Operation Manual

HEIDENHAIN CNC PILOT 640 289
4.6 Thread and undercut cycles
Recut API thread
Call the thread-cutting menu
Select API thread
Press the Recut soft key
 On: Inside thread
 Off: Outside thread
This optional cycle recuts a single or multi-start external or internal API
thread. Since you have already unclamped the workpiece, the CNC
PILOT needs to know the exact position of the thread. Place the
cutting tip of the tap drill in the center of a groove and transfer the
positions to the parameters measured angle and measured position
by pressing the Take over position soft key. From these values the
cycle then calculates the angle of the spindle at the starting point.
This function is available only in manual operation.
Cycle parameters
X1, Z1 Starting point of thread
X2, Z2 End point of thread
F1 Thread pitch (= feed rate)
D No. of gears (threads per unit)
U Thread depth – No input:
 Outside thread: U=0.6134*F1
 Inside thread: U=–0.5413*F1
I Maximum infeed
 I<U: First cut with cutting depth I — further cuts:
reduction of cutting depth
 I=U: One cut
 No input: Calculation from U and F1
WE Run-out angle (range: 0° <= WE < 90°)
W Taper angle (range: –60° < A < 60°)
C Measured angle
ZC Measured position
A Infeed angle (range: -60° <= A < 60°; default: 30°)
 A<0: Infeed on left thread flank
 A>0: Infeed on left right flank
R Remaining cutting depth—only with GV=4 (default:
1/100 mm)