Hi, thanks for respond but I set already "full" and it doesn't help me
Do you have any other idea?
@lukipap , I'm afraid, you can't do that as hole is broken in 2 portions. However, you can display it by adding sketch lines in other portion.
You can cosider opening an ER with GTAC .
ER7256282: The thread silhouettes are shown partially along length of the threaded hole.
In this case, it is designed behaviour. For threaded hole, cylindrical face is splitting into two disconnected faces and thread will be positioned on the face which will near to the thread origin.
Couple of workarounds that can be used:
1) Create general hole and apply separate threads to cylindrical faces
2) Split into two bodies
Create threaded hole with Boolean operation as none
Subtract hole body from one of the split body (Keep tool body)
Subtract hole body from other split body
Unite split bodies
The 'Thread' feature is applied only to the FACE of the Hole, not to the Hole feature itself. This means that when the face of the Hole was 'split' into two faces, only one of the faces retained the original object tag and therefore that's the one the Thread feature remains applied to. The other half of the Hole feature, its face has a new object tag and thus has no Thread feature assigned to it. If all you want is to make the view in the Drawing look correct, simply apply a second Thread feature to the face of the other half of the Hole. However, I agree that it would better if the Thread feature were enhanced such that it's applied to the face(s) of the Hole feature, no matter how many faces that might be, in this case two faces.