HEIDENHAIN MANUALplus 4110 - Manual (Page 338)

338 6 DIN Programming
6.15 Thr
ead Cy
cles
Thread single path G33
G33 cuts threads in any desired direction and position with variable
pitch (longitudinal, tapered or transverse threads; internal or external
threads). The thread starts at the current tool position and ends at the
"end point X, Z."
Parameters
 X end point of thread (diameter value)
 Z end point of thread
 F thread pitch
 B run-in length (default: 0): Distance required to accelerate to the
programmed feed rate
 P run-out length (default: 0): Distance required to decelerate the
slide
 C starting angle: Position of the spindle at the thread start
(default: 0°)
 Q number of spindle (default: 0=master spindle)
 H reference direction for thread pitch
(default: 3)
„ H=0: Feed rate on the Z axis (for longitudinal and taper threads up
to a max. angle of +45°/–45° to the Z axis)
„ H=1: Feed rate on the X axis (for transverse and taper threads up
to a max. angle of +45°/–45° to the X axis)
„ H=3: Contouring feed rate
 E variable pitch (default: 0)
„ E>0: Increase the pitch per revolution by E
„ E<0: Decrease the pitch per revolution by E
Example: G33
%33.nc
[G33]
N1 T45 G97 S1100 G95 F0.5 M3
N2 G0 X101.84 Z5
N3 G83 X100 Z5 I0.15
N4 G33 X120 Z-80 F1.5
N5 G33 X140 Z-122.5 F1.5
N6 G0 X150 Z5
N7 G80
END
„ "Cycle STOP" becomes effective at the end of a thread
cut.
„ Feed rate override is not effective during cycle
execution.
„ Feed forward control is switched on.