HEIDENHAIN MANUALplus 4110 - Manual (Page 182)

182 4 Cycle Programming
4.6 Thr
ead and Under
c
ut Cy
cles
Undercut DIN 509 E
Call the thread-cutting menu.
Select the "Undercut DIN 509 E" 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 DIN 509 type E, a
cylinder start chamfer, then the adjoining cylinder, and finishes with
the plane surface. You can define a finishing oversize for the area of
the cylinder. The cylinder start 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
 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 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
 B cylinder start chamfer —default: No start chamfer
 WB 1st cut angle —default: 45°
 RB chamfer radius —default: No chamfer radius
 U finishing oversize for the area of the cylinder—default: 0
All parameters that you enter will be accounted for—even if the
standard table prescribes other values. If the parameters I, K, W and
R are not defined, MANUALplus determines these values from the
cylinder diameter in the standard table (see “DIN 509 E, DIN 509 F—
undercut parameters” on page 527).