I have an assembly with parts created top-down, and for what ever reason, some of the parts are pointing to an assembly other than the one they were created in.
The dialog box to list external references wont allow me to redirect, is there a way to do this? I would hate to have to break all these relations.....
Much Appreciated
Not entirely....I was given the work around you have sugested (options/external references/allow multiple contexts for parts when editing in assembly) This allows me to edit what I need.
Still bothers me that there are still parts in the assembly that reference another assembly that they have nothing to do with...
I do have a greater respect for using external references now, and am looking into setting rules for their use.
Thank You!
Dennis,
You might want to check out this thread:
https://forum.solidworks.com/thread/62203?tstart=0
It looks like their could be some problems lurking in the process of renaming files.
Jerry S.
Dennis,
I have the same problems.
Did you found away to edit/redirect the external reference?
Peter
here is something to try. click the open file button in solidworks, and highlight the file you want to modify. in the lower right hand corner is a button that says "references" click that it will list all external references for that particular model. and each one can be modified to change its location if its referencing the wrong one. just double click the part you want to change and in the second open file window that opens find the correct reference point. you will know the file has canged cause it will highlight in the reference window
Thanks Brandon. It seams to work (i hope) But I have already saved all my virtual part with new namse as external files to be able to produce drawings. Your trick did changed to the correct Assembly in the List Externa Ref.. but i still have problems with Feature's Component. I might have to rename all the parts to the old virtual names again..... hmmmmmm I will try it with one part and see.
Thanks again
Peter
let me know how it works for you
Yes, it works. And once it had recognized the new (old) name, saved the assemble and then made a SW-rename back to the desired filename and that also updated correct in the parts external reference list.
Thanks again,
Peter
Dennis,
Did you ever get this worked out?
Did the assembly that the parts were defined in get renamed? That seems like one way to cause this type of difficulty. In that case, and assuming that you need to keep the renamed assembly, one way out of the difficulty is to allow SolidWorks to have references defined in multiple assemblies (check "Allow multiple contexts for parts when editing in assembly" in Tools/Options/System Options/External References).
Jerry S.