SOLIDWORKS Search Routine Order
When working in an assembly or drawing in a collaborative environment with multiple users sharing/editing the same files, chances are you may have seen the message below ‘Unable to locate the file…’ when file references cannot be found.
This message means a reference file has been moved, renamed, or deleted and now SOLIDWORKS cannot locate the file. Understanding the search routine SOLIDWORKS performs to find files may help explain why your file opened with this message or opened with a completely different file reference than expected.
The search routine listed below for SOLIDWORKS is followed every time a file is opened which contains references to another file:
- Search in memory (the computer’s RAM) for an open document.
- Search in the specified locations which have been added to Tools > Options > System Options > File Locations > Referenced Documents.
- Searches the path of the active document, then recursively searches the path where the referenced document was last saved.
- Searches the path where you last opened a document, then recursively searches the path where the referenced document was last saved.
- Searches the path where the software last found a referenced document.
- Search the full path where the document was last saved without a drive designation.
- Searches the full path where the document was last saved with its original drive designation.
- Allows user to browse to the document manually or suppress the missing reference and continue opening.
The sections below further define the general search routine steps in more detail.
Search in memory
The first place SOLIDWORKS searched for a reference document is within the computer’s RAM for files that are already opened with the same name. If files are named using generic names, this may cause problems if a file is opened with the same name as the one being referenced.
Example: If an assembly is opened that references a file named HOUSING.SLDPRT, and you currently have a part with the same name opened, used for another assembly or project, then SOLIDWORKS will display ‘Referenced document has non-matching internal ID. Would you like to use it?’ You can then choose to replace the HOUSING.SLDPRT being referenced with the file opened or continue to open the correctly referenced ones.
Search in Specified File Locations
The next place SOLIDWORKS will search for a file is in whatever folder that’s listed as a Referenced Documents folder in Tools > Options > System Options > File Locations > Referenced Documents. Click ‘Add’ to browse to a folder and add it as a Referenced Documents folder.
Once the assembly is opened and saved with the updated references, the component properties will automatically update and the Referenced Documents folder is no longer required the next time the file is opened.
Note, be sure to enable the options for ‘Search file locations for external references’ in Tools > Options > Systems Options > External References.
If you changed the name of the upper-level folder, you would only need to add the upper–level renamed folder and then the system will automatically search subfolders for the same sub-folder path and filename. For example, if your mapped network drive changed from ‘T:\Renamed Folder’ to ‘Z:\Renamed Folder’, then you can add ‘Z:\Renamed Folder’ to the Referenced Documents list to recursively search for references in that location.
Last Known/Saved Location
Searches the last saved location of the reference file. The last saved location of a component in an assembly can be viewed by right clicking the file in the FeatureManager Design Tree and then selecting Component Properties.
Browse for file
After the system has completed all the other search steps in the search routine, the user is prompted with the message ‘Unable to locate the file…’ with 3 choices to either browse to a new file, suppress the missing file, or suppress all missing files and continue opening.
Example: The HOUSING.SLDPRT file was renamed (not moved) to HOUSING_BELL.SLDPRT. The next time an assembly opens which references the HOUSING.SLDPRT file, the system will not be able to locate the file and then it will prompt the user to browse to the file. The user can select the HOUSING_BELL.SLDPRT file, save the assembly, and now SOLIDWORKS has updated the file references and “knows” where to find HOUSING_BELL.SLDPRT for that assembly.
If you have any questions regarding the SOLIDWORKS search routine or missing file references when opening files, feel free to reach out to MLC CAD Systems technical support. MLC CAD Systems can also provide services to assist with reviewing and possibly repairing/recovering larger data sets if file references are incorrect or missing.