Copyright DASSAULT SYSTEMES Assembly Design Fundamentals CATIA Training Foils Version 5 Release 8 January 2002 EDU-CAT-E-ASM-FF-V5R8
Copyright DASSAULT SYSTEMES Course Presentation 1 day Targeted audience New CATIA V5 Users Objectives of the Course In this course you will learn to create and manage CATProduct files Prerequisites: CATIA Part Design Fundamentals V5
Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to Assembly Designp 4 2. Assembling Componentsp Positioning Components Using Constraintsp Analyzing Assemblyp Editing Parts in an Assemblyp Working with Componentsp Flexible Sub-Assembliesp 177
Copyright DASSAULT SYSTEMES Introduction to Assembly Design Assembly Design QuickStart Assembly Design Workbench Presentation You will become familiar with the main work on assemblies such as inserting components and constraining them
Copyright DASSAULT SYSTEMES Accessing the workbench Exploring the User Interface Terminology Understanding the general process You will learn about the Assembly Design Workbench by : Assembly Design Workbench Presentation
Copyright DASSAULT SYSTEMES Accessing the Assembly Design Workbench (1/2) To access the Assembly Design Workbench, Start CATIA, then select the Start menu choosing Mechanical Design and Assembly Design. The first time you access the Assembly Design Workbench if no window is open, a new Product is created Assembly Design Workbench icon
Copyright DASSAULT SYSTEMES Accessing the Assembly Design Workbench (2/2) You can insert Assembly Design Workbench in a list of your favorite worbenches and acces it by the Workbench and Worbenches Toolbars. This Assembly Design Workbench can be now acces at the Top of the Start Menu 1 Select Tools / Customize and drop Assembly Design on the Favorites List 2a 2b Acces by Worbench Toolbar Acces by Worbenches Toolbar
Copyright DASSAULT SYSTEMES User Interface: Assembly Design Toolbars Constraint Assembly tree Components Product Structure Move Measure Standard Toolbar Compass Catalog Browser Weld Planner Annotation Annotations Scenes Filter Selection
Copyright DASSAULT SYSTEMES Update Snap Manipulate Explode Coincidence Constraint Contact Constraint Offset Constraint Angle Constraint Fix Component Fix Together Quick Constraint Flexible/Rigid Sub Assembly Change Constraint Reuse Pattern Manage Representation Fast Multi-Instanciation New Component New Product Existing Component Replace Component Measure Between Measure Item New Part Product structure Reordering Generate Numbering Product Init Catalog Browser Measure Inertia Weld Planner Flag Note with Leader Text with Leader User Interface: Assembly Design Icons
Copyright DASSAULT SYSTEMES A component is the general terminology. It can be a part or a assembly (inside an assembly it is called a sub-assembly). An Assembly or Product is a collection of components and constraints them. Assembly documents have the file extension CATProduct. Parts and assemblies have a Part Number (the Name of the component). All instances of a part or assembly have the same Part Number. Each instance can have its own Instance Name that identifies the instance. The active item is the item currently being edited. You make it active by double-clicking on it. Selected items are highlighted. Instance name by default is in parenthesis Active item is in blue Selected component is highlighted Component that is a part Component that is an sub-assembly Part Number Terminology
Copyright DASSAULT SYSTEMES General Process Create a new assembly or open an existing one Add, delete, and replace components Position components using constraints Analyze the assembly Capture various states of the assembly for analyzing the design and preparing for drafting Design parts in the context of the assembly
Copyright DASSAULT SYSTEMES Creating a New Assembly Document Adding Components Assigning Component Properties Saving an Assembly Document Assembling Components You will learn to create a new assembly, add components, assign properties, and save documents
Copyright DASSAULT SYSTEMES You will learn how to create a new Assembly Document Creating a New Assembly Document
Copyright DASSAULT SYSTEMES What is an Assembly Document ? An Assembly Document is a document that is also called a Product because of its file extension.CATProduct. An Assembly or Product is a collection of components blank sheet behind the component icon means that the component is linked with an external file A assembly may contain a another assembly, It is called a sub-assembly Full-clamp.CATProduct In this example, One file sub-clamp.CATProduct for 2 Instances Clamp-pad.CATPart
Copyright DASSAULT SYSTEMES Creating a New Assembly Document Ways to create a new document: 1- Start menu 2- File menu 3- Workbench Icon Assembly Design Workbench icon
Copyright DASSAULT SYSTEMES Product tab Properties Right-click the assembly 4 Key the Part Number and other properties Description information, called Product Properties, can be keyed for the new Assembly Document. Assigning Product Properties
Copyright DASSAULT SYSTEMES You will learn how to add new and existing components to an assembly Adding Components
Copyright DASSAULT SYSTEMES What are Components ? In its simplest form, a Component is a Part or Assembly that has been inserted into an assembly. However, a Component can also be represented by data that is not native to V5, such as V4 models, IGES, STEP, and VRML. The root assembly CATPart component CATProduct component V4 model component Component that exists only in the parent CATProduct and does not have its own file
Copyright DASSAULT SYSTEMES Most visible way is to select the assembly and use the icons in the Product Structure Toolbar 2 1 Fastest way is to right-click the assembly (that will receive the component) and use the Contextual Menu to insert the component 3 Last way is to select the assembly and use the Insert Menu There are three ways to insert components into an assembly: Contextual Menu, Product Structure toolbar, and Insert Menu. Adding Components
Copyright DASSAULT SYSTEMES Right-click the assembly 1 2 3b Double-click the file to insert Existing Component Often you will want to insert existing files as components. Inserted files are not copied into the assembly, they are just referenced by the assembly. You can import more than one component at a time by selecting with the mouse while holding the [SHIFT] or [CTRL] key 3a Choose a filter if desired (for example, CATPart, CATProduct, model, etc) Inserting an Existing Component
Copyright DASSAULT SYSTEMES If you pressed YES, select a point or a component to define the origin of the new part Press YES to define an origin for the new part that is different from the origin point of the assembly, otherwise press NO If you select a component, the origin point of the new part will be the same as the origin point of the selected component If you select a point, the origin of the new part will be exactly this point New parts (CATParts) can be inserted on-the-fly while designing an assembly. Key a Part Number for the new part. This sets the Part Number property. 3 2 New Part Right-click the assembly 1 Inserting a New Part
Copyright DASSAULT SYSTEMES Select Product Structure tab Select Product Structurebranch under Infrastructure node As a shortcut, Part Number properties can be keyed when inserting a new part in an assembly. 4 Activate Manual input Select Options... from the Tools menu Insert a New Part User Setting: Turning ON Manual Input of Part Numbers
Copyright DASSAULT SYSTEMES New assemblies (CATProducts) can be inserted on-the-fly. New Product Command will create a new sub assembly in the selected component but also a new external CATProduct file with the same name. Key a Part Number for the new assembly. This sets the Part Number property. 3 2 New Product Right-click the assembly 1 blank sheet behind the component icon means that the component is linked with an external file Inserting a New Product
Copyright DASSAULT SYSTEMES You can create a special type of component that exists only in the parent CATProduct and does not have its own file. Here are one component that exist in the parent CATProduct and do not have its own file. You can insert in it components Key a Part Number for the new assembly. This sets the Part Number property. 3 2 New Component Right-click the assembly 1 There is no blank sheet behind the component icon : there is no link with an external file. Inserting a New Component
Copyright DASSAULT SYSTEMES It can be useful to insert in your assembly standard components that are only available through Catalogs where they are referenced This screw which is referenced in a catalog needs to be inserted in your assembly Why Inserting a component from a catalog ?
