HEIDENHAIN TNC 410 ISO Programming - Manual (Page 236)

210 8 Programming: Cycles
8.3 Cy
cles f
o
r Dr
illing
, T
a
p
p
ing
and
Th
read Millin
g THREAD MILLING (Cycle G262, not TNC 410)
1 The TNC positions the tool in the tool axis at rapid traverse to the
programmed setup clearance above the workpiece surface.
2 The tool moves at the programmed feed rate for pre-positioning to
the starting plane. The starting plane is derived from the algebraic
sign of the thread pitch, the milling method (climb or up-cut milling)
and the number of threads per step.
3 The tool then approaches the thread diameter tangentially in a
helical movement. Before the helical approach, a compensating
motion of the tool axis is carried out in order to begin at the
programmed starting plane for the thread path.
4 Depending on the setting of the parameter for the number of
threads, the tool mills the thread in one, in several spaced or in one
continuous helical movement.
5 After this, the tool departs the contour tangentially and returns to
the starting point in the working plane.
6 At the end of the cycle, the TNC retracts the tool in rapid traverse
to set-up clearance, or—if programmed—to the 2nd set-up
clearance.
U U U U Nominal diameter Q335: Nominal thread diameter.
U U U U Thread pitch Q239: Pitch of the thread. The algebraic
sign differentiates between right-hand and left-hand
threads:
+ = right-hand thread
– = left-hand thread
U U U U Thread depth Q201 (incremental value): Distance
between workpiece surface and root of thread.
U U U U Threads per step Q355: Number of thread
revolutions by which the tool is offset, see figure at
lower right
0 = one 360° helical path to the depth of thread.
1 = continuous helical path over the entire length of
the thread
>1 = several helical paths with approach and
departure; between them, the TNC offsets the tool by
Q355, multiplied by the pitch
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation
G40.
The algebraic sign for the cycle parameter thread depth
determines the working direction. If you program the
thread depth = 0, the cycle will not be executed.
The nominal thread diameter is approached in a semi-circle
from the center. A pre-positioning movement to the side
is carried out if the pitch of the tool diameter is four times
smaller than the nominal thread diameter.