HEIDENHAIN CNC Pilot 4290 V7.1 Description of B and Y axes - Manual (Page 53)

HEIDENHAIN CNC PILOT 4290 53
1
.1
1
DIN PLUS (Y Axis): Milling Cy
cles
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
NS
Block number—reference to the contour description
H Cutting direction for side finishing (default: 0)
„ H=0: Up-cut milling
„ H=1: Climb milling
P (Maximum) milling depth (infeed in the working plane)
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)
J 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 Return to “retraction plane J.”