G36 Automatic Work Offset Measurement (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 is optional and requires a probe)

This G-code is used to set work offsets with a probe.

F - Feedrate
*I - Offset distance along X-Axis
*J - Offset distance along Y-Axis
*K - Offset distance along Z-Axis
*X - X-Axis motion command
*Y - Y-Axis motion command
*Z - Z-Axis motion command

*indicates optional

Automatic Work Offset Measurement (G36) is used to command a probe to set work coordinate offsets. A G36 will feed the axes of the machine in an effort to probe the work piece with a spindle mounted probe. The axis (axes) will move until a signal from the probe is received or the end of the programmed move is reached. Tool compensation (G41, G42, G43, or G44) must not be active when this function is performed. The point where the skip signal is received becomes the zero position for the currently active work coordinate system of each axis programmed. This G-code requires at least one Axis specified, if neither are found, an alarm is generated.

If an I, J, or K is specified, the appropriate axis work offset is shifted by the amount in the I, J, or K command. This allows the work offset to be shifted away from where the probe actually contacts the part.


This code is non-modal and only applies to the block of code in which G36 is specified.

The points probed are offset by the values in Settings 59 through 62. See the settings section of this manual for more information.

Do not use Cutter Compensation (G41, G42) with a G36.

Do not use tool length Compensation (G43, G44) with G36

To avoid damaging the probe, use a feed rate below F100. (inch) or F2500. (metric).

Turn on the spindle probe before using G36.

If your mill has the standard Renishaw probing system, use the following commands to turn on the spindle probe.

M59 P1134 ;

Use the following commands to turn off the spindle probe.

M69 P1134 ;

Also see M78, and M79.

% O60361 (G36 AUTO WORK OFFSET MEASUREMENT) ; (G54 X0 Y0 is at the top-center of the part) ; (Z0 is at the surface of part) ; (T1 is a Spindle probe) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 20) ; G00 G90 G54 X0 Y1. (Rapid to 1st position) ; (BEGIN PROBING BLOCKS) ; M59 P1134 (Spindle probe on) ; Z-.5 (Move the probe below surface of part) ; G01 G91 Y-0.5 F50. (Feed towards the part) ; G36 Y-0.7 F10. (Measure and record Y offset) ; G91 Y0.25 F50. (Move incrementally away from part) ; G00 Z1. (Rapid retract above part) ; M69 P1134 (Spindle probe off) ; (BEGIN COMPLETION BLOCKS) ; G00 G90 G53 Z0. (Rapid retract to Z home) ; 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.