G100 Cancel Mirror Image (Group 00)
G101 Enable Mirror Image (Group 00)
X X-axis command Y Y-axis command Z Z-axis command A A-axis command
Programmable mirror imaging is used to turn on or off any of the axes. When one is ON, axis motion may be mirrored (or reversed) around the work zero point. These G codes should be used in a command block without any other G codes. They do not cause any axis motion. The bottom of the screen will indicate when an axis is mirrored. Also see Settings 45 through 48 for mirror imaging.
The format for turning Mirror Image on and off is:
G101 X0. = Will turn on mirror imaging for the X axis.
G100 X0. = Will turn off mirror imaging for the X axis.
Image and Cutter Compensation
Turning on Mirror Image for only one of the X or Y axes will cause the cutter to move along the opposite side of a cut. The control will automatically switch the cutter compensation direction (G41, G42) and reverse the circular motion commands (G02, G03) as needed.
When milling a shape with XY motions, turning on Mirror Image for just one of the X or Y axes will change climb milling (G41) to conventional milling (G42) and/or conventional milling to climb milling. As a result, the type of cut or finish may not be what was desired. Mirror imaging of both X and Y will eliminate this problem.
Program Code for Mirror Imaging in the X-Axis:
Program Example Description % O3600 (Mirror image X axis) T1 M06 (Tool #1 is a 0.250” diameter endmill) G00 G90 G54 X-.4653 Y.052 S5000 M03 G43 H01 Z.1 M08 G01 Z-.25 F5. M98 P3601 F20. G00 Z.1 G101 X0. X-.4653 Y.052 G01 Z-.25 F5. M98 P3601 F20. G00 Z.1 G100 X0. G28 G91 Y0 Z0 M30 % % O3601 (Contour subprogram) G01 X-1.2153 Y.552 G03 X-1.3059 Y.528 R.0625 G01 X-1.5559 Y.028 G03 X-1.5559 Y-.028 R.0625 G01 X-1.3059 Y-.528 G03 X-1.2153 Y-.552 R.0625 G01 X-.4653 Y-.052 G03 X-.4653 Y.052 R.0625 M99 %
G100 Cancel Mirror Image G101 Enable Mirror Image