HEIDENHAIN TNC 640 User Manual page 334

11
Cycles: Special Functions | COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software
Cycle 291 is CALL-active.
Programming of M3/M4 is not required. In order to
describe the circular motions of the linear axes, you can
use CC and C coordinates, for example.
If you define the turning tool in the turning tool table
(toolturn.trn), we recommend working with parameter
Q561=1. This way, you convert the data of the turning
tool into the data of the milling tool, thus greatly
facilitating your programming effort. With Q561=1
you can use radius compensation RR and RL when
programming. (However, if you program Q561=0, then
you cannot use radius compensation RR and RL when
describing your contour. Additionally, you must program
the movement of the tool center path TCP without
spindle coupling. This kind of programming is much
more complicated!)
If you programmed parameter Q561=1, you must
program the following in order to complete the
operation of interpolation turning:
R0, overrides radius compensation
Cycle 291 with parameters Q560=0 and Q561=0,
overrides spindle coupling
CYCLE CALL, for calling Cycle 291
TOOL CALL overrides the conversion of parameter
Q561
When programming, remember that neither the spindle
center nor the indexable insert must be moved into the
center of the turning contour.
Program outside contours with a radius greater than 0.
Program inside contours with a radius greater than the
tool radius.
This cycle can also be used in a tilted working plane.
Before cycle call, define a large tolerance with Cycle 32
for your machine to attain high contour speeds. Program
Cycle 32 with HSC filter=1.
If Cycle 8 MIRRORING is active, the TNC does
perform the cycle for interpolation turning.
If Cycle 26 AXIS-SPECIFIC SCALING is active, and the
scaling factor for the axis does not equal 1, the TNC
does not
Please keep in mind that the axis angle must be equal
to the tilt angle before calling the cycle. Only then is
correct coupling of the axes possible.
This cycle is effective only for machines with servo-
controlled spindle.
Your TNC might monitor the tool to ensure that no
positioning movements at feed rate are performed while
spindle rotation is off. Contact the machine tool builder
for further information.
Software option 96 must be enabled.
334
perform the cycle for interpolation turning.
not
HEIDENHAIN | User's manual for cycle programming | 10/2017
option 96)