HEIDENHAIN MANUALplus 4110 - Manual (Page 312)

312 6 DIN Programming
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:
„ G817: Cycle starting point Z; last retraction diameter X
„ G818: Cycle starting point
Example: G817, G818
%817.nc
[G817, G818]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G818 P5 H2 I1 K0.3
N4 G0 X60 Z2
N5 G1 Z-15
N6 G1 X82 B2
N7 G1 X90 Zi-15
N8 G80
N9 G0 X120 Z-28
N10 G817 X90 P4 H0 I1 K0.3
N11 G0 X90 Z-28
N12 G1 Z-45 B-3
N13 G1 X102 B2
N14 G1 X120 A30
N15 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."