HEIDENHAIN MANUALplus 4110 - Manual (Page 180)

180 4 Cycle Programming
4.6 Thr
ead and Under
c
ut Cy
cles
Undercut DIN 76
Call the thread-cutting menu.
Select the "Undercut DIN 76" cycle.
With return soft key:
Off: When the cycle is completed, the tool remains at
the cycle end position (see figures at right).
On: Tool returns to the starting point (see figures on
next page).
The cycle machines a thread undercut according to DIN76, 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 "B" or "RB."
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
 T tool number
 S spindle speed / cutting speed
 F feed per revolution
 I undercut diameter —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
 P undercut oversize
„ P>0: Division into pre-turning and finish-turning—"P" is the
longitudinal oversize; the transverse oversize is always 0.1 mm
„ No input: Machining in one cut
 B cylinder start chamfer —default: No start chamfer
 WB 1st cut angle —default: 45°
 RB chamfer radius —default: No chamfer radius