Siemens SINUMERIK 840D sl Programming Manual page 210

Motion commands
9.6 Circular interpolation
Significance
G2:
G3:
CIP:
CT:
X Y Z :
I J K :
CR= :
AR= :
AP= :
RP= :
I1= J1= K1= :
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
210
Circular interpolation, clockwise
Circular interpolation, counterclockwise
Circular interpolation through intermediate point
Circle with tangential transition defines the circle
End point in Cartesian coordinates
Circle center point in Cartesian coordinates in X, Y, Z direction
Circle radius
Opening angle
End point in polar coordinates, in this case polar angle
End point in polar coordinates, in this case polar radius corresponding
to circle radius
Intermediate points in Cartesian coordinates in X, Y, Z direction
The following program lines contain an
example for each circular-path programming
possibility. The necessary dimensions are
shown in the production drawing on the right.
Comment
; Approach starting point
; Feed of the tool
; Circle end point, center point in
incremental dimensions
; Circle end point, center point in
absolute dimensions
; Circle end point, circle radius
; Opening angle, center point in
incremental dimensions
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals