Setting Up The Visualization Mode

This task shows you how to set up the Visualization mode for components in Product Structure context and how to manage Part Number conflicts when you shift to the Design Mode:

Setting up the Visualization Mode
Back into Design Mode
Managing Part Number conflicts when moving a CATIA document into Design Mode

The Visualization Mode uses documents in .cgr format. Only the external appearance of the component is visualized. The geometry is not available, which may be useful when you deal with sophisticated assemblies with large amounts of data but only need a few components to work on.

As only the external appearance is loaded and not its document, the Edit > Links functionality implies that the document is not loaded for any types of links.
By using the Edit > Links functionality, in the Status column, you can see the "not loaded" status of:

  • the Instance link:
  • the Copy / Cut / Paste link:
  You may wish to use the other edition mode referred to as the Design Mode.
  • In Visualization Mode, the button appears at all nodes' level and tree extension is possible, which allows partial load from the graph.
  • To accelerate the graph loading, the button is displayed every time a representation is associated to the document corresponding to the node, no difference is made between a product with an associated representation and a product containing a Part.
  • The "plus" status is updated when you click it. This means that you are allowing the partial loading of the graph only when you are in Visualization mode. If finally there is no children in the graph, for instance a document with an unloaded reference, "plus" status disappears:
  • The node's state is between Visualization Mode and Design Mode. If you click the node, the disappears and square brackets [] are replaced by parenthesis.
  • Double-Click again the same node and the product is set in Design Mode ("+" reappears).

Setting Up The Visualization Mode

  • Make sure that the Work with the cache system setting is activated in Tools > Options > Infrastructure > Product Structure > Cache Management. For more information, see Customizing Cache Setting.
  • Open the ManagingComponents01.CATProduct document.
    You can recognize that the CATProduct is in Visualization Mode because its components are written like this:
      Instance Name [Document Name]

Back into Design Mode

  1. Select CRIC_SCREW.1 [CRIC_SCREW.CATPart].

  2. Then select either:

  • the command Edit > Representation > Design Mode in the file-menu.

  • or select Representations > Design Mode from the contextual menu

  • or click the icon Design Mode .

If you do not click the root Product in order to make it active, the compass does not turn green when you move and place it on any part under the product and the part cannot be manipulated.

CRIC_SCREW.1 [CRIC_SCREW.CATPart] has turned into CRIC_SCREW (CRIC_SCREW.1) and the geometrical elements in CRIC_SCREW.1 can be seen, and therefore selected, in the Specification Tree because its branches are now expandable:

You can reapply the Visualization mode by selecting the CRIC_AXIS.1 for instance and clicking the Visualization Mode icon .

According to the mode you have chosen, you can see differences in the Specification Tree:
  • Design mode:

  • Visualization mode:

Managing Part Number Conflicts When Moving a CATIA document into Design Mode

Moving a CATPart document from Visualization Mode to Design Mode may lead to Part Number conflicts if you had already inserted another element with the same Part Number. This task shows you that you can solve this problem by renaming one of the conflicting Parts.
  1. Select ManagingComponents01.

  2. Click the Insert Existing Component icon .

  3. Choose CRIC_SCREWbis.CATPart and click Open and you obtain:

  4. Select CRIC_SCREW.1 [CRIC_SCREW.CATPart] and click the Design mode . A Part Number conflict window is displayed because both entities of CRIC_SCREW have the same Part Number:

    Renaming one of the Part Number is mandatory because the OK button is inactive in the Part Number conflict window.

  5. Rename CRIC_SCREWbis.CATPart and click OK:

  6. The Part Number is renamed and the conflict is solved:

    The second Part Number, CRIC_SCREWbis.CATPart, can be inserted in ManagingComponents01.CATProduct: