Export assembly as one single solid

[Anonymous]

Hello

Let me cut right to it.

Is it possible to export an assembly to one single solid step file?

I have tried shrinkwrap the assembly to one single solid, and export that to step file. when I import the step file and it shows multiple bodies, and not just one, eventhough there is only one solid body in the .ipt.

I then tried derive the .ipt to a new part. and choose "Single solid body" in derive style. export to step and the same thing happened when I import it again.

Both times i breaked the link to base component.

I'm looking forward to your answer.

[Sergio.D.Suárez]

Hi, In which program do you want to open the step file?
In some programs you have to adjust the import options for step files.
I ask what program you need to work on because maybe in that program there are the necessary tools to "combine" the parts into a single solid, or even in a multibody file.
Regards

[Anonymous]

Thank you for the answer.

It is not so much the import we should focus on.

I need it to be one solid body when I fx send it to a customer, so that they can't "make" their own version of my equipment.

[Sergio.D.Suárez]

Hi, if so, then my advice would be to first hide all unnecessary internal components of the assembly. Then you create a shrinkwrap, a file of part of a solid in one part. (avoid including bolts and other unnecessary information)

Then from this part file, you create a step file. You should not give much information in the step, just the general geometric information of the master assembly.
If you have multiple positions, create a shrinkwrap for each position and follow the same procedure mentioned.
I hope this helps you, regards

[Anonymous]

That is exactly what I have done.

Please se my screencast video.

Something went wrong with the screencast capture, so the mouse is a bit off.

d2a4c9f9-00f6-4d63-9835-64e2559ed005,640,620

[Anonymous]

Screencast:

https://knowledge.autodesk.com/community/screencast/d2a4c9f9-00f6-4d63-9835-64e2559ed005

[johnsonshiue]

Hi! Many thanks for the screencast! I think I know where the problem is. This is about a unique behavior in some Autodesk products like Inventor. Our modeler supports a concept called disjoint lumps per body. When you did the shrinkwrap and you selected Joint One Body option, the two non-overlapping bodies become two lumps in one body. In other CAD systems, such notion does not apply.

There is advantage and disadvantage here. Disjoint lumps allows Inventor to create features within one body regardless of merging or separating. But, it can be confusing to the users what a lump really is and how it would behave.

STEP as a neutral file format does not support disjoint lumps body. As a result, any disjoint geometry is considered a separate body. When the Shrinkwrap was exported to STEP, it was already separated as two bodies. As a result, importing it back becomes two solid bodies.

Many thanks!

[Anonymous]

Hi Thank you for your answer.

Is there some sort of workaround to make my models become a single solid body when exporting?

[johnsonshiue]

Hi! The only workaround I can think of is to use Shrinkwrap to create one solid body and then export such solid as SAT file. However, it will still depend on the receiving end if it supports disjoint lump solid body. If it does not, I think it will make the disjoint lump a separate solid body.

Many thanks!