Creating an Assembly Protected

You can create an assembly protected.

Before you begin: Open an existing assembly.
  1. From the Assembly section of the action bar, click Assembly Protected .

    The Choose a 3D Shape dialog box appears.

    In the Choose a 3D Shape dialog box:

    • The Product box displays the name of the active product.
    • 3DShapes either lists the available 3D shapes instanced under the active product or lists the available 3D shapes instanced under a selected product. In both cases, these 3D shapes can be modified.
    • The Create new command allows you to create a 3D shape.
      Important: When you create a new 3D shape in Assembly commands context, its Nature is set as Specification whatever your choice in the dialog box, and you cannot change the nature of this 3D shape after it has been created with this command. See Nature of a New 3D Shape Created in Assembly Commands Context.
    • The Automatically create new 3D Shape when none exists option allows you to create a 3D shape either under the active or selected product automatically. In this case, the Choose a 3D Shape dialog box does not appear.

  2. Click Create new in the Choose a 3DShape dialog box.

    The New Content tab appears.
  3. Click OK in the 3D Shape dialog box.
  4. Select the geometry in the assembly where you want to create the protected features.
    Important: A warning message is displayed when you select a geometry outside the active 3D Shape; the selected geometry does not belong to the current functional body.

    You are about to link the 3D shape functional body containing the assembly feature with the body element that supports the feature.

  5. Click OK in the Warning dialog box.
    • You exit the Assembly Feature Specificationapp.
    • The Protected Feature definition dialog box appears:
    • The Creation toolbar appears:
      • Launch Assembly Feature Definition: displays the Assembly Feature Definition dialog box at the end of the 3D shape feature creation.
      • Specification in No Show: toggles to hide/show the 3D shape feature at the end of its creation.
  6. Select the profile of the product from which you want to create the protected feature.
  7. Specify the protected feature properties and click OK in the Protected Feature definition dialog box.
    The Assembly Features dialog box appears.
  8. Select 3D shapes in the tree that will be affected by the protected feature.
    3D shapes are added to the affected list of the Assembly Features dialog box.
  9. Click OK in the Assembly Features dialog box.
    • You exit the Assembly Feature Specificationapp.
    • The Assembly Protected is created.
    • A solid linked to the Assembly Protected is created in the representation of each affected representation.
  10. From the standard area of the action bar, click Update .
    The protected feature is displayed.
    Important: You come back in the Assembly Design app.

 

See Also
About Assembly Features
Editing Assembly Features