Copyright DASSAULT SYSTEMES In standard toolbar, select the Catalog Browser Open chapters until you get the end chapter in which the element you want is referenced To insert the element inside your document you can either : - drag and drop it in the destination product (A) - make a copy with contextual menu of element and paste in destination product of your document (B) In the Assembly Design Workbench you can insert components from catalog referencing CATPart files or CATProduct files (B) (A) Inserting a component from a catalog
Copyright DASSAULT SYSTEMES Right-click the component to be copied Copy Right-click the assembly in which you want to paste the component After pasting there are two instances of the part Copy-and-Paste is an easy way to duplicate a component. 4 Paste You can also use shortcuts Another way to copy-and-paste a component is to press [CTRL] while dragging the component onto the assembly. [CTRL] key Instance name Copy-and-Paste a Component
Copyright DASSAULT SYSTEMES You will learn how to set component text properties Assigning Component Properties
Copyright DASSAULT SYSTEMES Component Properties can be assigned to distinguish or describe an instance of a component. Component Properties: Component Property values can vary by component. These properties are stored in the parent assemblys CATProduct file. Product Properties: Product Property values are the same for all instances of the component. When the component is a CATPart or CATProduct, these properties are stored in the CATPart or CATProduct. When the component is a V4 model, they are stored in the in the parent assemblys CATProduct file. Instance Name What are Component Properties ?
Copyright DASSAULT SYSTEMES Nodes Customization. Instance Name Part Number Select Tools / Options. Select Product Structure and Nodes Customization 2 3 Activate Customized Display and select yours desired options Assigning Component Properties (1/2)
Copyright DASSAULT SYSTEMES Product tab 5 6 Properties Right-click the component 4 Like other properties, component text properties can be easily accessed from the contextual menu. Component Property values can vary by component. Product Property values are the same for all instances of a part or assembly. Key an Instance Name and/or Description Assigning Component Properties (2/2)
Copyright DASSAULT SYSTEMES You will learn how to save an Assembly Document Saving an Assembly Document
Copyright DASSAULT SYSTEMES There are various ways to save an Assembly Document and child documents. Save will save the active components document and child documents of the active document Save As... is similar to Save, but it allows you to specify the name and folder for the active document Save All will save all the open documents that have been modified since last save Only those documents that have been modified will be saved or proposed to save. Save Management will propose saving all open documents and children of these document, but you can control names and locations of all of them Saving an Assembly Document...
Copyright DASSAULT SYSTEMES Save As… allows a file name and folder to be specified. It allows you to create a brand new document with new internal identifiers. 1 Activate the document to be saved 2 Save As... 4 Specify if you want to regenerate internal identifiers The active CATProduct document and any modified child documents will be saved Regenerating Internal Identifiers will avoid instantiation conflicts with the reference Specify a file name and folder 3 Saving a Document under another Name
Copyright DASSAULT SYSTEMES Save All is an easy way to save all modified documents which are not new or read only documents. 1 Save All 2a If all the documents modified since last save are not new (just created) or read only files, you wont have any message and CATIA will save them All modified open documents will be saved, regardless of which document is active 2b If some of the documents modified since last save are new (just created) or read only files you will have this message And clicking on OK will give you access to the Save All As command 3b Saving all Modified Documents
Copyright DASSAULT SYSTEMES This command is useful to save all the modified or linked documents under selected names and directories Modified Components What is Save Management ?
Copyright DASSAULT SYSTEMES This command is useful to save all the modified documents under other names and directories 1 Make modifications on components In this case, editing the Axis.CATPart file, we have increased the diameter of pad1 from 10 to 13 mm and the AxisNut.CATPart was impacted and modified also. We do have 4 modified documents Save Management (1/5)
Copyright DASSAULT SYSTEMES This command also remind you of what you have modified since last save. 2 Select Save Management … from File menu Number of unsaved modified files since last load If the file has been modified or saved since last load, it is indicated in the State column 3 Select the file you want to save No save as will be performed until you have clicked on OK Names of all files currently used are displayed... … and their paths as well. 4 Select Save as... Save Management (2/5)
Copyright DASSAULT SYSTEMES This command also remind you of what you have modified since last save. Select the destination folder and name of the new created file and select Save 5 Destination Folder Name Save is indicated for the selected document, and Save Auto for its child documents 6 Actions that will be performed when clicking Ok Save Management (3/5)
Copyright DASSAULT SYSTEMES If you click on OK as there are still unsaved files left, CATIA will display this message......and will save only the documents that have a Save or Save Auto Action If you select for the save as a CAT product and if other modified documents are referenced by it, those ones will get Save auto in the Action column and will be saved when clicking Ok Once you have saved a product in a new directory, you have the possibility to save the files referenced by the product into this directory just by clicking on the propagate directory button. This command automatically save impacted files too To know what are documents called by a CATProduct, use Links command from Edit menu or Desk from File menu Save Management (4/5)
Copyright DASSAULT SYSTEMES You can change your mind about the way you save the document thanks to Reset button and it is not mandatory to save a document under another name thanks to Save button. You can get back the original state of the document by selecting it and clicking on Reset You can choose to keep same name and folder for a document and in this case use the save button Save Management (5/5)
Copyright DASSAULT SYSTEMES Freely Moving Components Creating Assembly Constraints Updating Assembly Constraints Creating Quick Constraints Multi Constraints Modes Hiding Constraints Filtering Constraints You will become familiar with positioning components in an assembly using assembly constraints Positioning Components using Constraints
Copyright DASSAULT SYSTEMES You will learn how to use the Compass to freely move components which makes it easier to position components when setting assembly constraints Freely Moving Components
Copyright DASSAULT SYSTEMES How the Compass can be Used ? The Compass can be used to pan and rotate the entire session or freely drag and rotate components in an assembly. Panning and rotating the entire session Freely dragging and rotating components Here the entire session rotated around the X-axis. The rotation is temporary because it is not stored in CATPart or CATProduct documents. Here a component is freely rotated around the X-axis. The rotation may be permanent because it is stored in CATProduct documents. You will find it convenient to freely drag and rotate component to make it easier to create assembly constraints
Copyright DASSAULT SYSTEMES Move your cursor over the little red square of the compass to get this cursor icon 2 3 When the component is selectable, the compass takes the orientation of the geometric element that is under the compass. To select, release MB1. Positioning the Compass to Move a Component The first step in freely moving a component is to position the Compass on a component. Press and hold down MB1 to drag the compass. When moved, the compass takes this shape. If you release MB1 before any component selection, the compass will return to this point. A component is selectable when this point disappears Green highlighted compass means that a component is selected and that you can move it Once a component is selected, you can select any other one by clicking on it, and compass when moving will drag it.
