Centric Polygon - Finishing G844 - HEIDENHAIN CNC PILOT 640 User Manual

6

Centric polygon - finishing G844

G844 finishes centric polygons defined with G477-Geo (XY plane)
or 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 milling contour
NS: Block number of contour – reference to the contour
description
P: Milling depth – maximum infeed in the working plane
H: Mill cutting direction for side finishing (default: 0)
0: Up-cut
1: Climb
U: Overlap factor – defines the overlap of milling paths (default:
0.5) (range: 0 to 0.99)
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: Approach feed for plunging (default: active feed rate)
RB: Return plane (default: back to start position)
XY plane: Retraction position in Z direction
YZ plane: Return position in X direction (diameter)
Cycle run
1 Start 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 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 Repeat steps 4 to 7 until all polygonal surfaces are milled.
9 Returns to Return plane RB
596
DIN/ISO Programming for the Y axis | Milling cycles for the Y axis
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017