HEIDENHAIN CNC Pilot 4290 Description of the Y axis - Manual (Page 28)

Y Axis 28
Surface 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.
”U” defines the overlapping of the milling paths. ”V” defines the
distance by which the tool should pass the outside radius of the
workpiece (reference: tool diameter).
The tool moves to the working plane outside of the workpiece
material.
Cycle run
1 Starting position (X, Y, Z, C) is the position before the cycle
begins.
2 Calculates the cutting segmentation (infeeds to the working
planes, infeeds in the working plane).
3 Moves to the safety clearance and plunges to the first milling
depth.
4 Mills one plane.
5 Retracts by the safety clearance, returns and cuts to the next
milling depth.
6 Repeats steps 4 and 5 until the complete surface is milled.
7 Retracts to ”return plane J.”
Parameters
NS: Block number – reference to contour description
H: Cutting direction (relative to the machined edges) – default: 0
■ H=0: Up-cut milling
■ H=1: Climb milling
P: (Maximum) milling depth (infeed in the working plane)
U: (Minimum) overlap factor (overlap = U * tool diameter) –
default: 0.5
V: Overrun factor (overrun = V * tool diameter) – default: 0.5
F: Feed rate for infeed – default: Active feed rate
J: Return plane – no entry: Tool returns to the starting position
■ XY plane: Return position in Z direction
■ YZ plane: Return position in X direction (diameter)
2.3.4
Milling
Cycles
Y_4290BH.pm6 08.03.2005, 08:36 28