Copyright DASSAULT SYSTEMES CATIA Tools for Proficient Users CATIA Training Foils Version 5 Release 8 January 2002 EDU-CAT-E-PRO-FF-V5R8
Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will learn how to use tools dedicated to CATIA V5 Project Master such as the Catalog edition and Powercopy management 1 day Targeted audience Advanced Users Prerequisites: CATIA Basics, Sketcher, Part Design
Copyright DASSAULT SYSTEMES Table of Contents 1. Standart Knowledge Toolsp Using CATIA V5 Layers and Filtersp Customizing CATIA V5 User interfacep Creating and Using powercopies p Creating Catalogs of Components p From CATIA V4 to CATIA V5 Basics p 152
Copyright DASSAULT SYSTEMES You will learn how creating and using standart knowledge tools : Standart Knowledge Tools Introduction to Standart Knowledge Tools Creating and Using Parameters Creating and Using Formulas Creating and Using Design Table
Copyright DASSAULT SYSTEMES Accessing the Tools Seeing Terminology Checking Settings You will learn about the Standart Knowledge Tools : Introduction to Standart Knowledge Tools
Copyright DASSAULT SYSTEMES Accessing Standart Knowledge Tools From Knowledge Toolbar: From Tools + Formula… 1 2 Access to Formula Dialog Box
Copyright DASSAULT SYSTEMES Terminology RA relation is a generic name for knowledge features : formulas, design tables... A Formula defines how a parameter is to be calculated with respect to other parameters of the document Example : Length_of_Circle = 2 * Pi * Radius_of_Circle. A Parameter is a property of a CATIA document defined as a feature. It has a value and can be constrained by a Relation. ADesign Table is a Excel or text table constraining a set of parameters. Each column of the table defines possible values of a concrete parameter (its name is associated to the name of the column). Each row of the table defines a possible Configuration of this set of parameters. A Configuration is a set of coherent values of a set of parameters. Design Table User Parameter
Copyright DASSAULT SYSTEMES Customizing the specification tree (1) Displaying the parameters in the tree defined in the part document (2) Displaying the relations in the tree defined in the part document 1 2 Knowledge Settings (1/3)
Copyright DASSAULT SYSTEMES Select the corresponding option if you want … (1)the value of the parameter to appear in the tree (2)the formula driving the parameter to appear in the tree (3)to surround the parameter names by the Symbol Parameter names (4)To load extended language libraries wherever using measures in relations or user functions Knowledge Settings (2/3)
Copyright DASSAULT SYSTEMES Customizing the specification tree (1)Displaying the constraints and dimensions defined in the product document (2)Displaying the parameters defined in the product document (3)Displaying the relations defined in the product document 1 2 Knowledge Settings (3/3)
Copyright DASSAULT SYSTEMES Creating and Using Parameters You will learn how to create and manage parameters :
Copyright DASSAULT SYSTEMES Types of parameters About Parameters (1/2) 2 types of parameters: Intrinsic parameters define the intrinsic properties of the document User parameters define the extra pieces informations added to a document. You can define them at different levels: -Part level -Assembly Level -Feature Level Various types of parameters: Real, integer, String, Boolean, Length, Mass.. With single value (continuous) or multiple values (discrete). User parameters : - can be used to add specific information to a document - can be defined or constrained by relations - can be used as the arguments of relation User Parameters Intrinsic parameters
Copyright DASSAULT SYSTEMES Types of parameters About Parameters (2/2) Length Type User Parameter defined on a CATProduct User Parameter defined on a CATPart String Type
Copyright DASSAULT SYSTEMES General Process to create a User Parameter (1/2) Select the desired type and then specify Single Value or Multi Value option or. Click on New Parameter of type button Click on the F(x) icon Dont forget to click Apply The Formulas panel is displayed
Copyright DASSAULT SYSTEMES General Process to create a User Parameter (2/2) You can rename the parameter by typing a new name in the Edit name, value or formula field 6 The new parameter with default name (here Real.1) and default value 0 appears at the end of the parameter list 5
Copyright DASSAULT SYSTEMES Click Apply to confirm the creation of the new parameter The new parameter with default name (length.1) appears at the end of the parameter list. Creating a User Parameter with Single Value Click on the f(x) icon The Formulas panel is open Choose Single Value option Choose the type Length in the list of possible types 3 Click on New Parameter of type button Type of parameter
Copyright DASSAULT SYSTEMES Click on f(x) icon The panel of the Value List appears: -Type the first value in the first field, then Enter (Val.1 appears in second field) -Type the second value in first field, then Enter (Val.2 appears in second field) 1 5 Choose the type String and Multiple Values option 2 3 Click on New Parameter of type button Click OK to confirm 4 Creating a New Parameter with Multiple Values Double-Click the Parameter in the Specification Tree 6 Select your desired value
Copyright DASSAULT SYSTEMES Change the Parameters value & Click OK to confirm Editing a User Parameter Double-Click a Parameter in the Specification Tree Check the Parameter definition and edit it 3 A number of useful capabilities are available from the contextual menu of parameter edition box: 1-To edit Formula; 2-To specify a tolerance for the Length and Angle parameters; 3-To change step being incremented or decremented in the value field; 4-To specify interactively a measure….. 5-To specify the lower and upper bounds of the parameters value 6-To add comment or specify an existing one Right-Click the field value in the Edit Parameter Panel
Copyright DASSAULT SYSTEMES Creating and Using Formulas You will learn how to create and manage formulas :
Copyright DASSAULT SYSTEMES Formulas are features used to define or constrain a parameter.. A formula is a relation that you write with parameters, operators and functions.. The left of the relation is the parameter to be constrained, the right part is a statement.. Once it has been created, a formula can be manipulated like any other feature from its contextual menu. About Formulas
Copyright DASSAULT SYSTEMES General Process to create a Formula (1/2) 1 You can create formulas with dimensions or user parameters. Double-Click on the parameter in the specification tree and select Edit formula in the contextual menu (MB3).You can also click on the f(x) icon and select Add Formula button in the Formulas panel when creating a parameter Or …. Select the Parameter The formula Editor panel appears 2
Copyright DASSAULT SYSTEMES General Process to create a Formula (2/2) Enter the right side of the formula in the formula editor field. To enter a parameter, you can: - either check the 'Select Feature' box. Selecting a feature in the geometry area or in the specification tree enters the feature definition in the formula editor. - or check the 'Filter' box. Selecting a feature in the geometry area or in the specification tree highlights all the features below the selected feature in geometry area 3 Formula feature is displayed in the tree
Copyright DASSAULT SYSTEMES Referring to External Parameters in Formulas (1/4) In a formula, you can use parameters defined in external documents. This works between any types of document. For example, in a CATPart document, you can specify a formula referring to parameters defined in a CATDrafting document. External parameters can also be used when working within an assembly. You must activate the option Keep Link with selected object in Tools / Option Menu Click on the F(x) icon to display the Formulas dialog box. Select a parameter, then click Add Formula. The formula editor is displayed Select a feature in the external document tree. The External parameter selection panel is displayed In the External parameter selection dialog box, select the parameter(s) that you need in your formula and click OK Open Both documents and Select the Window->Tile Vertically command from the standard menu bar 1 5 Select the Edit->Links command from the standard menu bar. The dialog box which is displayed confirms there is a link between two documents. We can keep the link or choose « Isolate » in the links dialog box. If we click Isolate, the External Parameters node can no longer be expanded and the Length.2 parameter is added below the Parameters node. Activate
Copyright DASSAULT SYSTEMES Referring to External Parameters in Formulas (2/4) In a Formula, you can use parameters defined in external documents. This work is possible between any types of document. The following Assembly contains two parts. 2 In the Specification Tree, Double-click on the User Parameterdiam_disc to edit it. 1 Right-click on the Edit Parameter Dialog Box in order to select Edit formula option. The Formula Editor Panel is displayed
Copyright DASSAULT SYSTEMES Referring to External Parameters in Formulas (3/4) Select the second instance (ISO_SCREW). The External parameter selection panel is displayed. 4 Select the User parameter d_dia and then validate
Copyright DASSAULT SYSTEMES Referring to External Parameters in Formulas (4/4) Select the Edit->Links command from the standard menu bar. The dialog box which is displayed confirms there is a link between two documents. We can keep the link or choose « Isolate » in the links dialog box. If we click Isolate, the External Parameters node can no longer be expanded and the d_dia parameter is added below the Parameters node.
