HEIDENHAIN CNC Pilot 4290 - Manual (Page 156)

4 DIN PLUS 144
4.9 Dr
illing Cy
cles
Boring, countersinking G72
Use of G72: Boring, sinking, reaming, NC spot drilling or centering for
axial/ radial holes with stationary or driven tools.
G72 is used for bore holes with contour definition (individual bore hole
or hole pattern) in the following program sections:
■ FRONT
■ REAR SIDE
■ SURFACE
Parameters
NS:
Contour block number with geometry of bore hole (G49, G300/
G310-Geo)
E: Period of dwell (for chip breaking at end of hole) – default: 0
D: Retraction speed – default: 0
■ D=0: Rapid traverse
■ D=1: Feed rate
K: Retraction plane (radial holes, holes in the YZ plane: diameter) –
default: to starting position or to safety clearance
Cycle run
1 Approach starting position at rapid traverse
according to ”K”:
■ K not programmed: Approach to clearance height.
■ K programmed: Approach to ”K,” and then to
clearance height.
2 Start drilling bore hole at reduced feed rate (50%).
3 Move at feed rate to end of bore hole.
4 Retract at rapid traverse or feed rate according to
”D.”
5 Position to which tool retracts depends on ”K”:
■ K not programmed: Retract to starting position.
■ K programmed: Retract to position ”K.”
Hole pattern: ”NS” refers to the bore hole
contour (and not the definition of the
pattern).