Editing Imported Features

You can replace an imported feature with geometry from a new file.

To edit a feature created from an imported document:

  1. In the FeatureManager design tree, right-click the feature created from the imported document, and select Edit Feature.
    The Open dialog box appears.
  2. Optional: 3DEXPERIENCE Users: If the Open from 3DEXPERIENCE dialog box appears, click This PC.
  3. In the Files of type list, select the desired format.
  4. Browse to select the desired file to import.
    The file name appears in the File name box.
  5. Select the Match faces and edges check box, if desired. This does the following:
    • Propagates the dependencies of the old faces and edges in the old body, such as sketches or features, to the new faces and edges in the new body.
    • Ensures you get the correct results when you open a file that has imported features.
  6. Click Open.
    An imported solid is replaced only if the data in the new document can be successfully knitted into a body. A surface feature is replaced with the first surface in the new document, and subsequent surfaces in the new file are added to the model.
    You can edit only features that were created from an ACIS, Autodesk Inventor, IGES, Parasolid, Pro/ENGINEER, Solid Edge, STEP, VDAFS, or VRML file.
If you had added features to the imported body before selecting Edit Feature, SOLIDWORKS attempts to rebuild these features whenever possible.

For example, this STEP file contains an imported feature. You need to add a feature to the imported body.

  1. Select the bottom face of the imported body.

  2. Click Chamfer .

    The Chamfer PropertyManager appears.

  3. Under Chamfer Parameters, make the desired settings and click OK .
    The imported body now shows the additional chamfer feature on the bottom face.

  4. Right-click Imported1 in the FeatureManager design tree and select Edit Feature.
    A message box appears warning that this feature has a parent/child relation or is being referenced.

  5. Click OK.

    The Open dialog box appears.

  6. Optional: 3DEXPERIENCE Users: If the Open from 3DEXPERIENCE dialog box appears, click This PC.
  7. Select the STEP file and click Open.

    The STEP file opens with the imported body. The chamfer feature that you added to the imported body is rebuilt. You did not have to rebuild this feature that you had added to the imported body before selecting Edit Feature.