HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 205)

HEIDENHAIN TNC 320 205
8.2 Cy
cles f
o
r Dr
illing,
T
apping and Thr
ead Milling
THREAD MILLING (Cycle 262)
1 The TNC positions the tool in the tool axis at rapid traverse FMAX
to the programmed set-up 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 helical movement, in
several offset movements or in one continuous 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 at rapid traverse
to the set-up clearance, or—if programmed—to the 2nd set-up
clearance.
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation R0.
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 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 thread diameter.
Note that the TNC makes a compensating movement in
the tool axis before the approach movement. The length
of the compensating movement depends on the thread
pitch. Ensure sufficient space in the hole!
Use the machine parameter suppressDepthErr to define
whether, if a positive depth is entered, the TNC should
output an error message (on) or not (off).
Danger of collision!
Keep in mind that the TNC reverses the calculation for pre-
positioning when a positive depth is entered. This
means that the tool moves at rapid traverse in the tool axis
at safety clearance below the workpiece surface!