NX 6.0 Creating solid out of "empty space" in assembly

[johham9]

Hi everyone!
I would like to create a empty space-solid(yep, want to export the fluid).
I have a assembly with three metric tonnes of different small components, most of them completely irrelevant.
What I'm really interested in is the roughly the outer geometry and the interior geometry.

Anyways, I would like to find the easiest way to do this( Extracting surfaces and sew together is really not an option).

So, any ideas?

Cheers,
Johanna

 

[jerry1423]

Accomplishing that is really not as bad as you are making it seem.
Do you have WAVE?
Is it posiible to provide the file, or a picture of wwhat you are working with?

 

[johham9]

Waved out all components as bodies, and then did a half-ass attempt to make an assembly cut and tried something to try and unite them together. Can't remember exactly what I did.

Unfortunantly, I just signed a paper about not sharing any of the information I got from the company, so cannot share a picture. But I'm working with a drill bit, and I'm going to run som simulations on the drilling fluid, if that gives you a better picture of the situation?

 

[johham9]

And the result of that attempt was errors, of course...

 

[SDETERS]

Could you use simplify assembly? You need to have the advanced assembly license.

 

[JohnRBaker]

Not sure how easy it's going to be to follow, but if you look at the attached example you'll see where I modeled the 'empty space' inside of a 'valve assembly' using a workflow where I first WAVE linked all the parts into a single component, united them together and then used the Synchronous Modeling 'Delete Face' command to delete all of the OUTSIDE faces of the model leaving only the inside, which in this case represents the 'air' or 'empty space'. Just look at the component named 'empty_space' to see what I mean.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Toost]

I assume that you would like to subtract the drill and the shaft from the hole that the drill has cut, leaving the "drilled hole minus the drill minus the shaft" which would equal the fluid + material removed.
I assume that the type of drill is the type common in oil drilling operations, and not steel drilling.

Link all solid bodied that matter ( ignore irrelevant pieces such as ball bearings unless these are part of the fluid flow) into a separate part similar to what John showed, unite all bodies that can be united, use delete face to get rid of minor details, create/ extrude "help bodies" where needed to be able to unite ,( for example the complex conical thread which i have seen on this type of drill) then when you have a single solid body, create the "drilled hole" and subtract the drill from the hole.

If you intend to run the simulation in NX there might be smarter tools in the Simulation application.
There is a feature which can help in creating the "volume between" * but i have no experience of it.
* between the drill and a void in a separate body.


Regards,
Tomas

 

[johham9]

Thanks y'all!