HEIDENHAIN MANUALplus 4110 - Manual (Page 348)

348 6 DIN Programming
6.16 Under
c
ut Cy
cles
Undercut according to DIN 509 F with cylinder
machining G852
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
 I undercut depth (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 transverse depth (default: Value from standard table)
 A transverse angle (default: Value from standard table)
 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
 U finishing oversize for the area of the cylinder (default: 0)
Note:
Parameters that are not programmed are automatically calculated
from the diameter in the standard table (see “DIN 509 E, DIN 509 F—
undercut parameters” on page 527).
Blocks following the cycle call
Example: G852
%852.nc
[G852]
N1 T21 G95 F0.23 G96 S248 M3
N2 G0 X60 Z2
N3 G852 I3 K15 W30 R2 P0.2 A8 B5 RB2 WB30
E0.2 H1
N4 G0 X50 Z0
N5 G1 Z-30
N6 G1 X60
N7 G80
END N.. G852 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.