon Click on Reframe icon reframe the results window on the section 12 3 Manipulate the Section 4 View the generated section in a separate 3D viewer
Copyright DASSAULT SYSTEMES Computing Clash You will learn the different ways to Compute Clashes
Copyright DASSAULT SYSTEMES What is Computing Clash Check the Design You will see if : the Design has no interferences the minimum distance between the selected product and other components is OK, because of heat for example Modify the Design You will be able to see precisely which function or surface is to be modified to have a correct design Reading Results The Preview window displays selected interference according to options Clash: red intersection curves identify clashing products Contact: yellow triangles identify products in contact. Clearance: green triangles identify products separated by less than the specified clearance distance.
Copyright DASSAULT SYSTEMES How to Compute Clash Part to Part Clash This is the simplest tool for Clash Detection Select 2 parts then Click Apply The result is given by the traffic lights Check Clash Window This is the powerful tool for Clash Detection in Space Analysis This in fact the one you must know It is possible to save and keep results on the Specification Tree
Copyright DASSAULT SYSTEMES Analyze Part to Part Clashes Open Compute Clash 2 CTRL + Click on Apply 4 Check results 5 Check light : - green for clearance - yellow for contact - red for clash Check for clashes and clearances between parts in the document 1 Select the 2 parts Choose the kind of Analyze to perform: Clash (Parts occupying same space or in contact) Clearance (Parts occupying same space zone, in contact, or separated by less than the defined clearance distance - enter the value of the clearance) 3
Copyright DASSAULT SYSTEMES Computing Interferences Choose Computation type : - Clash: products occupy same space zone - Contact: products in contact -Clearance: products separated by less than the defined clearance distance Choose Selection type : Between all components : each product against all other products Inside one selection : within any one selection, tests each product of the selection against all other products in the same selection Between two selections : each product in the first selection against all products in the second selection Selection against all : each product in the defined selection against all other products in the document Select the products according to computation type Before Compute the Clash Operations, you will have to fill the Check Clash window Click apply to calculate the Clash The Results are displayed at the bottom of the Check Clash Box A Preview window displays the selected Clash 4
Copyright DASSAULT SYSTEMES Analyzing Interferences Basic List by Conflict Compute Clash Then Click on the results to be checked The Clearance/ Clash value is displayed The Status changed from not inspected to Relevant Filter Interferences to simplify result display, eventually Type: Clash/Contact/Clearance Value: Increasing/Decreasing Status: Irrelevant/Relevant/Not Inspected Compute status : New / Old / Modified Click on the Status value to change it into Relevant or Irrelevant, If necessary 3 Click on the Comment of the selected result to add/modify the Comment 5 Then Click Apply Filters 6 Click OK to Exit
Copyright DASSAULT SYSTEMES Analyzing Interferences Basic List by Product Compute Clash Then Click on the results to be checked The Clearance/ Clash value is displayed The Status changed from not inspected to Relevant Filter Interferences to simplify result display, eventually Type: Clash/Contact/Clearance Value: Increasing/Decreasing Status: Irrelevant/Relevant/Not Inspected Compute status : New / Old / Modified Click on the Status value to change it into Relevant or Irrelevant, If necessary 4 Click on the Comment of the selected result to add/modify the Comment 2 Click on « List by product » Tab to Display Clashes Product by Product Then Click Apply Filters 7 6 Click on OK to Exit
Copyright DASSAULT SYSTEMES Generating Reports and Numbering You will learn how to generate Bill of Material and Assembly Listing Reports and how to make Product Structure Numbering Bill of Material Reports Assembly Listing Reports Product Structure Numbering To Sum Up
Copyright DASSAULT SYSTEMES Bill of Material Reports You will learn how to generate Bill of Material Reports
Copyright DASSAULT SYSTEMES What are Bill of Material Reports? Bill of Material Reports list the components of assemblies. Components are listed by Part Number and the quantity of each Part Number is computed. BOM with the components of the active assembly One BOM for each sub-assembly Recap of leaf components from the active assembly and all sub-assemblies
Copyright DASSAULT SYSTEMES Generating Bill of Material Reports Bill of Material Reports can be interactively generated and viewed. Activate the assembly for which the BOM is to be generated 1 Analyze + Bill of Material 2
Copyright DASSAULT SYSTEMES Saving Bill of Material Reports Save As... Bill of Material Reports can be saved for viewing outside CATIA. 1 2 Specify a file name and folder 3 Specify a type: HTML, text, Excel
Copyright DASSAULT SYSTEMES Customizing Bill of Material Reports Define formats Bill of Material Reports can customized to display the properties of your choice and to arrange the order of properties. 1 Specify properties to be displayed 2 Arrange order of properties 3
Copyright DASSAULT SYSTEMES Removing a Component from the BOM A Product property can remove a component from the Bill Of Material This Component is not taken into account in the BOM… … Thanks to deactivation of this product properties
Copyright DASSAULT SYSTEMES Assembly Listing Reports You will learn how to generate Assembly Listing Reports
Copyright DASSAULT SYSTEMES What are Assembly Listing Reports? Assembly Listing Reports list the components of assemblies. Components are listed in a hierarchical or tree format. Hierarchy showing every component from the active assembly and all sub-assemblies
Copyright DASSAULT SYSTEMES Generating Assembly Listing Reports Assembly Listing Reports can be interactively generated and viewed. Activate the assembly for which the BOM is to be generated 1 Analyze + Bill of Material 2 Select the Listing Report tab 3
Copyright DASSAULT SYSTEMES Saving Assembly Listing Reports Save As... Assembly Listing Reports can be saved for viewing outside CATIA. 1 2 Specify a file name and folder
Copyright DASSAULT SYSTEMES Customizing Assembly Listing Reports Assembly Listing Reports can be customized to display the properties of your choice and to arrange the order of properties. Specify properties to be displayed 1 Arrange order of properties 2 Refresh 3
Copyright DASSAULT SYSTEMES Product Structure Numbering You will learn how to associate numbers usable for drafting to the different parts of your assembly
Copyright DASSAULT SYSTEMES What is Product Structure Numbering? The Generate Numbering command allows you to associate numbers or letters to the parts which make up your product. Those numbers will also appear when creating balloons on Drawings generated from the assembly Product Structure Numbering: Created Number Created Number appearing in a balloon
Copyright DASSAULT SYSTEMES Product Structure Numbering (1/2) (1) 1 Select the Generate Numbering icon 2 Select the root of the product The Generate Numbering command allows you to associate numbers or letters to the parts which make up your product. (2) 3 Select numbering mode (3) 4 5 The generated numbers appear in Properties dialog box (Product tab) Select what you do with already existing numbers Click on Ok (4) (5) 6a Created Number 6b The generated numbers also appear in the bill of Material (6b)
Copyright DASSAULT SYSTEMES Product Structure Numbering (2/2) 7 Generate a Drawing from the 3d 8 Select balloons icon In Drafting Workbench On a drawing generated from the product, when creating balloons on parts you will have by default the letter or number generated for the part in 3d. (8) (9) 9 When selecting an edge for ballooning, you will get the whole part.Click it 11 You can change it but the default value inside the balloon is the number of the selected part.Click Ok to validate 10 click on the sheet to place the balloon (10) (11)
Copyright DASSAULT SYSTEMES To Sum Up... You have seen how to generate reports: How to generated Bill of Material and Assembly Listing Reports How to save reports for viewing outside CATIA How to customize reports to display and re-order attributes How to associate numbers or letters to parts of your Assembly
Copyright DASSAULT SYSTEMES Generating Annotations You will learn how to create several types of annotations in CATProduct files Weld Planner Annotations Text Annotations Flag Note Manipulating Annotations To Sum Up
Copyright DASSAULT SYSTEMES Weld Planner Annotations You will learn how to add annotations concerning welding between components inside FD&T 3Dviews
Copyright DASSAULT SYSTEMES What Are Weld Planner annotations ? Weld planner annotations show specifications for welding between several components, Catia add them inside FD&T (Functional Dimensioning and Tolerancing ) 3D views.