Copyright DASSAULT SYSTEMES Place the compass on a component 2 Rotation around an axis Rotation around the origin of the compass Translation along a plane 3 With MB1 held down, move the component Freely moving a Component using the Compass Here are the basic steps for freely moving a component. Select the type of movement by moving the cursor on the Compass. The highlighted compass elements indicate the available movement. Translation along an axis To move a component while respecting the constraints, press [SHIFT] while pressing MB1 and moving the component. [SHIFT] key
Copyright DASSAULT SYSTEMES Place the compass on a component Translating a Component using the Compass Here are the basic steps for translating a component using the Compass. 2 Right-click on the compass and select Edit... 3a Specify translation distances by: Keying values; or 3b Move the component by: 4 Fix-Together the components if they will not otherwise be constrained Selecting elements using the Measure Distance… button Selecting one of these - and + buttons to move along the U, V, and W directions
Copyright DASSAULT SYSTEMES Place the compass on a component 2 Right-click on the compass and select Edit... 3a Specify a rotation angle by: Keying a value; or 3b Move the component by: Rotating a Component using the Compass Here are the basic steps for rotating a component using the Compass. 4 Fix-Together the components if they will not otherwise be constrained Selecting elements using the Measure Angle… button Selecting one these - and + buttons to rotate around the U, V, or W axis
Copyright DASSAULT SYSTEMES Select a component and the compass will jump to the origin of the selected component 3 Right-click on the compass and select Edit... 4a Specify a position by keying values 4b Move the component by pressing the Apply New Position button Setting the Absolute Position of a Component Here are the basic steps for setting the absolute position of a component. 1 Right-click on the compass and activate Snap Automatically to Selected Object The absolute position in the Compass Edit window is actually the position of the compass, not the position of the component.
Copyright DASSAULT SYSTEMES You will learn how to Position components setting Assembly Constraints Creating Assembly Constraints
Copyright DASSAULT SYSTEMES What are Assembly Constraints ? Assembly constraints provide an intuitive way to position components with respect to each other. The process for creating constraints is described here. 1 Using the Compass, freely drag and rotate components to make adding constraints easier Fix-in-space one component in each assembly that will serve as the base 2 3 Set the position of components by specifying constraints 4 Update (regenerate) the constraints to move the components into position
Copyright DASSAULT SYSTEMES Setting Assembly Constraints... You have several ways to reach constraints icons and several ways to use them 1 To set a constraint between two components, you can either: To reach the icons, you can either use: 2 the Constraint toolbar or the Insert Menu First click on the icon then select the Elements you want to constraint or first select or multi select the elements to constraint and click on the icon Note that in the second case you may have to use the [Ctrl] key to multi select elements whereas in the first case, CATIA will be waiting for a next selection
Copyright DASSAULT SYSTEMES Select Assembly Design branch under Mechanical Design node You control whether or not CATIA automatically updates assembly constraints (positioning of components) after making a change. Manual Update for Assembly Design Activate Manual 3 It is preferable to use Manual Update mode so that components do not move around before being fully positioned (fully constrained). 1 Select Options... from the Tools menu
Copyright DASSAULT SYSTEMES Select the component in the tree or in geometry 3 The component is fixed in space Fix Components that are Fixed in space return to their fixed-in-space position when constraints are updated (regenerated). Fixing a Component in Space (1/2) Its a good idea to fix-in-space one component in each assembly that will serve as the base
Copyright DASSAULT SYSTEMES Fixing a Component in Space (2/2) CRIC_FRAME cant move After Update Drag Cric Frame with the Compass
Copyright DASSAULT SYSTEMES Double-click the Fix constraint 3 Select the More>> button Fix Fixing a Component (1/2) Fix is like Fix in Space, but when constraints are updated, it will only stay at its current place and will not go back to a fixed in space position. 4 Deactivate the Fix in Space option
Copyright DASSAULT SYSTEMES Fixing a Component in Space (2/2) After Update Drag Cric Frame with the Compass
Copyright DASSAULT SYSTEMES Fixing-Together Components Components that are Fixed-Together move as a single entity when updating (regenerating) constraints. 1 2 Select the components to be Fixed-Together Fix Together As a matter of practice, its a good idea to Fix-Together components that will not otherwise be constrained. This will ensure that components are not unintentionally moved out of position.
Copyright DASSAULT SYSTEMES Select Assembly Design branch under Mechanical Design node Fix-Together constraints are used to glue components together. Using the Compass it is possible to unintentionally separate Fixed-Together components. User Setting: Turning On Fix-Together Warning We will activate the warning so that components belonging to a Fix Together constraint are not accidentally moved out of position. 3 Activate warning Select Options... from the Tools menu Use General tab 4
Copyright DASSAULT SYSTEMES You will be warned when attempting to move a component that is Fixed-Together. The warning can be disregarded, but beware that the new position is permanent. Disregarding the Fix-Together Warning For example, when attempting to Snap this component 1 You will see this warning 2 After pressing OK you can continue to move the component 3 But beware that pressing Update will not move the component back in position. It has a new position within the Fix-Together 4 Immediately press Undo if you did not intend to move the component.
