Siemens SINUMERIK 828D Programming Manual page 214

Motion commands
9.6 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 N30 CIP X80 Y120 Z-10
I1=IC(-85.35) J1=IC(-35.35) K1=-6
N40 M30
214
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
; Opening angle, circle end point
; Circle end point and intermediate
point
; Coordinates for all three geometry
axes
; End of program
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Fundamentals