Haas Mill G36 Automatic Work Offset Measurement

Haas G Codes Mill Reference

G36 Automatic Work Offset Measurement (Group 00)

(This G-code is optional and requires a probe)

F Feedrate in inches (mm) per minute
I Optional offset distance along X-axis
J Optional offset distance along Y-axis
K Optional offset distance along Z-axis
X Optional X-axis motion command
Y Optional Y-axis motion command
Z Optional Z-axis motion command

Automatic Work Offset Measurement (G36) is used to command a probe to set work fixture offsets. A G36 will feed the axes of the machine in an effort to probe the workpiece with a spindle mounted probe. The axis (axes) will move until a signal from the probe is received, or the travel limit is reached.
Tool offsets (G41, G42, G43, or G44) must not be active when this function is preformed. The currently active work coordinate system is set for each axis programmed. The point where the skip signal is received becomes the zero position. 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.


The points probed are offset by the values in Settings 59 through 62. Use G91 incremental moves when using a G36. Use the assigned M-codes (for example M53 and M63) with a dwell to turn the spindle probe on or off.

G04 P100

Program Example

O1234 (G36)
G04 P100
G00 G90 G54 X1. Y0
G91 G01 Z-1. F20.
G36 X-1. F10.
G90 G01 X1.
G04 P100
G00 G90 G53 Z0

G36 Automatic Work Offset Measurement