thread milling help

[BAD DOG]

need example for milling an internal 1.375 x 28 tpi x .312 deep thread with a single point cutter.

there is a center island (.75 diam) so I have to use a small thread tool to fit.

thanks

bad dog

new fanuc oi controller on doosan mv-3016

[dcoupar]

Let's try for a 1/4" dia. thread tool? If you need to make a thread at more than one location on the part, you should probably use nested subprograms. Store cutter radius in D01. Try this one ABOVE the part. Good luck.

O1000 (MAIN PROGRAM)
N1 G0 G17 G40 G80 G90
T01 M06
G00 G54 G90 X0 Y0 S6000 M03 (POSITION TO CENTER)
G43 Z0.1 H01 M08
M98 P1001 (CALL SUB)
X5.0 Y0 (POSITION TO 2ND CENTER)
M98 P1001 (CALL SUB)
G0 G91 G28 Z0 M05
G90 M30

O1001 (1-3/8 - 28 THREAD MILL SUB)
G91 X0.51 (POSITION OFF THE ISLAND)
G01 Z-.5 F20. (FEED TO 0.400 DEEP)
G41 X0.1775 D01 F1.0 (APPLY CRC)
M98 P121002 (CALL HELICAL SUB 12 TIMES)
G01 G40 X-0.1775 F20. (CANCEL CRC)
G90 Z0.1
M99

O1002 (HELICAL SUB)
G03 I-0.6875 Z0.0357
M99