Reply

Simplifying part made from .step files in ST6

I've received a large assembly .step file from a vendor that I need to use in my models, but don't ever need to be able to edit it (other than maybe putting some holes in it).

 

I bring the step file in as a sold edge part, and my tree looks like the photo below with a bunch of Design bodies, contruction bodies, part copies, and then it'll let you make 1 body feature. I really have no idea what any of that means.

 

tree.JPG

 

Is there a way to just combine all that junk into ONE body feature? Or just any suggestions for simplifying the thing so it's not making my models so hard to work with?

 

I've looked and found something about the "union" command, which I tried choosing that, then dragging over to select my entire model and get this error message...

 

error.JPG

4 REPLIES

Re: Simplifying part made from .step files in ST6

[ Edited ]

First you'll probably want to toggle all the construction bodies to design bodies. What I do if I don't want all the discrete bodies listed because I don't need them is open a new part and do an "insert part copy" of this converted part. That will make it one body. But I don't think it hurts to "carry around" all those bodies. Maybe someone can explain if it does have some processing or memory costs.

Edit: Oh yeah, do an optimize whenever you see the little "I" icon next to a body. It will change when done.

Bruce Shand
ST9 MP8 - Insight - Win10 - K4200

Re: Simplifying part made from .step files in ST6

Sometimes it is possible to turn all the construction bodies into a single body feature. The method I am showing you now results in a very minor geometry error as all the faces are shrunk by 0.02mm inwards. Since this is a vendor model this is a non-issue in my world, and in the bigger scheme of things an error of 0.02mm I can accept to obtain a single body feature.

 

Whenever there are point or edge conditions between bodies within a Solid Edge model. The result is then many bodies and a single body cannot be obtained. In the example video clip I show four bodies, with their edges touching. I first export a parasolid model and import it without being successful. I then offset the faces by a small fraction of 0.02, then export to parasolid file, which then I import into a successful single body feature part model.

 

I am also including the part file for you to play with first. Good luck, as each vendor model presents its own unique set of challenges when trying to convert into Solid Edge.

 

PS: I strongly recommend you spend some quality time trying to figure out those different kinds of junk (elements) you refer to. You will need to when converting third party models into Solid Edge.

 

Re: Simplifying part made from .step files in ST6

[ Edited ]

The offset trick is a good one if you can find the problem area. However, in all my importing of step files over several years I have yet to run up against this problem.

Just an FYI: You can also make the offset go in the other direction, so the bodies have no contact at all rather than a small overlap. Either way can give you one body.

Additionally, I always wonder why people export to another format like stp or parasolid so that they can then import it. Why do so when "insert part copy" is available, saving a step? Is there some advantage to exporting/importing over a part copy?

Bruce Shand
ST9 MP8 - Insight - Win10 - K4200

Re: Simplifying part made from .step files in ST6

There really isn't any issue with having multiple bodies and it avoids the "zero thickness non-manifold" issue, but I would recommend following @bshand's advice of making them Design Bodies asthey are far easier to work with in assembly and draft.


Thanks,
Ken

Production: ST9 MP7
Testing: ST10