HEIDENHAIN TNC 426, User Manual

Page: 252 / 502

226 8 Programming: Cycles
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
TAPPING with a floating tap holder (Cycle 2)
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 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 Total hole depth 2 (thread length, incremental value):
Distance between workpiece surface and end of
thread
U Dwell time in seconds : Enter a value between 0 and
0.5 seconds to avoid wedging of the tool during
retraction.
U Feed rate F : Traversing speed of the tool during
tapping
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
24 L Z+100 R0 FMAX
25 CYCL DEF 2.0 TAPPING
26 CYCL DEF 2.1 SET UP 3
27 CYCL DEF 2.2 DEPTH -20
28 CYCL DEF 2.3 DWELL 0.4
29 CYCL DEF 2.4 F100
30 L X+50 Y+20 FMAX M3
31 L Z+3 FMAX M99
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 R0.
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)