G136 Automatic Work Offset Center 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 Center Measurement (G136) is used to command a probe to set work offsets. A G136 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. Use a G31 cycle with an M75 to set the first point. A G136 will set the work coordinates to a point at the center of a line between the probed point and the point set with an M75. This allows the center of the part to be found using two separate probed points.
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.
Also see G31.
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 (M53 & M63) with a dwell to turn the spindle probe on or off.
M53 G04 P100 M63 Programming example to probe the center of a bore: O1234 (G136) M53 G04 P100 M63 G00 G90 G54 X0 Y0 Z-17. G91 G01 Z-1. F20. G31 X1. F10. M75 G01 X-1. G136 X-1. F10. G01 X1. M53 G04 P100 M63 G00 G90 G53 Z0 M30 Programming example to probe the center of a part: O1234 (G136) M53 G04 P100 M63 G00 G90 G54 X0 Y5. Z-17. G91 G01 Z-1. F20. G31 Y-1. F10. M75 G01 Y1. F20. G00 Z2. Y-10. G01 Z-2. F20. G136 Y1. F10. G01 Y-1. M53 G04 P100 M63 G00 G90 G53 Z0 M30
G136 Automatic Work Offset Center Measurement