Haas Mill G35 Automatic Tool Diameter Measurement

Haas G Codes Mill Reference

G35 Automatic Tool Diameter Measurement (Group 00)

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

F Feedrate in inches (mm) per minute
D Tool diameter offset number
X Optional X-axis command
Y Optional Y-axis command

Automatic Tool Diameter Offset Measurement function (G35) is used to set the tool diameter (or radius) using two passes of the probe; one on each side of the tool. The first point is set with a G31 block using an M75, and the second point is set with the G35 block. The distance between these two points is set into the selected (non-zero) Dnnn offset. Setting 63 (Tool Probe Width) is used to reduce the measurement of the tool by the width of the tool probe.
This G-code moves the axes to the programmed position. The specified move is started and continues until the position is reached or the probe sends a signal (skip signal).

Notes:

Also see G31.
Use the assigned M-code (M52) to turn the table probe on.
Use the assigned M-code (M62) to turn the table probe off.
Also see M75, M78, and M79.
Do not use Cutter Compensation with a G35.
Turn on the spindle in reverse (M04), for a right handed cutter.

O1234 (G35)
M52
T1 M06
G00 G90 G54 X0 Y1.
G43 H01 Z0
G01 Z-1. F10.
M04 S200
G31 Y0.49 F5. M75
G01 Y1. F20.
Z0
Y-1.
Z-1.
G35 Y-0.49 D1 F5.
G01 Y-1. F20.
M62
G00 G53 Z0 M05
M30

G35 Automatic Tool Diameter Measurement