Copyright DASSAULT SYSTEMES Creating Weld Planner(1/2) 1 3 When you create a Weld Planner annotation, you have to specify informations in two dialog boxes 2 4 Click on Weld Planner Icon Before creating Weld Planner features, your components have to be positioned with constraints (here constraints are not updated for the needs of the illustration) You will get two specification boxes Select Geometric Elements involved in the Welding In the first box, you will indicate Size of Welding Length of Welding Type of Welding Additional information about the Type This flag indicates the Welding is done on Working Site This Symbol indicates the welding is all around the part Indications about Welding on the other side Welding Process This switch will put the Main Welding indications up or under the center line to tell where the welding is (this side or the other) You can Import File about welding Process
Copyright DASSAULT SYSTEMES Creating Weld Planner(2/2) Creation of Weld Planner induces creation of a 3d view to support the annotation. 5 When finished with specifications click on OK (First Dialog Box) 6 2nd Dialog Box indicates... Name of the Weld Planner (editable) Geometric elements involved in the welding (selectable and reconnectable in the geometry) Two new nodes have appeared in the tree One Weld Planners node containing the just created feature One Annotation set node containing created 3d view Weld Planner annotation Supporting View 7 Those new features appear in the geometry too
Copyright DASSAULT SYSTEMES Text Annotations You will learn how to add text annotations on your assembly
Copyright DASSAULT SYSTEMES What Are Text Annotations ? Text annotations are some text that the user can see in the geometry and can edit when he wants.Text annotations are associated with geometric element of a component in the assembly. Command Dialog Box Associated Features
Copyright DASSAULT SYSTEMES Creating Text Annotations 1 4 When you create a text annotation, you implicitly use a FD&T view that will be created if not already existing 2 5 Validate Text Text Annotation and supporting view ares displayed in geometry and under annotation set in Structure tree. Select geometric element 3 Key Text (3) (4) Text Annotation Supporting View (2) (1) You can edit the annotation when you want by double clicking on it
Copyright DASSAULT SYSTEMES Flag Note You will learn how to add flag notes on geometric elements of your assembly that will call other electronic files (hyperlink)
Copyright DASSAULT SYSTEMES What Are Flag Notes ? Flag notes are some text annotation through which you can open any external files.Flag notes contain hyperlinks that you can connect or disconnect when you want. Command Dialog Box Associated Features
Copyright DASSAULT SYSTEMES Creating Flag Note (1/2) 1 4 When you create a flag note, you implicitly use a FD&T view that will be created if not already existing 2 5 Click on Browse Flag Select geometric element 3 Key text that will appear on flag (3) (4) (2) (1) 2x Double click on the file you want to attach (5)
Copyright DASSAULT SYSTEMES Creating Flag Note (2/2) 6 7a When consulting the linked file, you implicitly launch the application that can read it Hyperlink exists now, (7b) Flag Annotation Supporting View (7a) you can click OK to validate… 7b … or double click the link to consult the linked file You can edit the annotation when you want by double clicking on it
Copyright DASSAULT SYSTEMES Manipulating Annotations You will learn how to change annotations supporting view or how to change leader shapes. You will even learn how to project annotation views on drafting.
Copyright DASSAULT SYSTEMES What is Manipulating annotations ? You can change the FD&T 3D view supporting an annotation, and you can add or remove leader of annotation.You can even modify their symbol shape. The annotation is not supported by the right 3D view We would like to replace this ladder by another one snapping the right geometric element Here the leader is connected to another geometric element and has a different symbol shape Here the annotation is differently oriented because supported by another FD&T 3D View.
Copyright DASSAULT SYSTEMES Changing Annotation Supporting View CATIA Automatically chooses a supporting view when creating a Weld Planner but you may not be satisfied with the choice, so you have the possibility to change it. 1 To change supporting view... Select Transfer to View/Annotation Planein contextual menu of annotation 2 Select the new supporting View 3 The annotation is now supported by this view
Copyright DASSAULT SYSTEMES Manipulating Annotation Leaders (1/3) 1 To delete a leader First select the annotation Select Remove Ladder in contextual menu of the yellow point The Leader has disappeared Notice that if the Weld Planner feature has not any leader, the Weld process wont appear either CATIA Automatically puts a leader on your weld planner Feature but you may not be satisfied with the anchor point
Copyright DASSAULT SYSTEMES Manipulating Annotation Leaders (2/3) 1 To add a leader Select Add Leader in contextual menu of the Weld Planner Feature The new leader has appeared Click the Anchor Point leader in the Geometry Notice that only geometric elements involved in the annotation are selectable
Copyright DASSAULT SYSTEMES Manipulating Annotation Leaders (3/3) 1 To define Symbol Shape of a leader Select the weld planner feature The leader has a new Shape Select Symbol Shapein contextual menu of the yellow anchor... … and choose symbol in its submenu
Copyright DASSAULT SYSTEMES Projecting Annotation Views on a Drafting In the Drafting workbench, select View From 3D The View is now on the Drafting and displays annotations Select one of the 3D views in the 3D File You can dispose of FD&T 3D views in CATDrawing files Take care of having same Standards (ISO,ANSI) in 3D and 2D views otherwise you wont be able to add a view from 3D (default Standard in 3D Views is ANSI).
Copyright DASSAULT SYSTEMES To Sum Up... You have seen how to manage annotations: How to create Weld Planner Annotations How to create Text Annotations How to create flag notes How to change annotations
Copyright DASSAULT SYSTEMES Working with Large Assemblies You will learn how to work with large assemblies Hiding Components Deactivating Representations Deactivating a Component Product Init Using Visualization Mode Summary of Modes To Sum Up
Copyright DASSAULT SYSTEMES Hiding Components You will learn how to hide components to improve performance and reduce clutter in show space and exclude components from drawing views. Hiding components is similar to deactivation of representations, but with the added advantages of: excluding components from drawing views part elements accessible to design parts and assemblies
Copyright DASSAULT SYSTEMES What is Hiding Components ? Hiding components can improve performance and reduce clutter in show space. Hiding also excludes components from drafting views. Here one instance of the Connector Shell is hidden or no-shown. Hide/Show state is stored in CATProduct files so that the state is maintained when the assembly is opened. The components icon is dimmed in the tree. Hidden components are not visible in show space or in drafting views. Here an assembly is hidden.
Copyright DASSAULT SYSTEMES Differences between Show and Hide This table compares the capabilities of Show and Hide while in Design Mode.
