Service Home G136 Automatic Work Offset Center Measurement (Group 00)

G136 Automatic Work Offset Center Measurement (Group 00)

G136 Automatic Work Offset Center Measurement (Group 00)

This G-code is optional and requires a probe. Use it to set work offsets to the center of a work piece with a work probe.

F - Feedrate
* 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

* indicates optional

Automatic Work Offset Center Measurement (G136) is used to command a spindle probe to set work offsets. A G136 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 (skip 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 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 the measured center of the two probed points.

Notes:

This code is non-modal and only applies to the block of code in which G136 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 G136.

Do not use tool length Compensation (G43, G44) with G136

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

Turn on the spindle probe before using G136.

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

M59 P3 ;

Use the following commands to turn off the spindle probe:

M69 P3 ;

Also see M75, M78, and M79.

Also see G31.

This sample program measures the center of a part in the Y Axis and records the measured value to the G58 Y Axis work offset. To use this program, the G58 work offset location must be set at or close to the center of the part to be measured.

%
O61361 (G136 AUTO WORK OFFSET - CENTER OF PART) ;
(G58 X0 Y0 is at the center of part) ;
(Z0 is on top of the part) ;
(T1 is a spindle probe) ;
(BEGIN PREPARATION BLOCKS) ;
T1 M06 (Select tool 1) ;
G00 G90 G40 G49 G54 (Safe startup) ;
G00 G58 X0. Y1. (Rapid to 1st position) ;
(BEGIN PROBING BLOCKS) ;
M59 P3 (Spindle probe on) ;
Z-10. (Rapid spindle down to position) ;
G91 G01 Z-1. F20. (Incremental feed by Z-1.) ;
G31 Y-1. F10. M75 (Measure & record Y reference) ;
G01 Y0.25 F20. (Feed away from surface) ;
G00 Z2. (Rapid retract) ;
Y-2. (Move to opposite side of part) ;
G01 Z-2. F20. (Feed by Z-2.) ;
G136 Y1. F10. ;
(Measure and record center in the Y axis) ;
G01 Y-0.25 (Feed away from surface) ;
G00 Z1. (Rapid retract) ;
M69 P3 (Spindle probe off) ;
(BEGIN COMPLETION BLOCKS) ;
G00 G90 G53 Z0. (Rapid retract to Z home) ;
M30 (End program) ;
%