-Shenzhen Guanhong Automation Co.,Ltd.-
SZGH-CNC1000MDb Series
- 50 -
Fig3.17.2 coordinate system rotation
Note: When a decimal fraction is used to specify angular displacement (R_), the 1st digit corresponds to
degree units.
G code for selecting a plane: G17/G18/G19:
The G code for selecting a plane(G17 G18 or G19)
can be specified before the block containing the G code for coordinate system rotation(G68). G17,
G18 or G19 must not be designated in the mode of coordinate system rotation.
Incremental command in coordinate system rotation mode:
The center of rotation for an
incremental command programmed after G68 but before an absolute command is the tool position
when G68 was programmed.(See Fig3.17.3).
Center of rotation
: When
α_β_
is not programmed, the tool position when G68 was programmed
is assumed as the center of rotation.
Coordinate system rotation cancel command
: The G code used to cancel coordinate system
rotation (G69) may be specified in a block in which another command is specified.
Tool compensation
: Cutter compensation, tool length compensation, tool offset, and other
compensation operations are executed after the Coordinate system is rotated.
Limitations:
Commands related to reference position return and the coordinate system:
In coordinate
system rotation mode, G codes related to reference position return (G28,G26,G61,G30, etc.) and
these for changing the coordinate system(G52-G59, etc.)must not be specified. If any of these G
codes is necessary, specify it only after canceling coordinate system rotation mode.
Incremental command: The first move command after the coordinate system rotation cancel
command (G69) must be specified with absolute values. If an incremental move command is
specified, correct movement will not be performed.
Example1: Absolute/Incremental Position commands:
N1 G01 X-500 Y-500 F2000 G17;
N2 G68 X700 Y300 R60;
N3 G90 G01 X0 Y0 F2000;
(G91 X500.0 Y500.0)
N4 G91 X1000
N5 G02 Y1000 R1000
N6 G03 X-1000 I-500 J-500;
N7 G01 Y-1000
N8 G69