Copyright DASSAULT SYSTEMES Measure Functions in Formulas Insert parenthesis. As you need three arguments, insert two commas within the parenthesis. 2. Position the cursor where the first argument is intended to be typed. Then select the Spline feature in the specification tree. The curve argument is added to the length definition. 3. Position the cursor where the second argument is intended to be typed. Then select the Point feature in the specification tree. The point argument is added to the length definition. 4. Type a boolean for the third argument: True if the length is to be calculated from the origin, False if the length is to be calculated from the curve end. Measures, i.e. values captured from the geometry area can be used in formulas : distance between two points total length of a curve length of a curve segment volume of a PartBody or a closed surface area of a surface or a sketch Spline definitionPoint definitionBoolean: true or false 2 Check that the Load extended language libraries option is selected in the Knowledge tab of the General settings (Tools/Options) Select the Measures item from the Dictionary list. In the list of measures, select for example the length(Curve,Point,Boolean) item. The length function is added to the Formula Editor.. 1 wet area of a PartBody angle between two lines or two directions center of gravity returning points inertia axis on solid, surface, sketch
Copyright DASSAULT SYSTEMES if needed, use the icon to erase a formula Double-click on the formula Or Right-click the formula selected: Formula Object->Definition command From the contextual menu Editing a Formula Open the Relations node in the Specification Tree 3 Check the formula definition in the formulas Editor dialog box 1 The Incremental mode The Incremental mode allows you to display only the parameters of the features selected in the specifications tree. To use this mode, check the Incremental box, then select the feature you want to display parameter list, from either the specification tree or the geometry area. To write Formulas using functions and measures, use CATIA Knowledge Advisor Programming Guide for more information on how to write Formula. Select the formula to be edited 2
Copyright DASSAULT SYSTEMES Formulas Defined as Constant
Copyright DASSAULT SYSTEMES You will learn how to create and manage Design Tables …. Creating and Using Design Tables
Copyright DASSAULT SYSTEMES About Design Table A design table provides you with a means to create and manage component families. These components can be for example mechanical parts just differing in their parameter values. Screws are a good example of mechanical parts that can be described by a design table. In a design table, a set of parameter values is called a configuration and is registered in a row. A design table can be created from a CATIA document (the document data is then exported to the design table). It can also be applied to a document (the document data is then imported from the design table). The purpose of the design table is to drive the parameters of a CATIA document from external values. These values are stored in the form of a table either in a Microsoft ® Excel file on Windows or in a tabulated text file Knowledge Advisor Toolbar : Design Table icon It is possible to indicate the sheet number where the table is found
Copyright DASSAULT SYSTEMES Creating a Design Table (1/2) Click on the Design Table icon Select the parameters to add to the design table and use the arrows. Specify a file to contain the generated design table. Click Open button The Design Table creation panel is open. Select the option Create with current parameters values. Click OK
Copyright DASSAULT SYSTEMES Creating a Design Table (2/2) 5 A dialog box displays the newly created design table. This design table contains only one configuration. By default it is active. If you want to add other rows, click on the Edit table button The Design Table feature appears in the specification tree under the node Relations 6
Copyright DASSAULT SYSTEMES Double-click on the Design Table object in the specification tree to open the table panel 2 Click on Edit table Button to open the corresponding Excel file Under Windows NT Editing a Design Table (1/2)
Copyright DASSAULT SYSTEMES Editing a Design Table (2/2) You can change the Values on the excel file or add new rows 5 A CATIA panel confirming that the design table of CATIA document will be synchronized Click on OK to confirm Click Apply into the CATIA design table dialog box, the document is updated automatically 6 Save your Excel file and close your application 4
Copyright DASSAULT SYSTEMES Open Relations node in the Specification Tree, then Double-click on the design table element The design table panel is open. One of its rows (1) is selected. Select another one (Configuration2) 2 Click on OK to confirm 3 Using a Design Table
Copyright DASSAULT SYSTEMES Using CATIA V5 Layers and Filters You will learn how to create and use CATIA V5 Layers Usefulness of Layers and Filters Using Layers Using Visualization Filters
Copyright DASSAULT SYSTEMES You will learn when it can be useful to have layers and filters in CATIA V5 Usefulness of Layers and Filters
Copyright DASSAULT SYSTEMES Why Using Layers and Filters? You can use up to 1000 layers in a document to dispatch objects and organize the visualization using filters Objects on Different Layers DocumentFiltered visualization You can define as many filters as needed to adapt visualization to your needs. Default filter is All Visible, which means all layers are visible. LayersFilters You can dispatch objects onto layers, and create and apply filters to only view certain layers depending on your needs
Copyright DASSAULT SYSTEMES General Process Creating objects (*) Assigning objects to layers (*) Creating & Applying filters (*) Note that you can create objects directly on the desired layer (on the current layer)
Copyright DASSAULT SYSTEMES You will learn how to name layers and how to assign objects to them Using Layers
Copyright DASSAULT SYSTEMES What About Layers? Layers None (default): means there is no current layer and all document content is visible. Objects assigned to None will always be visible You can use up to 1000 layers numbered from 0 to 999 and name them as you like Using Layer Bodies and PartBodies can be assigned to layers Components of Products can be assigned to layers All features included in the selected (part)body inherit the layer assignment except for sketches Sketches remain on the None layer if not assigned to another layer You can rename layers and sort them out by number ([Num] tab) or by name ([Name] tab) Layers used Layer definition is stored in CATSettings. This allows for application of company standards When opening a CATIA V4 document, the layer organization is kept as is None 0 General 1 Layer 1 2 Layer 2 Other Layers...
Copyright DASSAULT SYSTEMES Assigning Objects to Layers 1 Select an object 3 Type the number of a layer (here 3) The selected object is assigned to layer 3 When you click on an object, the layer (number) to which it is assigned is displayed in the View toolbar You can create objects directly on a given layer. The object is then assigned to this layer To change the current layer, first make sure no object is selected, otherwise it will be assigned to this layer You can also select the layer in the list using the down arrow Note that Features making up the body inherit the layer assignement (except for sketches) 2 Display the Graphic Properties toolbar (View > Toolbars)
Copyright DASSAULT SYSTEMES Checking Objects Assigned to a Layer 1 2 Click on a layer Select Other Layers... The Named Layers dialog box is displayed The object(s) assigned to the selected layer are highlighted. Here, Body.3 was assigned to layer 3 None 0 General 1 Layer 1 2 Layer 2 Other Layers...
Copyright DASSAULT SYSTEMES Adding and Naming Layers 1 Select Other Layers... 2 The Named Layers dialog box is displayed Click on the New button 3 A new (numbered) layer is added to the list Click OK to confirm The new layer is also added to the layer list You can rename the layer by clicking slowly twice on the layer name Clicking the [Num] and [Name] buttons list layers in numerical and alphabetical order None 0 General 1 Layer 1 2 Layer 2 Other Layers... None 0 General 1 Layer 1 2 Layer 2 3 Layer 3 4 Layer 4 Other Layers...
Copyright DASSAULT SYSTEMES You will learn how to create visualization filters and how to apply them to the document Using Visualization Filters
Copyright DASSAULT SYSTEMES What About Filters? Filters A filter only displays the objects assigned to certain layers. Default filter is All visible, which means all layers are visible When you create a new filter you specify the layers that will be visible when applying this filter The Visualization Editor allows you to combine criteria and operators to specify the layers to make visible Criterium are operators (equal, different, lower, greater,...), the list of existing layers, and logical functions (and, or, not) to combine layers. Logical functions to combine layers Filter definition is stored in CATSettings. This allows for application of company standards When opening a CATIA V4 document, the filters organization is kept and can be used using a specific menu (Filter) List of layers Filter definition Operators Visualization Filters list Applying Filters You can create as many filters as needed You can apply only one filter at a time
Copyright DASSAULT SYSTEMES Creating and Applying a Simple Visualization Filter 1 2 Click Tools menu and Visualization option The Visualization Filters dialog box is displayed with default filter All visible Click button New to create a new filter The Visualization Filters Editor dialog box is displayed Select an operator Select a layer. This will edit the first line in the filter definition (never take layer 0) 5 Click OK to confirm The filter just created is added to the list. 6 Click Apply to apply it You can edit filters and delete them if needed (except for the All visible filter) 7 Click OK to confirm Note: Clicking on these functions will add new lines in the filter definition 3 4
Copyright DASSAULT SYSTEMES Applying Visualization Filters 1 Click Tools menu and Visualization option The Visualization Filters dialog box is displayed with existing filters Click Apply to apply the filter to the document Only objects assigned to layers involved in the filter definition will be visible 2 3 Select the filter to apply You can edit the filter before applying it to check the layers involved
Copyright DASSAULT SYSTEMES Customizing CATIA V5 User Interface You will learn how to create customized Workbenches and toolbars Customizing Favorite Workbenches Creating User Workbenches Inserting and Editing Toolbars Adding Commands in Toolbars
Copyright DASSAULT SYSTEMES You will learn how to put favorite workbenches into Welcome Panel Customizing Favorite Workbenches
Copyright DASSAULT SYSTEMES Favorite Workbenches are those that CATIA will display for you at each beginning of session in the Welcome panel. Welcome panel is empty by default What are Favorite Workbenches? This welcome panel is also available by clicking on Workbench icon Welcome Panel Favorite Workbenches
Copyright DASSAULT SYSTEMES Setting Favorite Workbenches (1/2) Favorite Workbenches are those that are displayed in Welcome Panel when you start a CATIA session 1 Select Customize in Tools menu 3 Select or multi select workbenches in the available list 4 Click on right arrow 2 Select Start Menu tab
Copyright DASSAULT SYSTEMES Setting Favorite Workbenches (2/2) Favorite Workbenches are those that are displayed in Welcome Panel when you start a CATIA session 4 Selected workbenches do appear now in the Favorites list 5 Click on Close when you have finished with customizing the interface Now, when beginning a CATIA session or when clicking on workbench icon, you will obtain this Welcome Panel
Copyright DASSAULT SYSTEMES You will learn how to create a new user Workbench Creating User Workbenches
Copyright DASSAULT SYSTEMES A user workbench is a workbench that a user may need and that does not exist by default in CATIA.So user has to create it What is a User Workbench? This Workbench is a user workbench, it contains two toolbars that belong to two different existing workbenches of CATIA: - Sketch Based Features toolbar belongs to Part Design Workbench - Wireframe toolbar belongs to Wireframe and Surface toolbar Wireframe toolbar This Workbench icon means it is a user workbench
Copyright DASSAULT SYSTEMES Creating a New User Workbench (1/2) You can create a new user workbench when editing a CATIA Document 1 Open the type of CATIA document your user workbench will be dedicated to 2 Select Customize from Tools menu 3 Select User Workbenches tab 4 Click on new 5 Key the name of your new User Workbench
Copyright DASSAULT SYSTEMES Creating a New User Workbench (2/2) The new workbench appears now in the list of user workbenches, it has become the current workbench The new workbench will be dedicated to the edition of only one type of file (the same type as the file you were editing when calling customize panel). Click on Close when you have finished with customizing the interface 6 7 User Workbench icon
Copyright DASSAULT SYSTEMES You will learn how to add existing toolbars in a workbench and how to create new ones Inserting and Editing Toolbars
Copyright DASSAULT SYSTEMES A workbench may not contain a command or a set of command that a specific user would need quite often when editing CATIA documents with it Why creating new toolbars? This wireframe toolbar is not present by default in the Part Design Workbench, it has been added by a user Part Design Workbench
Copyright DASSAULT SYSTEMES Creating New Toolbars (1/3) You can create new toolbars or add existing ones to the current workbench Select Customize from Tools menu Select Toolbars tab 1 Set the workbench in which you want to add toolbars as the current Workbench 2 3 You have the list of available toolbars in the current workbench Click on New 4
Copyright DASSAULT SYSTEMES Creating New Toolbars (2/3) You can either … …by selecting the workbench containing it … by keying a new name… 5a 6a … And click on OK 5b …Create a new empty toolbar…Or insert an already existing toolbar 6b … Selecting the toolbar… 7b … And click on OK (4b) (5b)
