Dividing a solid body face

[morauski]

is it possible to divide a solid body face?

i know in unigraphics/NX it is.

 

[williwang]

not in v5 I think

Forever Young.....

 

[krzychub]

Yes, you can do it. Not directly but with some work-around.
It depends what you need it for.

If you just need that divided surface as it is then you can extract the face fron solid using Extract function in GSD. Then use other GSD functionalities to divide that surface.

If you need to have that divided surface on solid then you can extract all faces of the solid, then divide the surface, then join all surfaces and make "Close surface" solid in Part Design.

Other way is for example to divide the line/curve already in the sketch which is used to make the feature (Pad/Pocket...).

/Krz

 

[Azrael]

I've worked with NX also and used that feature in rare occasions like setting up FEA and direct modeling. Could you elaborate some more, why do you want to do that, there may be another approach in catia to solve your issue.

 

[PeterGuy]

Extract the face
Cut to desired shape
Use sew surface in soilds (no not simplify)

 

[morauski]

in mold design we need a cavity half and a core half (and most times actions) i prefer to have all work done to the solid body so the face splitting is where the different mold components would come together. alot of times it is on a flat surface or on the radii.

i use this feature daily when i was on NX and was really surprised catia didn't have it. et al.

extracting surfaces and rejoining makes model basically dumb and i wanted to keep it smart

 

[williwang]

hehe, CATIA and UG are different. UG like a gun, CATIA like a knife, hold CATIA as a gun will cut your hand.

For die making, people can use solid operations, then use parting surface to get two halves.

Forever Young.....

 

[Azrael]

Ok. I guess that you are not using the Core & Cavity workbench. In catia you work with surfaces to get the splitting elements for core and cavity, it will actually be associative and quite stable for updates.

You could try to extract all surfaces, reflection line feature to split the surface twice, for core and cavity, extrude and sweep to get the oversize needed to split the tool with. This will be an associative model, the extract is actually a smart feature.

 

[jopal]

I agree with Azrael. But if your not using CCV, create you reflect line, extrude or sweep your runout surfaces, then trim to the original part surf to your runout surfaces twice (1 for core, 1 for cav.) Personally, I keep part data datum, join them all then do my pl, when i need to update the data, i just swap out the surfaces of join i need and everything updates. i find this the quickest and most efficient.

 

[morauski]

Thanks everyone i will give the suggestions a try.