Renaming Components

You can change the file name of a component directly from the FeatureManager design tree. You can specify an alternate component name without changing the file name.

Using Alternate Component Names

In Component Properties, you can specify an alternate component name to appear in the FeatureManager design tree without changing the component's file name.

By default, SOLIDWORKS identifies a component by its file name in the FeatureManager design tree. Using an alternate name can be useful if your company uses part numbers that are not descriptive. For example, if your assembly uses a flange with a part number P112728-101, you can specify flange as an alternate name to appear in the FeatureManager design tree.

To specify an alternate component name:

  1. In an assembly document, select a component and select Component Properties (context toolbar).
  2. In the dialog box, for Component Name, enter a name.
  3. Click OK.
    In the FeatureManager design tree, the component displays the name. The component's file name remains unchanged.

Changing Component File Names from the FeatureManager Design Tree

You can change component file names directly from the FeatureManager design tree.

You can update references to the renamed files in unopened documents at the same time.

If you want to change file names for many components, consider using Pack and Go. See Pack and Go Overview.

Before you begin:

To enable renaming, click Tools > Options > System Options > FeatureManager > Allow component files to be renamed from FeatureManager tree.

To change a component file name:

  1. In an assembly, in the FeatureManager design tree, do one of the following for the component whose file name you want to change:
    • Click-pause-click the component.
    • Right-click the component and click Rename Assembly or Rename Part.
    • Select the component and press F2.
  2. Enter a new name and press Enter.
  3. In the dialog box, select Temporarily rename document and, if prompted to rebuild, click Yes.
    The file name of the component changes in the SOLIDWORKS software, but is not changed in the Windows file system. Any open documents that reference the renamed file are updated in the SOLIDWORKS software to reference the new file name.
  4. Save the assembly.
    In the Rename Documents dialog box, you receive warnings of the following items:
    • Files that are temporarily renamed in SOLIDWORKS are renamed permanently in the Windows file system.
    • Other open documents that reference the renamed files are updated in the Windows file system.
    • References are broken in closed documents that reference the renamed files unless you select Update where used references and specify which documents to update.
  5. Optional: To avoid broken references in documents that are not open:
    1. Select Update where used references.
      The dialog box expands.
    2. Specify the folders to search for documents to update.
      Option Description
      File locations Lists the folders to search. Click Add Folder to browse for folders to add to the search. To remove a folder from the list, select it and click Remove.
      Include file locations - Referenced Document folders Specifies to search the folders listed under Referenced Documents in Tools > Options > File Locations.
    3. Click Search.
      Results are listed under Update where used references. By default, all items are selected.
    4. Clear items that you do not want to update.
        State Description
      Selected Items update to reference the new file name.
      Cleared Items continue to reference the old file name.
  6. Click OK.
    The component file is permanently renamed.