Creating an Assembly Added

You can create an assembly added.

Before you begin: Open an existing assembly.
See Also
About Assembly Features
Editing Assembly Features
  1. From the Assembly section of the action bar, click Assembly Added .

    The Choose a 3D Shape dialog box appears.

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

    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.

    The New Content tab appears.
  3. Click 3D Shape under Physical Product Structure node in the New Content tab.
  4. Click OK in the 3D Shape dialog box.
    The new 3D Shape is created under the active product.
  • Important: You switch from Assembly Design app to Assembly Feature Specification app.
    1. Select the geometry in the assembly where you want to create the added 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.

    2. Click OK in the Warning dialog box.
      • You are now in the Assembly Feature Specification app.
      • The added feature definition dialog box appears.
        Important:

        Trim to shell and Thick options are not taken into account on affected representations.

      • 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.
    3. Select the Profile/Surface box and select the profile element.
    4. Specify the Added Feature properties then click OK in the Added Feature dialog box
      The Assembly Features dialog box appears.
      Tip:

      The Assembly Added icon is displayed as reminder in the dialog box.

    5. Select 3D shapes in the tree that will be affected by the added feature.
      3D shapes are added to the affected list of the Assembly Features dialog box.
    6. Click OK in the Assembly Features dialog box.
      • You exit the Assembly Feature Specificationapp.
      • The Assembly Added is created.
      • A solid linked to the Assembly Added is created in the representation of each affected representations.
    7. From the standard area of the action bar, click Update .
      The added feature is displayed.
      Important: You come back in the Assembly Design app.