Siemens SINUMERIK 840D sl Programming Manual page 366

Coordinate transformations (frames)
12.7 Programmable mirroring (MIRROR, AMIRROR)
Program code
N10 G17 G54
N20 L10
N30 MIRROR X0
N40 L10
N50 AMIRROR Y0
N60 L10
N70 MIRROR Y0
N80 L10
N90 MIRROR
N100 G0 X300 Y100 M30
Example 2: Turning
Program code
N10 TRANS X0 Z140
...
N30 TRANS X0 Z600
N40 AMIRROR Z0
N50 ATRANS Z120
...
366
Comment
; Working plane X/Y, workpiece zero
; Machine first contour at top right
; Mirror X axis (the direction is changed in X)
; Machine second contour at top left
; Mirror Y axis (the direction is changed in Y)
; Machine third contour at bottom left
; MIRROR resets previous frames. Mirror Y axis (the
direction is changed in Y)
; Machine fourth contour at bottom right
; Deactivate mirroring
; Retraction, end of program
The actual machining is stored as a
subprogram and execution at the respective
spindle is implemented by means of
mirroring and offsets.
Comment
; Zero offset to W
; Machining of the first side with spindle 1
; Zero offset to spindle 2
; Mirroring of the Z axis
; Zero offset to W1
; Machining of the second side with spindle 2
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals