Sending files to vendor...'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?



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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.

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jeppe sorensen

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!).


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