G92 Threading Cycle (Group 01)

Classic Control - Lathe 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

G92 Threading Cycle (Group 01)

F(E) - Feed rate, the lead of the thread
*I - Optional distance and direction of X Axis taper, radius
*Q - Start Thread Angle
*U - X-axis incremental distance to target, diameter
*W - Z-axis incremental distance to target
X - X-axis absolute location of target
Z - Z-axis absolute location of target

* indicates optional

Programming Notes:

  • Setting 95/Setting 96 determine chamfer size/angle. M23/M24 turn chamfering on/off.

  • G92 is used for simple threading, however, multiple passes for threading are possible by specifying the X locations of additional passes. Straight threads are made by specifying X, Z, and F. By adding an I value, a pipe or taper thread is cut. The amount of taper is referenced from the target. That is, I is added to the value of X at the target. At the end of the thread, an automatic chamfer is cut before reaching the target; default for this chamfer is one thread at 45 degrees. These values can be changed with Setting 95 and Setting 96.

  • During incremental programming, the sign of the number following the U and W variables depends on the direction of the tool path. For example, if the direction of a path along the X-axis is negative, the value of U is negative.

G92 Threading Cycle: [1] Rapid, [2] Feed, [3] Programmed path, [4] Start position, [5] Minor diameter, [6] 1/Threads per inch = Feed per revolution (Inch formula; F = lead of thread) .

% O60921 (G92 THREADING CYCLE) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD thread tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, Spindle on CW) ; G00 G54 X0 Z0.25 (Rapid to 1st position) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; X1.2 Z.2 (Rapid to clear position) ; G92 X.980 Z-1.0 F0.0833 (Begin Thread Cycle) ; X.965 (2nd pass) ; X.955 (3rd pass) ; X.945 (4th pass) ; X.935 (5th pass) ; X.925 (6th pass) ; X.917 (7th pass) ; X.910 (8th pass) ; X.905 (9th pass) ; X.901 (10th pass) ; X.899 (11th pass) ; (BEGIN COMPLETION BLOCKS) ; G00 G53 X0 M09 (X home, coolant off) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

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.

Feedback