How to split IGES "assembly" that imports as single part

I have a vendor supplied IGES file of a latch. I believe it's surfaces, not solids (isn't that true of all IGES parts). Anyway, the file imports into Pro/E with the various components shown in different colors but it is not recognized as an assembly.



What can I do to break this apart?



View attachment 100

Here's the original IGES file:

One way of doing it is when you bring in the igs file you can go to Application>Legacy.

Then click on wire frame and delete whatever you do not need.

The same thing with surfaces. I know it is not the most efficient way. It works.

The only other way is to have the other person output the assembly as seperate files. Just like you can do int Pro. You can export as a single file or it would create single files as well as the assy file.



Hope this helps

I have not checked you specfic file, but this happened to me a little while ago. The mistake I made was I imported the file into a Pro/E part instead of an assembly. Start a new blank assembly and try to import it if you did what I did last time.

Another option:



Import the IGES file into a part. Put the import feature on a layer so you can blank it. Make a copy of the part for each component in the assembly. Open each part and make protrusion use quilt, selecting a different quilt in each part. Turn off the import layer, assemble all the parts by default and you should be all set!



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#Featur #Create #Solid #Protrusion and the optoin for Use Quilt is grayed out. The IGES model imports as one solid blob (i.e. model analysis is able to determine a mass and C.G.)



I think I know the answer is NO but is there any way to separate surfaces based on color?



-Bernie-

It is possible.



Drag-n-drop the IGES file into ProE. Choose #assembly. When the Iges file was exported as an assembly, you will get an imported assembly as well. But in this case it won't.

#Redefine the import feature in the 81-206 part and choose #attributes. Turn off the #make solid option.

Now create, as mentioned above, in this assembly empty parts wich will serve as the seperate components. Stay in assembly and choose #Modify #modify part and select the first empty part. Create the first feature with #Protusion #Use Quilt and select one of the closed surfaces of the imported part. The new parts will have a dependancy to this assembly. Set their colors as desired.



I've done this several times, with worse files. I tried it on your file and it works fine.



Huug



PS. Sorry for this late reply, but I had trouble with my login..

Thanks Huug,



Worked like magic in Pro/E 2001. I had know idea this was possible. I did in a couple of minutes what took the better part of a day in Cadkey (Cadkey 99 unfortunately looses the color attributes when importing IGES). As you probably noticed the red and gold surfaces are not individually closed which makes it a bit harder to break this into three separate parts but just separating out the handle is sufficent for my purposes.



I Guess there isn't any way to use color as a selection feature? That would be really convenient in spearating and repairing the pivot (gold surfaces) and lock (red surfaces).



-Bernie-