Siemens SINUMERIK 840D sl Programming Manual page 329

Meaning
MIRROR:
AMIRROR:
X... Y... Z... :
Examples
Example 1: Milling
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
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
Mirror absolute in relation to the currently valid coordinate system set with
G54 to G57, G505 to G599.
Additive mirror image with reference to the currently valid set or program‐
med coordinate system.
Geometry axis whose direction is to be changed. The value specified here
can be chosen freely, e.g. X0 Y0 Z0.
The contour shown here is programmed once
as a subprogram. The three other contours
are generated using mirroring. The workpiece
zero is located at the center of the contours.
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 di-
rection is changed in Y)
; Machine fourth contour at bottom right
;Deactivate mirroring
; Retraction, end of program
2.12 Coordinate transformations (frames)
Fundamentals
329