HEIDENHAIN TNC 410 ISO Programming - Manual (Page 225)

HEIDENHAIN TNC 410, TNC 426, TNC 430 199
8.3 Cy
cles f
o
r Dr
illing
, T
a
p
p
ing
and
Th
read Millin
g TAPPING with a floating tap holder
(Cycle G84)
1 The tool drills to the total hole depth in one movement.
2 Once the tool has reached the total hole depth, the direction of
spindle rotation is reversed and the tool is retracted to the starting
position at the end of the dwell time.
3 At the starting position, the direction of spindle rotation reverses
once again.
U U U U Set-up clearance 1 (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 2 (thread length, incremental value):
Distance between workpiece surface and end of
thread.
U U U U Dwell time in seconds : Enter a value between 0 and
0.5 seconds to avoid wedging of the tool during
retraction.
U U U U Feed rate F : Traversing speed of the tool during
tapping.
The feed rate is calculated as follows: F = S x p
Example: NC block
N13 G84 P01 2 P02 -20 P03 0 P04 100 *
X
Z
111
2
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation
G40.
Program a positioning block for the starting point in the
tool axis (set-up clearance above the workpiece surface).
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program DEPTH
= 0, the cycle will not be executed.
A floating tap holder is required for tapping. It must
compensate the tolerances between feed rate and spindle
speed during the tapping process.
When a cycle is being run, the spindle speed override knob
is disabled. The feed rate override knob is active only
within a limited range, which is defined by the machine
tool builder (refer to your machine manual).
For tapping right-hand threads activate the spindle with M3,
for left-hand threads use M4.
F Feed rate (mm/min)
S: Spindle speed (rpm)
p: Thread pitch (mm)