HEIDENHAIN CNC Pilot 4290 Description of the Y axis - Manual (Page 31)

HEIDENHAIN CNC PILOT 4290 31
Pocket milling - roughing G845
G845 roughs closed contours and figures that are defined in the XY
or YZ plane in the program sections:
■ FRONT_Y
■ REAR_SIDE_Y
■ SURFACE_Y
For machining with the C axis: see the User's Manual, section
”4.8.15 Milling Cycles.”
”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).
You can change the cutting direction with the ”cutting direction
H,” the ”machining direction Q,” and the direction of tool rotation
(see the User's Manual, section ”4.8.15 Milling Cycles”).
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 (if the milling contour passes the turning
contour)
■ 0: The defined contour is milled completely.
■ 0 < V † 1: Overrun = V * tool diameter
H: Cutting direction – default: 0
■ H=0: Up-cut milling
■ H=1: Climb milling
F: Feed rate for infeed – default: Active feed rate
E: Reduced feed rate for circular elements – no entry: Current
feed rate
2.3.4
Milling
Cycles
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)
Q: Machining direction – default: 0
■ Q=0: From the inside toward the outside
■ Q=1: From the outside toward the inside
Allowances are taken into account (G57:
X, Z direction; G58: equidistant oversize
in the milling plane).
Y_4290BH.pm6 08.03.2005, 08:36 31