Siemens Sinumerik 840D sl Programming Manual page 192

Motion commands
10.6 Circular interpolation
I1= J1= K1= :
=AC(...):
=IC(...):
Input in absolute and incremental dimensions
The G90/G91 defaults for absolute or incremental dimensions are valid for the intermediate
and circle end points.
With G91, the circle starting point is used as the reference for the intermediate point and end
point.
Turning technology
Note
The diameter programming of the interpolation parameter for the transverse axis is not
supported with CIP in the circular-path programming. The interpolation parameter for the
transverse axis must therefore be programmed in the radius.
Examples
Example 1: Milling
Program code
N10 G0 G90 X130 Y70.70 S800 M3
192
Interpolation parameters: Intermediate points in Cartesian coordinates (in X,
Y, Z direction)
The meanings are as follows:
Coordinate of the intermediate point in the X direction
I1:
Coordinate of the intermediate point in the Y direction
J1:
Coordinate of the intermediate point in the Z direction
K1:
Absolute dimensions (non-modal)
Incremental dimensions (non-modal)
In order to machine an inclined circular groove,
a circle is described by specifying the inter‐
mediate point with three interpolation parame‐
ters, and the end point with three coordinates.
Comment
; Approach starting point.
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
Fundamentals