Copyright DASSAULT SYSTEMES Creating New Toolbars (3/3) New created toolbars appear now in the list of toolbars that are available in the current workbench Click on Close when you have finished with customizing the interface 7 Existing Toolbar New empty Toolbar
Copyright DASSAULT SYSTEMES You will learn how to add commands to the current Workbench by inserting them in toolbars Adding Commands
Copyright DASSAULT SYSTEMES A command may not be available in a toolbar where a specific user could need it. So the user will have to make it become available Why adding commands? This button does launch the Save Management (old Save All as…) command and is not available in this toolbar by default. A user did put it there and assigned this icon to it(There was no icon by default). By default the only way to launch the Save management command is to select it in the File menu
Copyright DASSAULT SYSTEMES Adding Commands in Toolbars (1/3) You can add existing commands of CATIA in toolbars of current workbench Select Commands tab Select Customize from Tools menu 1 Make sure the toolbar in which you want to add the command is available in the current Workbench 2 3 Select the categorie (menu) containing the command you wannt to add 4 Select The command you want to add 5 (4)
Copyright DASSAULT SYSTEMES Adding Commands in Toolbars (2/3) You can add existing commands of CATIA in toolbars of the current workbench Click on this button to access the list of available icons Select the icon and Close the icon browser 6 (6)
Copyright DASSAULT SYSTEMES Adding Commands in Toolbars (3/3) You can add existing commands of CATIA in toolbars of the current workbench Drag and drop the command into the toolbar 6 drag drop Click on Close when you have finished with customizing the interface 7
Copyright DASSAULT SYSTEMES PowerCopy Presentation PowerCopy Creation Saving a PowerCopy PowerCopy Instantiation Creating and using Powercopies You will learn the Catalog workbench main features and tools to create and manage catalogs of reusable components
Copyright DASSAULT SYSTEMES You will learn what is a PowerCopy and how it can be used PowerCopy Presentation
Copyright DASSAULT SYSTEMES PowerCopy is a set of design features grouped together to be reproduced: it is a kind of advanced copying tool You can edit it (set contained features, entries, previews …) You can instantiate and customize it in the design of any part What is a PowerCopy?(1/2) PowerCopy tools are available in the Insert menu (Advanced Replication Tools) of those workbenches: Part design, Wireframe and Surface, SheetMetal Design The PowerCopy you want to create and instantiate is made up of… …One sketch (put on a face of a Pad) … One pocket based on this sketch… … And one thickness of a wall of this pocket
Copyright DASSAULT SYSTEMES What is a PowerCopy?(2/2) When instantiating the PowerCopy, you will be able to customize: …The face supporting the sketch… … the depth of the pocket… … The value of the thickness… … And the Position of the sketch (latitude and height parameters values)
Copyright DASSAULT SYSTEMES You will learn how to create a PowerCopy PowerCopy Creation
Copyright DASSAULT SYSTEMES Creating a Power copy consists in several steps that are to be made in the following order Creating a PowerCopy…. 0 Making the Part ready for the creation of the Powercopy 1423 Setting Definition Identifying and naming inputs Publishing Parameters Setting Icon and preview
Copyright DASSAULT SYSTEMES a Once you have the right geometry in your CATPart, you must build your powercopy with selected features Creating a PowerCopy (1/4) Select Powercopy creation in insert menu 1b Key the name of your Powercopy 1c Select features making up your PowerCopy
Copyright DASSAULT SYSTEMES a Once features making up your powercopy are selected, you need to identify and eventually rename geometric inputs Creating a PowerCopy (2/4) In our case, there is only one geometric input: This is the face supporting the Sketch making up the powercopy To rename a geometric input… 2c Key in the new name of the input Select inputs tab 2b Select the input to rename When editing inputs tab, required geometric inputs are shown in geometry Note that geometric inputs totally depend on which features you selected to create your Powercopy: in fact they are parent geometric elements that remain outside the Powercopy
Copyright DASSAULT SYSTEMES Once geometric inputs are identified and renamed, you have to choose and publish parameters of which you want to be able to set values when instantiating the Powercopy Creating a PowerCopy (3/4) Note that it will be easier for you to recognize them if you have already renamed parameters with knowledgeware tools 3a Select parameters tab To publish parameters… 3b Select parameter 3c Check published option 3d If necessary, give a public name to the parameter In our case, there are four renamed parameter to publish (keep their names as public names): - DepthOfPocket - Height - Latitude - Inside Thickness
Copyright DASSAULT SYSTEMES Once parameters are published, you can select the icon for your powercopy and make a grab screen to create a preview of your powercopy for catalogs Creating a PowerCopy (4/4) To prepare the grab screen, you can remove tree and compass from the window and get the correct zoom and orientation 3a Select icon tab 3b Select icon 3c Prepare the CATPart window for the grab screen Make a grab screen to have a preview 3d 3e You can now validate
Copyright DASSAULT SYSTEMES You will learn ways to save a Powercopy Saving a PowerCopy
Copyright DASSAULT SYSTEMES If not saved, a Powercopy will never be instantiated Saving a PowerCopy…. To save a powercopy, you must save the CATPart which contain the powercopy You can also create or update a catalog which makes reference to all powercopies of your CATPart Powercopies are stored under powercopy node of CATPart
Copyright DASSAULT SYSTEMES Saving a PowerCopy in a Catalog (1/2) To be able to make a « save as Catalog » the CATPart file must not have been modified since last save 1 Click on Save in Catalog command 2 Click on this button to access a browser if you are not satisfied with the path 3 Select correct path and key the name of the catalog
Copyright DASSAULT SYSTEMES The resulting catalog can be edited with catalog editor workbench Saving a PowerCopy in a Catalog (2/2) 4 Click on OK If you you want to see how the resulting catalog looks like, you can open it 5 6 Here is the resulting catalog
Copyright DASSAULT SYSTEMES You will learn how to paste with customized options features making up you powercopy PowerCopy Instantiation
Copyright DASSAULT SYSTEMES First step of the powercopy instantiation is accessing to the powercopy: you can make it: a) by selecting the CATPart file containing it b) by browsing a catalog having it as reference 1a Instantiating a PowerCopy (1/4) Select Instantiate from document 2b Select the CATPart file 1b Click on Catalog browser 2x 2b Double click on the feature
Copyright DASSAULT SYSTEMES Second step of the powercopy instantiation is defining the geometric inputs of the powercopy 3 Instantiating a PowerCopy (2/4) Select in the geometry the inputs of the powercopy When selected,geometric inputs are shown in the geometry (3)
