Why is my SOLIDWORKS Assembly opening the wrong components?

Has your SOLIDWORKS Assembly opened the wrong components with error: ‘Referenced document has non-matching internal ID‘? Don’t worry, it’s very easy to fix. Let’s take a look at why this happens and how to get it sorted via. referenced documents.

The SOLIDWORKS search routine for referenced documents

When you open a file such as an assembly or drawing, you’re not just opening that file, you’re also opening all other components used within that assembly or drawing. Understanding the search routine for referenced documents is key.

There is a specific search routine that SOLIDWORKS uses to find the referenced documents:

1: RAM

SOLIDWORKS will initially look in the RAM for a referenced file. Let’s say you have a part called plate already opened in SOLIDWORKS and you open an assembly which contains a part called plate within it, SOLIDWORKS would open the assembly and populate it using the plate opened in RAM. Even if it’s a different part to the one saved with the assembly. Therefore, it’s best to have unique file names for parts!

2: The paths that are specified in Tools->Options->System Options->File Locations->Referenced Documents

By adding a folder to this location, you can force SOLIDWORKS to look in this folder when searching for referenced documents. This can be useful if you’re moving an entire project from one location to another, or separating projects into different sub folders.

3: The Last Path Specified

SOLIDWORKS looks in the same location as where the assembly was opened from for referenced files. For example, In SOLIDWORKS you could pack and go an assembly to a single folder and transfer that folder from one machine to another. SOLIDWORKS can open the assembly correctly on the other machine because all referenced documents reside within the same single folder.

4: The Last Path Used by The System to Open a Document

If SOLIDWORKS didn’t locate the parts in the same folder as the assembly, it will look at the last path used by SOLIDWORKS to open a referenced file. SOLIDWORKS will skip this step in a fresh session where no other paths have been used.

5: The path where the referenced document was located when the parent document was last saved

When you save an assembly, it stores the locations of all the parts and subassemblies that are within it. The drive letter that the documents are saved to is not used at this stage. SOLIDWORKS uses the current drive. This means that if all your documents were stored on the C:\, and the drive letter was changed to D:\, SOLIDWORKS would still find the files because D:\ would be considered to be the current drive.

6: The path where the referenced document was located when the parent document was last saved with the original disk drive designation

This is basically the same as step 5, but the original drive letter is taken into consideration

7: Browse for file

If SOLIDWORKS still can’t find the file, it will give you the opportunity to browse for the file. This is useful if you have renamed the file through Windows Explorer. The assembly will not know that the file name has changed, so it allows you to replace the old reference name with the new one.

If you need to see where the referenced files have open from you can select File->Find References. This shows you every part within your assembly and the location it has been opened from.

That’s it! We hope you found that useful.

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	About the Author: This tutorial was written by Elite SOLIDWORKS Applications Engineer and Technical Support Manager, Alex Aprigliano. Alex Has been with the Visiativ Technical Support Team since 2007