Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set User Manual
Page 413
Axis Motion
Chapter 14
14-37
The axis word programmed with the G51.1 command is used to define the
location mirroring will be about. The defined location intercepts the
programmed axis at the programmed position. If only one axis is
programmed, the mirroring plane is perpendicular to that axis. If more
than one axis is programmed, the mirror plane passes through these points.
Important: The control only mirrors those axes that are programmed in
the G51.1 block. Axes not programmed in the G51.1 block execute
normally.
A G50.1 block cancels the mirror image function.
G50.1X__Y__Z__ ;
The control only cancels the mirror feature for those axes that are
programmed in the G50.1 block. Axes not programmed in the G50.1 block
remain mirrored. There is no significance to the axis value programmed
with the axis words in a G50.1 block. Axis values may or may not be
required depending on how the way AMP was configured by your system
installer. In either case, these values will be ignored by the control.
Example 14.14
Programmable Mirror Image
Main Program
Comment
(Mirror);
comment block, main program
G00G90;
rapid positioning, absolute mode
M98P8500;
call subprogram 8500
G51.1X75.;
mirror active on X
M98P8500;
call subprogram 8500
G51.1Y75.;
mirror active on Y (and X)
M98P8500;
call subprogram 8500
G50.1X0;
cancel mirror on X (active on Y only)
M98P8500;
call subprogram 8500
G50.1Y0;
cancel mirror on Y (no mirroring)
M30;
Subprogram
Comment
O8500;
program number
G00G90X60.Y90.;
rapid to start point
G01Y120.F50;
move 1
G03X30.Y90.R30;
move 2
G01X60.;
move 3
M99;
return from subprogram