Copyright DASSAULT SYSTEMES Third step of the powercopy instantiation is setting values of parameters that have been published at the creation of the powercopy 4 Instantiating a PowerCopy (3/4) Click on Parameters 5 Set values Click OK 6 If you want you can create on the fly formulas with parameters having same names
Copyright DASSAULT SYSTEMES The result of the powercopy instantiation is inserted after the in work object 7 Instantiating a PowerCopy (4/4) Click on OK The result of powercopy instantiation is a set of editable features.They are not linked to the original features of the powercopy
Copyright DASSAULT SYSTEMES A few advices for instantiation of powercopies: Additional Information (1/2) When you instantiate a powercopy from a CATPart containing several ones you can choose it through the reference Use identical names allows the automatic selection of the geometric inputs that have the same name as those used for the creation of the PowerCopy If you want to use the powercopies several times, check the repeat option
Copyright DASSAULT SYSTEMES Additional Information (2/2) When selecting a supporting face for a sketch, it is recommanded to select the face of a positionned and oriented local system instead of a face of the geometry: In the first case position and orientation of the axis in the created sketch will be controlled In the second case position and orientation of the axis in the created sketch will be uncertain Here, face selected to support the sketch is a face of a local axis system: origin of created sketch is the origin of the local axis and the H and V axis orientations are determined by the local system Here, face selected to support the sketch is a face of a the geometry: origin of the created sketch is a vertex of the selected face and orientation of H and V axis is not the expected one
Copyright DASSAULT SYSTEMES Catalog Workbench Presentation Browsing Catalogs Creating Catalogs Creating Chapters Creating Families Creating Keywords Creating Components Creating Part Family Components Referencing Data from External Catalogs Checking the Catalog preview Creating Catalogs in Batch Mode Creating Catalogs of Components You will learn the Catalog workbench main features and tools to create and manage catalogs of reusable components
Copyright DASSAULT SYSTEMES You will learn about the Catalog Workbench by Catalog Workbench Presentation Accessing the Workbench Exploring the User Interface Seeing Terminology Understanding General Process
Copyright DASSAULT SYSTEMES A Catalog is a file which provides fast access and previsualization of CATIA Documents, and features. It also classify the documents or features with Chapters and SubChapters, and keywords. A catalog references chapters and end chapters. Example: Fasteners can reference Screws, Nuts, Bolts... Syntax used for creating catalogs and query comes from Knowlegeware What is a Catalog?
Copyright DASSAULT SYSTEMES Anywhere from: 1- Start menu 2- File / New menu 3- File / Open menu Accessing the Workbench Note that when you are in another workbench, you can browse existing catalogs using the Catalog icon in the tools toolbar To create and edit catalogs 3-
Copyright DASSAULT SYSTEMES User Interface: Toolbars Chapter Toolbar Tree Structure of the catalog also called catalog navigator Content description and preview of the catalog entities Browsing Toolbar Data (description) Toolbar
Copyright DASSAULT SYSTEMES User Interface: Commands Chapter Link to other Catalog Part Family Keyword Component Family Catalog Preview Part Family Components Catalog filter Resolved Components
Copyright DASSAULT SYSTEMES Catalog (1): A way of classifying many objects. A V5 catalog is in the form of a tree structure made up of chapters and families Chapter (2): A set of references. Made of chapters and families Family (3): A set of references. Made of entities which have the same classification Terminology Keyword (4): The references are described using keywords such as name, type, diameter, length, etc. Keywords are then used to make a query in a catalog Component (5): Reference to an entity. It is displayed with its keyword values Entities (5): CATIA documents (CATPart or CATProduct...) referenced Structure tree of the catalog indicates if the feature is : a Catalog a Chapter a family if the feature comes from another catalog 2 3
Copyright DASSAULT SYSTEMES General Process Creating a new catalog Browsing catalogs to insert objects in a document
Copyright DASSAULT SYSTEMES Catalog Creation and Utilization V4 library.cvs file What you can do in CATIA V5: Catalog Edit component(s) in Part Design Insert component(s) in assembly Parts / features... (.catalog) Batch Batch* Additional Information Catalog workbench (interactive) *Not covered in this lesson Insert PowerCopy in Part Replay macros Insert Detail in Drafting Types of Components that can be Used CATPart, CATProduct, CATScript, CATGScript (Generative knowledge), and features such as Detail (Drafting), Power Copy, Formula, Rules, Check, and Rules Bases
Copyright DASSAULT SYSTEMES You will learn how to search and use objects from catalogs Browsing Catalogs Catalog browser dialog box
Copyright DASSAULT SYSTEMES The Catalog Browser is a tool available in several workbenches which allows you to consult catalogs. It means to have previews and descriptions of elements referenced in them, to sort them out with queries and to insert them in your current document. Catalog browser dialog box What is Browsing a Catalog? Query field to narrow down your search Access to father chapter Current chapter displayed Query Launcher Displays or hides descriptions table Selects another catalog Descriptions table Elements referenced in the current chapter Display Modes Selected element preview
Copyright DASSAULT SYSTEMES Click the Up one level icon to go back to the father chapter Click on an element icon to get its preview 2 x In a catalog, you can have chapters, families, documents and features referenced, you have to know how to navigate among them Click the Open icon to select a catalog Browsing Catalogs Click the Catalog icon. It opens the catalog browser 1 2 Double click a chapter icon to open it 3 3 You get the preview and the description of the selected object Click the Table button to show or hide the desciptions table
Copyright DASSAULT SYSTEMES Open chapters until you get the end chapter in which the element you want is referenced To insert an object you can also drag and drop it into your destination document Inserting a Component from a Catalog (1/2) Click the Catalog icon. It opens the catalog browser 1 Use contextual menu > Copy on the element Paste the object into your document 4 2
Copyright DASSAULT SYSTEMES Inserting a Component from a Catalog (2/2) x 2 Double-click on the desired component to insert 1 Inserting a Component from a Catalog : we can obtain a preview of the component to position it on the target document 2 A preview window appears 3 Select on the target component a point to position the new component
Copyright DASSAULT SYSTEMES When consulting a family, you can apply a filter so only components respecting your specifications will be displayed. Sorting Out Components with Queries (1/4) 1 2 First thing to do is to expand the Table Have a look at the keywords and keep in mind the exact spelling which is important to build correct queries