Copyright DASSAULT SYSTEMES Hiding Components Hiding can be performed on individual components, multi-selected components, or an entire assembly. Select the component to be hidden 1 2 Hide the component 3 The component is hidden You can hide more than one component at a time by selecting with the mouse while holding the [CTRL] key [CTRL] key
Copyright DASSAULT SYSTEMES Showing Components Showing a component makes it available for designing the assembly and inclusion in drafting views. Select the component to be shown 1 2 Show the component 3 The component is shown You can show more than one component at a time by selecting with the mouse while holding the [CTRL] key [CTRL] key
Copyright DASSAULT SYSTEMES Deactivating Representations You will learn how to deactivate representations to improve performance, reduce clutter in show space and no-show space, and exclude representations from mass property analysis. Deactivation of representations is similar to hiding components, but with the added advantages of: not cluttering no-show space improving performance when opening assemblies excluding representations from mass property analysis
Copyright DASSAULT SYSTEMES What is Deactivating Representations ? Deactivating representations can improve performance and reduce clutter in no-show space. Deactivation can also be used to exclude representations from mass property analysis. Here one instance of the Connector Shell is deactivated. More precisely, the geometric representation is deactivated. Deactivation state can be stored in CATProduct files. The default geometric representation is activated when opening an assembly. If there is only one representation, it is the default. A deactivation symbol appears in the tree. Deactivated representations are not visible in show space or no-show space. Deactivated representations are excluded from mass property analysis.
Copyright DASSAULT SYSTEMES Differences between Activation and Deactivation This table compares the capabilities of Activation and Deactivation while in Design Mode.
Copyright DASSAULT SYSTEMES Deactivating Representations Deactivation can be performed on individual components, multi-selected components, or all components in an assembly. Right-click the component to be deactivated 1 2 Deactivate Node 3 The geometric representation of the component is deactivated. Note that only the selected instance is deactivated. Use Deactivate Terminal Node to deactivate all parts within a selected assembly. You can deactivate more than one component at a time by selecting with the mouse while holding the [CTRL] key [CTRL] key
Copyright DASSAULT SYSTEMES Activating Representations Activating a representation makes it available for designing the assembly. Right-click the component to be activated 1 2 Activate Node 3 The default geometric representation is activated. Use Activate Terminal Node to activate all parts within a selected assembly. You can activate more than one component at a time by selecting with the mouse while holding the [CTRL] key [CTRL] key
Copyright DASSAULT SYSTEMES Saving Activation State (1/2) A command allows you to store activation state in CATProduct file : you first need to create the access to the command Select customize command from Tools menu 1 2 Select Commands tab 3 Select all commands 4 Drag and drop Save Activation State command into a toolbar Close Customize Panel 5
Copyright DASSAULT SYSTEMES Saving Activation State (2/2) This assembly has one component with deactivated shape This command will allow to keep activation state of components into the CATProduct files. If you save it without having clicked on the icon One click on the icon will make all save operations of CATProducts in the session,keep activation states of components. If you save it after having clicked on the icon… …You will obtain this next time you will open the CATproduct
Copyright DASSAULT SYSTEMES Using Deactivation when Opening an Assembly Performance can be improved by automatically deactivating representations when opening assemblies. Turn ON the option Do Not Activate Default Shapes on Open 1 4 Activate Node 2 Open an assembly 3 Multi-select the components to be activated
Copyright DASSAULT SYSTEMES Deactivate a Component
Copyright DASSAULT SYSTEMES Why Activate and Deactivate a Component ? Visualization (Shape Representation) BOM (Bill of Material) Accessibility (possibility of applying constraints) NO SHOW Hiding components NOYES YES, you can apply constraints between the hidden object and the other components in the show space. UNLOAD Unloading a Component NO Deactivating a Node NOYES YES, you can apply a constraint even if the shape is deactivated. Deactivating a Terminal Node NOYES Deactivating a Component NO
Copyright DASSAULT SYSTEMES Deactivating a Component (1/2) Select the instance and Right click to display the Contextuel menu 1 2 Select the Clamp2 object -> Activate/Deactivate Component Its shape is deactivated and there are no traces of its specifications in the Bill Of Material The symbol in the specification Tree shows you that it is still possible for you to reactivate it by the reverse operation
Copyright DASSAULT SYSTEMES Deactivating a Component (2/2) As oppose to Deactivate a Node, Deactivating a Component inside a assembly means deleting its representation in all the CATIA documents containing this assembly.
Copyright DASSAULT SYSTEMES Product Init You will learn how to determine what are the loaded components when opening an assembly
Copyright DASSAULT SYSTEMES What is Product Init ? The Product Init command allows you when you open a Product, to decide which component will be loaded or not and which component will be hidden or not. It is very useful when working with Large assemblies. Product Init: Unloaded component Loaded Component Loaded and hidden Component Product Init Dialog Box
Copyright DASSAULT SYSTEMES User Setting: Turning OFF the Automatic Load Select General tab 2 3 Select General node To get the Product Init command usable you have to Deactivate the option which makes CATIA automatically load documents referenced in the products Deactivate Load referenced documents 4 1 Select Options... from the Tools menu
Copyright DASSAULT SYSTEMES Product Init (1/2) Click on Product Init This box appears.Select in the tree the components you want to load The Product Init command allows you when you open a Product, to decide which component will be loaded or not and which component will be hidden or not. It is very useful when working with Large assemblies. 4 Click on load icon Open the product with unloaded referenced documents
Copyright DASSAULT SYSTEMES Product Init (2/2) Click on OK You can hide sets of components too with this tool but they have to be loaded first. Delayed actions appear in this areaPartial load and display are performed, you can see it in the tree and in the geometry Loaded Components Unloaded component
Copyright DASSAULT SYSTEMES Using Visualization Mode You will learn how to use Visualization Mode to improve performance.
Copyright DASSAULT SYSTEMES What is Visualization Mode? Substantial performance improvements can be gained by using a light form of parts and models, called Visualization Mode. Loading an assembly is faster when using Visualization Mode. Parts and models in Design Mode are fully loaded in memory, fully functional, and completely accessible. Notice that the screw branch is expandable and therefore the PartBody is accessible. When parts and models are in Visualization Mode, just a subset of the data is loaded in memory. The remaining data is loaded as needed. Assemblies can be loaded with parts and models: Fully resolved, called Design Mode; or In a light form, called Visualization Mode Parts and model in Visualization Mode are partially loaded in memory and therefore partially functional and accessible. Notice that the screw branch is not expandable and therefore the PartBody is not accessible.
Copyright DASSAULT SYSTEMES Differences between Visualization Mode and Design Mode
Copyright DASSAULT SYSTEMES User Setting : Turning On the Cache (1/2) Turning ON the cache system will cause CATIA to load automatically parts and models in Visualization Mode. 1 Select Options... from the Tools menu Select Cache Management tab 2 3 Select Product Structure branch under Infrastructure node Activate Work with the cache system 4 5 The cache system is not activated until CATIA is restarted
Copyright DASSAULT SYSTEMES User Setting:Turning On the Cache (2/2) Work without the Cache System Work with the Cache System You work with the cgr files: Notice that the branch is not expandable and therefore the PartBody is not accessible. You can edit items Right-clicking selecting Design Mode also switches the part or model to Design Mode:
Copyright DASSAULT SYSTEMES Manually Switching to Design Mode Parts and models can be switched manually to Design Mode. When opening an assembly, parts and models are in Visualization Mode Double-clicking a part or model in an assembly switches it to Design Mode. Note that all instances of the part or model switch to Design Mode when every instance is switched. 1 2a Right-clicking selecting Design Mode also switches the part or model to Design Mode 2b Right-clicking an assembly and selecting Design Mode switches all parts and model in the assembly to Design Mode.
