Filter
Top Products
Section Section 44 System ProgrammingSystem Programming
5858
Y=3, Z=4.5. The Machine Coordinates
remain unchanged at X=3, Y=3, Z=0.
G29 X4 Y4 Z0 Move the X and Y axes across and the Z
axis down to Program Coordinates X=4,
Y=4, Z=0, Machine Coordinates X=4, Y=4,
Z=-4.5
G01 X5 Z-1 Linear interpolation to Program Coordinates
X=5, Y=4, Z=-1, Machine Coordinates X=5,
Y=4, Z=-5.5
G28 Move the Z axis up and the X and Y axes
across to the Tool Change Position, Program
Coordinates X=2, Y=2, Z=4.5, Machine
Coordinates X=2, Y=2, Z=0
G49 Cancel Tool Length Compensation. The Z
axis Program Coordinate changes by -0.500,
the difference in Length Offset between the
current tool (#3: 1.000) and the tool
displayed in the Current Tool pull-down
menu when the program first began (#1:
1.500). The new Program Coordinates are
X=2, Y=2, Z=4. The Machine Coordinates
remain unchanged at X=2, Y=2, Z=0. At
this point the current tool should be removed
from the spindle.
G52 Local Coordinate System
The G52 command defines and activates a local coordinate system that LC uses in
place of your original Program Coordinates for all absolute positioning moves.
The X, Y and Z parameters indicate the offset from your original Program Zero
location to the origin for the local coordinate system.
For example, "G52 X1 Y2 Z-4" would activate a local coordinate system whose
origin is at a distance of 1, 2, -4 from the original Program Zero.
All absolute moves are made relative to the new local coordinate system. To
cancel use of the local coordinate system in the middle of a G-code file, use the
command “G52 X0 Y0 Z0”.
When LC reads a G52 command, it displays a magenta dot in the Tool Path View
Port showing the origin of the local coordinate system.
Note that the local coordinate system only applies to the G-code file being
executed. The G52 command has no effect on the Program Zero you set before
running the G-code file. LC automatically cancels the local coordinate system
when it completes execution of a G-code file.