HEIDENHAIN MANUALplus 4110 - Manual (Page 317)

HEIDENHAIN MANUALplus 4110 317
6.1
1
Cont
our
-Based T
u
rn
ing Cy
cles
Contour-parallel roughing G836
G836 machines the workpiece sections parallel to the contour. The
starting point of the contour is defined either in the cycle with X,Z or
in the G0 block after the cycle call. The blocks following G836 describe
the contour area. G80 concludes the contour description.
Parameters
 X starting point (diameter value)
 Z starting point
 P maximum infeed: The infeed depth is determined taking J into
account. The proportioning of cuts is calculated so that an "abrasive
cut" is avoided.
„ J=0: P is the maximum infeed depth. The cycle reduces the infeed
depth if the programmed infeed is not possible in the transverse
or longitudinal direction due to the cutting geometry.
„ J>0: P is the infeed depth. This infeed is used in the longitudinal
and transverse directions.
 I oversize X (diameter value)—(default: 0)
 K oversize Z (default: 0)
 J workpiece blank oversize —the cycle machines:
„ J=0: From the current tool position.
„ J>0: The area defined by the workpiece blank oversize.
 Q transverse roughing (default: 0): Longitudinal or transverse
machining
„ Q=0: Longitudinal machining
„ Q=1: Transverse machining
Note on the execution of the cycle:
„ MANUALplus automatically determines the cutting and infeed
directions from the current tool position relative to the starting point
/ end point of the contour area.
„ Tool position at the end of the cycle: Cycle starting point
Example: G836
%836.nc
[G836]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G836 P4 I1 K0.3
N4 G0 X80 Z0
N5 G1 Z-15 B-1
N6 G1 X102 B2
N7 G1 Z-22
N8 G1 X90 Zi-12 B1
N9 G1 Zi-6
N10 G1 X100 A80 B-1
N11 G1 Z-47
N12 G1 X110
N13 G0 Z2
N14 G80
END
„ At the start of the cycle, the tool must be located
outside the defined contour area.
„ Cutting radius compensation: Active.
„ G57/G58 oversizes are taken into account if I/K is not
programmed. After the cycle has been executed, the
oversizes are canceled.
„ Safety clearance after each step: Parameter "Current
parameters—Machining—Safety distances."
„ For workpiece blank oversize J>0: Set the “infeed
depth P” to the smaller infeed, if the maximum infeed
differs for the longitudinal and transverse directions due
to the cutting geometry.
„ The cycle parameter workpiece blank oversize J is
available as of NC software versions 507 807-16 and
526 488-08. With earlier software versions, the cycle
starts the machining operation from the current tool
position.