Siemens SINUMERIK 840DE Programming Manual page 124

Programming Motion Commands
4.5 Circular interpolation types, (G2/G3, CIP, CT)
Example of milling
The following program lines contain an example for each circular programming possibility.
The necessary dimensions are shown in the production drawing on the right.
N10 G0 G90 X133 Y44.48 S800 M3
N20 G17 G1 Z-5 F1000
N30 G2 X115 Y113.3 I-43 J25.52
Or
N30 G2 X115 Y113.3 I=AC(90) J=AC(70)
Or
N30 G2 X115 Y113.3 CR=-50
Or
N30 G2 AR=269.31 I-43 J25.52
Or
N30 G2 AR=269.31 X115 Y113.3
Or
N30 N30 CIP X80 Y120 Z-10
I1= IC(-85.35)J1=IC(-35.35) K1=-6
N40 M30
4-18
;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 radius
;Aperture angle, center point in
;incremental dimensions
;Arc angle, circle end point
;Circle end point and intermediate
point:
;Coordinates for all
;three geometry axes
;End of program
Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1
Fundamentals