Simple Drilling G71 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Drilling cycles

Simple drilling G71

G71 is used for axial and radial bore holes using driven or stationary
tools.
Parameters:
ID: Hole dimensions – name of the hole definition
NS: Starting block no. of contour – beginning of contour
section
Reference to the contour of the hole (G49, G300 or G310-
Geo)
No input: Single hole without contour description
NF: Position mark – reference at which the cycle stores the
hole positions (range: 1 to 127)
XS: Start point of radial hole (diameter value)
ZS: Start point of axial hole
XE: Final point of radial hole (diameter value)
ZE: Final point of axial hole
K: Boring depth (alternative toXE and ZE)
A: Tap/Drill. lth (default: 0)
V: Bore variant – feed rate reduction 50 % (default: 0)
0: Without reduction
1: At end of the hole
2: At start of the hole
3: At start & end of hole
RB: Return plane (default: retract to starting position or to
safety clearance; diameter value with radial holes and holes in
the YZ plane)
E: Period of dwell for chip breaking at end of hole (default: 0)
D: Retraction type
0: Rapid traverse
1: Feed rate
BS: Start elem.no. – number of the first hole to be machined in
a pattern
BE: End: elem.no. – number of the last hole to be machined in
a pattern
H: Brake off (1) (default: 0)
0: Spindle brake on
1: Spindle brake off
Single hole without contour description: Program XS
or ZS as alternative.
Hole with contour description: Do not program XS, ZS
Hole pattern: NS refers to the hole contour, and not
the definition of the pattern
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
373