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Zip Gaps with imported iges


New member
I'm still finding my feet with PRo/E (2001), and currently I'm begining to think we should have purchased an alternative product!

Anyway, I'm trying to import an iges file into part format so I can make it solid to incorporate some changes to the design. The iges file is full of gaps. The 'Auto Select' command zipped some gaps, but even with the 'MaxGapDist' set to the maximum I cannot zip the remaining gaps manually. Every time I try, the edges remain yellow! I'm currently close to throwing the thing out of the window, but I don't think my boss will appreciate it! Can anyone offer any help?


New member
Can you receive the data in STEP format? I think IGES is a last resort protocol these days. If you can get it in .stp Pro/E is much more likely to pull in a solid, if not a water-tight surface quilt.



New member
The iges file was created with 'Rhinoceros', the supplier tells me it can't export in STEP format!? Any other suggestions?


New member
That's really odd because I have Rhino at home and it allows me to export in .stp format. .stp is basically the industry standard now days for data exchange between software packages. Have you tried manually fixing the surfaces (boundry ect.)? Pro/E's geometry heal functions aren't exactly what I would call intuitive but once you can learn the finer points and some of the shortcuts it can actually be a fairly powerful just takes forever to learn it well. I really wish it had an option similar to Rhino where you can drape a surface over any existing geometry, it's a real time-saver.


New member
Ask your supplier if his model is a solid model. I work with Industrial Designers and they use Rhino to develop their concepts. Their models usually can not be converted into solid Rhino models. Our boss will not pay for any type of training, so the files they export are usually junk that can not be converted into solids ( I also suggest step). We usually end up creating thin protrusions and/or projected datum curves on individual surfaces that we can dimension in a draw, and then recreate the file.



New member
You can manually exclude the surfaces that are a problem as long as the software will exclude them. Then do a surface merge on each surface. In most cases the software will stitch the surfaces back together. Strange why it would not do this during the initial import, but that's Pro-E. I know this can be a time consuming task, but if you don't have any other choice this will work. Believe me I have used quite often.


New member

You can try setting the option fix_boundaries_on_import to yes.

You can also try modifying accuracy. There are two ways to do this; 1) import the IGES then change the accuracy or 2) start a new part change the accuracy then Insert/Data from File (in earlier versions File/Import/Append to Model). The next question would probably be what do I sent my accuracy to? I usually will try different values but if you open the IGES file in a text editor, the accuracy value the model was originally created in will be in the header information. If you have access to PTC


New member
My experience is that most imported quilts were never closed (ever saw a design with gaps of millimeters?), the designer never figured it might be important. So the problems you have might not created by export/import issues but by unprofessional designers.

One last resortI often use is to recreate the original untrimmed surfaces. That obviously only works if the surfaces are trimmed e.g. bigger then what you see on the screen. Try create/surface/new/advanced/freeform and click the surface you want to "untrim". It will recreate (read approximate)the original surface. If it's the same as the oneyou already had, then the original design was not made with

Clearly you totally screw up the quality of the surface... it is quite senseless importing nurbs surfaces in pro/e just to approximate them. Anyway, repeat this procedure with all surfaces you needand merge them all into a new closed quilt.

Good luck