Siemens CNC Milling | MIRROR-AMIRROR | Programmable Mirroring

Programmable Mirroring Introduction

MIRROR and AMIRROR can be used to mirror workpiece shapes on coordinate axes. All traversing motions of axes for which mirroring is programmed are reversed in their direction with programmable mirroring function.

MIRROR and AMIRROR Codes Format

MIRROR X0 Y0 Z0 ; Programmable mirroring, clears old instructions for offset, rotation, scaling factor, mirroring
AMIRROR X0 Y0 Z0 ; Programmable mirroring, additive to existing instructions
MIRROR ; Without values: clears old instructions for offset, rotation, scaling factor, mirroring

The instructions that contain MIRROR or AMIRROR each require a separate block. The axis value has no influence. A value, however, must be specified.

Note : Any active tool radius compensation (G41/G42) is reversed automatically when mirroring.

The direction of rotation of the circle G2/G3 is also reversed automatically when mirroring.

Programmable Mirroring Examples

MIRROR CNC Program Example – 1

Siemens CNC | CNC Program Example for MIRROR

See the following illustration for example for mirroring with the tool position shown:
Mirroring in different coordinate axes with influence on an active tool radius compensation and G2/G3:

N10 G17 ; X/Y plane, Z standing vertically on it
N20 L10 ; Programmed contour with G41
N30 MIRROR X0 ; Direction changed in X
N40 L10 ; Mirrored contour
N50 MIRROR Y0 ; Direction changed in Y
N60 L10
N70 AMIRROR X0 ; Mirroring once more, but now in X
N80 L10 ; Twice-mirrored contour
N90 MIRROR ; Mirroring off