HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 505)

HEIDENHAIN MANUALplus 620, CNC PILOT 620/640
505
6.7 Milling cy
cles f
o
r the Y axis
Area milling—finishing G842
G842 finishes surfaces defined with G376-Geo (XY plane) or G386-
Geo (YZ plane). The cycle mills from the outside toward the inside. The
tool moves to the working plane outside of the workpiece material.
Parameters
ID Milling contour—name of the contour to be milled
NS Block number—reference to the contour description
P Milling depth (maximum infeed in the working plane)
H Cutting direction for side finishing (default: 0)
 H=0: Up-cut milling
 H=1: Climb milling
U (Minimum) overlap factor. Defines the overlap of milling paths
(default: 0.5).
Overlap = U*milling diameter
V Overrun factor. Defines the distance by which the tool should
pass the outside radius of the workpiece (default: 0.5).
Overrun = V*milling diameter
F Feed rate for infeed (default: active feed rate)
RB Retraction plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Cycle run
1 Starting position (X, Y, Z, C) is the position before the cycle
begins.
2 Calculate the proportioning of cuts (infeeds to the milling planes,
infeeds in the milling depths).
3 Move to the safety clearance and plunge to the first milling depth.
4 Mill the first plane.
5 Retract by the safety clearance, return and cut to the next milling
depth.
6 Repeat steps 4 and 5 until the complete area is milled.
7 Returns to retraction plane RB.