Joined part, broke ext refs, what now?

I have been trying to figure this one out for a while. I imported an
assembly, and decided I wanted a single part out of the assembly. So
I joined the assembly. I then decided I did not care to keep the
original assembly, so I broke the external reference link and deleted
the original assembly. Well I forgot (this has happened to me before)
the joined part is always going to reference the original assembly it
was created in.
My question is can I wash this joined file from any reference it had
to its creator? Every time I open the assembly this joined part is
in, I get a message that it can't find the parent assembly.
Everything works fine otherwise. It's just that annoying message on
loading.
Mike

 

Right-Click on the Part name at the top of the design tree. In the list
select "List External Refs......." In the dialog that comes up select Break
All at the bottom you will probably have a dumb part then.

Corey Scheich

 

Mike,
Since it's a joined part you probably aren't going to be doing anything with
it?
How about creating a STEP file and re-inserting it in your assembly?

Richard

 

Sorry about that.

If you set the option

External References
Load Referenced Documents

to NONE

you will not get this error.

Corey

 

Or, better than STEP, use Parasolid...

--Todd

 

If you're using 2003 or later you can save an assembly as a part without
using the join command. You might keep this in mind for the future. We
use it all the time for assemblies we get from customers. This method
brings no references with it.

Dave H

 

I didn't see that. Save an Assembly as a part. That's great you can
even save it as surfaces or solids. I did not know this was possible.
It was probably in a presentation somewhere, but I may have been
zoning at the time. That's why I like this group. Everyone knows
some other method.
I've used the translate through the step format before and that works,
but it just seemed like a going from NY to Chicago via Miami type of
things. It's just too bad that you can't remove or change that
relationship in solidworks explorer. The reference shows up but
doesn't allow a change. Thanks everyone for all the great
suggestions!
Mike