18 Replies Latest reply on Oct 28, 2009 3:30 PM by Lenny Bucholz

    STEP conversion takes forever and has errors

    Chris Mellen

      I have been trying to save an assembly file as a STEP AP203 file.  I was finally able to get it converted, but it took 1hr 40min.  I then sent it to my client who wanted to forward it on to his suppliers.  His tested it out by importing it into ProE, but was not successful.  The program hung and never imported all the way.  He sent me a log file that indicated the STEP file was importing with many errors (this log file is attached).  I don't know know if the original files are corrupted somehow (they seem to be built robustly) or if there is a bug in the SW that's preventing a good STEP file conversion.  I'm wondering if others have been having similar issues when trying to convert to STEP (or even IGES - I don't know if a problem with IGES conversion would be related).  The files I'm converting (all assembly files and part files) add up to about 170MB.  I don't think that's too humongous to work with, but I could be wrong.  If anyone has any input, I would appreciate it.  Thanks!

       

      -Chris

        • Re: STEP conversion takes forever and has errors
          Daniel Smith

          The Rx doesn't apear to show any issues, unless I'm missing something.

          Converting a 170mb file to step may take a long time, I've never tried to convert a file that large.  I would open the step file and confirm on your system, maybe the import into Pro-E is the problem?

            • Re: STEP conversion takes forever and has errors
              Chris Mellen

              Thanks for the response Daniel.  I haven't yet tried importing the step file into SW.  I was assuming this wouldn't work cause the file is so large, but I'll give it a shot.

              The log file seems to indicate processing problems and warnings for a few parts...cup shelf, grill, frame lower.  I really don't know how to interpret these errors, but it does indicate that a lot of things (surfaces, curves, etc.) were "skipped."

                • Re: STEP conversion takes forever and has errors
                  Daniel Smith

                  Was the step 170mb or your sw file?  I just tried a little experiment with an asm of mine that was 15mb and saving it as a step blew it up to 59 mb.  After saving it I opened the step file (which took nearly 10 min.) and several parts had rebuild errors.  I also noticed that on my asm that the parts with errors were missing faces and surfaces (similar to what you described).  OOoooooooohhhhh, It actually creates a huge problem.  CREATE A SEPARATE FOLDER IF YOU TRY TO OPEN THE STEP AND OPEN IT FROM THERE.

                  Can you customer import a SW doc into Pro-e?  Maybe taking out a step (no pun intended)  will be les problematic.

                    • Re: STEP conversion takes forever and has errors
                      Daniel Smith

                      Saving as an iges made my file 99mb...  And it locked up my system when I tried to open it.

                       

                      I guess my next question is this, can you save the asm as a part?  Do they need your model as an assembly?  

                        • Re: STEP conversion takes forever and has errors
                          Chris Mellen

                          We've tried IGES as well, but as you found out, it actually creates a larger file than step.  And, the iges files also have errors.  STEP is the preferred format which is why I'm focusing on that and I'm under the impression that step files tend to be less problematic than iges, but I could be wrong.

                           

                          I don't know if saving the assembly as a part would help, but we do need the assemblies intact.

                        • Re: STEP conversion takes forever and has errors
                          Chris Mellen
                          The step file ended up being 148mb.  The main assembly file is about 27mb but all the files (main assembly file, all subassembly files and all part files) add up to 178mb.  I tried opening the step file, but force quit after about 40 mins.  I may try opening it again tonight when there is more time to let it run.  What you discovered with your step file is interesting.  Maybe there is something wrong with the step conversion in SW.  I wonder what can be done in that case?  I actually asked my client if he tried taking the solidworks files into ProE before exporting as a step (he has both ProE and SW, but I only have SW) but he hasn't gotten back to me yet about that.  Do you know if ProE can open native SW files or do you need to convert them to ProE from SW first?  I tried to convert to ProE this morning but had to force quit after the program got hung up a while.  Again, I can't let the program process the conversion for hrs at the moment.  May try tonight.  Thanks for all your input Daniel.
                        • Re: STEP conversion takes forever and has errors
                          Jerry Steiger

                          Chris,

                           

                          No doubt you are far past worrying about the particular files that you were having trouble with, but I would try saving the individual parts to STEP that had problems according to the log, then import them back into SolidWorks. If they come in with problems, try Tools/Check with "Stringent solid/surface check" checked on the original SW parts to make sure that they don't have problems. If they fail the part check, find and fix the problems before exporting them.

                           

                          If the original SW parts don't have problems but the imported parts do, try fixing the problems with the Import Diagnostics tools. If necessary you might have to use other SW tools to fix some. The point of doing this is that sometimes you can fix the problems and re-export them and get better files. (You'll have re-import into SW to see if it helped.) If you do get better files, you will need to make an export assembly with the improved parts replacing the originals.

                           

                          Jerry Steiger

                            • Re: STEP conversion takes forever and has errors
                              Chris Mellen

                              Jerry,

                              Thanks for your reply.  I ended up doing pretty much what you said.  But, even the STEP files that looked good in SW were still showing errors in the log file when my customer imported into ProE.  I still don't know the answer to that one.  In the end, I exported the main assembly as a ProE file (something my customer said he tried in the beginning but said was not working - he runs both SW and ProE).  There was one part that did not export as ProE so I saved it as a STEP instead and imported that into SW to fix any problems with import diagnostics (as you said Jerry).  Import D. fixed the problem and I exported that file as ProE.  I delivered all the ProE files to my customer and he said he was able to open the files with no errors...problem solved.

                               

                              So, if anyone is interested, the following is the short list of what ended up working...

                               

                              1. Tools>Options>System Options>Performance....Checked the box next to "Verification on rebuild."


                                   This did a more thorough than normal check on my original solidworks files.  It showed some problems with my original files that was not as evident before.  I was able to fix this with a little rebuilding.

                               

                              2.  Ran another check with Tools>Check>Stringent Check on all the part files that were problematic.  Everything checked out.

                               

                              2.  Exported the main assembly file as ProE.

                               

                                   This worked for all files but one part file.  For that file, I did the following...

                               

                              3.  Exported the file as STEP and re-imported into solidworks and fixed a general geometric error with import diagnostics, then exported the file agian as ProE.  I sent all the files to my customer who was able to open the main assembly file with all parts and subassemblies within it (in ProE).

                               

                              I still don't know why my customer was having problems with a lot of my STEP files.  May have something to do with how SW exports to STEP or how ProE reads the STEP.  Maybe STEP conversion has problems with certain geometry while other file conversions work.  I don't know.  This will hopefully get better with future software upgrades.

                               

                              Thanks for everyone's input!

                               

                              Chris

                                • Re: STEP conversion takes forever and has errors

                                  Hi Chris,

                                   

                                  I'm using Inventor 2010 and used to have pretty good luck with STEP files from Solidworks; however, I have several vendors and clients that use SW and the STEP files now are often plagued with problems.  These are usually missing faces.  I called my Autodesk tech up and asked what the issue was; apparently SW converts with significantly lower accuracy than INV, and you end up with faces not meeting and holes in the models.

                                   

                                  I downloaded  IDA-STEP which is a free STEP viewer and the same problems occur using that.  So I would definitely say the problem is with SW and its STEP converter.

                                   

                                  I'm currently looking for a good way to get solid data out of SW into INV.

                                   

                                  Regards,

                                  Jim