HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 175)

159 HEIDENHAIN TNC 410, TNC 426, TNC 430
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.
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 depth parameter determines
the working direction.
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.
ú Setup clearance (incremental value): Distance
between tool tip (at starting position) and workpiece
surface. Standard value: approx. 4 times the thread
pitch
ú Total hole depth (thread length, incremental value):
Distance between workpiece surface and end of
thread
ú Dwell time in seconds: Enter a value between 0 and
0.5 seconds to avoid wedging of the tool during
retraction.
ú Feed rate F: Traversing speed of the tool during
tapping
The feed rate is calculated as follows: F = S x p,
where
F is the feed rate in mm/min),
S is the spindle speed in rpm,
and p is the thread pitch in mm
Retract tool if program is interrupted (not TNC 410)
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.
X
Z
8.3 Dr
illing Cy
cles
Example NC block:
N13 G84 P01 2 P02 -20 P03 0 P04 100*
Kkap8.pm6 29.06.2006, 08:06 159