Posted: 23 September 2008 at 11:08am | IP Logged

I want to convert an assembly into a single part file and maintain the solid volume as closely as possible.

When I export as STEP and then open into a part, the location of all the components are not correct (each default position).  I tried IGES and I loose some geometry.  Not sure what is happening there, but it apears that some parts are assembled multiple times come in only once or on top of each other.  Or maybe because they are thin with respect to there overall size.  Shrinkwrap fails. 

The assembly is not very "clean".  It has interfering geometry, poor modeling and assembly techniuqe, etc.  I tried some of the other formats to export and import gemetery with no luck either. 

Anyone have any suggestions?

Posted: 23 September 2008 at 12:05pm | IP Logged

What release and datecode of Pro/E are you using? When you tried the shrinkwrap what quality level did you use?  How many components are in your assembly and are they complex?

Seems like shrinkwrap would be your best bet using the "Merged Solid" creation method. This gives you a single solid that has the same mass props and colors as the original assembly. I've done some fairly large assemblies and it's been hard to tell the difference. If quality level 10 doesn't work for you keep backing if off until you get it to work, sometimes it's hit or miss so it takes some patience.

Play around with the "Fill Holes" and other special handings until you get something that works for you. I'd say if it's consistently crashing no matter what you do then it's lost cause but it takes some trial and error.

Posted: 23 September 2008 at 3:12pm | IP Logged

WF 2.0 M280

All the way up to level 7 results in a different volume from the actual model.  Anything higher will fail.  I need a nearly exact volume for what I am doing.  I am using a simplified assembly to test these methods and it is not working, at some point I will be doing it with a fairly complex assembly.

Posted: 23 September 2008 at 5:46pm | IP Logged

How?

In the old days we used a "master model merge" technique to merge the geometery of one part into a new part.  I never used used it for for merging multiple parts, I will look into that tomorrow.

Thanks!

Posted: 23 September 2008 at 5:56pm | IP Logged

ReinhardN wrote: you could try to merge all parts of your assembly into a new part

Yeah, this might be the solution. Only drawback is having to create a merge feature for each component but it should give him what he wants. If this is a complex assembly it might take a while.

In a part, go to Insert>Shared Data> Merge/Inheritance, browse for the compnent you want and assemble each using "Default". You can then choose if you want it to be an external ref, dependent, etc.

Edit: Sorry, in this case you are going to have to insert a new part into your assembly, then activate the part. You then have access to the command to add merge features except now it will add the features in the correct locations as a merge feature instead of an external merge (there are advantages/disadvantages for both). If you do it outside of the assembly it won't know where to place the components unless you define the constraints for each feature and in this case you are basically recreating the assembly again. Trying to save you some work so all you have to do is go with the default constraint for each part.  

Posted: 24 September 2008 at 3:29am | IP Logged

No No No! I doubt very much you would be successful in merging all your componts into one single part.

The best way is to use Shrinkwrap using merged solid. I usually use a setting of around 6 > 7. Once you have created your shrinkrap model you will see two features in the model tree - copied geometry and a solidfy. I normally add additional features like protrusions to block off sensitive internal fesatures to customers and add any weldments since you are now in part mode and are able to add chanfers between surfaces etc.

Once you have done all this you can then produce a STEP file.

Posted: 24 September 2008 at 7:57am | IP Logged

Another long and not so good way is to create a new part in the assembly. Activate the part and then make surface copy (surf and bound) of each part. Merge all the surface files together and then solidify.

Krow72

Posted: 24 September 2008 at 10:06am | IP Logged

I agree, doing each part indivually is not an option it would take too long.  Again, Shrinkwrap will not work.  If you compare the solid volume of the original assembly to that of the shrinkwrap model it is greatly different.  What I need is an accurate volume representation of the assembly preferably in a part.

Thanks anyway.

Posted: 24 September 2008 at 1:48pm | IP Logged

Just another thought.  Are all your parts set to the same "ABSOLUTE ACCURACY"?  This could cause your shrinkwrap to fail.

Krow72