HEIDENHAIN CNC Pilot 4290 - Manual (Page 168)

4 DIN PLUS 156
Pocket milling – roughing G845
G845 roughs closed contours and figures in the following program
sections:
■ FRONT
■ REAR SIDE
■ SURFACE
You can change the cutting direction with the ”cutting direction H,”
the ”machining direction Q” and the direction of tool rotation (see
table G846).
Parameters
NS:
Block number – reference to contour description
P: (Maximum) milling depth (infeed in the working plane)
I: Oversize in X direction
K: Oversize in Z direction
U: (Minimum) overlap factor – overlap of tool paths (overlap = U *
cutter diameter) – default: 0.5
V: Overrun factor – no significance for machining with the C axis
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 – default: Current feed
rate
J: Retraction plane – default: return to starting position
■ Front or rear face: Retraction position in Z direction
■ Lateral surface: Retraction 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
Programming in the Y axis See ”CNC PILOT 4290 with Y Axis”
User's Manual.
Oversizes are taken into account with
G845 (G57: X, Z direction; G58: equidistant
oversize in the milling plane).
4.1
1 Milling Cy
cles
Cycle run
1 Starting position (X, Z, C) is the position before the
cycle begins.
2 Calculate the cutting segmentation (infeeds to the
working planes, infeeds in the working plane).
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 surface is
milled.
7 Retract to ”return plane J.”