HEIDENHAIN MANUALplus 4110 - Manual (Page 318)

318 6 DIN Programming
6.1
1
Cont
our
-Based T
u
rn
ing Cy
cles
Contour finishing G89
G89 finishes the contour area defined in the subsequent blocks (see
“Contour definition” on page 310).
In the NC block after G89, the tool-tip radius compensation (TRC) is
called with G41/G42 (without parameters) and allows you to define the
position of the tool (reference: contour direction):
„ G41: Tool moves to the right of the contour.
„ G42: Tool moves to the left of the contour.
MANUALplus switches off the TRC at the end of the cycle. If you do
not define G41/G42, the TRC function does not become effective.
Parameters
 B chamfer/rounding at start of contour
„ B>0: Radius of rounding
„ B<0: Width of chamfer
 I oversize: Equidistant oversize—a negative oversize is permitted.
 K retraction mode at the end of cycle —defines the tool position
at the end of the cycle:
„ No input: Return to starting point of cycle
„ K=0: Tool remains at cycle end position
„ K>0: Tool retracts by K
 J element position: When the contour section begins with a
chamfer/rounding, J defines the position of the "imaginary reference
element" (default: 1).
Reference element:
„ J=1: Transverse element in the positive X-axis direction
„ J=–1: Transverse element in the negative X-axis direction
„ J=2: Longitudinal element in the positive Z-axis direction
„ J=–2: Longitudinal element in the negative Z-axis direction
Example: G89
%89.nc
[G89]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X70 Z2
N3 G89 B-2 I2 K1 J1
N4 G42
N5 G0 X40 Z0
N6 G1 Z-20 B3
N7 G1 X60 B-2
N8 G1 Z-32
N9 G25 H5 W30
N10 G1 X70
N11 G80
END
Oversizes: An oversize programmed with G58 is taken
into account if I is not defined in the cycle. After the cycle
has been executed, the oversize is canceled.