[klosr]

hello, was trying out thread milling, is it possible to do it with manually written program?

[Geof]

Sure, I do it all the time. Here is the code to cut a 16tpi internal thread 1.500" major diameter about 0.650" long.

N5000 T5 M06 (THREAD MILL 16TPI)
N5001 G43 H05
N5002 M03 S8000
N5003 G00 X0. Y0. Z1.
N5004 Z-0.59 M08
N5005 G41 D05 G00 Y-0.4
N5006 G03 I0. J0.575 Y0.75 F30.
N5007 G91 G03 I0. J-0.75 Z0.0625 F30. L3
N5008 G90 G03 I0. J-0.575 Y-0.4
N5009 G40 G00 X0. Y0. Z1.
N5010 M99

[klosr]

Sure, I do it all the time. Here is the code to cut a 16tpi internal thread 1.500" major diameter about 0.650" long.

N5000 T5 M06 (THREAD MILL 16TPI)
N5001 G43 H05
N5002 M03 S8000
N5003 G00 X0. Y0. Z1.
N5004 Z-0.59 M08
N5005 G41 D05 G00 Y-0.4
N5006 G03 I0. J0.575 Y0.75 F30.
N5007 G91 G03 I0. J-0.75 Z0.0625 F30. L3
N5008 G90 G03 I0. J-0.575 Y-0.4
N5009 G40 G00 X0. Y0. Z1.
N5010 M99

thanks! is the L3 meant for subprogram just for each pitch increment for Z ? or L3 works itself for 3 repetition with g91 in the line of code?

[Geof]

This was written for a Haas mill which can have an L count in a G03 command.

This is an internal right hand thread so the thread mill has to 'screw' itself out.

N5004 drops the mill to the thread depth.

N5005 sets tool comp with a small Y negative move.

N5006 enters the cut tangentially through a 180 degree arc.

N5007 does three counterclockwise circles incrementing up 0.0625 per circle. Not all machines can do this so this may have to be written as three absolut moves on some machines.

N5008 exits tangentially.

N5009 cancels tool comp.

[klosr]

i see.,, thanks

[Anders6612]

Just add Z depth to a 360 deg interpolation block.
And by making it a sub program, you can repeat it
as many times as you want, until final depth.