170
G CODES
96-8000
June 1999
AUTOMATIC W ORK O FFSET M EASUREMENT (G36 , G136)
G36 Automatic Work Offset Center Measurement (This G-code is optional and requires a probe)Group 00
G136 Automatic Work Offset Center Measurement Group 00
F Feed rate in inches (mm) per minute
I Optional offset distance along X-axis
J Optional offset distance along Y-axis
K Optional offset distance along Z-axis
X Optional X-axis motion command
Y Optional Y-axis motion command
Z Optional Z-axis motion command
A Optional A-axis motion command
The automatic work offset measurement operation is a non-modal operation that causes a linear move of the X,
Y, Z, and A axes until the skip signal is received or the end of the programmed motion. The X, Y, Z, and A axes
are moved to the programmed position in a linear move but will stop early if the skip signal is received. Tool
offsets must not be active when this function is performed. M78 or M79 may be used to test if the skip signal
was received. The currently active work coordinate system is set for each axis that is programmed. The point
where the skip signal is received becomes the work zero position. The work coordinate system may be se-
lected in this block or in a previous block.
The points probed are offset by the values in Settings 59 through 62.
A G36 will set the work coordinates to the point where the probe is hit. The G136 will set the work coordinates
to a point at the center of a line between the probed point and the point set with M75. This allows the center of
a part to be found using two separated probed points.
Note that the X, Y, Z, or A programmed into this block are interpreted in the coordinate system that is about to
be set. Thus, the end point of the move will be interpreted in the old work coordinate value. For this reason, it is
easier to program these moves as incremental (G91).
If an I, J, or K is specified, the appropriate axis work offset is shifted by the amount in the I, J, or K. This allows
the work offset to be shifted some distance away from where the probe actually hits.
CUTTER C OMPENSATION (G40, G41, G42)
G40 Cutter Comp Cancel Group 07
G40 will cancel the G41 or G42 cutter compensation. Programming a D00 will also cancel cutter compensa-
tion.
G41 2D Cutter Compensation Left Group 07
G41 will select cutter compensation left; that is the tool is moved to the left of the programmed path to com-
pensate for the size of the tool. A Dnn must also be programmed to select the correct tool size from compen-
sation memory. If compensation memory contains a negative value for cutter size, cutter compensation will
operate as though G42 was specified.
To Next Page
Loading...
Need help?
General