Copyright DASSAULT SYSTEMES Sorting Out Components with Queries (2/4) 3 Apply a filter Key your specification in the Filter field
Copyright DASSAULT SYSTEMES Same kind of expression as for the numeric values (but only == does work as Operator and you need to delimit Reference value with ) The way to build a specification will be different whether the value of the concerned keyword is numeric or alphanumeric Sorting Out Components with Queries (3/4) 1 For numeric values (Length, Weight…) use expressions like : x.Diameter =0 Key your specification in the Filter field Click on to apply the filter 2 Only components respecting the specification are displayed 3 To select all the values of the keyword containing the chain of characters CHC-M6
Copyright DASSAULT SYSTEMES You can combine effects of two specifications to build a query Sorting Out Components with Queries (4/4) Intersection of results of both specifications Union of results of both specifications Result of first specification Result of 2nd specification
Copyright DASSAULT SYSTEMES You will learn how to create catalogs file from scratch Creating Catalogs A catalog
Copyright DASSAULT SYSTEMES There are several options to create CATIA V5 Catalogs… Creating Catalogs… …You can create an empty catalog from scratch… …You can save a CATPart containing Powercopies as a catalog … …Or you can save CATDrawing files containing details sheets and dittos as a catalog
Copyright DASSAULT SYSTEMES Activate the catalog workbench using the Start or the File menu A new catalog is created with one chapter Accessing the Catalog Editor workbench will create an empty catalog with a first chapter Save the catalog to name it (File > Save As...) Creating a New Catalog (1/2) Chapter 2 Chapter.1 can be renamed
Copyright DASSAULT SYSTEMES Creating a New Catalog (2/2) Creating a new catalog Adding chapters & families Defining keywords Linking components to CATIA documents Saving the catalog To choose to create a catalog interactively implicates all this process
Copyright DASSAULT SYSTEMES You can save CATdrawing files containing details sheets and dittos as catalogs Creating a Catalog from a CATDrawing file (1/2) Only 2dComponents that are in detail sheets will be referenced in the created catalog 1 Select Save as… command from File menu 2 Select catalog for the type of the file
Copyright DASSAULT SYSTEMES You can save CATdrawing files containing details sheets and dittos as catalogs Creating a Catalog from a CATDrawing file (2/2) Save the catalog file 4 The result catalog will contain one family for each detail sheet of the drawing.Each family will contain as many components as there were 2D Components in the corresponding Detail Sheet
Copyright DASSAULT SYSTEMES You will learn how to create chapters Creating Chapters
Copyright DASSAULT SYSTEMES A chapter is a set of references. It will reference other chapters or Families Chapter Definition Box Chapter referencing another chapter What is a Chapter? Chapter referencing two Families
Copyright DASSAULT SYSTEMES Select theChapter icon 3 A chapter is a set of references. It can refer to other chapters or to families Edit the Chapter under which you want to create a new chapter Type the name of the Chapter A Family will reference CATIA documents or features whereas a Chapter will reference other Chapters or Families You can not create any Chapter under a Family Click OK to confirm the chapter creation Adding a Chapter to a Catalog 4 The chapter is added in the tree 1 5 Open the catalog you want to modify (File > Open)
Copyright DASSAULT SYSTEMES You will learn how to create families that can contain reference to CATIA documents and Features Creating Families
Copyright DASSAULT SYSTEMES A family is a set of references. It references components that can be CATIA documents (CATProduct or CATPart) or CATIA Features (Details or Powercopies). Family Definition Box Families What is a Family?
Copyright DASSAULT SYSTEMES Select Family icon 3 A family is a set of references. It refers to CATIA documents (CATPart or CATProduct) or features (Drawing Details or Power Copy) 4 5 Edit the Chapter under which you want to add the family Key in the name of the family to create A Family will reference CATIA documents or features whereas a Chapter will reference other Chapters or families You can not create any Chapter under a Family Click OK to confirm the creation The new family appears in the tree Adding a Family 1 Open the catalog you want to modify (File > Open)
Copyright DASSAULT SYSTEMES You will learn how to create keywords in order to describe contents of chapters and families Creating Keywords
Copyright DASSAULT SYSTEMES Keywords allow you to characterize references in a chapter or family. Values of keywords will help you sort them out when searching for an object (query) Keywords name Keywords value What is a Keyword?
Copyright DASSAULT SYSTEMES Activate the Family or Chapter in which you want to add a keyword 1 Select the Keyword icon The keywords allow you to characterize the references in the chapter or family. Values of keywords will help you to sort out references with queries 3 Type the name of the keyword Display the list and select the desired type of the keyword 4 The new keyword appears in the Table tab in the result window 6 Click OK Creating a Keyword in a Catalog To modify a keyword you can use the contextual menu on a chapter (objectname... > Keywords...) or on a component (Keywords...) 5 Set the default value of the Keyword This option will determine if values of this keyword are visible through the browser or not
Copyright DASSAULT SYSTEMES You will learn how to create references to CATIA documents or Features Creating Components
Copyright DASSAULT SYSTEMES A Component is a reference to an external document or feature. The components keyword values are displayed. Description definition box A component What is a Component? Path of the CATIA document
Copyright DASSAULT SYSTEMES Select the Component icon A Component is a reference to an external file or feature described with keyword settings 4 2 Activate the family in which you want to add a component Select the desired CATIA file 3 Click on Select document to link a CATIA document In the Keyword tab, set values for keywords by selecting the keyword typing the value Description is created 6 Click OK Adding a Component 1 You can edit the default name The path of the selected document will be displayed in the File Name field 5 The Select external feature allows you to select PowerCopies or Details You can preview the associated documents (Preview tab)
Copyright DASSAULT SYSTEMES You will learn how to create whole sets of components from single CATPart files Creating Part Family Components
Copyright DASSAULT SYSTEMES Part Family Components are sets of components generated from a single Part which has several configurations referenced in a Design Table. For each configuration described in the Design Table, a part family component will be created. What are Part Family Components? (1/2) This icon allows you to generate a complete family from a single CATPart All possible configurations of this part are stored in the file leading the Design Table (Exel file or tabulated text file) Keywords will be created directly from names of the parameters(columns) in the Design Table In the Design Table where all the configurations are defined, a column describing the PartNumber is required.
