catia v5r16 boolean warnings

[liquidlunch]

I am getting a warning when I try to do boolean operations to my part. I have probly 100 or so boolean operations with no warnings but for some reason I am now getting them. The warning reads

" You are trying to create a boolean operation which breaks relation order between geometrical elements. Operand body will not be move under the boolean feature. Do you want to continue "

There are no links to any other features or geometry. Am I losing it or does someone have any idea how to properly diagnose this warning??

 

[jackk]

are you using Hybrid bodies?

are all the PartBody icons green?

 

[liquidlunch]

Yes hybrid is on.

 

[jackk]

and are all the PartBody icons green gears? (or are they yellow and/or gray?)

 

[liquidlunch]

large gear is green, small gear is blue

 

[jackk]

(here's what I think is happening. I don't work with Hybrid bodies, so I'm not speaking from experience)

Since you're working with Hybrid Bodies (which are "ordered") you must have everything in sequential/historical order in the tree. The error message says that the boolean operation will move something that is a child in front of it's parent. The result would be out of the sequential order.

You say there are "no links," but are you sure there are no parent/child relationships? such as a sketch made on a plane in another body?

What happens if you continue after you receive the warning mesage? Is there any other info that might help you figure out what is related to what?

You say the icon is the big green gear - are ALL the PartBodies green gears?

As a work-around, you MIGHT be able to copy & paste special with link the part body into a new partbody and then do the boolean with the linked solid.

The only other solution I can think of is to re-create the body being booleaned AFTER you add the boolean to the tree.

 

[slcad]

Yeah, another one of hybrid design´s "benefits"...

I agree with Jack, there MUST be some parent-child relationship causing this. You must identify what feature cause you problems (probably a sketch) and try to reorder or duplicate (copy-paste) it in orde to break the relationship. What I noticed is that usually you cannot move sketches into another (open-)body via the contextual command ("Change geometrical set"), neither does the reordering usually work. What I do when dealing with sketches is simply copy-paste it inside the desired body, replace the original sketch with its copy and delete the original.

What happens if you go further without doing anything? Nothing else except that you are left with a bunch of bodies outside the part body, which is naturally unpleasant. But the actual boolean operation DOES take place. The geometry of the body IS operated in the part body, only that the operated body does not move under the boolean feature in the tree structure.

Regards,
Stely

 

[liquidlunch]

A querry on parent child relationships show there are none. I have made new simple features such as body with an extrude and tried the operation with it, nope, I have tried rolling back up and down the tree to different points and trying the operation. Nothing seems to work. I deleted and re-unioned a previous feature and it worked. This would seem to support the parent child issue on the new feature but the search yeilds nothing.

I have been using catia for some time and have never experienced this before. Could it be some kind of bug in V5r16? I will post if I find something.

Thanks you very much for your replies!

 

[slcad]

This problem also occurs when you mix hybrid and non-hybrid bodies. But then, as Jack was pointing in his questions, the icons of the bodies should look different. For a quick identification, perform a "Tools -Parametrisation analysis" and choose "Bodies" from the drop-down menu. It should find all the body features in your files, and there you can see faster if their icons differ.

Good luck!