Have you tried it using Solidworks explorer, as in the Solidworks explorer program and not the right click thing? I've had the same trouble for a while. My VAR replicated the behavior and was told from Solidworks that we need to use explorer. They are also not sure when its going to be fixed.
I can tell you however that since using the full Solidworks explorer program everything has behaved as expected.
Unfortunately, using Pack and Go within the Solidworks Explorer did not correct the problem. The external references still did not update.
Here when I do a Pack & Go I want it to be totally disconnected from the original sketches, parts or assemblies. My issues were they stayed connected then when I wanted to work on a "New" assembly a pop up would come up telling me I can only update in the original assembly/part etc.. Then I need to break all connections/relations and re-connect in the new pack and go file..
Me and Pack & Go just don't get along, I loose patience and Pack & Go just packed up and went where it wanted to.....
I found a work around that should be usable until SolidWorks programmers fix the issue.
- Create a new folder, name it whatever you want
- Copy and paste the desired assembly file in the new folder.
- Go to the original assembly file and right click, then go to SOLIDWORKS > Rename.
- When the Rename Document dialog box pops up, type in a new name for your assembly.
- Click the check box next to "Include virtual components." If a Warning dialog box pops up, just click OK.
- Click on the "Search" button. A few check boxes should populate under the "Update where used by" box.
- Deselect every check box EXCEPT for the one next to your original assembly.
- MAKE SURE the check box next to your copied assembly in the new folder is DESELECTED.
- Click OK. The assembly's name should be updated (along with it's external references.)
- Move the copied assembly back to the original folder and delete the new folder.
Hopefully this helps others dealing with this issue.
A good colleague of mine pointed me to a solution. In my case I had to copy a complete project to another folder (duplicate project) with find/replace on project number. This worked well, until I opened the main assembly from the new folder. It referenced to parts from the older folder as the OP describes.
Take note that when you opened the new main assembly, it opened with all assembly's and parts on lightweight. My colleague showed me that if you open the assembly from Solidworks and select 'Resolved' at the open dialog box on the dropdown menu 'Mode', that it worked. Now it showed all assembly's and parts from the new folder.