Copyright DASSAULT SYSTEMES What are Part Family Components? (2/2) You have choice : You can edit a Chapter and create in it a Part Family referencing all components described by the Design Table Or you can edit an already existing family and create in it all references of components described by the Design Table
Copyright DASSAULT SYSTEMES Select the add Part Family icon A Part Family will display several components but all of them will be generated from configurations of a single CATpart file. Those configurations are defined in a Design Table. 4 2 Activate the chapter under which you want to add the part family Select the desired CATIA file 3 Click on Select document to link a CATIA document Adding a Part Family (1/2) You can edit the default name The path of the selected document will be displayed in the File Name field 1 In the Design Table where all the configurations are defined, a column describing the PartNumber is required.
Copyright DASSAULT SYSTEMES if not resolved, description of each component will refer to the same.CATPart File Adding a Part Family (2/2) Click OK 5 The Part family is created and contains as many components as there was rows in the Design Table of the Part 6 Each component has an available preview A Part Family will display several components but all of them will be generated from configurations of a single CATpart file.Those configurations are defined in a Design Table.
Copyright DASSAULT SYSTEMES Select the add Part Family Component icon A Part Family component is a set of components. All of them will be generated from configurations of a single CATpart file. Those configurations are defined in a Design Table. 4 2 Activate the family under which you want to add the part family component Select the desired CATIA file 3 Click on Select document to link a CATIA document Adding a Part Family Component (1/2) You can edit the default name The path of the selected document will be displayed in the File Name field 1 In the Design Table where all the configurations are defined, a column describing the PartNumber is required.
Copyright DASSAULT SYSTEMES If not resolved, description of each component will refer to the same.CATPart File Adding Part Family Components(2/2) Click OK 5 The Part family Component is created and contains as many components as there was rows in the Design Table of the Part 6 Each component has an available preview
Copyright DASSAULT SYSTEMES Part Family Resolution(1/2) You can choose to generate in a storage folder all files corresponding to components of your PartFamily Unresolved: Part Family Components refer to the same single CATPart file which is driven by a Design Table Resolved: each component does refer to its proper CATPart File which has no external Link
Copyright DASSAULT SYSTEMES Part Family Resolution(2/2) Whole PartFamily resolutionSingle PartFamily Component resolution Path of Storage Folder is a Setting :
Copyright DASSAULT SYSTEMES Additional Information You have to make a selection or multi selection in this list before clicking on OK If the document selected to create a PartFamily is driven by several Design Tables, CATIA will give you choice between them.
Copyright DASSAULT SYSTEMES You will learn how to create references to chapters of other catalogs and to create sets of components that are the result of a query on an external catalog Referencing Data from External Catalogs
Copyright DASSAULT SYSTEMES Click the Link to other catalog icon 1 Open the catalog where you will add a link to an external chapter (File > Open) 3 If the Chapter you need to create already exist in another catalog, this command allows you to add a link to this chapter from the current catalog 5 Select the chapter or family to import A new chapter appears in the destination Catalog. A link has been created If you change anything in the linked chapter it will be changed in both catalogs Adding a Link to Another Catalog Open the catalog from which you want to get the chapter (File > Open) 2 4 Activate the chapter under which you want to add the link. When a family or a chapter comes from another catalog it is indicated on its item in the tree. Family from another catalog Chapter from another catalog If you want to know precisely where it comes from, use the Edit>Links command
Copyright DASSAULT SYSTEMES What are Catalog Filter Resolved Components Result of a query on all components of the external catalog External Catalog Now you can create lists of components that are result of filter on components of an external catalog: those lists are Catalog Filter resolved Components
Copyright DASSAULT SYSTEMES Catalog Filter Resolved Components (1/2) Activate the Family Select the external catalog Create your query Validate 1 2 Select the command You first need to select the external catalog and create your query
Copyright DASSAULT SYSTEMES Catalog Filter Resolved Components (2/2) 2 x Generated components of selected query Resolved Query Components generated from a query are referenced as external description Next step consists in making resulting components of the query available by resolving the query 6 Select Generative Data tab 7 Double click the query 8 Click on Resolve Query Button 9 Click on OK
Copyright DASSAULT SYSTEMES You will learn how to create catalogs file from scratch Checking the Catalog Preview A catalog
Copyright DASSAULT SYSTEMES What is Catalog Preview? You wont have the same view of a Catalog whether you open it with the Catalog Editor or with the Catalog Browser. Catalog Editor Catalog Browser A Browser icon is available in the Catalog Editor workbench in order to browse the Catalog currently edited. Let us have a look at the differences between the views.
Copyright DASSAULT SYSTEMES Catalog Preview (1/3) You have a global view of the structure of your catalog Structure tree of the catalog indicates if the feature is : a Catalog a Chapter a family if the feature comes from another catalog The Table tab displays all the contents of the active Chapter or Family The active Chapter or Family is blue Highlighted View from the Catalog Editor... To get a Chapter or a Family active, just double click on it
Copyright DASSAULT SYSTEMES Catalog Preview (2/3) 2 x View from the Catalog Browser... You will load the currently edited Catalog by clicking on this icon You only have a view of the contents of the consulted chapter or family The folder icon behind the main icon means that there is a content (it can be Chapters, Families or Components).When you do not have folder icon behind the main icon, it means that there is not any content and that it is a Component To see the content of an element, just double click on it
Copyright DASSAULT SYSTEMES Catalog Preview (3/3) From the editor, you can modify the icons affected to the chapters or family but you will see them only through the browser. Icons representing the chapters or family can be different wether you are browsing or editing the Catalog To change the icon, click there … And select the icon If you do not touch to the icons with the editor, you will have the same icons in the browser In contextual menu of the chapter or family, select Definition Click on OK
Copyright DASSAULT SYSTEMES Keywords Visibility From the editor, you can decide if values of a keyword will be visible through the browser or not. Deactivate this option Select the keyword Star indicates this keyword is not visible We would like to hide values of this keyword in the browser In contextual menu of the family, select Keywords Default values Keyword is hidden 5 Click on OK 4
Copyright DASSAULT SYSTEMES You will learn how to create catalogs in batch mode using Text or Excel files and macros Creating Catalogs in Batch Mode Definition file.csv
Copyright DASSAULT SYSTEMES CATIA documents (parts or assemblies) referenced in catalogs Catalog files generated after running a macro Macro scripts used to generate catalogs Text or Excel files (.csv format) used to create & define, and modify catalog content Reports generated by macros Sample source files Catalogs can be stored with parts they reference. Otherwise, the Search Order must be correctly set What is Behind Catalogs?
