(This G-code is optional and requires a probe)
This G-code is used to set tool length offsets.F - Feedrate
Automatic Tool Length Offset Measurement (G37) is used to command a probe to set tool length offsets. A G37 will feed the Z-Axis in an effort to probe a tool with a tool-setting probe. The Z-Axis will move until a signal from the probe is received or the travel limit is reached. A non-zero H code and either G43 or G44 must be active. When the signal from the probe is received (skip signal) the Z position is used to set the specified tool offset (Hnnn). The resulting tool offset is the distance between the current work coordinate zero point and the point where the probe is touched. If a non-zero Z value is on the G37 line of code the resulting tool offset will be shifted by the non-zero amount. Specify Z0 for no offset shift.
The work coordinate system (G54, G55, etc.) and the tool length offsets
(H01-H200) may be selected in this block or the previous block.
This code is non-modal and only applies to the block of code in which G37 is specified.
A non-zero H code and either G43 or G44 must be active.
To avoid damaging the probe, use a feed rate below F100. (inch) or F2500. (metric).
Turn on the tool-setting probe before using G37.
If your mill has the standard Renishaw probing system, use the following commands to turn on the tool-setting probe.
Use the following command to turn off the tool-setting probe.
Also see M78 and M79.
This sample program measures the length of a tool and records the measured value on the tool offset page. To use this program, the G59 work offset location must be set to the tool-setting probe location.