9: PROGRAMMING
table
l The P number is 0
Set Coordinate System (G10 L2)
To define the origin of a work offset coordinate system,
program: G10 L2 P~ <axes R~>
l P~ is the number of coordinate system to use (G54 = 1,
G59.3 = 9)
l R~ is the rotation about the rotation about the Z-axis
The G10 L2 P~ command doesn't change from the current
coordinate system to the one specified by P. Use G54 through
G59.3 to select a coordinate system.
The coordinate system whose origin is set by a G10 command
may be active or inactive at the time the G10 is executed. If
it's currently active, the new coordinates take effect
immediately. For example, if a G92 origin offset was in effect
before G10 L2, it continues to be in effect after.
Optionally program R to indicate the rotation of the XY axis
around the Z-axis. The direction of rotation is counterclockwise
(viewed from the positive end of the Z-axis). When a rotation
is in effect, jogging an axis only moves that axis in a positive or
a negative direction — not along the rotated axis. To cancel a
rotation for the active coordinate, program G10 L2 P0 R0.
Troubleshooting
It's an error if:
l The P number does not evaluate to an integer in the
range 0-500
l An axis other than X or Z is programmed
Set Tool Table (G10 L10)
To change the tool table entry for tool P so that if the tool
offset is reloaded with the machine in its current position and
with the current G5x and G92 offsets active, program: G10
L10 P~ R~
l P~ is the tool number
l R~ is the radius of tool
The current coordinates for the given axes become the given
values. The axes that are not specified in the G10 L10
command are not changed. This could be useful with a probe
move (G38).
Troubleshooting
It's an error if:
l Cutter Compensation is on
l The P number is unspecified
l The P number is not a valid tool number from the tool
table
l The P number is 0
Set Tool Table (G10 L11)
G10 L11 is just like G10 L10, except that instead of setting
the entry according to the current offsets, it's set so that the
current coordinates would become the given value if the new
tool offset is reloaded and the machine is placed in the G59.3
coordinate system without any G92 offset active. This allows
you to set the G59.3 coordinate system according to a fixed
point on the machine, and then use that fixture to measure
tools without regard to other currently active offsets.
Program: G10 L11 P~ X~ Y~ Z~ R~
l P~ is the tool number
l R~ is the radius of tool
Troubleshooting
It's an error if:
l Cutter Compensation is on
l The P number is unspecified
l The P number is not a valid tool number from the tool
table
l The P number is 0
Set Coordinate System (G10 L20)
G10 L20 is similar to G10 L2, except that instead of setting
the offset/entry to the given value, it is set to a calculated
value that makes the current coordinates become the given
value.
Program: G10 L20 P~ X~ Y~ Z~ A~
l P~ is the number of coordinate system to use (G54 = 1,
G59.3 = 9)
l X~ is the X-axis coordinate
l Y~ is the Y-axis coordinate
l Z~ is the Z-axis coordinate
l A~ is the A-axis coordinate
Troubleshooting
It's an error if:
l The P number does not evaluate to an integer in the
range 0 to 9
l An axis other than X, Y, Z, or A is programmed
©Tormach® 2024
Specifications subject to change without notice.
Page 181 UM10811: 1500MX Operator's Manual (Version 0424A)
For the most recent version, see tormach.com/support
To Next Page
Loading...