Copyright DASSAULT SYSTEMES Constraining Parts in Visualization Mode Parts and models switch automatically to Design Mode when defining Assembly Constraints. Parts and models switch automatically to Design Mode after assembly constraint is defined. When a constraint icon has been selected, the mouse cursor has a feather on it when hovering over a part or model that is in Visualization Mode. When opening an assembly, parts and models are in Visualization Mode 2 3 Activate the option Automatic Switch to Design Mode 1
Copyright DASSAULT SYSTEMES Automatic Switch to Design Mode 1 This setting allows you to put constraints between components that are on visualization mode 2 Check that the Automatic switch to Design Mode option is activated Around a geometry, the cursor will have this shape Click the geometry 3 Select the Constraint Command Note that constraint commands are available even if no components are on Design mode 4 The Component on which you selected a geometric element is now on Design Mode. Select next element. 5 Last component is now on Design mode and constraint is created. (2)
Copyright DASSAULT SYSTEMES Updating Assembly Constraints and Visualization Mode In order to update constraints, parts have to be in Design Mode. Use Analyze + Dependencies to identify the parts in the constraint network. Select Dependencies… from the Analyze menu Select the component that was repositioned The graph lists the parts and model that should be switched to Design Mode 2 Right-click the part or model and select Expand All to see the components in the network of constraints
Copyright DASSAULT SYSTEMES Summary of Modes You will see a summary of the capabilities of Visualization Mode, Hide and Deactivate. Visualization Mode Deactivation Hide
Copyright DASSAULT SYSTEMES Differences between Modes This table highlights some key reasons for using Visualization Mode, Deactivation, and Hide.
Copyright DASSAULT SYSTEMES To Sum Up... You have seen how to work with large assemblies by: Reordering components to arrange in a logical order Hiding components to reduce clutter and exclude components from assembly drawings Deactivating of Representations to reduce clutter and improve performance while working and to exclude representations from mass property analysis Using Visualization Mode to improve performance when opening assemblies Using Proximity to operate on components within or outside a proximity
Copyright DASSAULT SYSTEMES Designing & Managing Contextual Parts In this lesson you will learn how to design and manage contextual parts Creating Contextual Parts Sketch and Design in Context Knowledgeware and Design in Context Editing Contextually-related Parts Creating Assembly Features Analyzing Contextual Parts Isolating Contextual Parts Saving Contextually-related Documents Deleting Contextually-related Components To Sum Up
Copyright DASSAULT SYSTEMES Creating Contextual Parts You will learn how to design parts that are contextual, or geometrically driven by other components.
Copyright DASSAULT SYSTEMES What are Contextual Parts? Contextual parts have geometry that is driven by other components. Changing geometry in another component can automatically cause changes to a contextual part. This bottom face of the brown part contextually rests on the top face of the green component. The brown face was sketched on the green face. The width of the brown rib is contextually controlled by the edges of the slot in the green component. The sketch of the brown rib was projected from the edges of the slot. The depth of the rib is contextually controlled by the depth of the slot. The depth of the rib is defined as up-to-plane of the slot bottom. This rounded edge and the hole are contextually concentric with the pin in the green component. The sketch of the rounded edge and hole are explicitly constrained to be concentric with the pin.
Copyright DASSAULT SYSTEMES Examples of Contextual Parts in Action Here are some examples of how contextual parts can be driven by changes to other parts. Here the width of the slot has been changed. Notice how the width of the rib is driven by the edges of the slot. Here the depth of the slot has been changed. Notice how the depth of the rib is driven by the depth of the slot. Here the location of the pin has been changed. Notice how the location of the hole is driven by the location of the pin.
Copyright DASSAULT SYSTEMES Contextual Parts in the Tree The tree indicates whether a part is contextual and therefore has External References to other components. External geometry is copied from driving parts to contextual parts that are being driven. The copies are organized in the the External References branch of the part. The green gear signifies the original instance of a part that is contextual (driven by another part). The brown gear signifies the second or subsequent instance of a part that is contextual. It identifies a part out of is context. The reason for distinguishing between the original and subsequent instances of contextual parts is that the geometrical definition of contextual parts is dependant upon neighboring components in the assembly. The white gear signifies the original instance of a part defined in context of an intermediate document.
Copyright DASSAULT SYSTEMES Creating Contextual Elements Contextual elements can be established while designing sketches and features in-context. Turn ON the option Keep Link with Selected Object 1 Sketch on the face of another component to link the sketched face with the other component 2 3 Use geometry of other components to define sketches. For example: Project edges onto the sketch plane Constrain sketch elements to edges of other components Limit features up-to other components 4 Turn ON Keep Link with Selected Object only when you want to create a contextual element. Turn it OFF when you are done.
Copyright DASSAULT SYSTEMES Constraining Contextual Instances of Parts Assembly constraints are forbidden when there is a potential conflict between geometric and assembly constraints. Assembly constraints are always forbidden when any element in a sketch is associative. Here the small brown pad is sketched on a face of the large green component. The pads sketch has external links to the green component. The offset constraint is forbidden because it would cause a potential conflict between the sketch and assembly constraint Attempt to define an assembly offset constraint Here the round blue pad is limited up-to-plane of the small brown component. The pads length has external links to the brown component. Attempt to define an assembly offset constraint The offset constraint is permitted. There is no potential conflicts between the pad length and assembly constraint.
Copyright DASSAULT SYSTEMES Constraining Non-Contextual Instances of Parts Assembly constraints can be used when there is no conflict between assembly and geometry constraints. In the simpliest case this means that assembly constraints can be used on non-contextual instances. This is the original instance of the brown part. In this example, it cannot be positioned using constraints because there would be conflicts between assembly and geometric constraints. This instance of the brown part can be positioned using assembly constraints because no geometric elements of the part were contextually defined within this instance of the part.
Copyright DASSAULT SYSTEMES Sketch and Design in Context You will learn how to use sketches of other parts in the assembly to design parts in context.
Copyright DASSAULT SYSTEMES Why using Sketch in Context ? It can be much more useful to select same sketch to define two different parts than using projections of edges of one part to define the other. In the first case, edges are projected from one part into the sketch of the other, this way creates a lot of external references to synchronize In the second case, the sketch of one part is directly used to create the pad of the other part, now there is only one external reference to synchronize
Copyright DASSAULT SYSTEMES Using a Sketch as an External Reference (1/2) Simply use the sketch of another part to design the new part and take care to keep link with selected object. Edit the Part in which you want to create a pad or another Sketch Based feature 1 Click on Sketch Based Feature you want to edit 2 Select Sketch in another part as profile 3 Key the Length 4 5 Click on OK 6 Pad1 is based on a copy of the selected sketch which is an External Reference
Copyright DASSAULT SYSTEMES Using a Sketch as an External Reference (2/2) Simply use the sketch of another part to design the new part and take care to keep link with selected object. Activate the root assembly and try to move the newly created component 7 8 You will see that the representation becomes red due to the fact that the part is no longer up to date. Now if you click on Update… You will see that position of the component relative to the original sketch impacts its geometry Relative positions of Pad (linked to the external referenceSketch1) and reference planes of the part have changed. Sketch1 remain an exact copy of MasterSketch 9 Reference planes of FixtureCoverWithExternalRef
Copyright DASSAULT SYSTEMES Knowledgeware and Design in Context You will learn how to use parameters of other parts in the assembly to design parts in context.
