NX -> Pro/E import / conversion?

[JonathanHodgson]

Does anyone here have a working knowledge of NX?

I've been provided with some client models in NX format, but as I don't use NX I'm importing them into Pro/E to incorporate in a new assembly, and in some cases to modify - although for illustration rather than manufacture.

I've opened the assembly in NX, exported as STEP, and imported into Pro/E (WF4). In principle this has worked, but many of the more complex parts (cast gearbox casings) have failed to solidify, in one case with myriad tiny gaps, e.g. at the edges around drilled hole points. This is making them rather awkward to modify.

Does anyone know either a) a better way to do the conversion, or b) some settings I can change (probably in the NX export) to improve the STEP accuracy?

IDD isn't an option - I've tried on a couple of models and the Search tool fails to find any gaps; hunting them down manually would take hours, and finding the last ones would be almost impossible.

Thanks!

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[RadovanMíček]

Hi Jonathan

I am not sure, however if you have NX and Pro/E on the same PC, you can open NX geometry directly. (NX.prt)

You can try PTC Distributed Batch too.

Regards

Radovan

[JonathanHodgson]

Thanks Radovan.

I have access to both, but they're network installs running from a licence manager - will that work?

[RadovanMíček]

I hope so.

At this time you must have special licence: check http://www.ptc.com/product/creo/interface-for-nx

Check this idea (NX in Creo 3.0)

http://communities.ptc.com/ideas/1477 (copy/paste this link)

[JonathanHodgson]

Ah... we don't have that licence.

[DaveClark]

have you tried exporting the items as parasolid files (x_t)? i've had greater success with this than step.

[RadovanMíček]

Yes, all depends on export/import settings. Set Retrieve External Accuracy in import process.

[JonathanHodgson]

Hi Radovan,

Where do I set this? Normally I just open the STEP file and I get no further prompts.

[RadovanMíček]

0:19 sec (use Tempalte and set this option).

I hope this works from Wildfire 5.0

[JonathanHodgson]

Just tried exporting one component as Parasolid. It has one missing surface that I can see, and I've just spent the last half hour failing to patch this using IDD. It also has several large holes that appear to be 'skinned over' with geometry that I don't seem to be able to select.

Also, I couldn't make NX export the whole assembly as Parasolid - is this supported?

[DaveClark]

As I look back through NX parts I've received from clients, it seems that every NX assembly is really a multiple body part, where I have to select each one to export separately. I have no idea why I receive assemblies this way.

I did run a quick test, where I threw two parts together to make an assembly to export as a parasolid. I couldn't seem to select the assembly. I had to select the parts individually, but I could get all of them in one file. Creo did recognize the the parasolid file as an assembly, but it started naming the parts test_1.prt, test_2.prt instead of the names that were used in NX.

My apologies if this wasn't much help. I just try all the options I can before ruling something out.

[JonathanHodgson]

Thanks, it was worth a try.

I've just tried Parasolid on another, simpler component - but both the STEP import and the Parasolid version refuse to solidify, despite showing no single-sided edges in wireframe view.

[TomD.inPDX]

I have never had problems with NX files unsing STEP 214 format exports. Assemblies have always been exported as assemblies but you do have to select all the components you want to export. There are issues with NX if it is tied to TeamCenter but normally the issues are on import, not export.

If you want me to take a look at your file, let me know. I've healed a few files using Cadkey '99

[JonathanHodgson]

Thanks Antonius, but it's customer data so I can't share it.

I've just tried importing into Creo2 but the parts still arrive with tiny gaps. I miss the old (2001?) 'Zip Gaps' function - it wasn't perfect but it was a darn sight easier to do something with than the current IDD.

Radovan, the default accuracy option seemed to be External - I've tried that and Automatic, with neither producing a solidified component.

Oh, and it takes about half an hour to import the STEP each time (flat out on one CPU core).

[JonathanHodgson · Accepted solution]

Well, that turned out to have an easier fix: I slackened the Absolute Accuracy from our default of 0.01 (mm) to 0.05. Both the problem parts were suddenly able to be solidified.

Wish I'd tried that one sooner...

[TomD.inPDX]

Since there are several places where accuracy is managed; exactly how and where did you set this?

[JonathanHodgson]

Working in the (already imported and saved as Pro/E) .prt file, Edit->Setup->Accuracy.

Since the import had picked up our start parts, it was already set to Absolute, and changing it from 0.01 to 0.05 fixed the two components I was particularly interested in.

[TomD.inPDX]

Darn, that is not what I was thinking. I was hoping the import operation had a manageable accuracy setting.

Thank you for clarifying this.