G53: Basic Machine Coordinate System Selection - Mitsubishi Electric MELSEC iQ-R16MTCPU Programming Manual

G53: Basic machine coordinate system selection

Moves to command positions on the basic machine coordinate system.
Code Format
G53
G53 X x
Processing details
• The basic machine coordinate system is used to indicate positions specifically determined by the machine.
• The G53 command is unmodal. It is only valid for the specified block.
• The G53 command moves by an incremental value based on the selected coordinate system when in incremental value
command mode (G91). To move to a position on the basic machine coordinate system, use the G53 command in absolute
value command mode (G90). When operating in incremental value command mode (G91) up until the block before, set
absolute value command mode (G90) before the G53 command.
• The G53 command moves by cutting feed or fast forward in accordance with command modal (G00, G01). When the G53
command and circular interpolation command (G02, G03) are commanded in the same block, linear interpolation is
performed to the end point coordinates but the modal is a circular modal.
• When the G53 command is executed, the compensation vector of the tool radius in the applicable block is cancelled.
However, the compensation amount for the tool radius at axes commanded from the next point onwards is not cancelled.
(1)
• Movement to the coordinate command of the G53 command block starts after the completion of deceleration stop at the
previous block.
• The tool length compensation amount set by tool length compensation (G43, G44), is temporarily cancelled.
Program example
■Program that performs positioning to the specified position of the work coordinate system
after positioning to the specified position of the basic machine coordinate system in absolute
value mode
Operation Program
(1) G90
(2) G53 X10. Y10.
(3) G01 X10. Y10. F20.
Y Y
10
(2)
(3)
10
10
Y y Z z
Coordinate on basic machine coordinate system
(2) (3)
Current position
X
10
Work coordinates
X
Basic machine [Unit: mm]
coordinates
: Tool center path
: Program path
(G41)
(1) G91 G01 X60. Y30.
(2) G90 G53 X10. Y10.
(3) X30. Y40.
(4) X70. Y50.
Remarks
Absolute position command
Move to basic machine coordinates X10,Y10
Move to work coordinates X10,Y10
5 G-CODE CONTROL PROGRAMS
5
141
5.6 G-Code