Operation Manual

HEIDENHAIN CNC PILOT 640 291
4.6 Thread and undercut cycles
Undercut DIN 76
Call the thread-cutting menu
Select Undercut DIN 76.
 Off: When the cycle is completed, the tool remains
at the cycle end position.
 On: Tool returns to the starting point
The cycle machines a thread undercut according to DIN 76, a thread
chamfer, then the cylinder, and finishes with the plane surface. The
thread chamfer is executed when you enter at least one of the
parameters cylinder 1st cut length or 1st cut radius.
Cycle parameters
X, Z Starting point
X1, Z1 Starting point of cylinder
X2, Z2 End point on plane surface
FP Thread pitch (default: value from standard table)
E Reduced feed rate for the plunge cut and the thread
chamfer (default: feed rate F)
I Undercut depth (default: value from standard table)
K Undercut length (default: value from standard table)
W Undercut angle (default: value from standard table)
R Undercut radius on both sides of the undercut (default:
value from standard table)
P1 Undercut oversize
 No input: Machining in one cut
 P>0: Division into pre-turning and finish-turning. P is
longitudinal oversize; the transverse oversize is preset
to 0.1 mm
G14 Tool change point (siehe Seite 140)
T Turret pocket number
ID Tool ID number
S Spindle speed/cutting speed
F Feed per revolution