Copyright DASSAULT SYSTEMES Why using parameters in Context ? It can be interesting to have parameters of a part driven by parameters of another part of the assembly or by parameters of the assembly itself. In this case, we would like this parameter concerning FixtureCoverForKWE component to be equal to … …this other parameter concerning Holder component which himself could be equal to… …this user parameter of the root assembly
Copyright DASSAULT SYSTEMES Linking Parameters of Two Parts in the Assembly (1/3) Creating a relation involving parameter of another part is possible, a linked copy of this parameter will be created under External Parameter node. Edit the part on which you want to create a relation 1 Select Formula icon 2 Select the parameter you want to drive 3 Add a formula 4 Editing the formula, select in an other part of the assembly the driving Parameter 5 2 x (5a) First select the other part in geometry so CATIA will know that you want to select a parameter outside the active part (1) (2) (3) (4) (5a)
Copyright DASSAULT SYSTEMES Linking Parameters of Two Parts in the Assembly (2/3) Creating a relation involving parameter of another part is possible, a linked copy of this parameter will be created under External Parameter node. Validate formula 6 Validate the Parameters edition (5b) The External parameter selection box has appeared (5c) Click on a feature of the other part to focus parameters filter on it and make the parameters appear in 3D (5d) Select driving parameter in 3D (5e) Validate the External Parameter selection (6) (7) 7
Copyright DASSAULT SYSTEMES Linking Parameters of Two Parts in the Assembly (3/3) Creating a relation involving parameter of another part is possible, a linked copy of this parameter will be created under External Parameter node. 8 the component still has a yellow wheel indicating it is not contextual to the assembly A parameter with green light(indicating synchronization with external document) has appeared under External Parameter node Here is the result Created formula is under Relations node Parent and Children box of « Length.1 » parameter displays the link to the external Parameter and indicates its owner document 9
Copyright DASSAULT SYSTEMES Using a Parameter of the Assembly to design a part (1/3) You can also drive a parameter of a Part of the Assembly with a parameter of the Assembly itself. Edit the Part in which you want to create a relation 1 Click on Formulas icon 2 2 x (1) (2) Select the parameter you want to be driven 3 (3) Add a Formula 4 Editing the formula, select a Parameter in the root assembly 5 (5a) First select the root node of the assembly so CATIA will know you want to select a parameter outside the active part
Copyright DASSAULT SYSTEMES Using a Parameter of the Assembly to design a part (2/3) You can also drive a parameter of a Part of the Assembly with a parameter of the Assembly itself. 6 (5d) (5b) The External parameter selection box has appeared (5c) Select driving parameter (5d) Validate the External Parameter selection (6) Validate the formula 7 Validate the Parameter edition (7)
Copyright DASSAULT SYSTEMES Using a Parameter of the Assembly to design a part (3/3) The component using an external parameter in the assembly becomes contextual. the component still have a yellow wheel indicating it is not contextual to the assembly A parameter with green light(indicating synchronization with external document) has appeared under External Parameter node 8 Here is the result Created formula is under Relations node Parent and Children box of « Length.1 » parameter displays the link to the external Parameter and indicates its owner document 9
Copyright DASSAULT SYSTEMES Editing Contextually-related Parts You will learn how to edit parts that drive, or are driven by, other parts.
Copyright DASSAULT SYSTEMES What is Editing Contextually-related Parts ? With regard to editing parts, there are two notions to consider: editing contextual parts that have external references and are therefore driven; and editing parts that drive contextual parts. Here we are editing a contextual part that has External References and is therefore driven by geometry in other components. Here we are editing a part that drives geometry in other parts that are contextual.
Copyright DASSAULT SYSTEMES What is Editing Driving Parts ? Editing a part that drives other contextual parts will cause changes to geometry in the other parts. Here the width of the slot in the driving part has been changed. The width of the rib is driven by the edges of the slot.
Copyright DASSAULT SYSTEMES What is Editing Contextual Parts ? Parts that are contextual (driven) by other components can be edited within or outside the context of the assembly in which the contextual elements were defined. However, you can also edit a contextual part via instances of the part that are not the original instance. This can be useful when defining new contextual elements that are dependant on the position of an instance that is not the original instance. You can also edit contextual parts without opening the assembly, but contextual elements cannot be completely updated because the context (assembly and components) in which the contextual elements were defined is not available. Typically you will want to edit the original instance of a contextual part because often many of the contextual elements were probably define here.
Copyright DASSAULT SYSTEMES Editing Driving Parts After editing driving parts you will have to update contextual (driven) parts in-context of the assembly. Double-click the driving part to be edited 1 Edit the driving part 2 Double-click and update contextual parts that are driven by the edited part 3 You can edit parts outside the context of the assembly, but the assembly must be opened to fully update contextual parts because contextual elements can be updated only in the context in which they were defined.
Copyright DASSAULT SYSTEMES Automatically Synchronizing Changes when Editing Driving Parts You can set an option to synchronize all contextual elements when simply pressing Update. Turn ON the option Synchronize All External References for Update 1 Edit the driving part 2 All contextual elements in driven parts are synchronized with driving parts by simply pressing Update Double-click and update contextual parts that are driven by the edited part 3
Copyright DASSAULT SYSTEMES Manually Synchronizing Changes when Editing Contextual Parts You can set an option to synchronize individual contextual elements. Turn OFF the option Synchronize All External References for Update 1 Edit the driving part 2 Right-click the feature to be updated in the contextual part and select Parent/Children… 3 Right-click the node of interest and select Show All Parents to see External References 4 Right-click on External Reference of interest and select Update Link 5
Copyright DASSAULT SYSTEMES Editing Contextual Parts When editing contextual parts pay close attention to the creation and editing of contextual elements. To edit or create non-contextual elements, double- click any instance of the part 1 Edit the part 2 To edit or create a contextual element, double-click the instance of the part in which the contextual elements is defined (or will be defined) 1 Edit the part 2 Added fillets Added a pad and limited it up-to-surface of the light blue component. This contextual element had to be defined in the right insert instance in order to reference the near-by blue component. You can also make non-contextual changes by opening only the CATPart.
Copyright DASSAULT SYSTEMES Fully Constraining Contextual Parts It is important to fully constrain contextual parts to avoid unintentional distortion of geometry. Here the small brown pad is sketched on a face of the large green component. The pad has external links to the green component. The slot is not fully constrained to the pad Suppose a component is temporarily moved Updating the small brown part projects the contextual sketch back onto the large green part. But the slot appears to be in the wrong location. Fully constraining the slot ensures that it maintains the expected location relative to the small brown pad.
Copyright DASSAULT SYSTEMES Fixing-in-Space Contextual Parts Moving a component can unintentionally cause geometry to move within a contextual part. Here the slot is fully constrained to the pad Suppose a component is temporarily moved Updating the small brown part projects the contextual sketch back onto the large green part. But the pad appears to be in the wrong location. Fix-in-space contextual components To avoid unintentionally moving geometry in contextual parts, ensure that components are in their assembled position before updating contextual parts. To make this easy: Update the assembly to move components back in position before updating contextual parts Unintentionally moving geometry in contextual parts may have adverse affects on scenes and drawings.
