How to split part to bodies

[valtokrhm]

Hi,

How can I split part that has made in one body to different bodies?

In solidworks I can use split command and keep both bodies on both sides of the split plane.




In Catia split command deletes the other side of the plane, so is it possible to keep both different bodies?



Thanks! -VK

 

[MrCATIA]

As a workaround, you could Pocket a very thin slice across the part, keeping two bodies (domains)

 

[MrCATIA]

Another workaround: Copy and Paste the PartBody so you have two shapes (bodies) of your part. Split first one with arrow up, and Split the copy with the arrow down.

 

[valtokrhm]

Yes, I have made it like this but then I can't make drawing and apply links to different bodies because these are still the same body.

 

[valtokrhm]

Another workaround: Copy and Paste the PartBody so you have two shapes (bodies) of your part. Split first one with arrow up, and Split the copy with the arrow down.

With this method there is problem that copied body is not in date if I want to make changes in main body.

 

[MrCATIA]

Copy the PartBody and use Paste Special + Result With Link. Do this twice so you have two copied Bodies. Then Hide the PartBody, and Split the pasted bodies. Any changes made to the PartBody, will update in the copied/linked Bodies.

 

[Rickyt]

If you don't want the extra hidden body in your file.

You could take your unwanted shape and paste special as result with link. So now you have two of the unwanted shapes.

Create 2 new bodies.
Do a boolean add of one of your unwanted shapes to one of the new bodies.
Do another boolean add of the other unwanted shape to the other new body.

Now you can do a split in each of the new bodies after the boolean operation.

One body will have the parametric history with a split afterwards. And the other will have a linked body with a split afterwards.