STEP files from SW to Pro-E

[cmellen]

I have been trying to send a customer STEP files of parts and assemblies that were created in SolidWorks. My customer is opening the STEP files in Pro-E. They are not opening up perfectly, however. He is running log files when importing and a lot of errors are showing up. Sometimes the parts look stable on screen, but the log files are telling us they are not stable.

Can anyone help with this issue? I am not sure if the files need to be rebuilt, or if our attempt at getting perfect STEP file conversion is futile.

I have uploaded one of the STEP files I've delivered to my customer along with the log file to yousendit.com. You can download them by clicking on the following link:

https://rcpt.yousendit.com/730533675/91ac36d696166eaddf6cad96292bea39

Thank you to anyone who could help!

-Chris

 

[DesignerGuy16]

STEP files are neutral format 3D files, but being neutral means it isn't always perfect depending on what/how they are imported.

I've not used Pro/E, but I know a lot of STEP files I import into Solidworks I end up running a surface check and maybe 30% of the time I have to manually fix faces so the geometry is correct/error free. The only perfect import is going to be directly into the native format, but that's not going to happen.

Is the problem that the end user isn't proficient enough to correct any surfacing errors?

James Spisich
Design Engineer, CSWP

 

[cmellen]

Thanks for the reply James.

I don't know that the end user is not proficient in ProE. I think he is expecting perfectly stable files with no post import work needed. I am beginning to think it's a pipe dream cause I've been trying to fix this issue for a week now. I was hoping there was a definitive answer to my problem, but the conversion process may just be too inconsistent to expect perfect results with every type of geometry. Thanks for sharing your experiences.

My customer has been under the assumption that my geometry is faulty. That is really what i've been trying to get to the bottom of. He insists he's gotten perfect conversion from SW to ProE through STEP files in the past.

Haven't ruled out the possibility that there may be things I could change with how i've constructed the files. I just don't know what that would be yet. Seems to be a complex and geometrically sensitive thing.

Chris

 

[PDMAdmin]

Have you tried IGES? Or maybe a different flavor of STEP (203 vs. 214)?

 

[cmellen]

We did try IGES at the beginning of the process and were getting mixed results, some parts ok, others with errors. The customer preferred STEP so that's what I concentrated on. I've also heard that STEP files are generally more reliable than IGES, but I suppose one should always be tried when the other isn't working.

I also tried STEP AP214 as well as AP203, though I don't know the difference. I got the same results with both. Do you know the difference between the two?

 

[CorBlimeyLimey]

See the Help > Index files for export documents.

SW can Save as to Pro/E part (.prt) or assy (.asm) formats? Have you tried these?

 

[cmellen]

My customer said he tried saving ProE files from my original SW files (he has ProE and SW) and was unsuccessful doing so.

I tried saving the entire assem in ProE earlier today. Halfway through it said it was unable to export one of the parts. Everything else seemed to export. I'll try to save that one part individually, give these to the customer and see what he says.

This does not mean he will be able to export STEP or IGES successfully from ProE, however (which is the ultimate goal). We'll see I guess.

 

[CorBlimeyLimey]

?? I'm sure there's probably a good reason, but why go through the hassle of converting to Pro/E only to re-export as STEP or IGES?

Which versions of Pro/E and SW does your client have? His version of Pro/E may be ahead of the version his SW can export to.

 

[kellnerp]

Here is a standard sanity check on the SW end.

[ul]
[li]Turn on Verification on Rebuild in Options. CTRL Q rebuild.[/li]
[li]While that is on do a TOOLS/CHECK with all options checked.[/li]
[li]Round trip check[/li]
[ul square]
[li]Export as STEP, IGES, PARASOLID[/li]
[li]Re-import from the STEP, etc.[/li]
[li]Do the first two steps on the imported parts. [/li]
[/ul]
[li]Fix any problems that show up. [/li]
[/ul]
You would be surprised how many time SW has trouble with it's own neutral files. General faults are really bad.

Finally consider that SW and Pro/E are competitors. This means they don't give a rip about what the other guy's software does. SW won't license Granite and it is not likely that Pro/E will have the parasolid module. Add to that that the two represent solids differently internally and it doesn't matter that SW writes perfect STEP and that Pro/E reads it perfectly.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[cmellen]

I finally got a set of files to my customer that he said import fine!

I went the save as ProE route. It wasn't working for my customer before, but this time we got it. May be due to a few adjustments I've made to the files over this whole process. Don't know for sure. I did have to perform a work around with one of the parts that wasn't saving as ProE...I saved as STEP first, imported to SW, fixed a "general geometry problem" with import diagnostics and saved that as ProE.

Anyway, he opened the whole batch of files in ProE and they seem to be ok.

Still don't know why the direct STEP from SW wasn't importing right in ProE. I hope to figure that out at some point.

kellnerp, that's good advice about the sanity check within solidworks. I actually learned the verification on rebuild trick earlier this week and it helped me fix a couple hidden problems. All the files check out after going through those steps, but the STEP issue still remains.

Thanks so much to everyone for their input. I hope this might be helpful to others reading this string of posts.

I will let u all know if I figure out the STEP issue.

-Chris

 

[DesignerGuy16]

For Pro/E & Solidworks STEP & Parasolid are the BEST neutral formats to go between. IGES files are pure surface models, and honestly from having to deal with IGES files in the past can be a pain to deal with. Pro/E and Solidworks are completely different in structure and coding so it's bound to happen you'll get errors going directly from one to another.

A good example would be the internal PDF maker built into Solidworks isn't as clean as say an external PDF printer. Sometimes I still export a PDF and get blank views, etc. Not because the PDF was corrupt, just that Solidworks glitched and didn't render the view(s).




James Spisich
Design Engineer, CSWP