HEIDENHAIN MANUALplus 4110 - Manual (Page 355)

HEIDENHAIN MANUALplus 4110 355
6.1
8
Dr
illing Cy
cles
Deep-hole drilling cycle G74
You can use cycle G74 with stationary tools for drilling axial holes in
the turning center and with driven tools for drilling axial and radial
holes.
The hole is drilled in several passes. After each pass, the drill retracts
and advances again to the first drilling depth, minus the "safety
clearance." The drilling depth is reduced with each subsequent pass.
Parameters
 X end point of axial hole (diameter value)
 Z end point of radial hole
 R safety clearance no input: Value from "Current parameters—
Machining—Safety distances"
 P 1st hole depth —no input: Hole will be drilled in one pass
 I reduction value (default: 0): With each subsequent pass, the
drilling depth is reduced by "I," however, without falling below "J."
 B return distance (default: Retract to starting point of hole)
 J minimum hole depth (default: 1/10 of P)
 A drilling lengths (default: 0)
 E dwell time for chip breaking at end of hole (default: 0)
 V drilling variants —Feed rate reduced by 50% during both pre-
drilling and through-boring
„ 0: No feed rate reduction
„ 1: Feed reduction for through-boring
„ 2: Feed reduction for pre-drilling
„ 3: Feed reduction for pre-drilling and through-boring
 K drilling depth (radial holes: radius)
„ K is defined: The starting point of the hole is calculated from the
hole end point and "K."
„ K is not defined: "K" is calculated from the hole end point and the
current tool position.
 D retreat retraction speed and infeed within the hole—default: 0
„ 0: Rapid traverse
„ 1: Feed rate
Example: G74
%74.nc
[G74]
N1 M5
N2 T49 G197 S1000 G195 F0.2 M103
N3 M14
N4 G110 C0
N5 G0 X80 Z2
N6 G745 XK0 YK0 Z2 K80 Wi90 Q4 V2
N7 G74 Z-40 R2 P12 I2 B0 J8
N8 M15
END