Haas 96-8000 - G29 Return from Reference Point (Group 00); G31 Feed until Skip (Group 00); G35 Automatic Tool Diameter Measurement (Group 00)

144
96-8000 Rev AC
May 2010
Example 2 (same work and tool offsets as Example 1)
Program segment:
G54;
G43 H02;
G00 G91G28 Z0
The G28 block will move directly to machine coordinate Z = 0 since incremental
positioning is in effect.
G29 Return From Reference Point (Group 00)
The G29 code is used to move the axes to a specic position. The axes se-
lected in this block are moved to the G29 reference point saved in G28, and
then moved to the location specied in the G29 command.
G31 Feed Until Skip (Group 00)
(This G-code is optional and requires a probe)
F Feedrate in inches (mm) per minute
X X-axis absolute motion command
Y Y-axis absolute motion command
Z Z-axis absolute motion command
A A-axis absolute motion command
B B-axis absolute motion command
This G-code moves the axes to the programmed position. It applies only to the
block in which G31 is specied. The specied move is started and continues
until the position is reached or the probe receives a signal (skip signal). The
control will beep when the end of travel is reached.
Do not use Cutter Compensation with a G31.
Use the assigned M-codes (for example M52 and M62), with a dwell, to turn
the table probe on and off
For example:
M53
G04 P100
M63
Also see M75, M78 and M79.
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 rst 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