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Import surfaces or solid bodys into a partbody?

MrCATIA

Super Moderator
Assuming you are not using Hybrid Design,

nothing special needs to be done. Just TRIM or SPLIT the solid by using the surface as the trimming element.

The surface's definition stays in the Geometric Set, but it comes a parent element to the solid in the PartBody. So, you will see the surface twice in the Spec Tree.
 

Chang

New member
If you want to have surface in partbody then you must activate hybrid design or you can make thick surface from the surface in other body then use remove (boolean operation) to cut what you want.
 

douger

New member
If these surfaces/solid bodies are located in another CATPart, it is best to publish them in that CATPart (Tools > Publication, then select the surfaces/bodies). After doing this you would Copy then 'Paste'/'Paste Special" into the new CATPart. Paste Special, As Result with Link will maintain an associative link between the resultant Surfaces/Body so when the original part is modified the pasted geometry in the second part will update to the new specifications after syncronization of the Published Surface.
 

3-foot

New member
You can put the surface into the part body, even if hybrid is turned off, sort of.

With hybrid turned off....

It is possible to insert a geo-set into the part body, then paste the surface into that geo-set. This way you have your surface in the tree at the point where it was used, but you're not voilating the "no hybrids" rule that many OEM's are imposing. You're only building one tree this way.

With Hybrid turned on......

I'd do it the same way as I stated above except you must use an ordered geo-set. Don't put surface and wireframe directly into the part body, use an OGS for that.
 

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