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Although Pro/ENGINEER was originally designed to be an assembly mode modeler, there are more mature ways to do what you set out to do in your explanation.
Its called top down design and the term comes from software programming. See Wikipedia.
Other terms used to describe specify to proe is skeleton modeling or copy geometry.
A) Does the 3d data change? or what you are sent is the final version?
B) Are you the only one working on the files?
C) Do you expect to have variations of your design that you will need to show as possible options?
D) Are you able to use a skeleton part?
E) How accurate are the models you are sent? e.g.: are they built as the nominal size of a manufactured part or a concept part just to show form
I create templates with the neccesary datums, parameters, saved views etc. that I require and then use these to create parts fromfor top down design activities. I establish a master datum which I then assemble most major components to, this enables easy reassembly (should it be required) and a good reference point for copy geometry fetaures within the parts. The master datum in your case should probably be the engine datum. By the way you need an AXX (Advanced Assembly eXtension) license to create or modify skeletons.
nofalloff - As some have indicated, thereis a lot of 'it depends' here.
To start off, assemble it to things that make sense for what it does. In you motor mount example, to assemble that to the chassis or engine default CYS doesn't make a lot of sense to me. When I open the mount alone, it's going to be offset quite a bit from the default planes, Drawing views are then much bigger than the part and overlap, causing difficulties working with the drawing. Worst of all, the position of the part in the assembly has no relationship at all to what it will actually be mounted to. If the chassis changes and the mounts move forward 2", your mount won't.
So I'd try to assemble it to the frame rail and the features on the framethat define it's position. You might think that makes it less robust, and I guess technically you'd be right. If the features it's mounted too change, the mount's position might fail. Good. If the features change in such a way to make the mounting scheme invalid, I want it to fail. That signals to me that there'sproblem that I need to address in the design or with the guy responsible for the frame.
That said, the big question becomes is external references permissible? If yes, then we start talking about how to accomplish that. There are several ways to do so, more thanI can cover here, but one thing I don't do is directly reference other parts in that assembly or other sub assemblies. It can create a tangled web of dependencies that's tough to unravel and manage.
In your mount example, I suspect that the engine & chassis guys don't want to have dependencies to their models. If so, then I spend some time measuring the assys, building neededref geometry in my mount model to represent bolt holes, mating surfaces, etc. I'll build in part mode and go back and check in the assy. Use real design dims. In other words, if you need to maintain a 4" dim from a mounting hole to the mating surf make the feature so the dim controlling it is 4", not 3" from a datum plane that happens to be 1" away from the hole.
I would still use top down design to assembly a motor assembly. That way leverages Pro/ENGINEER and compensates for my lack of intelligence. Some of you are probabably hitting IQ of 150! I am at the 1st grade only IQ141 as I recall.
Anyway...
I think of Pro/ENGINEER and the top down design as Teddy Roosevelt's big stick analogy. A complex mechanism becomes a much more simple problem where I can find and narrow down solutions efficiently.
To make a more direct reference to your assembly (without actually referencing your assembly) one can use copy geometry .... i have recently incorporated this type of excersie in a class...
1 design your part without actually making a parent child relationship to the surface reference from your copy geom. Say for example you are creating a heat shield to an exhaust manifold that requires a 20 mm offset. in the end you siimply delete your copy geometry and the rest of your geometry does not fail because we made only sketcher relationships.
Oh, I agree. I don't design anything with 2 or more parts without a skeleton anymore. Exactly what you said, it helps me keep track of stuff. There are times where the folks you are working with- either the client or the other folks on the project - don't want the external refs. Particularly if it's a client requirement, you've got to dowhat they're comfortable with.
One of our customers found too much top down bogged down their assembly so much it brought the entire project to a halt. Anything over 2500 parts in an assembly that has top down design might be excessive. As computer get faster and users gain more advanced skills we can only hope we push the envelope. pun intended.
My second example from above would be :
2 use a simple IGES export of the significant part of the exhaust manifold. Offset that geometry and use that to design your heat shield. With the new tools in Wildfire users can easily delete the IGES reference and manage a simple fail and ... no references to anything exterior.
Thanks guys. What this illustrates to me is that I clearly need some training. Bart, It's too bad I'm not near Chi town. I have spoken to out reseller in the past about classes and they are about as interested in helping me as .
dgs, I often have the problem you described. When I import my start part and align it to the default CS, it is then off in space when I open the part separately. I've been avoiding external references by coping all needed references into the new part. it is rare that i get revisions that are so different that an externally referenced part will fail but the parts files have to be able to stand on their own with out any of the other files from the assembly being present for reference. Most of the way I've been doing things have been methods I have devised on my own with no formal guidance. It doesn't always work smoothly but I have managed to make it work.
I had access to the PTC.com/learning but there didn't seem to be anything there that was applicable to this. Our account has since expired.
I am new this forum and have been re-educating myself with WF3 for two months now after a couple years away from it. (SW & ACAD) Nofalloff and I walk similar paths and have similar questions so I thought I would add to this thread.
If I wasdesigning weld fixtures around assembly weldments,where I have many parts(ie.100) used to to create my fixture parts, (ie.50) and there can be no references between the two assemblies all said and done...would the modeling advicebe any different?
Currently I create a master fixture assembly via a start assembly, bring in a model assembly using default, thenbring ina fixture assembly(s) underneath. As you can imagine, if I leave any mates between the assemblies...Pro_e has some extra work for me to do.
And, is there a way you can mirror a part in assembly mode and retain the same name?Mirror is a quicker route to create geometry that is symetrical as opposed to copy & paste and without the remating, buthas a tendancy to create a rather lengthy BOM stucture of 1ea.
Don't mean to ramble but one day soon with any advice at all, I will master this software! Thanks for any and all comments.
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