When you open an assembly or drawing in SOLIDWORKS, you are not just opening a single file, you are opening all the referenced files too. So if you open an assembly, SOLIDWORKS opens the assembly, as well as all the sub-assemblies and part files within it.
There is an order to which SOLIDWORKS looks for these referenced files. This is as follows:
SOLIDWORKS will initially look in the RAM for a referenced file. So, if you have a part called bracket already opened in SOLIDWORKS and you open an assembly which contains a part called bracket within it, SOLIDWORKS would open the assembly and populate it using the bracket opened in RAM. Even if it is a different part to the one saved with the assembly. This is why it is 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 really handy if you are moving an entire project from one location to another, or separating projects into different sub folders.
3. The Last Path Specified
SOLIDWORKS will look in the same location as where the assembly was opened from for referenced files. As an 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
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. Interestingly, 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 taking 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 really 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.
We hope you found that useful!
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