HEIDENHAIN MANUALPLUS 620 User Manual

HEIDENHAIN MANUALplus 620 287
4.21 Undercut Cycles
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).
Parameters that are not programmed are automatically calculated
from the diameter in the standard table (see "Undercut cycle G85" on
page 284).
Blocks following the cycle call
Example: 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 Surface 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 Cut-in angle (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 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.

HEIDENHAIN MANUALPLUS 620 Specifications

General

Brand	HEIDENHAIN
Model	MANUALPLUS 620
Category	Control Systems
Language	English