Coupling Interpolation Turning (Cycle 291, Din/Iso: G291, Software Option 96); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Cycles: Special Functions | COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software
option 96)
11.7 COUPLING INTERPOLATION TURNING
(cycle 291, DIN/ISO: G291, software
option 96)

Cycle run

Cycle 291 COUPLG.TURNG.INTERP. couples the tool spindle to the
position of the linear axes, or cancels this spindle coupling. With
interpolation turning the cutting edge is oriented to the center of a
circle. The center of rotation is defined in the cycle by entering the
coordinates Q216 and Q217 . Cycle 291 COUPLG.TURNG.INTERP. is
run in milling mode and is CALL-active.
Cycle run if Q560=1:
1 The TNC first stops the spindle (M5).
2 The TNC orients the tool spindle to the specified center of
rotation. The specified angle for spindle orientation Q336 is
taken into account. If an "ORI" value is given in the tool table, it
is also taken into account if so defined.
3 The tool spindle is now coupled to the position of the linear
axes. The spindle follows the nominal position of the reference
axes.
4 To terminate the cycle, the coupling must be deactivated by
the operator. (With Cycle 291 and end of program/internal stop
resp.)
Cycle run if Q560=0:
1 The TNC deactivates the spindle coupling.
2 The tool spindle is no longer coupled to the position of the linear
axes.
3 Machining with the interpolation turning cycle 291 is terminated.
4 If Q560=0, the parameters Q336, Q216, Q217 are irrelevant.

Please note while programming:

This feature must be enabled and adapted by the
machine tool builder.
After defining Cycle 291 and CYCLE CALL program the operation
you wish to perform. In order to describe the circular motions of
the linear axes linear/polar coordinates are used, for example. A
programming example is provided at the end of this section, See
page 353.
HEIDENHAIN | User's manual for cycle programming | 10/2017
11
333