HEIDENHAIN MANUALplus 4110 - Manual (Page 366)

366 6 DIN Programming
6.20 F
a
ce Mac
h
ining
Area milling, face G797
Depending on "Q," G797 mills surfaces, polygons or the figure defined
in the command following G797.
Parameters
 X limiting diameter
 Z milling top edge
 ZE milling floor
 B width across flats (omit for Q=0): B defines the remaining
material. For an even number of surfaces, you can program "B" as an
alternative to "V."
„ Q=1: Remaining thickness
„ Q>=2: Width across flats
 V edge length —omit for Q=0
 R chamfer/rounding arc —omit for Q=0
„ R<0: Chamfer length
„ R>0: Rounding arc
 A slope angle (reference: see graphic support window)—omit for
Q=0
 Q number of surfaces (default: 0):
Range: 0 <= Q <= 127
„ Q=0: G797 is followed by a figure definition
„ Q=1: One surface
„ Q=2: Two surfaces offset by 180°
„ Q=3: Triangle
„ Q=4: Rectangle, square
„ Q>4: Polygon
 P maximum infeed (default: Total depth in one infeed)
 U overlap factor (default: 0.5): Minimum overlap of milling paths =
U*milling diameter
 I oversize contour-parallel
 K oversize Z (in infeed direction)
 F feed rate for infeed (default: Active feed rate)
 E reduced feed rate for circular elements (default: Active feed rate)
 H cutting direction (default: 0): The cutting direction (see
graphic support window) can be changed with H and the direction
of tool rotation.
„ H=0: Up-cut milling
„ H=1: Climb milling
Example: G797
%797.nc
[G797]
N1 T70 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G797 X100 Z0 ZE-5 B50 R2 A0 Q4 P2 U0.5
N6 G100 Z2
N7 M15
END