Inserting a Part into Another Part

Use Insert Part to insert a base part into another part document.

When you insert a part into another part:
  • The part into which you insert it becomes a multibody part.
  • The part that you insert becomes a solid body.
  • If the inserted part contains mate references, you can use the references to position the inserted part. A Body-Move/Copy feature is added to the FeatureManager design tree. You can move and rotate the body after you place it.

To insert a part:

  1. With a part document open, click Insert Part (Features toolbar) or Insert > Part.
  • Click to pin the PropertyManager if you want to insert multiple parts without having to reopen the PropertyManager.
    1. Select a part from the list, or click Browse to open an existing document.
      When you open the Insert Part PropertyManager and no parts are available under Open documents, the Open dialog box opens automatically so that you can browse for a part to insert.
    2. If the part has multiple configurations, select a configuration from the list.
    3. In the Insert Part PropertyManager, under Transfer, select the items from the inserted part to include in the derived part. You can include items like custom properties, cut list properties, sketches, and model dimensions.
      All transferred elements of the inserted part are placed in folders under the inserted part in the FeatureManager design tree.
    4. Under Locate Part, select Locate part with Move/Copy feature to define a location for the inserted part in the Locate Part PropertyManager.
    5. Optional: To edit the features of the inserted part without affecting the original part, under Link, click Break link to original part.
      You can break the link to the original part at a later time by listing the derived part's external references and selecting Break All. After you break the link to the original part, you cannot restore the link.
    6. Click .
      After you insert a part, you can move, copy, rotate, or mate it using Move/Copy Bodies (Features toolbar).

    To change the configuration of the inserted part:

    1. Right-click the part and click External References.
    2. Select a configuration in Configuration, and click OK.
      You can control the configuration with a design table. See Base Parts in Configurations.