I have imported an IGES file from a customer. It is around 50MB, and consists of 757 surfaces. What I would like is a solid, but I am not confident that going in and manually knitting the surfaces will work, and it will be very time consuming. Features are not important, but the ability to check interference would be great. What I really need is a smaller file that does not make SWX so slow. I am running SWX2003 SP2.1 (I could upgrade SP but don?t think that will help much) on a Win2K AMD Athlon XP 2600+ with 1.00 GB RAM.
What system generated the IGES file ? If you open it in a text editor, the first few lines will tell you
The best solution is to have the customer send you a STEP file instead of IGES. Of course that would depend on whether or not they have the translator. Most newer systems have this capability right out of the box.
IGES doesn't work very well for translation between todays solid modelers. If you're stuck with it you might want to consider sending it to a service bureau. Otherwise you'll have to manually mess with it untill you can get it to knit. It is, what it is mathematically. The only way to make it read in better is to regenerate it in the originating system with different settings.
I've heard that some IGES files can be healed by reading them into Rhino, and translating them out using the SW settings.
Mike, When you opened the file was the "Try to knit to solid" option checked in the Option dialog area? You should not have to manually knit all 757 surfaces. If it was checked, then try to get a Parasolid format(x_t or x_b) that is the native format for Solidworks.
You can highlight all IGES parts in the feature tree and apply the FIX mate to them simultaneously. This keeps the parts together in their proper position. You would have to use the join command to turn everything into one part and I am not sure that really buys you anything.
I used to bring in lots of surfaces and have to try and sort them out. I found using the diagnostics tool quite useful, and then when it had done it's thing, exporting the file again and re-importing - sometimes SW would patch even more up each time so eventually you would get a solid.
The other thing is to try selecting the faces you need for interference detection (use the face filter for this and drag to select areas can speed things up a lot!) and then exporting only the selected faces - then reimporting these ones and stitching them to make a solid. This can be frustrating ad time consuming if there are lots of fiddly faces where holes appear. However, you can see a 'hole' using the tools>check command, then remember where it is, use filter>edges, right-click one of the edges and use 'select open loop' which should run a selection round the hole. Then use surface>fill to patch it up. If there are a few small holes, which can be frustratingly impossible to see using SW, this can work a treat. Once you have patched all the holes try knitting and forming solid - if this fails try exporting the new surfaces again and re-importing with the 'try forming solids' option ticked.
my key tips are:
- offset surfaces before exporting as then if you miss one you don't have to reselect them all again, you can simply select the offset surface from the tree.
- make use of the filter keys ('x' for faces , 'e' for edges, etc) or the filter toolbar.
- use the right-click> 'select tangency (for faces) and 'select loop' or 'open loop' for edges.
- export and reimport after using the diagnostics.
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