HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 297)

HEIDENHAIN MANUALplus 620, CNC PILOT 620/640
297
4.1
9
Thr
ead cy
cles
Simple thread cycle G32
G32 cuts a single thread in any desired direction and position
(longitudinal, tapered or transverse thread; internal or external thread).
Parameters
X End point of thread (diameter)
Z End point of thread
XS Starting point for thread (diameter)
ZS Starting point for thread
BD External/internal thread:
 0: External thread
 1: Internal thread
F Thread pitch
U Thread depth
No input: The thread depth is calculated automatically:
 External thread (0.6134 * F)
 Internal thread (0.5413 * F)
I Maximum cutting depth
IC Number of cuts. The infeed is calculated from IC and U. Usable
with:
 V=0 (constant chip cross section)
 V=1 (constant infeed)
V Type of infeed (default: 0)
 0: Constant cross section for all cuts
 1: Constant infeed
 2: W/ remaining cutting (with distribution of remaining cuts).
First infeed = Remainder of the division of thread depth/
cutting depth. The last cut is divided into four partial cuts:
1/2, 1/4, 1/8 and 1/8
 3: Infeed is calculated from the pitch and spindle speed
 4: Same as MANUALplus 4110
H Type of offset for smoothing the thread flanks (default: 0)
 0: Without offset
 1: Offset from the left
 2: Offset from the right
 3: Tool is offset alternately from the right and left
K Run-out length at thread end point (default: 0)
W Taper angle (–45° < W < 45°)—(default: 0)
Position of the taper thread with respect to longitudinal or
transverse axis:
 W>0: Rising contour (in machining direction)
 W<0: Falling contour