Haas 96-8000 - G37 Automatic Tool Offset Measurement (Group 00)

146
96-8000 Rev AC
May 2010
position.
If an I, J, or K is specied, 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.
Notes:
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.
Example:
M53
G04 P100
M63
Program Example
O1234 (G36)
M53
G04 P100
M63
G00 G90 G54 X1. Y0
Z-18.
G91 G01 Z-1. F20.
G36 X-1. F10.
G90 G01 X1.
M53
G04 P100
M63
G00 G90 G53 Z0
M30
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 specied 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.