Tapping G73 - HEIDENHAIN CNC PILOT 640 User Manual

4

Tapping G73

G73 cuts axial and radial threads 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
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)
F: Thread pitch (prevails over the contour description)
B: Run-in lgth
S: Return speed (default: tapping speed)
J: Retract length with use of floating tap holders (default: 0)
RB: Return plane (default: back to start position)
P: Chip breaking depth
I: Return distance
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
The starting position is calculated from the safety clearance and the
Slop.length B.
Parameter combinations for single holes without contour
description
XS, XE
XS, K
XE, K
Retract length J: Use this parameter for floating tap holders. The
cycle calculates a new nominal pitch on the basis of the thread depth,
the programmed Thread pitch and the Retract length. The nominal
pitch is somewhat smaller than the Thread pitch of the tap. During
tapping, the tap is pulled away from the chuck by the Retract length.
With this method you can achieve higher service life from the taps.
376
ZS, ZE
ZS, K
ZE, K
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
DIN/ISO programming | Drilling cycles