HEIDENHAIN TNC 426, User Manual

Page: 237 / 502

HEIDENHAIN TNC 426, TNC 430 211
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
PECKING (Cycle 1)
1 The tool drills from the current position to the first plunging depth
at the programmed feed rate F.
2 When it reaches the first plunging depth, the tool retracts in rapid
traverse FMAX to the starting position and advances again to the
first plunging depth minus the advanced stop distance t.
3 The advanced stop distance is automatically calculated by the
control:
n
At a total hole depth of up to 30 mm: t = 0.6 mm
n
At a total hole depth exceeding 30 mm: t = hole depth / 50
n
Maximum advanced stop distance: 7 mm
4 The tool then advances with another infeed at the programmed
feed rate F.
5 The TNC repeats this process (1 to 4) until the programmed depth
is reached.
6 After a dwell time at the hole bottom, the tool is returned to the
starting position in rapid traverse FMAX for chip breaking.
U
Set-up clearance 1 (incremental value): Distance
between tool tip (at starting position) and workpiece
surface
U
Depth 2 (incremental value): Distance between
workpiece surface and bottom of hole (tip of drill
taper)
U
Plunging depth 3 (incremental value): Infeed per cut
The total hole depth does not have to be a multiple of
the plunging depth. The tool will drill to the total hole
depth in one movement if:
n
the plunging depth is equal to the depth
n
the plunging depth is greater than the total hole
depth
U Dwell time in seconds : Amount of time the tool
remains at the total hole depth for chip breaking
U Feed rate F : Traversing speed of the tool during
drilling in mm/min
Example: NC blocks
5 L Z+100 R0 FMAX
6 CYCL DEF 1.0 PECKING
7 CYCL DEF 1.1 SET UP 2
8 CYCL DEF 1.2 DEPTH -15
9 CYCL DEF 1.3 PECKG 7.5
10 CYCL DEF 1.4 DWELL 1
11 CYCL DEF 1.5 F80
12 L X+30 Y+20 FMAX M3
13 L Z+2 FMAX M99
14 L X+80 Y+50 FMAX M99
15 L Z+100 FMAX M2
X
Z
11
2
3
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.