Copyright DASSAULT SYSTEMES Creating a Coincidence Constraint (1/2) Coincidence creates alignment that can be coaxial, coplanar, or merged points. coaxial coplanar merged points 1 Coincidence 2 Select the two elements to specify the constraint The constraint is created and the elements are aligned
Copyright DASSAULT SYSTEMES Creating a Coincidence Constraint (2/2) Concerning coplanar alignment, CATIA gives a choice of orientation with two green arrows 1 2 Just click one of those green arrows to invert the orientation of the moving component. Select two planes as geometric elements for the constraint When putting a constraint between two components, the moving component will be the first selected if it is not fixed or fixed in space 1st selection 2nd selection 3 Coincidence 4 Click on OK when the orientation is correct
Copyright DASSAULT SYSTEMES Creating a Contact Constraint Contact mates two planes or faces. 1 Contact 2 Select the two elements to specify the constraint The constraint is created and the elements are mated Notice that the Pre-selection Navigator to select elements that are hidden
Copyright DASSAULT SYSTEMES b Key the offset Creating an Offset Constraint Defines an offset between two elements. 1 Offset 3a Select the orientation 2 Select the two elements to specify the constraint 1st selection Click on Ok when you are satisfied with specifications By selecting an orientation in the Orientation Combo box 4 By clicking on a green arrow 2nd selection
Copyright DASSAULT SYSTEMES b Key the angle Creating an Angle Constraint (1/2) Defines angle, parallelism and perpendicularity. 1 Angle 3a 2 Select the two elements to specify the constraint The constraint is created and the elements are offset Select the type 4
Copyright DASSAULT SYSTEMES Creating an Angle Constraint (2/2) Concerning parallelism between two planes, CATIA gives a choice in the orientation of the components. 1 Angle 3 2 Select two planes as geometric elements to specify the constraint Click OK when satisfied with specifications Select the type Select the orientation By selecting an orientation in the Orientation Combo box By clicking on a green arrow 5
Copyright DASSAULT SYSTEMES Constraint Rules There are a few simple rules that CATIA automatically enforces. (1) This constraint cannot be applied because Product K does not belong to the active component Product B. To define this constraint, Product A must be made active. (2) This constraint cannot be applied because Product E and Product F both belong to a component other than the active component Product B. To define this constraint, Product D must be made active. (3) This constraint can be applied since Product C belongs to the active component Product B and also Product E is contained within Product D which is contained within the active component Product B. You cannot apply a constraint between two components belonging to the same sub-assembly if this sub-assembly is not the active component. You can apply constraints only between the child components of the active component. You cannot define constraints between two geometric elements belonging to the same component
Copyright DASSAULT SYSTEMES This assistant will warn you when you make mistakes putting constraints 2 Assembly Assistant This warning appears when you have switched on the setting only use the published geometry and try to select a non published element for a constraint This warning appears when you try to constrain two elements which belong to the same component 3 (4 ) This warning appears when you try to constrain a component which does not belong to the active product
Copyright DASSAULT SYSTEMES You will learn how to Update assembly constraints Updating Assembly Constraints
Copyright DASSAULT SYSTEMES What is Updating Constraints ? Updating or regenerating constraints is the way to move components into their assembled positions as specified by the constraints. Here the coincidence constraint is not updated Here the coincidence constraint is updated
Copyright DASSAULT SYSTEMES Updating Constraints... The scope of the update can be applied to all constraints or just individual constraints. To update all the constraints and parts of the assembly, click on the Update icon in the Update Toolbar To update an individual constraint, right-click on a constraint in the tree or 3D and select Update Update needed Update done Update needed Update done As a matter of practice, its a good idea to update an assembly before saving it. This will enable improved performance when opening assemblies, especially when using Manual Update. Its also a good idea to update sub-assemblies before activating another assembly. This avoids unintended results when updating constraints
Copyright DASSAULT SYSTEMES Options for Updating Assembly Constraints Updating can be Manual or Automatic. Updating can be applied to the active level of the assembly or all levels. Click on Options in the Tools menu Select the Assembly Design branch under Mechanical Design node Make your choices in Update options Select Manual because Automatic will modify your assembly with each constraint creation
Copyright DASSAULT SYSTEMES Handling Update Errors When Updating, constraints are checked for conflicts where are also called over-constraints. Updating will display the Diagnosis Window if there are problems such as over-constrained components 1 Select a record 2 Select Deactivate or Edit Deactivate is a way to turn OFF a constraint without deleting it. Later the problem can be examined and the constraint deleted or re-activated Edit displays the Constraint Definition window where the constraint can be edited or reconnected to a different element. 3
Copyright DASSAULT SYSTEMES What is analysing Update ? Analyzing Update allows you to know what are constraints and components in your assembly that are updated or not and update them separately directly from where you are constraints and components to be updated Update Analysis Dialog Box
Copyright DASSAULT SYSTEMES Analysing Update (1/2) Thanks to this command you will exactly know what constraints and components are updated or not in your assembly and its sub-assemblies 1 Select Update from Analyze menu Update Analysis dialog box appears and displays: 2 analyzed component In Analyse tab Constraints of the analyzed component that are to be updated Sub Assemblies of the analyzed component that are to be updated Constraints of the sub assemblies that are to be updated Representations of parts that are to be updated
Copyright DASSAULT SYSTEMES Analysing Update (2/2) This command displays also for you a selector which allows you to choose and update any unresolved feature directly from where you are 3 In Update tab List of the unresolved components Select or multi- select in the list the features you want to update 4 Click on Update icon 5 Component is updated in the geometry and does no more appear in the list 6 Once you have finished with Update Analysis, Click on OK This combo Box displays all assemblies and sub_assemblies available for analyze
Copyright DASSAULT SYSTEMES You will learn how to ease the creation of constraints using the Quick Constraint capability Creating Quick Constraints
Copyright DASSAULT SYSTEMES What are Quick Constraints? Quick Constraint is a way to create constraints while letting the system partially decide which type of constraint to create. You simply select two elements and let CATIA decide which type of constraint to create 1 If you wanted a different type of constraint, just click Change Constraint 2 You can set the preference for automatic constraints using Tools + Options (Assembly Design Node + Constraints tab) 3
Copyright DASSAULT SYSTEMES Quick Constraint 2 Select the two elements to specify the constraint Creating Quick Constraints Creating a Quick Constraint is as simple as selecting two elements.
