G100/G101 Disable/Enable Mirror Image (Group 00)

Next Generation Control Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue
*X - X-Axis command
*Y - Y-Axis command
*Z - Z-Axis command
*A - A-Axis command
*B - B-Axis command
*C - C-Axis command

* indicates optional

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 indicates when an axis is mirrored. Also see Settings 45, 46, 47, 48, 80, and 250 for mirror imaging.

The format for turning Mirror Image on and off is:

G101 X0. (turns on mirror imaging for the X-Axis) ; G100 X0. (turns off mirror imaging for the X-Axis) ;

X-Y Mirror Image

Mirror Image and Cutter Compensation

Turning on Mirror Image for only one of the X or Y axes causes the cutter to move along the opposite side of a cut. The control automatically switches the cutter compensation direction (G41, G42) and reverses 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 changes 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 eliminates this problem.

Mirror Image and Pocket Milling

Program Code for Mirror Imaging in the X-Axis:

% O61011 (G101 MIRROR IMAGE ABOUT X AXIS) ; (G54 X0 Y0 is at the center of part) ; (Z0 is on top of the part) ; (T1 is a 0.250 in. diameter endmill) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G00 G54 X-.4653 Y.052 (Rapid to 1st position) ; S5000 M03 (Spindle on CW) ; G43 H01 Z.1 (Activate tool offset 1) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G01 Z-.25 F5. (Feed to depth of cut) ; M98 P61012 F20. (Call contour subprogram) ; G00 Z.1 (Rapid retract above part) ; G101 X0. (Mirror imaging on for X Axis) ; X-.4653 Y.052 (Rapid to 1st position) ; G01 Z-.25 F5. (Feed to depth of cut) ; M98 P61012 F20. (Call contour subprogram) ; (BEGIN COMPLETION BLOCKS) ; G00 Z0.1 M09 (Rapid retract, Coolant off) ; G100 X0. (Mirror imaging off for X Axis) ; G53 G49 Z0 M05 (Z home, Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; % % O61012 (G101 CONTOUR SUBPROGRAM) ; (Subprogram for pocket in O61011) ; (Must have a feedrate in M98) ; G01 X-1.2153 Y.552 (Linear move) ; G03 X-1.3059 Y.528 R.0625 (CCW arc) ; G01 X-1.5559 Y.028 (Linear move) ; G03 X-1.5559 Y-.028 R.0625 (CCW arc) ; G01 X-1.3059 Y-.528 (Linear move) ; G03 X-1.2153 Y-.552 R.0625 (CCW arc) ; G01 X-.4653 Y-.052 (Linear move) ; G03 X-.4653 Y.052 R.0625 (CCW arc) ; M99 (Exit to Main Program) ; %
*X - X-axis command
*Z - Z-axis command

* indicates optional. At least one is required.

Programmable mirror image can be turned on or off individually for the X and/or Z Axis. The bottom of the screen indicates when an axis is mirrored. These G codes are used in a command block without any other G codes and do not cause any Axis motion. G101 turns on mirror image for any Axis listed in that block. G100 turns off mirror image for any Axis listed in the block. The actual value given for the X or Z code has no effect; G100 or G101 by itself has no effect. For example, G101 X 0 turns on X-axis mirror.

note: Settings 45 and 47 may be used to manually select mirror image.

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback