The Tow Hook

The scenario developed below is intended to show how to create and instantiate an assembly template into a .CATProduct file.
To perform this scenario, you will need the following files:

Create the Assembly Template

  1.  Open the PktTowHook.CATProduct file.

  1. From the Start > Mechanical Design menu, access the Drafting workbench. The New Drawing Creation Window is displayed.

  2. Select the All views configuration and click OK.

  3. The drawing corresponding to the pad is generated.

  1. Save your drawing and close the file. Click here to see the generated drawing.

  1. Go back to the PktTowHook.CATProduct file to create an assembly template.
    From the Insert menu, select Document Template Creation .... The Document Template Definition window is displayed.

  1. In the Document Template Definition window, define the document template. 

  • Click the Inputs tab. In the geometry, expand the Support node and select the following items located below the Isolated External References node:
    • Surface.1
    • Curve.1
    • Surface.2
  • Select Surface.1 and assign it a new name: PlanarFace
  • Select Curve.1 and assign it a new name: Center_CircularEdge
  • Select Surface.2 and assign it a new name: Axis_CylindricalFace
  • Click the Published Parameters tab and click Edit List... .
  • In the Select parameters to insert window, select the Support\Tube_Thickness parameter using the arrow button.
  • Click OK to validate. The Document template is displayed below the KnowledgeTemplates node.
  1. Save your file and close it. Click here to open the result .CATProduct file.

Instantiate the Assembly Template

  1. Open the PktDestinationProduct.CATProduct file.

  1. From the Start > Knowledgeware menu, access the Product Knowledge Template workbench.

  2. Click the Instantiate from Document icon () and select the PktTowHook_result.CATProduct file in the File Selection window. The Insert Object dialog box is displayed.

  3. Select the visible face of the pad. Face is displayed in the Insert Object dialog box.

  4. Select the pocket in the Geometry.

  5. Expand the Input_Cylinder node and select the Extract.1.

  6. Click OK to validate. The assembly template is instantiated...

and the associated drawing is updated accordingly (click here to open the generated drawing).