Try saving the assembly as a part and then save the part in the desired solid format.
No need to work too hard. You can do this in 2 minutes.
1. Insert your assembly in another dummy assembly.
2. Create a SpeedPak of the top level assembly with only the faces or bodies that you want to preserve.
3. Save the dummy assembly with the SpeedPak configuration active.
4. Send them only the dummy assembly file.
They will be able to insert it in their own assemblies if so desired, without being able to touch the faces you had not preserved.
I would save it as a step file first and then open it back up SW and then save it as a SW part file if the end user is using SW, otherwise just give them a step file.
There are tricks to hide some features first though... You can make component level configurations and remove (defeature) some of the more important features of the file.
@ Kevin, Alin and Steve.
Thank you for your replys, but i must sadly say thay none of them worked.
We need to create a IFC2x3 file, which architects use in their software, like Revit.
i have inserted a small dummy model i have been experimenting with, before trying the solutions on the much larger ones. and as you can see there is still a model tree, where the customers can deactivate the parts and look into our products. This model tree should have been reduced to only 1 part which they can hide or unhide.
- Open the main assembly.
- Select all internal components (use quick select for that)
- Suppress them
- Add a new part inside main assembly
- Edit the new part
- Use the "Join" command with the "Force surface contact" on.
- Send them this new part.
Theoretically, the "Force surface contact" setting should eliminate the zero thickness conditions. In real life, it does not always work, but give it a try.
One more thing. In the newly created part, run Intersect and fill all the cavities, so you will eliminate the external faces.
My apologies for my post.
I didn't read far enough and what I posted was redundant and worthless.
Thank you for your replys everyone.
I think i will go with the defeature command even though it is not the solution i wanted. But if you by chance should stumble upon a way to just "save as" one single solid, let me know .
(thread can be closed)
I have found the solution.
First defeature the model.
Second use the intersect Tool on all the solids in the model.
now if I save it in my IFC format it comes out as one solid piece.