Haas Mill G37 Automatic Tool Offset Measurement

Haas G Codes Mill Reference

G37 Automatic Tool Offset Measurement (Group 00)

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

F Feedrate in inches (mm) per minute
H Tool offset number
Z Required Z-axis offset

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 table mounted 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 offset between the work zero point and the point where the probe is touched.
The coordinate system (G54-G59, G110-G129) and the tool length offsets (H01-H200) may be selected in this block or the previous block.
Notes:
Use the assigned M-code (M52) to turn the table probe on.
Use the assigned M-code (M62) to turn the table probe off.

Cutter Compensation may not be active during a skip function.
Also see M78 and M79.
Specify Z0 for no offset.

O1234 (G37)
T1 M06
M52
G00 G90 G110 X0 Y0
G00 G43 H1 Z5.
G37 H1 Z0. F30.
G00 G53 Z0
M62
M30

G37 Automatic Tool Offset Measurement