Copyright DASSAULT SYSTEMES Change Constraint 3 Select the type Changing a Constraints Type You can change the type of any Assembly Constraint whether or not it was created using Quick Constraint. 1 Select the constraint
Copyright DASSAULT SYSTEMES You will learn how to choose the way you will put several constraints one after the other Multi Constraints Modes
Copyright DASSAULT SYSTEMES When you have double clicked on a Constraint command, you will have three ways to put the several constraints: What are Multi Constraint Modes? Default Mode when no geometric element is shared between constraints Stack Mode when a geometric element is shared between all the constraints Chain Mode when several geometric elements are each shared between two constraint
Copyright DASSAULT SYSTEMES This mode allows you to select two after two, geometric elements involved in constraints Select Default Mode in MultiConstraint Mode Toolbar 2 Double click on the Constraint you want to apply several times 3 Default Mode for Multi Constraint (1) Select elements one after the other, you will see that as soon as two elements are selected, a constraint is created between them Once you have obtained all the needed constraints, you must deactivate the command by clicking on it 4 (4)
Copyright DASSAULT SYSTEMES Once you have obtained all the needed constraints, you must deactivate the command by clicking on it 1 This mode allows you to select only once a geometric element that is shared between several constraints of the same type Select Stack Mode in MultiConstraint Mode Toolbar 2 Double click on the Constraint you want to apply several times 4 Select the first geometric element that will be shared between the next created constraints 3 Stack Mode for Multi Constraint (1) 5 Select one after another geometric elements you want to constrain with the shared element. (3) (4) (5)
Copyright DASSAULT SYSTEMES This mode allows you to select only once the shared element between two consecutive constraints Select Stack Mode in MultiConstraint Mode Toolbar 2 Double click on the Constraint you want to apply several times 3 Chain Mode for Multi Constraint (1) Select one after t-he other the elements to be constrained, specifying at each time the parameters values, and each next constraint will take as first geometric element the last one selected for the previous constraint Once you have obtained all the needed constraints, you must deactivate the command by clicking on it 4 (4) (3)
Copyright DASSAULT SYSTEMES You will learn how to Hide assembly constraint symbols in the geometry Hiding Constraints
Copyright DASSAULT SYSTEMES What is Hiding Constraints ? Hiding constraints can help remove clutter. Cluttered screen Un-cluttered screen You can Hide individual constraints You can also Hide a bunch of constraints at the same time
Copyright DASSAULT SYSTEMES Hiding Constraints... You can hide constraints as any other component of your assembly just by selecting them and clicking on Hide/Show icon You can either select the constraint in the tree, in the geometry or with selecting tools such as Search Hide/Show icon is either reachable on View toolbar and View menu or through the contextual menu of the constraint
Copyright DASSAULT SYSTEMES Hiding Individual Constraints Hiding can be limited to one or more selected constraints. 1 Select a constraint in the tree or 3D 2 Select Hide/Show You can hide more than one constraint at a time by selecting with the mouse while holding the [CTRL] key. [CTRL] key
Copyright DASSAULT SYSTEMES Hiding Constraints relative to a Component An option in contextual menu of the component can be used to find and select all the constraints which involve the component and can be subsequently hidden. 1 Right click on the component in the tree 2 Select Components Constraints 3 4 Select Hide/Show Constraints relative to the component are selected
Copyright DASSAULT SYSTEMES Hiding all the Constraints of an Assembly You can hide at once all the constraints of an assembly. 1 Select first Constraint under Constraints node in the tree 2 Keeping Shift Key Pressed, select last constraint under Constraints node 3 Select Hide/Show [Shift] key (1) (2)
Copyright DASSAULT SYSTEMES You will learn how to filter Hide assembly constraint symbols in the geometry Filtering Constraints
Copyright DASSAULT SYSTEMES What is Filtering Constraints ? Constraint filter Options... Displays the constraints according to their type Defines the filter level: if Conditional Filter is selected, the filters below are available Displays the constraints according to their status: Verified only, unverified only or all of them Displays the constraints on the active product
Copyright DASSAULT SYSTEMES Filter Constraints on an Active Product Show only constraints of the active Product
Copyright DASSAULT SYSTEMES Select or deselect the desired types Filter by Type (1/2) You can filter and displays constraints according to their type
Copyright DASSAULT SYSTEMES Filter by Type (2/2)
Copyright DASSAULT SYSTEMES You will become familiar with tools created to analyze an assembly Measuring Computing Clash and Clearance Viewing Mechanical Properties Analyzing Constraints Analysing Degrees of Freedom Analyzing an Assembly
Copyright DASSAULT SYSTEMES You will learn how to measure an assembly Measuring an Assembly
Copyright DASSAULT SYSTEMES Distance and angles can be measured. Individual geometric elements can also be measured. What is Measuring an Assembly ? Measuring distance between the axis of two different components Measuring the length of a line
Copyright DASSAULT SYSTEMES Measure Between 2 Optionally define how you want to measure 3 Select the reference and target elements 4a Minimum distance and angle are displayed in 3D and in the results window 4b The window also displays components of distance vector and coordinates of Reference and Target points Measuring between Items (1/2) You can measure angle and distance between geometric entities. To select sub-elements like the axis of a hole, right-click and select Other Selection...
Copyright DASSAULT SYSTEMES Right click the geometric element 2 Select Other selections 3 Expand the tree appearing in Other selections dialog box 4 Select the sub element Measuring between Items (2/2) You can select sub elements thanks to Other selections option. 5 Sub element is now under selection in CATIA and highlighted
Copyright DASSAULT SYSTEMES Measure Item 2 Select the item Measuring Items You can measure geometric items. 3 Properties of the selected item are displayed in 3D and in the results window Click the Customize… button to see the information that is available for each type of element
Copyright DASSAULT SYSTEMES Measure Inertia 2 Select the item Measuring Inertia You can measure Inertia of components or geometric elements. 3 Properties of the selected item are displayed in 3D and in the results window Click the Customize… button to see the information that is available for each type of element
Copyright DASSAULT SYSTEMES When Creating your measure, activate the Keep Measure option 2 Each created measure will be kept in the tree… Keeping Measure You can keep results of measures as features in the tree … And in the Geometry… And be saved in the CATProduct file Those measure features contain parameters that can be used in any formula of the Knowledgeware
Copyright DASSAULT SYSTEMES You will learn how to test for clash and clearance violations between components Computing Clash and Clearance
Copyright DASSAULT SYSTEMES Clash analysis is used to check for interference between components. Clearance analysis is used to ensure the proper clearance between components. What is Clash and Clearance ? A clash violation occurs when one component penetrates another component A clearance violation occurs when a minimum distance between components is not respected For more powerful clash and clearance analysis, see the DMU Space Analysis workbench
Copyright DASSAULT SYSTEMES Multi-select the components using the [CTRL] Key 3b Click on Apply 4b Clashes are highlighted 1 Click on Compute Clash in the Analyze menu 3a Select Clash from the list 4a Clash violation is signaled in the window The Assembly Design workbench enables checking for interference between two components. Computing Clash between 2 Components
Copyright DASSAULT SYSTEMES Multi-select the components using the [CTRL] Key 1 Click on Compute Clash in the Analyze menu Select Clearance in the list Key in the clearance value 3b 3a 2 3c Click on Apply 4b Components not respecting the clearance are highlighted 4a Clearance violation is signaled in the window The Assembly Design workbench enables checking to ensure clearance is respected between two components. Computing Clearance between 2 Components
