HEIDENHAIN SW 54843x-03 DIN Programming - Manual (Page 319)

HEIDENHAIN MANUALplus 620, CNC PILOT 640 319
4.21 Under
c
ut cy
cles
Undercut according to DIN 509 F with cylinder
machining G852
G852 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 Cut-in length (1st cut length)
or Cut-in radius (1st cut radius).
The Steuerung calculates unentered parameters automatically from
the diameter in the standard table (see “Undercut cycle G85” on
page 316).
Blocks following the cycle call
Beispiel: G852
%852.nc
[G852]
N1 T2 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
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 Face depth (default: value from standard table)
A Face angle (default: value from standard table)
B Cut-in length (1st cut length)—no input: No chamfer machined
at start of cylinder
RB Cut-in radius (1st cut radius)—no input: 1st cut radius is not
machined
WB 1st cut angle (default: 45 °)
E Reduced feed for machining the undercut (default: active feed
rate)
H Type of departure (default: 0):
 0: Tool returns to the starting point
 1: Tool remains at the end of the plane surface
U Grinding oversize for the area of the cylinder (default: 0)
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 on 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 is active.
 Oversizes are not taken into account.