Thread Milling (Cycle) - HEIDENHAIN ITNC 530 User Manual

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 nominal 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
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!
Enter in MP7441 bit 2 whether the TNC should output an
error message (bit 2=1) or not (bit 2=0) if a positive depth
is entered.
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!
330 8 Programming: Cycles