Tapping g36, 1 8 dr illing cy cles – HEIDENHAIN MANUALplus 4110 User Manual
Page 357
HEIDENHAIN MANUALplus 4110
357
6.1
8
Dr
illing Cy
cles
Tapping G36
You can use cycle G36 with stationary tools for cutting axial threads in
the turning center and with driven tools for cutting axial and radial
threads.
Meaning of "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
X end point
of thread for axial machining (diameter value)
Z end point
of thread for radial machining
F feed per revolution:
Thread pitch
B run-in length
(default: 2 * thread pitch F1): Distance for reaching
the programmed spindle speed and feed rate
Q number of spindle
Q=0: Master spindle (stationary tool)
Q=1: Driven tool
H reference direction
for thread pitch (default: 0)
H=0: Feed rate on the Z axis
H=1: Feed rate on the X axis
S retraction speed
(default: Same spindle speed as for tapping)
K drilling depth
(radial holes: radius)
K is defined: The starting point of the hole is calculated from the
hole end point and "K."
K is not defined: "K" is calculated from the hole end point and the
current tool position.
Retraction length J
(default: 0) when using floating tap holders
Notes:
The control starts execution of the cycle at the current tool and
spindle position. The starting point is approached at rapid traverse.
Axial hole:
Do not program "X."
Define "Z."
Radial hole:
Define "X."
Do not program "Z."
X and Z are programmed: The control uses the "tool orientation" to
decide whether a radial or an axial hole is machined (see “Tapping
tools” on page 424).
Example: G36
%36.nc
[G36]
N1 T50 G97 S1000 G95 F0.2 M3
N2 G0 X0 Z5
N3 G71 Z-30
N4 G14 Q0
N5 T51 G97 S600 M3
N6 G0 X0 Z8
N7 G36 Z-25 F1.5 B3 Q0
END