Copyright DASSAULT SYSTEMES Creating Assembly Features You will learn how to Create Assembly Features
Copyright DASSAULT SYSTEMES What are Assembly Features ? Assembly features are features that are applied not only to a single part (in Part Design Workbench )but to a set of several parts of an assembly. Available Assembly Features are : SplitHolePocketAddRemove
Copyright DASSAULT SYSTEMES What are affected Parts ? Linked feature is created in affected part Affected parts are parts of the assembly that will be involved in the assembly feature Creation and edition at the level of the assembly Affected parts become contextually linked List of affected parts and linked features in them
Copyright DASSAULT SYSTEMES Specifying Affected Parts Whatever assembly feature you want to create you have to specify affected parts in the first appearing dialog box (Assembly Feature Definition dialog box). Parts of the assembly that are not yet affected by the assembly feature.Select them by clicking them and using Ctrl and Shift keys Parts of the assembly that will be affected by the assembly feature. Select them by clicking them and using Ctrl and Shift keys Affecting Tools: Move all parts of upper field into lower field Move selected parts of upper field into lower field Move all parts of lower field into upper field Move selected parts of lower field into upper field This option allows you to highlight in geometry parts that will be affected
Copyright DASSAULT SYSTEMES Assembly Split You need a surface or a plane to make a split, this surface can belong to one of the affected parts or not. Split 1 Select splitting surface 2 3 Specify affected Parts 4 Select orientation of the split 5 Validate the command 6 Affected parts are splitted
Copyright DASSAULT SYSTEMES Assembly Hole Reference edges When creating an assembly hole, you will create a sketch that will belong to the part containing the reference plane Hole 1 Select reference edges and surface for the Hole 2 3 Validate 5 (a) Specify affected parts 4 Specify hole parameters values and types Reference face (b) 6 The hole goes through all affected parts
Copyright DASSAULT SYSTEMES Assembly Pocket The created pocket goes through all affected parts Pocket is a Sketch based feature that requires an existing sketch, this sketch can belong to one of the affected parts or not. Pocket 1 Select sketch 2 4 Specify pocket parameter values and types 5 Specify affected parts 3 Validate the command 6
Copyright DASSAULT SYSTEMES Adding a Body to an Assembly The body you want to add to several parts can belong to one of these parts? It can even be its Partbody Add 1 Select the body 2 4 Validate the command Specify affected parts 3 5 A linked copy of the body is added to each affected part Hiding all parts except one, you will see that there is an added body to it
Copyright DASSAULT SYSTEMES Removing a Body from an Assembly The body you want to remove from several parts can belong to one of these parts.It can even be its whole partbody Remove 1 Select the body 2 4 Validate the command Specify affected parts 3 6 A linked copy of the body has been removed from each affected part
Copyright DASSAULT SYSTEMES Additional information Existing Split Existing Hole Existing Pocket For every kind of Assembly feature, you can define its feature properties by selecting an already existing Part Design feature Properties of the assembly feature are simple unlinked copies of the Part Design feature properties
Copyright DASSAULT SYSTEMES Analyzing Contextual Parts You will learn how to inquiry about the relationships between driving and driven parts.
Copyright DASSAULT SYSTEMES What is Analyzing Contextual Parts ? To help understand contextual parts, inquires can be made about relationships between driving and driven components, elements, and documents. Here we are inquiring about the relationships between driving and driven components. In this case the top block component is a contextual part that is driven by the bottom block component. In turn, the top block drives the round pad component which is another contextual part. Here we are inquiring about the relationships between driving and driven elements and documents. In this case sketch.1 has some External References to Pad.1 in the bottom block instance of another CATPart.
Copyright DASSAULT SYSTEMES Inquiring about Parent and Child Components Analyze dependencies to understand the relationships between driving and driven components. Select the component to be analyzed 1 Analyze + Dependencies 2 Activate the Associativity option and deactivate the Constraints option 3 Right-click and select Expand All to show the parents and children 4 Parents drive the part being analyzed Children are driven by the component being analyzed
Copyright DASSAULT SYSTEMES Inquiring about Parent and Child Elements & Documents View parent/children to understand the relationships to external elements and documents. Right-click the feature to be updated in the contextual part and select Parent/Children… 1 Right-click on the node of interest and select Show All Parents to see External Reference elements and documents 2 To help you graphically see the relationship between driving and driven elements, temporarily show (un-hide) External Reference elements and then select elements to highlight them.
Copyright DASSAULT SYSTEMES Isolating Contextual Parts You will learn how to severe the contextual relationships between driving and driven parts.
Copyright DASSAULT SYSTEMES What is Isolating Contextual Parts ? At times you may want to severe the contextual relationships between driving and driven parts. Here we are severing all contextual relations in the selected part. Here we are severing an individual contextual relation while leaving other contextual relations intact Contextual elements may be severed because: The part is being released and you want to avoid inadvertent changes The design is stable and you no longer have a need to drive changes from one part to other parts You inadvertently deleted the assembly and/or components that define the context for contextual elements
Copyright DASSAULT SYSTEMES Isolating All Elements in Contextual Parts Isolating a part severs the contextual relationship with the driving components so that changes to driving parts no longer cause changes to the part that was formerly driven. Right-click the part to be isolated and select Isolate Part 1 The geometry in the External References branch transfers to the Open Body branch
Copyright DASSAULT SYSTEMES Isolating Individual Elements in Contextual Parts You can isolate several individual contextual elements so that some elements remain driven. Right-click the feature to be isolated in the contextual part and select Parent/Children… 1 Right-click the node of interest and select Show All Parents to see External References 2 Right-click the External Reference of interest and select Isolate 3
Copyright DASSAULT SYSTEMES Saving Contextually-related Documents You will learn how to save documents that are explicitly or implicitly related to contextual CATParts.
Copyright DASSAULT SYSTEMES What is Saving Contextually-related Documents ? Special attention is required when saving documents that are explicitly or implicitly related to contextual parts. Here the Small Block part references elements in the bottom block instance of the Large Block part Contextual parts reference: Elements in driving CATParts Specific instances of CATParts in specific CATProducts Saving one document with a new file name may require that a related document also be saved
Copyright DASSAULT SYSTEMES Saving Driving CATParts Open the assembly that references the CATPart to be Saved As Save contextual CATParts that are driven by the CATPart that was Saved As After saving a driving CATPart with a new file name you will also need to save the driven CATParts and the parent CATProduct because they reference to the driving CATPart file name. Save As the driving CATPart 1 Click OK to proceed with the save Save the CATProduct that is the parent of the CATPart that was Saved As You might find it more convenient to use Save All As
Copyright DASSAULT SYSTEMES Saving Contextual CATParts Open the assembly that references the CATPart to be Saved As Save the CATProduct that is the parent of the CATPart that was Saved As After saving a contextual CATPart with a new file name you will also need to save the parent CATProduct because it references the driving CATPart file name. Save As the contextual CATPart 1 Click OK to proceed with the save You might find it more convenient to use Save All As
Copyright DASSAULT SYSTEMES Saving Parent CATProducts Open the assembly that is to be Saved As Save contextual CATParts that were defined in-context of the CATProduct that was Saved As After saving a CATProduct with a new file name you will also need to save contextual CATParts that were defined in-context of the CATProduct because these CATParts reference the CATProduct file name. Save As the CATProduct 1 Click OK to proceed with the save You might find it more convenient to use Save Management
Copyright DASSAULT SYSTEMES Deleting Contextually-related Components You will learn how to delete components that are contextual or that drive contextual parts.
