incontext references

I have a sheet metal assembly made up of parts and sub-assemblies. I
like to etch mark mating parts when laser cutting for our welders to
locate parts. I do the etching by adding sketches to the parts, while
working in the assembly; this uses the edges of welded parts for
sketch references. The etching is shown on the flat layout drawings
and transfered into the laser g-code program from a dxf of the
drawing.

My question - why can't I add an incontext reference to a part that
already has another incontext reference in either the main assembly,
or its sub-assembly?

Of course I use it anyway but, why does SW not let me make this an
incontext reference?

Thanks for any help. Davis

 

Hello Davis-
Have you tried this?
"Edit In-Context" each part and create a sketch, using the edges you
require. Now click on "Display Relations" and delete all "external"
relations. The sketch will turn blue. Now dimension the sketch or "fix" as
needed. Don't extrude cut yet, just exit the sketch. Repeat this process as
needed while still "in-context". Now, "exit" "in-context" rebuild and save.
Now open the part file. Double check that each sketch has no external
relations. Edit each sketch and extrude cut. This can be done a couple of
different ways, the goal is to grab what you need and then delete each
external relation before moving on to the next feature.
Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com

 

My question - why can't I add an incontext reference to a part that

tools>options>system options>external references> check the box for "allow
multiple contexts for parts ..."

 

Be very careful. You can get into boatloads of trouble when you have
multiple contexts. In particular, renaming assemblies becomes a nightmare.
Parts will end up keeping their associations to the "old" assemblies. It
seems that we have had parts reestablish the old associations after they
have been changed, but I'm guessing this is actually pilot error, that we
only thought we had fixed the associations. Going through and breaking all
of the relations, then reestablishing them to the correct assembly is a real
pain.

It sure would be nice if SW allowed you to break relations one at a time, or
one feature/sketch at a time, instead of breaking every relation in the
part.

Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"

 

Be very careful. You can get into boatloads of trouble when you have

i use sw explorer and haven't noticed any anomalies. do you use sw explorer
to rename?

 

We've renamed assemblies both with SW Explorer and inside SW. I don't know
for sure which method was used on the assemblies we've had trouble with, but
I think they were renamed with SWE, as that was the method we used the most.

Jerry Steiger
Tripod Data Systems
"take the garbage out, dear"

 

Thanks for the responses.

I don't really want to delete the relationships from the sketches back
to the assemblies. We will typically prototype a new weldment, then
wait 6 months or longer until the production release by our customer
(we are a job shop fabricator). The production release always involve
numerous revisions to parts and the assemblies. If I delete the
relationships, then that adds work in updating to the latest
revisions.

This particular customer uses an old version of ACAD, so we aren't
sharing SW files, the way we do with customers running SW. They also
do other fun stuff, like reusing part numbers from obsolete items -
same part number, different usage, different description. Allowing
parts to have multiple would be a bit scary.

Thanks again for the input. Davis