Clearance in lathe threading violates clearance/retract settings on internal threading. I have a 2" 4tpi internal acme thread. The minor diameter is 1.76" my threading bar is 1.69". I only want to clear by .03" radial and is what I have set in the radial heights. Which would put me at about 1.7". Part feeds out of the thread to 1.49" and would rub the back side of the tool.
Hi @Lonnie.Cady
Thanks for posting! My apologies for the late response on this thread.
Would you mind sharing the part you are working with me? I looked into this a bit today and got some varied results with different tool compensations. Some of these compensation strategies are hard to make sense of mathematically, but I found that everything does appear to be posting correctly when using the "Insert Center" for the tool compensation. Does your code appear to post correctly if you use the Insert Center as the compensation point (when in the tool editor)?
I've also reached out to some other CAM resources that may be able to provide more detail on this behavior and will keep this thread updated with anything I have to share. Feel free to let me know if you have any questions!
I am not really sure how to explain it differently. I have attached the file. I tired different tip compensations and it always violates the clearance I have set. I have a bore that is 1.76" in diameter that needs to be threaded. I have a bar that I want to use that is 1.69" from the cutting tip to the backside of the bar. There for I can't really retract past 1.69". I mean I could realistically by a small margin since the bore is .07" bigger than the cutting tool.
I set the clearance to -.03 below the bore which would mean the tool would retract to (1.76" - (.030" * 2)) = 1.700".
However the operation does not obey that setting and feeds the tool down to 1.49" which causes the backside of the tool to rub the threads.
In the attached file it is the final operation in the second setup.
(Thread2) T1111 G98 G97 S500 M3 G54 M8 G0 Z0.25 X1.7 Z-0.1864 G1 X1.7923 F39.37 G32 Z-2.3138 F0.25 X1.49 F0.25 <------------------------past clearance plane, tool hits on back side of bar. Clearance is set to be 1.7" G0 Z-0.1879 X1.7 G1 X1.8056 F39.37 G32 Z-2.3153 F0.25
Hi @Lonnie.Cady
Thanks for attaching the file! I had another look this morning and you are correct - the clearance and retract planes are not being respected in the output code. I found that they were also not respected when output with the dumper post, which suggests that we have found a bug. I've logged a ticket (CAM-9071) about this behavior and development will be working to provide a fix. We appreciate you bringing this to our attention!
I found that the only way I was able to get the output to respect the clearance and retract planes was to use a very small thread depth with the "Fade Thread End" flag enabled. Either increasing the thread depth (to anything greater than the built in default in Fusion), or disabling the Fade Thread End option would result in the clearance/retract planes not being respected and the tool moving further towards the center. The deeper the thread depth, the more towards the center the tool was allowed to move. As decreasing the thread depth is not really a workaround, I think that the easiest way to move forward with your design will be to edit the code by hand - I apologize for any inconveniences this may cause. I have marked the ticket as a high priority issue and hope that it will be resolved soon.
Please let me know if you have any questions!
@paul.clauss Don't mark it high priority on my behalf. 
Parts were done before I posted the issue.
Thanks for following this thru and getting it logged.
