HEIDENHAIN MANUALplus 4110 - Manual (Page 315)

HEIDENHAIN MANUALplus 4110 315
6.1
1
Cont
our
-Based T
u
rn
ing Cy
cles
Note on the execution of the cycle:
„ MANUALplus automatically determines the cutting and infeed
directions from the current tool position relative to the starting
point / end point of the contour area.
Tool position at the end of the cycle:
„ G827: Cycle starting point X; last retraction diameter in Z
„ G828: Cycle starting point
Example: G827, 828
%827.nc
[G827, G828]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G827 Z-15 P5 H0 I1 K0.3
N4 G0 X120 Z-15
N5 G1 X62 B3
N6 G1 Z-8 B2
N7 G1 X40 B-2
N8 G1 Z0 B-2
N9 G1 X30
N10 G80
N11 G0 X120 Z-15
N12 G828 Z-38 P4 H1 I1 K0.3
N13 G0 X120 Z-38
N14 G1 X103 B-3
N15 G1 Z-25
N16 G1 Z-15 A195 B2
N17 G1 X80
N18 G80
END
„ Descending contour elements are not machined.
„ The tool must be located outside the defined contour
area.
„ Cutting radius compensation: Active.
„ G57/G58 oversizes are taken into account if I/K is not
programmed. After the cycle has been executed, the
oversizes are canceled.
„ Safety clearance after each step: Parameter "Current
parameters—Machining—Safety distances."