HEIDENHAIN MANUALplus 4110 - Manual (Page 364)

364 6 DIN Programming
6.20 F
a
ce Mac
h
ining
Contour and figure milling cycle, face G793
G793 mills figures or (open or closed) "independent" contours on the
face. G793 is followed by:
„ The figure to be milled with:
„ Circle (G304), rectangle (G305) or polygon (G307)
„ Conclusion of milling contour (G80)
„ The independent contour with:
„ Starting point of milling contour (G100)
„ Milling contour (G101, G102, G103)
„ Conclusion of milling contour (G80)
Parameters
 Z milling top edge
 ZE milling floor
 P maximum infeed (default: Total depth in one infeed)
 U overlap factor: Machining of contour or pocket (default: 0)
„ U=0: Contour milling
„ U>0: Pocket milling—minimum overlap of milling paths =
U*milling diameter
 R approaching radius: (Radius of approaching/departing arc)—
(default: 0)
„ R=0: Contour element is approached directly; feed to starting
point above the milling plane—then vertical plunge.
„ R>0: Tool moves on approaching/departing arc that connects
tangentially to the contour element.
„ R<0 for inside corners: Tool moves on approaching/departing arc
that connects tangentially to the contour element.
„ R<0 for outside corners: Length of linear approaching/departing
element; contour element is approached/departed tangentially.
 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: G793
%100.nc
[G100, G101, G102, G103, G793]
N1 T70 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G793 Z2 ZE-5 P2 U0.5 R0 I0.5 F0.15 H0 Q0
N6 G100 XK20 YK5
N7 G101 XK50 B5
N8 G103 XK5 YK50 R50 Q1 B5
N9 G101 XK5 YK20 B5
N10 G102 XK20 YK5 R20 B5
N11 G80
N12 M15
END