HEIDENHAIN CNC Pilot 4290 Description of the Y axis - Manual (Page 27)

HEIDENHAIN CNC PILOT 4290 27
2.3.4
Milling
Cycles
2.3.4 Milling Cycles
Contour milling G840
G840 mills, finishes, engraves or deburrs figures or ”free contours”
(open or closed) in the following program sections:
■ FRONT_Y (with Y axis)
■ REAR_SIDE_Y (with Y axis)
■ SURFACE_Y (with Y axis)
Machining with the Y axis operates as with the C axis (see User's
Manual, section ”4.8.15 Milling Cycles”).
Surface 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.
”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
P: (Maximum) milling depth (infeed in the working plane)
I, K: Allowance in X, Z direction
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)
Allowances are taken into account (G57:
X, Z direction; G58: equidistant oversize
in the milling plane).
Y_4290BH.pm6 08.03.2005, 08:36 27