Create simplified model from complex assembly

[alexit]

What is best way to make external surface only type model?

I tried saving as sldprt part choosing external faces option but this is only surfaces not solid. I have also exported as iges, step, stl, etc. and re-imported to try to make this. Only close with export as stl selecting flatten and save in single file, then re-importing as graphic solid...this is time wasting so I hope you have better methods.

Thanks for looking,
Alex
SW2005SP3.1
4000hours using/0hours training

 

[SBaugh]

What is best way to make external surface only type model?.... I tried saving as sldprt part choosing external faces option but this is only surfaces not solid.

So what do you want Surfaces or a solid... you can't have both when saving.

If surfaces are all you want, then you have already done. Save as part and pick external surfaces.

If you want a solid then choose one of the other 2 options you get when saving an assembly to a part - "External Components" or "All Components".

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[wes616]

Alex, what you probablly want is the save as solid - external features only option.

Wes C.
------------------------------
In this house, we OBEY the laws of thermodynamics! - Homer Simpson

 

[alexit]

Problem is I want a monolithic solid created only from the external faces.

The 'save as part - external components only' gives customer too much information. Imagine auto motor, if I send this solid, you get all the internal geometry of block casting too.

I guess I can make special configuration for each extenal part with all internal features suppressed, but some assemblies have more than 500 parts...it would be nice if this was easy.

I find now the STL option I do earlier wont work, file was >22MB from 7MB test file.

Maybe I can knit the external faces...

 

[CorBlimeyLimey]

Does it really have to be a solid? What's wrong with giving them the external surfaces only? It will have no internal details ... just a hollow shell.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[rfus]

People often spend so much time looking for the magic button that in that time they could have just done what was needed and had it out the door.

Saving all external faces into a part and then knit into a solid with some work sounds like the way you wanna go.

Save assembly as part, select solid and external components, open the part and start combining solids which should swallow up some stuff, and use other features to bring solids together or deleting solids with too much info. Zero thickness can be a problem with combining solids from assemblies.

Then save as parasolid.

Saving as stl is making polygons out of your CAD geometry, probably not what you want.

 

[MElam]

Try saving "external components only". Then open the new part and use the Combine feature (Insert/Features/Combine)

This will merge all of the bodies into one chunk - if they are touching with no zero thicknesses

 

[alexit]

Thank you all for suggestions, I try each one.

The knit idea fails, each single surface is all external surfaces for a single part, so it curves funny and the command doesn't work on any join of two surfaces.

Cor:
They must have a solid for their software to create the imagery/rendering they desire. I send surfaces and it fails. I tried thicken too (very small thicken), but this fails as many parts cannot thicken.

Rfus/Melam:
When I save as parasolid and re-import I get back feature tree with everything I did, easy to delete those extrudes or combines used to fill important information and get back to saved external solid bodies. Also easy to cut single solid with sections and get to internals...am I doing the save wrong?

I try this also, I make big block to fit over all and subtract parts from it to get negative to try to make single part. But I cannot subtract in assembly mode, not offered.

I mail disc of 22MB STL model today, they can play with this while I find better way.

 

[MElam]

Sorry, my response should have been more clear.

I was talking about saving the assembly as a part file (.sldprt) not parasolid. Saving as external components only will give you a multibody part. The Combine feature will merge the bodies you place in the seletion box into one single dumb body.

The subtract you are looking for in assembly mode just may be the cavity feature. Look it up.

 

[SBaugh]

I try this also, I make big block to fit over all and subtract parts from it to get negative to try to make single part. But I cannot subtract in assembly mode, not offered.

It is offered, you can only subtract if you are doing a Cavity. (Mold Tools) Insert\Mold\Cavity - you have to be editing the part within in the assembly.

See Mold\Cavity in the help

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[alexit]

Cannot make cavity from sub assemblies only single parts can be selected, I will try smash assembly, then make cavity when I get next chance.