HEIDENHAIN MANUALplus 4110 - Manual (Page 337)

HEIDENHAIN MANUALplus 4110 337
6.15 Thr
ead Cy
cles
Single thread G32
G32 cuts a simple thread in any desired direction and position
(longitudinal, tapered or transverse thread; internal or external thread).
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
 U thread depth
„ U>0: Internal thread
„ U<=0: External thread (lateral surface or front face)
„ U= +999 or –999: Thread depth is calculated
 I maximum infeed
 B remainder cuts (default: 0)
„ B=0: The last cut is divided into four partial cuts: 1/2, 1/4, 1/8 and
1/8.
„ B=1: Without distribution of remaining cut
 Q number of air cuts after the last cut (default: 0)
 K run-out length at end point of thread (default: 0)
 W taper angle (default: 0): Position of the tapered thread with
reference to longitudinal or transverse axis. For cutting a descending
tapered thread, W must be programmed with a negative algebraic
sign.
Range: –45° < W < 45°
 C starting angle: Position of the spindle at the thread start
(default: 0°)
 H type of tool offset (default: 0)
„ H=0: Without offset
„ H=1: Offset from the left toward the thread base
„ H=2: Offset from the right toward the thread base
„ H=3: Tool is offset alternately from the right and left (zigzag)
Internal or external threads: See algebraic sign of "U."
Infeeds: If the division U/I provides a remainder, the first feed is
reduced. The last cut is divided into four partial cuts: 1/2, 1/4, 1/8 and
1/8
Example: G32
%32.nc
[G32]
N1 T45 G97 S800 M3
N2 G0 X16 Z4
N3 G32 X16 Z-29 F1.5 U-0.9 I0.2
END
„ Transverse threads are machined with recessing tools.
„ "Cycle STOP" becomes effective at the end of a thread
cut.
„ The feed rate and spindle speed overrides are not
effective during cycle execution.
„ Feedforward control is switched off.