HEIDENHAIN MANUALplus 4110 - Manual (Page 335)

HEIDENHAIN MANUALplus 4110 335
6.15 Thr
ead Cy
cles
6.15 Thread Cycles
Universal thread cycle G31
G31 cuts threads in any desired direction and position (longitudinal,
tapered or transverse threads; internal or external threads). You can
also machine successions of threads.
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
 R difference in radii (default: 0): Difference between the
diameters at the start of thread (XA) and end of thread (X). With
descending contours, R must be programmed as a negative value.
R=(X–XA)/2
 B run-in length: Distance required to accelerate to the
programmed feed rate.
No input: Internal calculation (see “Thread run-in / thread run-out”
on page 163)
 P run-out length: Distance required to decelerate the slide.
No input: Internal calculation (see “Thread run-in / thread run-out”
on page 163)
 A feed angle: Range: 0° < A < 60°
No input: A=arctan (0.5*F/U)
 V type of approach (default: 0)
„ V=0: Constant cross section for all cuts
„ V=1: Constant feed
„ V=2: With distribution of remaining cut
„ V=3: Without distribution of remaining cut
 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)
 Q number of air cuts after the last cut (default: 0)
 C starting angle: Position of the spindle at the thread start
(default: 0°)
„ G31 without contour definition: "X, Z" is programmed. The thread
starts at the current tool position and ends at the end point X, Z.
Example: G31
%31.nc
[G31]
N1 T45 G97 S800 M3
N2 G0 X20 Z5
N3 G31 Z-50 F1.5 I0.2
END