HEIDENHAIN SW 54843x-03 DIN Programming - Manual (Page 530)

530 DIN programming for the Y axis
6.7 Milling cy
cles f
o
r the Y axis
Centric 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. 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 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) and the spindle positions.
3 Spindle turns to the first position. The tool moves to the safety
clearance and plunges 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 The tool returns to "retraction plane J." The spindle turns to the
next position. The tool moves to the safety clearance and plunges
to the first milling depth.
8 Repeat steps 4 to 7 until all polygonal surfaces are milled.
9 Return to retraction plane RB.