Thread Milling Example:

Classic Control - Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

This program I.D. thread mills a 1.5 diameter x 8 TPI hole with a 0.750" diameter x 1.0" thread hob.

  1. To start, take the hole diameter (1.500). Subtract the cutter diameter .750 and then divide by 2. (1.500 - .75) / 2 = .375

    The result (.375) is the distance the cutter starts from the I.D. of the part.

  2. After the initial positioning, the next step of the program is to turn on cutter compensation and move to the I.D. of the circle.

  3. The next step is to program a complete circle (G02 or G03) with a Z-Axis command of the amount of one full pitch of the thread (this is called Helical Interpolation).

  4. The last step is to move away from the I.D. of the circle and turn off cutter compensation.

You cannot turn cutter compensation off or on during an arc movement. You must program a linear move, either in the X or Y Axis, to move the tool to and from the diameter to cut. This move will be the maximum compensation amount that you can adjust.

Thread Milling Example, 1.5 Diameter X 8 TPI: [1]Tool Path, [2] Turn on and off cutter compensation.

note: Many thread mill manufacturers offer free online software to help you create your threading programs.
% O60023 (G03 THREAD MILL 1.5-8 UNC) ; (G54 X0 Y0 is at the center of the bore) ; (Z0 is on top of the part) ; (T1 is a .5 in dia thread mill) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G00 G54 X0 Y0 (Rapid to 1st position) ; S1000 M03 (Spindle on CW) ; G43 H01 Z0.1 (Activate tool offset 1) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G01 Z-0.5156 F50. (Feed to starting depth) ; (Z-0.5 minus 1/8th of the pitch = Z-0.5156) ; G41 X0.25 Y-0.25 F10. D01 (cutter comp on) ; G03 X0.5 Y0 I0 J0.25 Z-0.5 (Arc into thread) ; (Ramps up by 1/8th of the pitch) ; I-0.5 J0 Z-0.375 F20. (Cuts full thread) ; (Z moving up by the pitch value to Z-0.375) ; X0.25 Y0.25 I-0.25 J0 Z-0.3594 (Arc out of thread) ; (Ramp up by 1/8th of the pitch) ; G40 G01 X0 Y1 (cutter comp off) ; (BEGIN COMPLETION BLOCKS) ; G00 Z0.1 M09 (Rapid retract, Coolant off) ; G53 G49 Z0 M05 (Z home, Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; %

N5 = XY at the center of the hole

N7 = Thread depth, minus 1/8 pitch

N8 = Enable Cutter Compensation

N9 = Arcs into thread, ramps up by 1/8 pitch

N10 = Cuts full thread, Z moving up by the pitch value

N11 = Arcs out of thread, ramps up 1/8 pitch

N12 = Cancel Cutter Compensation

note: Maximum cutter compensation adjustability is .175.

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.