Copyright DASSAULT SYSTEMES You will learn how to check the mechanical properties of parts and assemblies Viewing Mechanical Properties
Copyright DASSAULT SYSTEMES Mechanical Properties indicate physical characteristics of parts and assemblies. What are Mechanical Properties ? Structural Properties are assigned to materials Materials are assigned to parts Mechanical Properties are computed based on material that is assigned to parts 1 2 3
Copyright DASSAULT SYSTEMES Mechanical Properties can be viewed, but not directly modified. Viewing Mechanical Properties Right-click the assembly 12 Properties 3 Mechanical tab
Copyright DASSAULT SYSTEMES Materials can be applied to components directly from the Assembly Design Workbench. Applying a Material to a Part of the Assembly Select Apply Material icon 1 2 Drag and drop the material onto the component 3 Drop the material when you have this cursor on the component you want to apply the material to. Material is applied and appears in specification tree of the part
Copyright DASSAULT SYSTEMES You will learn how to analyze the status of constraints and the relationship between constraints and components Analyzing Constraints
Copyright DASSAULT SYSTEMES You will analyze a constraint by seeing its status and by identifying the components involved in it. What is Analyzing Constraints ? A constraint is set between at less two components (except for the fixing constraint), you will see them thanks to its display in specification tree or with the dependences tree Those are the components involved in the constraint (CRIC_TOP.1 and Set1.1 are linked with Surface Contact.6) A coincidence constraint can ( as any other type of constraint ) be : Not updated DeactivatedUnresolvedActive In the Tree In Constraint Analysis Dialog Box Constraint Status can be seen :
Copyright DASSAULT SYSTEMES Constraints can be examined to determine their status and how they relate to other components. Analyzing Constraints... The status of constraints can be viewed to the tree A global perspective of constraint status can be viewed in an on-line report The relationships between components and constraints can be dynamically navigated
Copyright DASSAULT SYSTEMES Analyzing Constraints in the Tree The status of constraints can be viewed in the tree. This symbol indicates that the constraint not updated. This symbol indicates that the constraint is deactivated. This symbol indicates that the constraint is unresolved which means either: The constraint is broken (for example, related component deleted); or The constraint is impossible (for example, geometry modified and constraint no longer possible) Select the plus-sign (+) on the Constraints branch to expand the branch 1
Copyright DASSAULT SYSTEMES Analyzing Constraints in the on-line Report 2 Select Constraints… from the Analyze menu Activate the assembly to be analyzed A global status of constraints can be viewed for the active assembly. The Constraints Analysis Window appears and shows the status of the constraints 1
Copyright DASSAULT SYSTEMES Analyzing Constraint Relationships The relationship between constraints and components can be dynamically navigated. 2 Select Dependence… from the Analyze menu Activate the assembly to be analyzed 1 3 Right-click on a constraint and select Expand All to see which components are associated with the constraint You can also expand a component, even the top assembly
Copyright DASSAULT SYSTEMES You will learn how to analyze Degrees of Freedom on a component Analyzing Degrees of Freedom
Copyright DASSAULT SYSTEMES There are 6 Degrees of Freedom for each instance: 3 Degrees of Rotation and 3 Degrees of Translation What is a DOF ? When there is no constraint on a instance. All Degrees are free When a instance is full-constrained, all Degrees are fixed. If you decide for example to fix a instance, there is no degree of freedom
Copyright DASSAULT SYSTEMES Degrees of freedom Analysis You can select one instance and analyse its degrees of freedom
Copyright DASSAULT SYSTEMES You will learn how to edit parts in-context of an assembly Designing in-context of an assembly without external links Aligning Components for Sketching Using Local Axis for Snapping Editing Parts in an Assembly
Copyright DASSAULT SYSTEMES You will learn how to design a part in-context of an assembly without External References Designing in-context of an Assembly without external links
Copyright DASSAULT SYSTEMES Part features and sketches can be design in-context of an assembly. What is Designing in-context of an Assembly ? Parts can be sketched on the face of neighboring components 3D elements from other components can be projected onto and intersected with the sketch plane Sketch constraints can be defined using elements in other components Features can be limited up-to other components Parts can be edited in context of an assembly
Copyright DASSAULT SYSTEMES Designing in-context of an Assembly without links Part features and sketches can be design in-context of an assembly with the Keep link with selected object option deactivated. No associativity in case of Design modifications Design in-context : these sketch elements are copied from the Reference Part ones into a Open Body.
Copyright DASSAULT SYSTEMES Designing in-context of an Assembly with links Part features and sketches can be design in-context of an assembly with the Keep link with selected object option activated. For more details, see the Assembly Design Advanced Course to design in-context with associativity. Notice the green color of the wheel icon Keep links in case of design modification
Copyright DASSAULT SYSTEMES Double-click the branch that is just below the one you expanded The part is active and the last workbench used to edit a CATpart document is displayed Editing a Part In order to edit a part, the part must be activated. Select the plus-sign (+) next to the part you want to edit 1 The branch represents the instance of the part The branch represents the actual part Another way to easily activate a part is to double-click the part in 3D
Copyright DASSAULT SYSTEMES Select the Sketcher icon in the Part Design workbench 4 Select a face on a component Sketching on the Face of a Component A part can be sketched on the face of another component. 5 Sketch on the face Notice that a copy of the face appears in the Open_body of the active part
Copyright DASSAULT SYSTEMES Select one element from the sketch and another from a neighboring component 7 Define a constraint just as you would when constraining two elements within the sketch Defining Sketch Constraints using other Components Sketch constraints can be defined using elements in other components. Notice that a copy of the element from the other part appears in the Open_body of the active part
Copyright DASSAULT SYSTEMES Project 3D Elements 3 Isolate the projected element from the original element by right-clicking the element and selecting xxx.object + Isolate Projecting 3D Elements onto the Sketch Plane 3D elements from neighboring components can be projected onto the sketch. 2 Select an element from a neighboring component You can also project other types of elements such as points and faces (which projects the edges of the face)
Copyright DASSAULT SYSTEMES Intersecting 3D Elements with the Sketch Plane 3D elements from neighboring components can be intersected with the sketch. 1 Intersect 3D Elements 2 Select an element from a neighboring component You can also intersect other types of elements such lines (which creates a point at the intersection) 3 Isolate the projected element from the original element by right-clicking the element and selecting xxx.object + Isolate
Copyright DASSAULT SYSTEMES Limiting Features up-to other Components You can select geometric elements of other components to design features of your part 1 When defining features such as a pad, set the limit up-to-plane or up- to-surface 2 Select a face in a neighboring component
Copyright DASSAULT SYSTEMES You will learn how to align components so that the sketch plane of one component is parallel to another component that is being sketched on Aligning Components for Sketching
Copyright DASSAULT SYSTEMES Sometimes it is convenient and intuitive to align a part that is being sketched with another component so that the sketch is parallel to the other component. What is Aligning Components ? However, sometimes the part being sketched is not oriented so that it is parallel to the component being sketched on When designing in-context you will find it useful to sketch on the face of another component The Snap function can be used to align the part being sketched so that it is parallel to another component In this case we want to sketch a new part on this face 1 2 3
