HEIDENHAIN MANUALPLUS 620 User Manual

HEIDENHAIN MANUALplus 620 411
5.7 Milling Cycles for the Y Axis
5.7 Milling Cycles for the Y Axis
Area milling—roughing G841
G841 roughs surfaces defined with G376-Geo (XY plane) or with
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
ID Milling contour—name of the contour to be milled
NS Block number—reference to the contour description
P Milling depth (maximum infeed in the working plane)
I Oversize in X direction
K Oversize in Z direction
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 Approach feed for infeed (default: active feed rate)
RB Return plane (default: back to starting position)
 XY plane: Retraction position in Z direction
 YZ plane: Retraction position in X direction (diameter)
Oversizes are taken into account:
 G57: Oversize in X, Z direction
 G58: Equidistant oversize in the milling plane
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 Returns to retraction plane RB.

HEIDENHAIN MANUALPLUS 620 Specifications

General

Brand	HEIDENHAIN
Model	MANUALPLUS 620
Category	Control Systems
Language	English