Siemens SINUMERIK 840DE Programming Manual page 133

Further information
Full circles (traversing angle 360°) cannot be programmed with AR=, but must be
programmed using the circle end point and interpolation parameters. The center point
coordinates I, J, K are normally entered in incremental dimensions with reference to the
circle starting point.
You program the absolute center point non-modally with reference to the workpiece zero
with: I=AC(...), J=AC(...), K=AC(...). An interpolation parameter I, J, K with value 0 can be
omitted but the second associated parameter must always be specified.
Example for milling
Programming a circle with arc angle and center point or end point
N10 G0 X67.5 Y80.211
N20 G3 X17.203 Y38.029 AR=140.134 F500
Or
N20 G3 I–17.5 J–30.211 AR=140.134 F500
Fundamentals
Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1
4.8 Circular interpolation with arc angle and center point (G2/G3, AR=)
Programming Motion Commands
4-27