Catia V5R14 Partbody icon color

[michalr]

Hello,

can someone explain me the difference between Partbody when icon is green (normal one), grey or yellow?

I have a problem. I have part from other person and the partbody icon is grey. I would like to add another body using assembly boolean operation (this body icon is green). Catia does it but body that I want to add doesn't come under partbody. It remains in its place. It generates problem when I want to check what is the weight of the hole part (body I want to add is a pocket).

Regards,
Michal Raczko

 

[jackk]

Michal...

In R14 (or R15), Dassault introduced something called Hybrid Design which is what the different colored part body symbols mean.

(Hybrid Design allows wireframe and surface geometry to be part of the part body, with the solid. Most users seem to think this causes confusion, so most uses do not use Hybrid Design.)

In Tools + Options you can enable or not-enable Hybrid Design. Once a part is made with Hybrid Design enabled, it's very difficult to change it back.

If your partbody icon is green, it means your current part is the same as your current tools setting. You have a non-hybrid part and Hybrid Design is not enabled. Or, you have a hybrid part and Hybrid Design is enabled.

A yellow part body means you have a hybrid part, but Hybrid Design is not enabled.

A gray symbol means you have a non-hybrid part, but Hybrid Design is enabled.

 

[jackk]

Michal... (I just reread your post)

I was unaware of Hybrid Design causing any problems, until you reported the problem with booleans.

Try turning off the Hybrid Design mode, and see if that makes a difference with your boolean assemble.

 

[michalr]

Ok, it worked. I turned off Hybrid Design in Tools Options and all the Partbody's became green. Thanks