Section Section 44 System ProgrammingSystem Programming
4848
an incremental move, the ending point is defined relative to the current tool
location. The G90/G91 commands tell the system which of these two modes to
use (described below).
While there will be cases where incremental programming is useful, generally you
should define your moves as absolute since it is a less error prone method of
programming. All of the examples in the following section use absolute
positioning unless otherwise noted.
G and M Code Reference
G00 Rapid Tool Positioning
The G00 command moves the tool to the designated XYZ coordinate at the rapid
rate using 3-Axis linear interpolation. The rapid rate is calculated from the
Maximum Feedrates defined in the Feedrate/Ramping Setup dialog box.
Example:
G00 X1.0 Y2.0 Z1.5 Moves the tool directly to the Program
Coordinate X=1.0, Y=2.0, Z=1.5 at the rapid
rate (assuming G90 is active). If G91 is
active then it moves the tool a distance 1, 2,
1.5 from the current location.
When using G00, there are several things to keep in mind:
• You do not need to specify all three coordinates, only the ones for
which you want movement.
Example:
G00 X4.0 Y3.0 Moves the tool to Program
coordinate X=4.0, Y=3.0, leaving the
Z position unchanged.
• This is a modal command, meaning that all successive moves will be
treated as rapid moves until another modal move command (G01, G02
or G03) occurs.
Example:
G00 X1.0 Y2.0 Z1.5 Rapid Move
X4.0 Y6.5 Z1.0 Rapid Move
G01 X3.0 Y3.0 Z1.4 Feedrate Move
X2.8 Y1.4 Z0 Feedrate Move
• The interpretation of the coordinates depends on the G90/G91
command in effect.