Managing Representations    

This task shows you how to use several documents (CATShapes) to describe one part.
Open the ManageRep.CATProduct document.

  1. Click Manage Representations in the Representation toolbar or right-click Cylindre (Cylindre.1) and select the Representations > Manage Representations... contextual command. The Manage Representation dialog box appears:

    It displays:

    • the Name of the representation,

    • the Source file of the representation,
    • the Type of the representation,
    • whether the representation is the Default representation of the product,
    • whether the representation is Activated or not.

    In this window you can see one Shape: Cylindre_s.CATShape.

The default name given for a .cgr and .CATShape file is Shape X (X=1, 2, …. Depending on the number of files you have created). For example, it could be Shape 1.

  1. Click Associate... and the Associate Representation dialog box appears.

  2. Select Cylindre_d.CATShape from the online\pstug\samples folder and click Open.

A second CATShape appears in the Manage Representation dialog box:

  1. Select the Cylindre_d.CATShape line. As a result Cylindre_d.CATShape is visible in the Geometry space.

The Rename button becomes active.

  1. Click Rename and enter Detailed in the Rename Representation box. Click OK. Cylindre_d.CATShape appears with the name Detailed, in the Manage Representation dialog box:

  1. Cylindre_d.CATShape is still selected. Click Set As Default button. This representation is activated and set as the default representation. Therefore by default, Cylindre_d.CATShape is visible when opening Cylindre Product.

You can associate as many representations as you need, but only one must be Set As Default. In this case other representations are not displayed in the Specification Tree and in the Geometry area.

  • To change the default representation of a product, select one of its representations and click the Set As Default button.

  • To deactivate a representation of a product, select a representation in the Manage Representations dialog box and click the Deactivate button. The representation is deactivated from Product in the specification tree and in the geometry area. The Activated column of the Manage Representations dialog box displays "No".

  • To activate a representation of a product, select a representation in the Manage Representations dialog box and click the Activate button. The representation is activated in the specification tree and in the geometry area. The Activated column of the Manage Representations dialog box displays "Yes".

  • To replace a representation, select a representation in the Manage Representations dialog box and click the Replace... button. The Replace Representation dialog box is displayed. Select the model document from the chosen directory and click Open. The representation is replaced in Product in the Specification Tree, in the geometry area and in the Manage Representations dialog box.
    When you replace a constrained representation, even if its constraints have been deleted, you are in the reconnect representation context.
    See Reconnecting a Replaced Representation, in CATIA - Assembly User's Guide. When you replace a deactivated representation, the replacing representation is automatically activated.

  • To rename a representation, select a representation in the Manage Representations dialog box and click the Rename... button. The Rename Representation dialog box is displayed. Define a new name or select an existing name in the combo box. The representation is renamed in the Manage Representations dialog box. However, this has no effect on the feature names in the specification tree as there is no relation between representation names and feature names.

  • Renaming the instance name of the Part with this character "!" breaks the Publication Links, a warning message appears and you cannot rename it.

  • To remove a representation, select a representation in the Manage Representations dialog box and click the Remove button. The representation is removed from the Product in the specification tree, in the geometry area and in the Manage Representations dialog box.

  • If you copy / paste a .model As Spec (Paste Special > As Spec) into a CATProduct in CATIA V5, it is the same like doing a Add New Representation that is to say adding this model as a New Representation in the CATProduct. Copying As Spec consists in transferring of the solid with the Geometry and History tree. For more information about the Copy / Paste Special > As Spec, please refer to Copying 3D from CATIA Version 4 to CATIA Version 5 in the CATIA - V4 Integration User's Guide.

  • .cgr, .model, .CATShape and some other 3D graphic formats can be associated to a product. A CATPart or a CATProduct cannot be associated as an alternate representation to a product.

  • Activate representation operation is not persistent.

If you want to know how to manage representations as alternate shapes automatically, in DMU Optimizer, see Customizing DMU Optimizer Settings in CATIA -  Infrastructure User's Guide.

From CATIA V5, new alternate shapes can be saved in ENOVIAVPM, directly in the database. When the dialog box entitled Synchronization is displayed, you can click on OK. For more information about alternate shapes in VPM, refer to Managing Alternate Shapes - Saving and Deleting Alternate Shapes in VPM User's Guide.
 

About CATParts and CATShapes
CATPart / CATShape differences?

A part contains a "Product" description that does not exist in a CATShape:
What is a CATShape?

A CATShape is designed to be used as a representation in a Part, product or component, which CATParts cannot.
What is the CATShape's role?

The role of a CATShape is to give a description to a product.

You can use several documents to describe a product. These documents can be divided in two groups:

  • a document describing the geometry, for instance: Cylindre_s.CATShape in our exemple.
  • another document giving other specifications: cf. Cylindre_d.CATShape.
A CATPart contains both:
  • the CATProduct's data, that is to say the product definition of the CATPart,

  • and the CATShape's data or the geometry definition of the CATPart.

But there is a constraint: there is always a CATShape set as default. And the CATProduct (product definition of the CATPart) cannot have sons, it can have other Shapes but cannot set them as default. Moreover, the CATShape (geometry definition of the CATPart) can be considered as the second half of the CATPart and it has priority before the other Shapes.

CATShape is only available with a license for one of the following products: CNA.prd, EQT.prd, HGR.prd, HVA.prd,
PIP.prd, RCD.prd, TUB.prd, WAV.prd (they are the shipbuilding products and you can find their full name under
Equipment&Systems.