NX to SW via .stp

[Cityjackit]

Evening all,

Its been some time since quality productive SW usage. Back on plastic parts for my current company.
They have been receiving production injected parts for many years without a fully dimensions print, much less critical dims with tolerances. Nobody. Molder or my company included seemed to have current models. Or at least that anybody could track down. All changes were done via cocktail napkin sketches or "nice to have" email communications. Nothing has been tracked or revisions.
I finally got the shop who made the molds to give me their most recent models. They gave me native NX files as well as .stp files. When I bring the .stp files in, they are a solid body. Correct but not editable features.
Question; is there any way to get an NX files, native or .stp into sw where I can change, ads, or subtract individual features?

Thank you ill and have a good week.

[gerard]

Pretty much your only option is the recognize features functionality.

Saying that, the process creates fairly oddly created models. Typically they are not dimensioned, will be referenced to planes other than the base (added planes) and complex features often don't get recognized.

This all makes the models coming out of the process of limited usefulness.

You can add or subtract from an imported "blob", you just can't parametrically change it.

good luck,

g

[Glenn Schroeder]

Can you get them to send parasolids instead of step files? I can't make any promises, but SW often plays nicer with parasolids.

[DanPihlaja]

As @gerard says, the short answer is no.

The long answer is.....bring in the solid blobs, and add/subtract only when needed, and make drawings of them.

Short of remodeling (recognize features is ONLY useful if your part is basically a plate with a couple of holes in it [I am exaggerating, but seriously, it is only useful for things that you can remodel in less time than it takes to run the feature recognition feature]), there really is nothing else you can do.

[gerard]

Can you get them to send parasolids instead of step files? I can't make any promises, but SW often plays nicer with parasolids.

I've had mixed results at least with models from CREO.

Yes the solids seem better behaved, but the last one I had, the step file had the full suite of sub assemblies, and the parasolid assembly was completely flat, no sub assemblies.

[zxys001]

..you'll need to directly edit "Insert/Face/Move" or cut/extrude/add/subract/,..

[Cityjackit]

Thank you guys. Well, it looks like what I thought. Bring in the solid "blob", then add and cut as needed. Make drws from this then.

Thanks guys for all replying.

[Cityjackit]

ZXYS001, not sure where you are going here. What is the path you are providing? I'm not sure if you are saying to just add and cutaway what I need or don't want or are providing a way to remodel to something I can control.

Sorry, I do not follow, but thank you sir.

[Cityjackit]

Can you get them to send parasolids instead of step files? I can't make any promises, but SW often plays nicer with parasolids.

Can NX export a parasolid? Not sure what a parasolid is. Its worth a try for sure.

Thank you

[DanPihlaja]

Can NX export a parasolid? Not sure what a parasolid is. Its worth a try for sure.

Thank you

Solidworks native kernel is parasolid (x_t format). This means that there is no translation happening when Solidworks saves as a parasolid. That is all that is happening is that the software is just saving out the geometry.

NX's kernel is also parasolid.

Therefore, there is not translation happening when saved as a parasolid.

If you save out the NX stuff as a STP file, then it is translating it to STP. Then when you open that STP file in Solidworks, another translation is happening.

This is akin to having 2 people trying to talk through 2 different interpreters.

So Parasolid is the way to go here.