Siemens Sinumerik 840D sl Programming Manual page 180

Motion commands
10.6 Circular interpolation
Examples
Example 1: Milling
Program code
N10 G0 G90 X133 Y44.48 S800 M3
N20 G17 G1 Z-5 F1000
N30 G2 X115 Y113.3 I-43 J25.52
N30 G2 X115 Y113.3 I=AC(90) J=AC(70)
N30 G2 X115 Y113.3 CR=-50
N30 G2 AR=269.31 I-43 J25.52
N30 G2 AR=269.31 X115 Y113.3
N30 CIP X115 Y113.3 Z-10 I1=IC(-...) J1=IC(...) K1=IC(-...)
N40 M30
180
The following program lines contain an exam‐
ple for each circular-path programming possi‐
bility. The necessary dimensions are shown in
the production drawing on the right.
Comment
; Approach starting point
; Tool infeed
; Circle end point, center
point in incremental dimensions
; Circle end point, center
point in absolute dimensions
; Circle end point, circle ra-
dius
; Opening angle, center point
in incremental dimensions
;Opening angle, circle end
point
; Circle end point and inter-
mediate point: Coordinates for
all three geometry axes
; End of program
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
Fundamentals