G92 Set Work Coordinate Systems Shift Value (Group 00)

Next Generation 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 G-code does not move any of the axes; it only changes the values stored as user work offsets. G92 works differently depending on Setting 33, which selects a FANUC, HAAS, or YASNAC coordinate system.


If Setting 33 is set to FANUC or HAAS, a G92 command shifts all work coordinate systems (G54-G59, G110-G129) so that the commanded position becomes the current position in the active work system. G92 is non-modal.

A G92 command cancels any G52 in effect for the commanded axes. Example: G92 X1.4 cancels the G52 for the X-Axis. The other axes are not affected.

The G92 shift value is displayed at the bottom of the Work Offsets page and may be cleared there if necessary. It is also cleared automatically after power-up, and any time ZERO RETURN and ALL or ZERO RETURN and SINGLE are used.

G92 Clear Shift Value From Within a Program

G92 shifts may be canceled by programming another G92 shift to change the current work offset back to the original value.

% O60921 (G92 SHIFT WORK OFFSETS) ; (G54 X0 Y0 Z0 is at the center of mill travel) ; G00 G90 G54 X0 Y0 (Rapid to G54 origin) ; G92 X2. Y2. (Shifts current G54) ; G00 G90 G54 X0 Y0 (Rapid to G54 origin) ; G92 X-2. Y-2. (Shifts current G54 back to original) ; G00 G90 G54 X0 Y0 (Rapid to G54 origin) ; M30 (End program) ; %


If Setting 33 is set to YASNAC, a G92 command sets the G52 work coordinate system so that the commanded position becomes the current position in the active work system. The G52 work system then automatically becomes active until another work system is selected.

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.