Subtracting error: the tool and target do not form a complete intersection

[JoachimAlly]

Hi all,

I am designing a cap for EEG-investigation of a Sprague Dawley rodent. I wanted to make grooves in the top of my cap by:
- Drawing curves on the top surface by making a sketch and project this sketch on the top surface
- Use these projected curves to make tubes with the command 'Tube'
- Subtract the cap with the tubes

The last step didn't work out. I got the error the tool and target do not form a complete intersection and I don't know how to fix it? In my opinion, what I want to do must be very clear for the program but there must be some reason why it is not possible for Siemens NX to cut these grooves in the cap. The attachment is a screenshot that clarifies the problem even more.

Does someone see what the problem could be? If yes, do you know how to fix it?

Thanks in advance and kind regards from a Belgian student,
Joachim

 

[cowski]

Try extending the tube so that it cuts entirely through the wall of the hole.

Alternatively, create and subtract the tubes before creating the hole features.

www.nxjournaling.com

 

[Jaydenn]

The hole in the "Target" body is likely tangent to the end of the "Tool" body. The result is a zero thickness, zero area body. It won't work. It's called "Non-Manifold".

See my simple example attached.

Like Cowski said, extend the tube tool more, or put the holes in later.

J


NX 6.0.5.3

 

[JoachimAlly]

Thank you very much, cowski and Jaydenn. Due to your help, I discovered the problem and was able to fix it.

Actually, I had already curves, but when I projected them to the upper surface, the curves weren't project on the holes, because the holes were part of the surface. So I just drew another plane that is the same but without the holes and projected the curves on this plane, which evolved in longer tubes and avoiding the error. In attachment you can see the result I wanted and have reached.