Copyright DASSAULT SYSTEMES What is Deleting Contextually-related Components ? Additional options are available for managing data when deleting components that drive contextual parts or when deleting contextual components. Here we are deleting the original instance of a contextual part. We are warned to establish another component as the new original instance. Here we are deleting a component that drives a contextual part. We have the option to delete the contextual components that are driven by the component being deleted.
Copyright DASSAULT SYSTEMES Deleting Driving Components When deleting a component you will be optionally able to delete any contextual components that it drives because contextual components are children of driving components. 2 Press More >> Specify whether or not to delete: Select the component to be deleted and press 3 1 Assembly constraints Contextual components that are driven by the component being deleted Note that Delete all children is not checked.
Copyright DASSAULT SYSTEMES Deleting Contextual Components After deleting a contextual component you will have to isolate any remaining instances or establish one as the new original contextual component. Select the component to be deleted and press 1 Press OK 2 Isolate remaining instances of the contextual part or Change Context 3 If Changed Context, delete any assembly constraints on the instance and move it to the position of the original instance 4
Copyright DASSAULT SYSTEMES To Sum Up... You have seen how to design and manage contextual parts by: Creating contextual parts that have External References to other components Using Sketches as External References to design parts in context of the assembly Using Design Parameters of parts of the assembly to design other parts Editing driving parts thereby causing changes to contextual parts Creating Assembly Features Analyzing contextual parts to understand how they related to other components, documents, and elements Isolating contextual parts so they are no longer driven by other components Keeping external references to file names up-to-date when contextual parts, driving parts, and parent assemblies Deleting contextual parts and driving parts
Copyright DASSAULT SYSTEMES Creating and Using Published Geometry In this lesson you will learn what is published geometry and in which conditions it can be used Creating Published Geometry Using Published Geometry Usefulness of Published Geometry To Sum Up
Copyright DASSAULT SYSTEMES Creating Published Geometry You will learn how to publish geometric elements of components
Copyright DASSAULT SYSTEMES What is Publishing Geometry ? Publishing geometry of a component is associating a name to it so it will be recognized by other documents. There the name Sketch has been affected to Sketch1 feature The published elements will be seeable only in product structure tree
Copyright DASSAULT SYSTEMES What Kind of Geometry can be Published ? Here is the list of geometry you can publish Assumption : elements you want to publish must be useable in MML, it means you can cut or copy them and paste them with the option as result with link (Paste Special) In V5R9, the following elements can be published: ¨ Wireframe features (Points, Lines, Curves, Planes) ¨ Whole sketches ¨ Generative Shape Design features (Extruded Surfaces, Offsets, Joins etc.) ¨ Free Style Design features (Planar Patches, Curves etc.) ¨ Sub Elements of all Geometrical Elements (Faces, Edges, Vertices etc.)
Copyright DASSAULT SYSTEMES Published Elements in the Tree The tree displays names of published elements of a component under its Publication node. When an external reference is connected to a published geometry, it is shown also. Copies of external geometry that are synchronized with published geometry are signaled with the capital P The green gear signifies the original instance of a part that is contextual (driven by another part) Here are the published elements of the component 2ndSurfaces Capital P will be green when the link to external geometry is updated ( ) and be replaced by this red symbol when not synchronized ( ) This node will appear only in the product even if the published component is a part
Copyright DASSAULT SYSTEMES Publishing Geometry (1/3) Publication will concern the active component and is available both in Assembly Design Workbench and Part Design Workbench Activate the component in which you want to publish geometry 1 Select Publication in Tools Menu 2 3 Select geometric element you want to publish As soon as selected, the element is added in the list of published geometry, to modify its published name, select its row then its name cell 4 2 x (3) (4a) (4b)
Copyright DASSAULT SYSTEMES Publishing Geometry (2/3) You can publish as many elements as you want. Key the name you want associate to the selected element 5 6 Repeat step 3 to 5 to publish other elements (5) Click on OK (8) Published geometry is displayed under Publication node of the component It is not mandatory to publish all the geometry in one shot, you can come back later to the Publication of the component and add some other published geometry 7
Copyright DASSAULT SYSTEMES Publishing Geometry (3/3) Part Design Workbench Tools Menu Concerning part components, you can as well publish their geometry from Part Design Workbench as from Assembly Design Workbench Published Geometry in Part Specification tree
Copyright DASSAULT SYSTEMES Changing a Published Element You can also replace the published element by another one select the row Select Publication in Tools Menu 2 Edit the Part or component on which you want to change the published geometry 1 3 select the new element in geometry answer yes to this question 4 5
Copyright DASSAULT SYSTEMES Additional information (1/3) A few setting are useful when publishing geometry When this option is activated, selection of sub-elements(edges,vertex…) is possible When this option is deactivated, only selection of whole features (elements of the tree) is possible This panel allows you to rename published features with their publication name: it can be never, always or after a validation through this kind of dialog box
Copyright DASSAULT SYSTEMES Additional information (2/3) You can overload publication of components in sub assemblies Browse command is available only in Assembly design Workbench and allows you to make a selection among published elements of components of the active assembly Bolt assembly is made of one nut (H_M8_8) and one screw (H_M8_50) which already have published elements We want Bolt publication to concern those already published elements
Copyright DASSAULT SYSTEMES Additional information (3/3) Publication names are by default same as in components but you can modify them Re-Published elements will appear under publication node of the active component
Copyright DASSAULT SYSTEMES Using Published Geometry You will learn in which cases you can use published geometry.
Copyright DASSAULT SYSTEMES When can you use Published Geometry ? Published geometry can be used in any command that requires geometric elements. It means in assembly constraint edition and design in context You can use published geometry to specify geometric elements involved in assembly constraints You can use published geometry as external reference for design in context. In this case, to design MouseCarter Part, we used two published elements of PublishedReferences component : Sketch_Carter and Ref_Surf In this case, we had the setting only use the Published geometry activated and could only select published geometry to define the coincidence constraint
Copyright DASSAULT SYSTEMES User Setting : use published geometry to Constrain (1/3) There is a setting that prevent from using other geometry than published one when creating Assembly Constraints. 1 Select Options... from the Tools menu Select the Assembly Design branch under Mechanical Design node 2 Activate one of the Use published geometry options 4 Select Constraints tab 3
Copyright DASSAULT SYSTEMES User Setting : Use Published Geometry to Constrain (2/3) When imposing the use of published geometry, you can choose between two behaviors Only these two geometric elements are published at the level of the bolt assembly This face is published at the level of the nut component and not at the level of the bolt assembly We have inserted the bolt assembly in another assembly also containing two plates We have selected these two faces in order to put a contact constraint between them The behavior of CATIA wont be the same whether the active option is… …This one… …or This one.
