Sending files to vendor...

So...you've just designed a car in SW. You need to send the files for
the external sheet metal out to your fabrication shop. They have SW.
You only want to send the relevant files. They don't need the nuts,
bolts, washers, suspension, glass, engine, seats, etc. The design is
top-down and has lots of external relations to alignment sketches,
planes and, of course, lots of mates.

How do you do this? How do you extract 12 parts and a few assemblies
to send out to a vendor?

Best I can figure is to use "pack and go" to flatten the design.
Then, manually separate the files you want. And, finally, go one-by-
one and lock all external relations.

How do you avoid sending the design for the whole car to the guy who
just has to make your hood ornament?

Thanks,

-Martin

 

Send them a Parasolids or STEP file instead. Then you can hide
everything you don't need to send and then export just those that the
vendor needs.

 

Please see below:
Best regards
Jeppe

Good for the design phase. Bad for the production phase.

And how will you handle the revisions that you will inevitable get?

When moving to the production phase you have to lock or break all the
external references. Otherwise you will have a design spagetti. Move one
line and everything else changes...

Avoid working with external references in the first place.

 

Avoid working with external references in the first place.

What's the point of using a parametric CAD system then? Not using
external references exponentially increases the potential of making
costly mistakes.

Yes, if the wrong approach is used with external references you can
end-up with a fine mess. I, of course, learned this the hard way when
I was getting started with SW.

My rule at this point is simple: Do no mate or create references to
part geometry whatsoever unless absolutely necessary. Instead use
reference sketches and planes at the top-level assembly and EVERYTHING
is referenced and mated to them. You can easily transfer reference
geometry to lower level assemblies by creating reference sketches or
planes within them that refer to the master assembly. The only
exception to this rule are parts, components or assemblies that you
purchase. Those should exist on their own and not depend on
relationships to other assemblies.

Revisions are relatively simple. You move or re-dimension top level
sketches and rebuild. What's neat is that you can completely take out
parts from the assembly and things don't explode on you. Example:
Engine->head gasket->valve head assembly. You can delete the gasket
and nothing breaks because everything else is mated and dimensioned to
reference sketches rather than faces or vertices or features of other
parts or assemblies. You can then substitute the gasket with an
entirely different part (or assembly) and, again, nothing breaks.

I learned this lesson two-fold when using FloWorks with SW. We
created test assemblies where hundreds of different configurations
needed to be simulated. As the simulations were run in batch mode the
only way to safely "morph" the assembly from one configuration to
another was to use top-level reference sketches and geometry as much
as possible. With that in place, using a design table and Excel to
radically alter the morphology of the unit under test was child's
play. You could change dimensions, mates, suppression states, even
sub-assembly part configurations and geometry. With everything
remaining mated to top-level reference entities nothing ever broke and
we could run hundreds of simulatied scenarios spanning many days of
processing without trouble (well, outside of FW/SW crashing that is!).

-Martin