HEIDENHAIN CNC Pilot 4290 Pilot - Manual (Page 81)

81
Dr
illing cy
cle gr
oup
Deep drilling G74
G74 can be used for axial and radial holes on the end faces or lateral
surface using driven or stationary tools. The hole is drilled in several
passes.
The cycle is used for:
■ A single hole without contour description
■ Boring with contour description (single hole or hole pattern)
Parameters
NS:
Contour block number with boring geometry (G49, G300- or
G310-Geo) – no input: single hole without contour description
X, Z: Position, length – end points of axial/radial holes (X diameter)
P:
1st drilling depth
I: Reduction value – default: 0
B: Return distance
default: Retract to ”starting point of hole”
J: Minimum hole depth - default: 1/10 of P
E: Delay (dwell time for chip breaking at end of hole)
default: 0
V: Feed rate reduction (50%) – default: 0
■ V=0 or 2: Feed rate reduction at start
■ V=1 or 3: Feed rate reduction at start and end
■ V=4: Feed rate reduction at end
■ V=5: No feed rate reduction
Exception for V=0 and V=1: No feed rate reduction when
boring/drilling with indexable inserts and twist drills with 180°
angle
D: Retraction speed and infeed within the hole – default: 0
■ D=0: Rapid traverse
■ D=1: Feed rate
K: Retraction level (radial holes: diameter) – no
input: tool returns to starting position/moves
to clearance height
• Single hole without contour description:
Program „X or Z“ as alternative.
• Hole with contour description: Do not pro-
gram „X, Z“.
• Hole pattern: ”NS” refers to the bore hole
contour (and not the definition of the
pattern).
• A ”feed rate reduction at end” goes into
effect only at the last drilling stage.