Copyright DASSAULT SYSTEMES Snapping Components into Alignment The Snap function provides a quick way to align components. Snap 1 2 Select the planes and/or faces that are to be made coplanar 3 Click on the green arrow to change the orientation of the moved part 4 Click somewhere in the geometric space to validate the position 5 Components are correctly positioned relative to each other Notice that first selected component will move
Copyright DASSAULT SYSTEMES You will learn how to use local axis to snap components to each other Using Local Axis for Snapping
Copyright DASSAULT SYSTEMES Why Snapping Local Axis? The Snap function provides a quick way to align components but lines and points in the geometry are needed for that.If you do not have any, Local Axis are useful In this assembly, to build the cylindrical part perpendicular to the upper surface of the other part, we needed Local Axis
Copyright DASSAULT SYSTEMES Snapping Local Axis of Components into Alignment The Snap function provides a quick way to align components and you can select planes, axis and point of Local Axis System to perform it. Snap 1 2 Select the planes and/or faces that are to be made coplanar 3 Select the green arrow to invert the direction of the component 4 Click somewhere else in the geometry to validate 5 Planes are now aligned 6 For snapping you can select on Local Axis System: PlanesAxis Points
Copyright DASSAULT SYSTEMES You will learn how to manage components of your assemblies Using Visualization mode Deleting Components Duplicating Components Replacing Components Restructuring Components Reordering Product Structure Working with Components
Copyright DASSAULT SYSTEMES You will learn how to use Visualization Mode to improve performance. Using Visualization Mode
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 Turning ON the cache system will cause CATIA to automatically load parts and models in Visualization Mode when opening assemblies. User Setting : Turning On the Cache (1/2) 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 Parts and models can be manually switched to Design Mode. Manually Switching 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 any 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 Parts and models automatically switch to Design Mode when defining Assembly Constraints. Constraining Parts in Visualization Mode Parts and models automatically switch 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 This setting allows you to put constraints between components that are on visualization mode 2 Automatic Switch to Design Mode 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 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 Updating Assembly Constraints and Visualization Mode
Copyright DASSAULT SYSTEMES You will learn how to delete components and their associated constraints Deleting Components
Copyright DASSAULT SYSTEMES Removing a component from an assembly is called deleting the component. What is Deleting Components ? Deleting a component removes the component from the assembly But deleting a component does not delete the referenced file from the hard drive
Copyright DASSAULT SYSTEMES Press the key Uncheck this box to not delete the assembly constraints associated with the component Deleting a Component When deleting a component, you decide whether or not to delete the constraints associated with the component. In the tree of 3D, select the component to be deleted 3 These constant will be deleted Components can also be deleted by right-clicking the component and selecting Delete from the contextual menu 1
Copyright DASSAULT SYSTEMES You will learn how to duplicate components Duplicating Components
Copyright DASSAULT SYSTEMES Right-click the component to be copied Copy Right-click the assembly in which you want to paste the component After pasting there are two instances of the part Copy-and-Paste a Component Copy-and-Paste is an easy way to duplicate a component. 4 Paste You can also use shortcuts Another way to copy-and-paste a component is to press [CTRL] while dragging the component onto the assembly. [CTRL] key Instance name
Copyright DASSAULT SYSTEMES Setting Copy-and-Paste Options You control whether constraints are copied-and-pasted when copying-and-pasting components. 1 Select Options... from the Tools menu Click Assembly-Design 2 3 Set the Paste components option to either: 4 Without the assembly constraints With the assembly constraints only after a Cut Copying constraints when copying a component will cause both components to be constrained in exactly the same way. This is okay, but you will have to manually edit or delete and recreate some constraints. Two Lug Nuts with a coincidence constraint to the same Stud Select Constraints Tab
Copyright DASSAULT SYSTEMES Instanciating Multiple Instances of a Component Components can be duplicated along a line. Beware that in this in case the components are not automatically constrained. Define Multi Instanciation 1 Select a component 2 Specify the number of instances and space between them 3a Select a direction 3b Use the Fast Multi Instanciation icon to re-use the Default multi- instanciation definition
Copyright DASSAULT SYSTEMES Creating a Pattern of Components (1/3) Patterns in parts can be used to automate the duplication of a component and creation of constraints. Reuse Pattern 1 Select a component Select the pattern to follow Specify the constraints to re-use 2 3a 3b Notice that the constraints for the duplicate components are correct.
Copyright DASSAULT SYSTEMES Creating a Pattern of Components (2/3) Keep link with the pattern…. The reuse pattern command create an Assembly Feature « Pattern » that is associative in case of modification of the part design pattern that was used as input. Component to instantiate Pattern Disk Lug Nut
Copyright DASSAULT SYSTEMES Creating a Pattern of Components (3/3) When you modify the instances in the design pattern, the assembly pattern is « out of date » and the update of the assembly will add/delete generated components
Copyright DASSAULT SYSTEMES Symmetrical Sub-Assemblies
Copyright DASSAULT SYSTEMES What Symmetrical Sub-Assembly ? Create a symmetrical sub-assembly from an original one, based on a symmetry plane. Generation: The result of the generation of a symmetrical sub-assembly is another sub- assembly with a similar product structure. The User chooses between both options, The parts building the symmetrical sub-assembly are : Either a symmetrical part from the source part. This involves creating a new part, outside any assembly context, with a new « PartNumber ». A typical example is the left door in a car, relatively to the right door. Either a new instance of the source part, in a position symmetric to the original part. A typical example is a cars front left wheel, relatively to the front right wheel.
Copyright DASSAULT SYSTEMES Creating a Symmetry on Component (1/2) Select the icon You can find it on the Product Structure Tools Toolbar 1 2 The Assembly Mirror Wizard dialog box appears: The reference plane is now displayed in green. Select the mirror plane 3 Select the sub-assembly to be mirrored
Copyright DASSAULT SYSTEMES Creating a Symmetry on Component (2/2) By default, CATIA create a new component by each Part 4 Results: 4 components created New Part Number
Copyright DASSAULT SYSTEMES Create New Instances On this following example, you need to create new instance about the Wheel and Disk Parts. Select one component and activate Symmetry wih new instance option New instance When the user chooses to create a new instance of a source part, at a mirrored position, a new instance is created in the symmetrical sub-assembly, then its position is chosen with respect to the symmetry plane, at creation time. Only reference plane of the part can be used in determining the transformation
Copyright DASSAULT SYSTEMES Keep Links Once the symmetrical sub-assembly has been generated, changes in the source sub-assembly shall allow updating it « FORM » associativity: A change in geometrical shape of the source part leads to update the symmetrical part. « POSITION » associativity: A change of relative position of a component of the source sub-assembly leads to updatethe position of the symmetrical component in the symmetrical sub-assembly. « STRUCTURE » associativity: A change in structure of the source sub-assembly (adding/removing components) leads to update the structure of the symmetrical sub-assembly.
Copyright DASSAULT SYSTEMES You will learn how to replace components Replacing Components
Copyright DASSAULT SYSTEMES Replacing a component is a shortcut to deleting a component and adding another component in its place. What is Replacing Components ?
