Can someone send me a sample of a thread mill operation? I need to compare this to what our CAM software (Bobcam) is posting . The problem is that the thread mill does not want to travel helical Z. Sharp said I am missing a "G33" ?

This is the post that "Bobcam" provides

(JOB 2 THREAD MILLING)
(TOOL #3 0.3720 THREAD MILL)

N59 T03
N60 M06
N61 T01
N62 G90 G54 X0. Y0. S841 M03
N63 G43 H03 Z.1 M08
N64 G01 Z-2. F3.3679
N65 X-.186 Y.5
N66 G02 X.314 Y0. I0. J-.5
N67 X.314 Y0. I-.314 J0.
N68 X-.186 Y-.5 I-.5 J0.
N69 G01 X0. Y0. Z13.
N70 G00 Z.1
N71 M09
N72 M05
N73 G28 Z0.
N74 G59 X0. Y0.

(END OF FILE)
(END OF PROGRAM)

N75 M30
%

Hello Arcticigloo ,I also have a sharp 2412 , G33 does not apply to threadmilling its more for single point thread cutting.
It looks like your cuting a 1 inch dia thread don't know the pitch.

The program looks wrong line N65 will place the cutter well outside the 1 inch circle. Also theres no Z while cutting therefore no movement.

Also the cutter should climb out of the hole G3 insted of G2

Lets say you want to threadmill a 1x 10 tpi . 5 deep thru hole with no cutter comp. and no lead in or lead out .

(JOB 2 THREAD MILLING 1 X 10 TPI)
(TOOL #3 0.3720 THREAD MILL )
T03M6
G0 90 G54 X0 Y0 S1000 M3
G43 H3 Z.1 M8
G1 Z-.650 F50
X-.314 F5
G3 I-.314 Z -.550
G1 X0
G0Z6M9
M30

Note G3 I-.314 Z -.550 cuts a full circle while Z rises 1 full pitch.

It might be the same reason thar my high speed maching was not working.
if you open your post and look on line 64 you should have somthing like
x_f,y_f,Z_f,. This teels the z to post in a three axis arc.
If your using v23. I have a sharp also but only used it for the high speed maching and it would not put a z on any lines with a g2 or g3.