HEIDENHAIN iTNC 530 (340 420) - Manual (Page 262)

234 8 Programming: Cycles
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
U U U U Set-up clearance Q200 (incremental value): Distance
between tool tip (at starting position) and workpiece
surface. Standard value: approx. 4 times the thread
pitch
U U U U Total hole depth Q201 (thread length, incremental
value): Distance between workpiece surface and end
of thread
U U U U Feed rate F Q206: Traversing speed of the tool during
tapping
U U U U Dwell time at bottom Q211: Enter a value between 0
and 0.5 seconds to avoid wedging of the tool during
retraction
U U U U Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface.
U U U U 2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices) can
occur.
The feed rate is calculated as follows: F = S x p
Retracting after a program interruption
If you interrupt program run during tapping with the machine stop
button, the TNC will display a soft key with which you can retract the
tool.
Example: NC blocks
25 CYCL DEF 206 TAPPING NEW
Q200=2 ;SAFETY CLEARANCE
Q201=-20 ;DEPTH
Q206=150 ;FEED RATE FOR PLUNGING
Q211=0.25 ;DWELL TIME AT DEPTH
Q203=+25 ;SURFACE COORDINATE
Q204=50 ;2ND SAFETY CLEARANCE
F Feed rate (mm/min)
S: Spindle speed (rpm)
p: Thread pitch (mm)