Product to Part and Generate CATPart from Product

This task will show you how to filter a CATProduct into a CATPart, i.e. how to remove sensitive information from a CATProduct and create a new CATPart with the remaining geometry as follows:
Shown geometry
Graphic attributes
Axis system
Naming		 always kept
Colors and attributes on instance and subelements optional

Any data other than the ones described above are removed in the newly created CATPart.
An option is also available to merge the bodies of each part into one body.
Note that the In Work Object in the result part is always the PartBody.

In this task, you will find:

  • To avoid the transfer of integrity errors in data, and to improve the filtering performances,
    we recommend that you use CATDUA V5 and make sure the data are up-to-date before performing any Product Data Filtering.
  • If a memory error or a memory warning occurs, or if the input document is corrupted, the output part will be empty or partial.
  • If the geometry to filter is not up-to-date, the result will not be coherent.
Open the 01_Cric_Assembly.CATProduct from the samples directory. It looks like this:

  1. Click Product to Part or select Tools > Generate CATPart from Product...  menu and select the node Assembly_01.

  2. The dialog box is displayed.

    In Assembly Design:

    In Product Data Filtering:

  3. Click OK. A progress bar is displayed while Assembly_01_AllCATPart is created.

    It looks like this:

Standard behavior

  • You can select any node in the CATProduct structure. Only this node and the elements it contains will be processed, enabling you to create a CATPart with only a portion of your product.
  • A CATPart is created. Its default name is "Name_of_Node_of_Original_CATProduct"_AllCATPart and can be edited.
  • A body is created in the resulting CATPart for each body containing shown geometries under the node you have selected.
    Its name is the full path of the instance in the original CATProduct.
  • The geometries found are transferred as solids, surfaces or wireframes and placed in the corresponding bodies in the resulting CATPart.
  • The solids are created with the graphic properties (color, line type, line thickness, transparency) of their original body,
    the surfaces and wireframes are created with the graphic properties of their original feature.
  • All positions of the geometries are kept in the resulting CATPart.
    The origin of the resulting CATPart is created relatively to the higher root product currently open in V5
    (which is not necessarily the node you have selected).
  • The reference planes are always hidden.
 

 

Options

You can select several options to transfer some elements that are not transferred in the standard behavior. For more information, see the Product to Part Options chapter.