Siemens SINUMERIK 840D sl Programming Manual page 761

Program code
N80 X0 Y0 Z0 A0 B0 C0 G17 T1 D1 F12000
N90 TRAORI(1)
N100 B4=-1 C4=1
N110 G41 ORID CUT3DF G64 X10 Y0 Z0
N120 X30
N130 Y20 A4=1 C4=1
N140 B3=1 C3=5
N150 B3=1 C3=1
N160 X-10 A5=1 C5=2 ORIC
N170 A3=-2 C3=1
N180 A3=-1 C3=1
N190 Y-10 A4=-1 C4=3
N200 X-20 Y-20 Z10
N210 X-30 Y10 A4=1 C4=1
N220 A3=1 B3=0.5 C3=1.7
N230 X-20 Y30 A4=1 B4=-2 C4=3 ORID
N240 A3 = 0.5 B3=-0.5 C3=1
N250 X0 Y30 C4=1
N260 BSPLINE X20 Z15
N270 X30 Y25 Z18
N280 X40 Y20 Z13
N290 X45 Y0 PW=2 Z8
N300 Y-20
N310 G2 ORIMKS A30 B45 I-20 X25 Y-40 Z0
N320 G1 X0 A3=-0.123 B3=0.456 C3=2.789 B4=-1 C4=5
B5=-1 C5=2
N330 X-20 G40
N340 M30
Example 2: NC program (section) generated from a CAD system with CUT3DFD
Program code
N01 G710
N03 T="12"
N06 S5305 M03
N07 G642
; Approaching the starting position in the MCS taking the tool length into account.
G00 G90 X-250.62787 Y-38.37944 A=DC(253.12719)
B-12.49543
G00 G90 Z251.80052
; End of positioning in the MCS.
;
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
Comment
; Selection of the tool.
; Select orientation transformation.
; Definition of the plane.
; Activate tool offset.
; Outside corner, new plane definition.
; Change in orientation with ORID.
; Change in orientation with ORID.
; Change in orientation with ORIC.
; Change in orientation with ORIC.
; New plane definition.
; Inside corner with previous block.
; Inside corner, new plane definition.
; Change in orientation with ORIC.
; Change in orientation.
; Path movement, new plane,
; orientation with relative programming.
; Spline begin, relative programming of the orien-
tation
; remains active during spline.
; Helix, orientation with axis programming.
; Path movement, orientation, non-constant plane.
; Deactivation of the tool radius compensation.
Comment
Work preparation
3.13 Tool offsets
761