HEIDENHAIN MANUALplus 4110 - Manual (Page 349)

HEIDENHAIN MANUALplus 4110 349
6.16 Under
c
ut Cy
cles
Undercut according to DIN 76 with cylinder
machining G853
The cycle machines the adjoining cylinder, the undercut, and finishes
with the plane surface. It also machines a cylinder start chamfer when
you enter at least one of the parameters "B" or "RB."
Parameters
 FP thread pitch
 I undercut diameter (diameter value) (default: Value from standard
table)
 K undercut length (default: Value from standard table)
 W undercut angle (default: Value from standard table)
 R undercut radius (default: Value from standard table)
 P oversize
„ P is not defined: The undercut is machined in one pass
„ P is defined: Division into pre-turning and finish-turning
– P = longitudinal oversize
– The transverse oversize is preset to 0.1 mm
 B cylinder 1st cut length —no input: No chamfer machined at
start of cylinder
 RB 1st cut radius —no input: No chamfer radius is machined
 WB 1st cut angle (default: 45°)
 E reduced feed rate (default: Active feed rate): For the plunge cut
and the thread chamfer
 H type of departure (default: 0):
„ H=0: Tool returns to the starting point
„ H=1: Tool remains at the end of the plane surface
Note:
Parameters that are not programmed are automatically calculated
from the standard table (see “DIN 76—undercut parameters” on
page 525):
„ FP from the diameter
„ I, K, W, and R from FP (thread pitch)
Blocks following the cycle call
Example: G853
%853.nc
[G853]
N1 T21 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G853 FP1.5 I47 K15 W30 R2 P1 B5 RB2
WB30 E0.2 H1
N4 G0 X50 Z0
N5 G1 Z-30
N6 G1 X60
N7 G80
END
N.. G853 FP.. I.. K.. W.. /Cycle call
N.. G0 X.. Z.. /Corner point of cylinder start chamfer
N.. G1 Z.. /Undercut corner
N.. G1 X.. /End point of plane surface
N.. G80 /End of contour definition
„ Undercuts can only be executed in orthogonal, paraxial
contour corners along the longitudinal axis.
„ Cutting radius compensation: Active.
„ Oversizes: are not taken into account.