Creating Annotations in Assembly Context

You can create 3D Tolerancing & Annotation features in an assembly, such as annotations and dimensions.

Important: You can manage the selection of elements according to Assembly Context options.

Before you begin: Open an assembly.
See Also
About Annotations in Representation
  1. Double-click the root product to activate it.
  2. From Product Edition section of the action bar, click Insert New Representation .

    The New Content dialog box appears.

  3. Under the Physical Product Structure category, select the representation type to be created.
  4. Click OK in the New Content dialog box.
    The representation is added.
  5. Double-click the created representation and activate the 3D Tolerancing & Annotation app.
  6. Create a dimension between two parts (respectively Representation_A and Representation_C in this example).

    Important:
    • The green diamond as contextual symbol appears on the 3D shape representation icon in the tree , indicating that the 3D shape is involved in context minimal (that is, when the relation and the two components belong to the same parent component) in the assembly.
    • The External References node appears under the 3D Shape representation, containing links with involved geometries in the dimension , a green thumb displays the link status as OK . Contextual links are hidden by default.
    • The Annotation Set node appears under the 3D Shape representation, containing the dimension. It contains an annotation plane and the dimension , a green thumb displays the dimension status as OK.
    • Three engineering connection nodes with one engineering connection are created:
      • One Engineering Connections node appears under each product in relation with the dimension, with a UserDefined engineering connection containing the PLM information to validate the dimension.
      • As a reminder another Engineering Connections node appears under the first parent product containing the active 3D Shape representation. Here the root product itself.

      These three UserDefined engineering connections are the same object.

  7. Right-click one UserDefined engineering connection and select UserDefined.1 > Definition....

    You are back in the previous product context app.

  8. Right-click the same UserDefined engineering connection again and select UserDefined.1 > Definition....
  9. In the Engineering Connection Definition dialog box, select FTA.

    This section displays information related to the annotations contained in the engineering connection.

    • In the Name column, the annotation name is displayed.

      Double-click the annotation name to rename it.

    • In the User Surface column, the first icon represents the geometry class, and the other icons below represent the related geometries.
    • In the Action column, the remove option is available for each row.

      The remove action is performed on all the selected rows.

  10. Click OK.