HEIDENHAIN TNC 128 (77184x-02) - Manual (Page 439)

FACE MILLING (Cycle 233) 17.4
17
TNC 128 | User's Manual HEIDENHAIN Conversational Programming | 5/2014
439
Strategy Q389=4
4 The tool subsequently approaches the starting point of the
milling path on a straight line tangential arc at the programmed
feed rate for milling.
5 The TNC machines the level surface at the feed rate for
milling from the outside toward the inside with ever-shorter
milling paths. The constant stepover results in the tool being
continuously engaged.
6 The process is repeated until the programmed surface has been
completed. At the end of the last path, the TNC positions the
tool at rapid traverse
FMAX back to the starting point
1 .
7 If more than one infeed is required, the TNC moves the tool in
the spindle axis to the next plunging depth at the positioning
feed rate.
8 The process is repeated until all infeeds have been machined. In
the last infeed, only the finishing allowance entered is milled at
the finishing feed rate.
9 At the end of the cycle, the tool is retracted at
FMAX to the 2nd
set-up clearance.
Limits
The limits enable you to set limits to the machining of the level
surface so that, for example, side walls or shoulders are considered
during machining. A side wall that is defined by a limit is machined
to the finished dimension resulting from the starting point or the
side lengths of the level surface. During roughing the TNC takes
the allowance for the side into account, whereas during finishing
the allowance is used for pre-positioning the tool.
Please note while programming:
Pre-position the tool in the machining plane to the
starting position with radius compensation
R0. Keep
in mind the machining direction.
The TNC automatically pre-positions the tool in the
tool axis. Note the
2nd set-up clearance Q204.
Enter the 2nd set-up clearance in Q204 so that no
collision with the workpiece or the fixtures can occur.
If the starting point in the 3rd axis Q227 and the
end point in the 3rd axis Q386 are entered as equal
values, the TNC does not run the cycle (depth = 0
has been programmed).