HEIDENHAIN CNC Pilot 4290 Description of the Y axis - Manual (Page 30)

Y Axis 30
Polygon milling finishing G844
G844 finishes centric polygons defined with G477 Geo (XY plane)
or with G487 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. (”U, V” refer to the 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) and the spindle position.
3 Spindle turns to the first position. The tool 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 The tool retracts to ”return plane J.” The spindle turns to the
next position. The tool moves to the safety clearance and
plunges to the first milling depth.
8 Repeats 4 to 7 until all polygonal surfaces are milled.
9 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 30