HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 249)

HEIDENHAIN CNC PILOT 4290 249
4.23 Dr
illing Cy
cles
Tapping G73
G73 cuts axial/radial threads using driven or stationary tools. G73 is
used for holes with contour definition (individual hole or hole pattern).
The starting position is calculated from the safety clearance and the
run-in (slope) length B.
Retraction 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 pitch, and the “retract length.” The nominal pitch is
somewhat smaller than the pitch of the tap. During tapping, the drill is
pulled away from the chuck by the retraction length. With this method
you can achieve higher service life from the taps.
Parameters
NS Block number of contour. Reference to the contour of the
hole (G49-Geo, G300-Geo or G310-Geo)
B Slope length (default: machining parameter 7 “Thread starting
length [GAL]”)
S Retraction speed (default: Tapping speed)
K Retraction plane (radial holes, holes in the YZ plane:
diameter)—(default: retract to starting position or to safety
clearance)
J Retraction length when using floating tap holders (default: 0)
H1 As of software version 625 952-04:
Spindle brake (H1 is evaluated if the brake is entered in
machine parameter 1019, ..)—default: 0
„ 0: Activate the spindle brake
„ 1: Deactivate the spindle brake
„ Hole pattern: NS refers to the hole contour, and not the
definition of the pattern.
„ “Cycle STOP” becomes effective at the end of the
tapping operation.
„ Feed rate override is not effective.
„ Do not use spindle override!