Copyright DASSAULT SYSTEMES Replacing a Component A single instance of a component can be replaced. Right-click the component to be replaced 1 2 Replacement Component 3b Double-click the file 3a Choose a filter if desired (for example, CATPart, CATProduct, model, etc) Dont forget that you have to manually revise any references (such as constraints) to the component that was replaced Notice that the instance name is not modified This option make replaced all instances that have same reference as selected component
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 You will learn how to move components from one assembly to another assembly while maintaining constraints Restructuring Components
Copyright DASSAULT SYSTEMES Sometimes it is necessary to restructure components by moving components from one assembly to another assembly. What is Restructuring Components ? Move to sub-assembly Move to parent assembly Move to peer assembly
Copyright DASSAULT SYSTEMES Setting Cut-and-Paste Options You control whether constraints are maintained when moving a component to another assembly. 1 Select Options... from the Tools menu 2 Select Assembly Design node under Mechanical Design branch Set the Paste components option to: 3 With the assembly constraints only after a Cut
Copyright DASSAULT SYSTEMES Moving a Component to Another Assembly Components can be dragged to another assembly while maintaining constraints. 1 Click the component and hold down the left mouse button 2 Drag the mouse over the target assembly and release the mouse button In this case two constraints are also moved to the target assembly because both associated components exist in the target assembly The component is moved to the target assembly 3
Copyright DASSAULT SYSTEMES You will learn how to change the order in which components are displayed in the tree Reordering Product Structure
Copyright DASSAULT SYSTEMES What is Reordering Product Structure? This command allows you to reorder components display in the tree under a selected product Tree to reorderReordered tree a b
Copyright DASSAULT SYSTEMES This command allows you to reorder components display in the tree under selected product 3a Product Structure Reordering (1/2) Select the Graph Tree Reorder Command Select the Product in which you want to reorder components (2) Select the Component you want to reorder (3) 4a Click one of these arrows to move the selected component of one level
Copyright DASSAULT SYSTEMES b Select another component to reorder 4b Click this icon and click the component above which you want to place the selected component 5 Click Ok to get the reordered tree 6 Here is the reordered tree Product Structure Reordering (2/2) There are two ways available to reorder components in the tree
Copyright DASSAULT SYSTEMES Flexible Sub-Assemblies What can you do with Flexible Sub-Assemblies? Managing Flexible Sub-Assemblies with Several Levels Propagating Position to Reference You will become familiar with positioning components in an assembly using assembly constraints Flexible Sub-Assemblies
Copyright DASSAULT SYSTEMES You will learn how to get a Flexible Sub-Assembly and to see impacts on positioning matrix and constraints Flexible Sub-Assemblies
Copyright DASSAULT SYSTEMES A flexible Sub-Assembly is a Sub-assembly whose child components can be moved disregarding the fact it is not the active component. Relative positions of its child components can be different than those stored in the reference CATProduct File. What are Flexible Sub-Assemblies? Icon with purple wheel means Flexible Sub- Assembly There you can see four instances of Leg sub-Assembly : notice that components of leg are not positionned the same way in each instance, it is possible because instances of Leg Assembly are flexible Leg.1 Leg.2 Leg.3 Leg.4 Relative positions of components in the reference of the Sub- Assembly Leg
Copyright DASSAULT SYSTEMES Rigid/Flexible sub-Assembly command is a switch: you can have components of the sub- assembly in same relative position as in the reference CATProduct (Rigid Sub-Assembly) or in relative positions that are contextual to the assembly (SoftSub-Assembly) Select the Sub-Assembly 2 Flexible/Rigid Sub-Assembly 3 Making a sub-Assembly flexible (1) Selected Sub- Assembly is now Flexible Note that you can make the sub-Assembly rigid again using the same icon Purple wheel means means flexible instance (2)
Copyright DASSAULT SYSTEMES You can position components by freely moving them with the compass or by constraining them. In both cases Rigid/Flexible state is important. Freely moving Components Positioning Components of a Flexible Sub-Assembly(1/2) In this case the compass has been put on a component of a Rigid Sub-Assembly. In this case the compass has been put on a component of a Flexible Sub-Assembly. Root assembly is active, so the compass will drag the whole Rigid Sub-Assembly Root assembly is active, but as the sub-Assembly is flexible, the compass will only move the selected component
Copyright DASSAULT SYSTEMES Relative Positions of components of a Flexible Sub-Assembly are stored with instance informations in containing CATProduct. Constraining Components Positioning Components of a Flexible Sub-Assembly(2/2) When you create a constraint between : a component of the active assembly … … And a component of a rigid sub-assembly … Constraint involves the component and the whole Rigid Sub-Assembly And a component of a Flexible sub-assembly … a component of the active assembly … When you create a constraint between : Constraint involves the component and the selected component of the Flexible sub-assembly flexible instance
Copyright DASSAULT SYSTEMES There are two types of structure when you use flexible Sub-Assemblies What is Mechanical Structure? Product Structure Tree shows which assemblies and sub-assemblies Parts and constraints belong to Mechanical Structure Tree shows what components you can constrain together (they are at the same level) Components and constraints of Flexible Sub-Assemblies are considered as direct childs of the root assembly in mechanical Structure tree Flexible Sub-assembly does not exist anymore in Mechanical Structure tree Product Structure Mechanical Structure
Copyright DASSAULT SYSTEMES There are two types of structure when you use flexible Sub-Assemblies Viewing Mechanical Structure 1 Activate the Assembly or Sub-Assembly you want to analyze 2 Select Mechanical Structure from Analyze menu Mechanical Structure of the instance Mechanical Structure of the reference Combo box
Copyright DASSAULT SYSTEMES You will learn to manipulate Flexible Sub-Assemblies What can you do with Flexible Assemblies?
Copyright DASSAULT SYSTEMES Once the sub-assembly is flexible, Numerical Value, Activity status, Orientation (Same or Opposite), Driven/Driving property can be overload to modify locally its internal definition, or deal with under/over constrained situations What can you Overload with Flexible Sub-Assemblies? Flexible Sub-Assembly Rigid Sub-Assembly
Copyright DASSAULT SYSTEMES Activate / Deactivate Status Concerning methodology using flexible sub-assemblies, you can change the Activity Status on a constraint flexible Sub-Assembly
Copyright DASSAULT SYSTEMES Numerical Value On a flexible sub-assembly, you can modify numerical values without impacting others instances Flexible Sub-Assembly Rigid Sub-Assembly
Copyright DASSAULT SYSTEMES Propagating Position to Reference
Copyright DASSAULT SYSTEMES Propagating Position (1/2) 1 Modify position of the Flexible Base Instance. : flexible instance : rigid instance This Product contains 2 sub-assemblies : Base.CATProduct Base_unit.CATProduct Flexible sub-assembly
Copyright DASSAULT SYSTEMES Apply overloaded position to reference Select the flexible Base instance MB3+ ….object+Propagate position to reference Propagating Position (2/2) Result : all rigid instances should have the same position than the flexible one. Internal position of flexible instances are not impacted by the command. V5R8
Copyright DASSAULT SYSTEMES To Sum Up... You have seen CATIA V5 Assembly Design User interface: How to access the workbench Its user interface and tools The terminology that will be used The general design process... and Basic functions: How to add components How to position components How to analyze an assembly How to design a part in context of the assembly How to manage components How to manage Flexible Assembly Sum Up …