Copyright DASSAULT SYSTEMES How Does it Work?.csv Catalog in CATIAChapter definition End-chapter definition CATIA document Macro Chapter Family Filenames of parts Filenames of catalogs Terminology: A chapter references catalogs An end-chapter references CATIA parts / products Keywords are used in queries to search for parts
Copyright DASSAULT SYSTEMES csv E:\users\images\screw.bmp.cs v When you create catalogs of parts, you define chapters and families (see example below) Save the files as.csv (usable on UNIX) You can check the report resulting from the catalog creation Edit csv files: define chapters and families, keywords, names of referenced catalogs or parts & products, and component characteristics (Knowledgware syntax) CATIA settings: reference (if not already done) the CclTypeLib library from intel_a\code\bin using Tools > Options > General > Automation > Add Edit macro BuildCatalog.CATScript (input & output catalog names & location) & Run it You can customize a catalog icon by entering the location and name of the image to be used in cell C1 of the table 5 Creating chapter2. catalog From chapter2. csv Batch successfully ended ' Define the absolute path of the input csv file csvFile ="...\Online\Samples\Infrastructure\chapter2.csv" ' Define the absolute path of the output catalog file catalogFile ="...\chapter2.catalog" * Note that you can define absolute location of catalogs and parts 1 You can have one macro per catalog. Then, you do not need to edit the macro each time (input / output names already defined) Creating Catalogs in Batch Mode
Copyright DASSAULT SYSTEMES You will learn how to read a simple CATIA V4 model and copy it into a V5 document, and to manage your visualization using layers and filters Working with a CATIA V4 Document From CATIA V4 to V5 Basics
Copyright DASSAULT SYSTEMES You will learn how to copy CATIA V4 data using CATIA V5 Working with a CATIA V4 Document V4 model loaded in CATIA V5
Copyright DASSAULT SYSTEMES V5 Files About CATIA V4 and CATIA V5 Analogy V4 Files Solid.model 3D.CATPart (Body) Surface.model 3D.CATPart(Open Body) Wireframe.model 3D or 2D.CATPart (Open Body) Drawing.model DR.CATDrawing Part Positioning.session,.asm, ditto.CATProduct Library.lib.catalog PRJNative Data(Description)
Copyright DASSAULT SYSTEMES User Interface: CATIA V4,V3,V2 Workbench Geometry Check : Check by transferring the solids geometry through Copy-Paste Special as CATIA_Result Using the Check Tools Geometry Specification : Check by transferring the solid with geometry and the history tree through Copy-Paste Special as CATIA_Spec V4 Integration workbench Check Tools
Copyright DASSAULT SYSTEMES About Copy and Paste Options CATIA_RESULT: the result is a Boundary Representation feature i.e. Brep feature Example: V4 surface becomes a surface in an Open Body & V4 solid becomes a Solid in a Part Body CATIA_SPEC: the result is a full Spec containing entire history of the actions performed to obtain the V5 Part. Note : you can modify the features in the history tree Using the Paste Special Tools
Copyright DASSAULT SYSTEMES In CATIA V5 you can read a V4 model, check its content, and manipulate the geometry, but not save it directly. First, you need copy it into a V5 document. There are two methods: What are the Different Methods? AB Copy without historyCopy with history A simple copy generates a Solid object which cannot be modified but can be used as reference A special copy takes into account the V4 specifications and generates V5 features. You can edit the part body as well as the features (as shown on right picture)
Copyright DASSAULT SYSTEMES General Process Interactive mode using: Copy Paste Special CATIA_SPEC + Update Using Part Design Workbench capabilities to analyze/check the result CATPart Batch mode (not covered in this course) Saving the integrated document As a.CATPart 43 Before Copying the CATIA model: Checking its Geometry and Specifications Integrating V4 CATIA model to CATIA V5 CATPart Document Two ways of doing : From CATIAV4,V3,V2 workbench Opening & Visualizing a CATIA model 2 1
Copyright DASSAULT SYSTEMES You need to check either the geometry or the specification of CATIA V4 model data 2 The Check Validity dialog box appears Click Geometry Check icon Open the CATIA V4 model and select one or more geometrical elements in the geometry area Checking CATIA V4 Model Data before Copying it to CATIA V5 Document (1/2) CATIA V4Integration workbench & toolbar "3 operations not implemented" : 3 operations will be unavailable in a migration to CATIA V5. Click Specifications Check icon. The Check Validity dialog box appears 3 You can transfer the solids geometry only through copy - paste special - As a Result. 1
Copyright DASSAULT SYSTEMES To view the results of a specification check, double-click on the contents of the selected line in the Check Validity dialog box. The $ symbol means that the Pipe item is an unresolved feature in V5 (same symbol in the V4 tree). Checking CATIA V4 Model Data before Copying it to CATIA V5 Document (2/2) 4 5 Right-click the red element to discover the problem In the Check Validity dialog box there are four columns: The first column showing the overall result, color-coded as follows: G (green): will be copied as is to CATIA Version 5. The check is OK. R (red): will NOT be copied to CATIA Version 5 as is. This is a KO Check. Y (yellow): will NOT be copied to CATIA Version 5 as is because of a link to a red-coded item. This is KO Check due to the element supporting by the solid. CATIA identifies the identifier & the format i.e. Specifications The Message column provides the number and type of problems.
Copyright DASSAULT SYSTEMES File > Open Open a (new) V5 document V4 Workspaces 1 V4 Integration workbench & tools Select mode Geometry check 3 Click V4 geometry (if simple part) or the desired object in the tree, then Copy (Edit menu or MB3) 4 Click in V5 tree, then Paste Special (Edit menu or MB3) Click CATIA SPECS then OK to keep the V4 model history Edit > Update the geometry to visualize it 7 Double click MASTER to see its content Copying a CATIA V4 Solid into CATIA V5 6 Resulting tree. 5
Copyright DASSAULT SYSTEMES You have seen some advanced functionalities of CATIA V5 such as : Standart Knowledge Tools Using V5 Layers and Filters Customizing CATIA V5 User Interface Creating and Using Powercopies Creating Catalogs of Components Using CATIA V4 Documents Sum Up …..