catia v5r16 boolean warnings
catia v5r16 boolean warnings
(OP)
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??
" 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??





RE: catia v5r16 boolean warnings
are all the PartBody icons green?
RE: catia v5r16 boolean warnings
RE: catia v5r16 boolean warnings
RE: catia v5r16 boolean warnings
RE: catia v5r16 boolean warnings
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.
RE: catia v5r16 boolean warnings
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
RE: catia v5r16 boolean warnings
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!
RE: catia v5r16 boolean warnings
Good luck!