Problem

When a document has referenced files with many revisions saved in different file locations, mismatches may occur. This article goes over how to fix incorrect file references. The files SOLIDWORKS opens as references are not random. We can see which file is being accessed in the assembly, drawing, or part by going to File> Find References.

If one of these files is being pulled from the “wrong” location, you may consult the SOLIDWORKS search routine to find which step is causing this file to be opened:
Understanding the SOLIDWORKS Search Routine Order

Tips to prevent file reference mismatch:

1. Unique File Names: This applies to files of the same extension. You may have a part, drawing, assembly, PDF, and Word document all of the same name, but not 2 part documents of the same name. If there is no duplicate file name for your part files, there is no chance that the wrong file will be used.
2. SOLIDWORKS PDM: SOLIDWORKS PDM (product data management) offers robust data management to store files with revision control in a PDM Vault. Users have a working folder where copies of checked-out files are stored to be viewed or modified. In this case, as long as there are no other locations (most commonly on shared drives or test folders) that have files of the same name, the correct file will be referenced.
3. Referenced Documents Search Path: If alternate save locations must be used, adding a referenced documents search path may solve any referencing issues. This option is found in Tools > Options > System Options > File Locations > Referenced Documents.

Solution 1: Open Correct Files First

1. Open SOLIDWORKS
2. Open the correct referenced file(s) in SOLIDWORKS before opening the assembly or drawing file.
3. Open the assembly or drawing file that needs references fixed
4. Rebuild the file with CTRL+Q
5. Save the file to update the references

Solution 2: Rename Incorrect Files

1. Close SOLIDWORKS
2. Rename the old files located in the original directory. Note: This will cause SOLIDWORKS to be unable to find the source location and will use the search routine to find the correct files. This method is faster, but gives less control.
3. Open the assembly or drawing file that needs references fixed
4. Rebuild the file with CTRL+Q
5. Save the file to update the references

Solution 3: Manually Fix References with File > Open

1. Open SOLIDWORKS
2. Go to File > Open

3. Select the file with references to fix, but do not open it, and then click the "References" button

   

4. In the "Edit Reference File Locations" window, click each cell in the "In Folder" column to browse to the correct file path

   

5. Once all file references have been updated, click "OK" to close the Edit Reference File Locations" window and then open the file using the updated references.

   

6. Rebuild the file with CTRL+Q and verify the references are updated from File > Find References

   

7. Save the file

This video goes over an example of this solution: How to Fix SOLIDWORKS File References

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.