Copyright DASSAULT SYSTEMES User Setting : Use Published Geometry to Constrain (3/3) When imposing the use of published geometry, you can choose between two behaviors With this option… … It will not be possible to constrain because the face of the nut is not published at the required level … Contact constraint will be created because the face of the nut is published at least at a sub-level With this option…
Copyright DASSAULT SYSTEMES Using Published Geometry in Assembly Constraints You can select published geometry to define assembly constraints between components. If all elements involved in the constraint are published... If at least one element involved in the constraint is not published... 1 You can activate one of the use Published geometryoptions 2 Select your constraint 3 Select Elements directly in geometry 1 Select your constraint 2 Select non published elements in geometry 3 Select published element under publication node in the tree or in the geometry (2) (3)
Copyright DASSAULT SYSTEMES User Setting: Published Elements for External References This setting prevent you from selecting other geometry than published one when creating external reference With this option activated, selection of external reference that is not published will not be possible, cursor will have this shape when moving around non published elements. 1 Select Options... from the Tools menu Select the Part Design branch under Mechanical Design node 2 3 Activate the Only use published elements for external selectionoption
Copyright DASSAULT SYSTEMES Using Published Geometry in Contextual Design (1/2) You can select published geometry as external reference to design associative parts in context of the assembly. 1 Activate the Part that you want to design in context 2 x 2 Create a Pad 3 Select as profile the Sketch_Carter publication of Published Reference 4 Select up to surface as type of first limit and select as limit the Ref_surf publication of Published Reference component (you can either select it in the tree or in the geometry) (3a) (3b) (3c) 5 Click on OK 6 Here is the result
Copyright DASSAULT SYSTEMES Using Published Geometry in Contextual Design (2/2) Red lightning indicates that the Wireframe & Surface element is a datum (non associative element that you can not modify) ( ) Published geometry as any other geometry does appear under External Reference node when used to design another part in context of the assembly. 7a Copies of published geometry are under External References node of the part and are associative If the option keep link with selected object was on while editing the part If the option keep link with selected object was off while editing the part 7b Copies of published geometry are under an open Body of the part and are not associative a b Capital P indicates that the element is linked to an external reference that is published ( )
Copyright DASSAULT SYSTEMES Usefulness of Published Geometry You will learn in which cases it can be useful to use published geometry.
Copyright DASSAULT SYSTEMES What are cases when published geometry is useful ? Published geometry becomes useful when you replace a component and when the replaced component is involved in a constraint or driving other contextual components. With published geometry, constraints involving the replaced component can be preserved Without published geometry, constraints involving the replaced component must be reconnected Concerning Design in Assembly context, the best way to replace a component driving geometry of other components is to use Published geometry. In this case, the part containing all the driving geometry(Sketches and Surfaces) has been replaced.
Copyright DASSAULT SYSTEMES Reconnecting a Constraint (1/2) A constraint can become unresolved after a replacement of a component or connected to a wrong geometric element.You have the possibility to redefine geometric elements involved in it. Edit the constraint you want to reconnect 1 2 Expand the dialog box 4 Click on Reconnect 3 Select in dialog box geometric element to reconnect 5 2 x (1) (2) (3) (4)
Copyright DASSAULT SYSTEMES Reconnecting a Constraint (2/2) The Constraint dialog box let you have a look at geometric elements involved in it. Select the new connected geometric element 5 Edited constraint is now connected to the just selected element.You can Click on OK and Update the constraint 6
Copyright DASSAULT SYSTEMES Replacement of a non Published Driving Component (1/3) When you replace a component which contains geometry leading other contextual components of the assembly, driven components will have to be re-designed to be reconnected to the new driving geometry. 1 Those two external references are synchronized (green light) with geometry of the driving component Unpublished References Replace Unpublished References with another Part (PublishedReferences.CATpart) MouseCarter part is contextual to FirstMouse assembly and linked to Unpublished References part 0 2 x A first Warning appears about contextual data that will be lost 2 Click on OK A second Warning appears precising what are the data that are not synchronized 3
Copyright DASSAULT SYSTEMES Replacement of a non Published Driving Component (2/3) When you replace a component which contains geometry leading other contextual components of the assembly, driven components will have to be re-designed to be reconnected to the new driving geometry. 4 7 References are no more synchronized because the component they are referencing is no more in the assembly Contextual data are no more synchronized and you have to re-design the contextual part PublishedReferences is not recognized by contextual geometry of MouseCarter 2 x 5 Edit MouseCarter part 6 Edit Pad1 feature 8 Select sketch of replacing component as Profile Select surface of replacing component as Limit 9 Click on OK
Copyright DASSAULT SYSTEMES Replacement of a non Published Driving Component (3/3) [CTRL] + +[DEL] Re-design parts in context creates other external references, you have to delete the old ones that have become useless. 10 Delete useless External References 11 Contextual part references now only geometry of the replacing component
Copyright DASSAULT SYSTEMES Published Geometry and Assembly Constraints (1/2) When you replace a published component that is involved in assembly constraints, it is possible thanks to published geometry to have automatic reconnection of the constraints. 0 Two constraints in the assembly are connected to published elements of Cric_Screw component 1a Cric_Screw has been replaced with Cric_Screw_2 which has not the same published geometry Constraints are connected to published elements Constraints have become unresolved Cric-Screw Cric-Screw-2 Published Geometry No Published Geometry in Cric_Screw_2 No reconnection
Copyright DASSAULT SYSTEMES Published Geometry and Assembly Constraints (2/2) 0 Two constraints in the assembly are connected to published elements of Cric_Screw component 1b Cric_Screw has been replaced with Cric_Screw_3 which has the same published geometry Constraints are connected to published elements of Cric_Screw Constraints are connected to published elements of Cric_Screw_3 Cric-Screw Cric-Screw-3 Published Geometry You Have to take care of the exact spelling when you publish geometry. Reconnection
Copyright DASSAULT SYSTEMES Published Geometry and Contextual Design (1/2) When you replace a published component which contains geometry leading other contextual components of the assembly, there can be automatic reconnection to the external references thanks to published geometry. 0 1a External references are synchronized with published geometry of Published Reference External references are no more synchronized with any geometry You have warnings about non synchronized geometry Those two published geometric elements of PublishedReferences are used to design MouseCarter PublishedReferences has been replaced with UnPublishedReferences which has not published geometry MouseCartercomponent has been designed contextually to published geometry of PublishedReferences No published geometry in Unpublished References No More Synchronization
Copyright DASSAULT SYSTEMES Published Geometry and Contextual Design (2/2) You Have to take Care of the exact spelling when publishing Geometry. 0 1b External references are synchronized with published geometry of Published Reference External references are synchronized with published geometry of 2ndSurfaces Those two published geometric elements of PublishedReferences are used to design MouseCarter Those two published geometric elements of 2ndSurfaces are used to design MouseCarter PublishedReferences has been replaced with 2ndSurfaces which has the same published geometry MouseCartercomponent has been designed contextually to published geometry of PublishedReferences Re-Synchronization
Copyright DASSAULT SYSTEMES To Sum Up... You have seen how to have and manage published geometry by: Creating Published Geometry Using Published Geometry Usefulness of Published Geometry
Copyright DASSAULT SYSTEMES Course Summary You have seen some advanced functionalities of the Assembly Design Workbench such as : Managing Scenes Measuring, Sectioning, Clash Generating Reports Generating Annotations Working with Large Assemblies Designing Managing Contextual Parts Creating and Using Published Geometry