Need Help!- Sharp SV 2412s Question Thd Milling

[arcticigloo]

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
%

[timlkallam]

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.

[laserkey]

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.