HEIDENHAIN TNC 640 User Manual page 337

Cycles: Special Functions | COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software
option 96)
These three possibilities of defining the tool are described in more
detail below:
Define a turning tool in the tool table (tool.t) as a milling
tool
If you are working without option 50, define your turning tool
as a milling cutter in the tool table (tool.t). In this case the
following data from the tool table a taken into account (including
delta values): length (L), radius (R), and corner radius (R2). The
geometry data of the turning tool are converted to the data of a
milling cutter. Orient the turning tool to the spindle center and
enter this spindle orientation angle in the parameter Q336 of
the cycle. For outside machining the spindle orientation equals
Q336, and for inside machining the spindle orientation equals
Q336+180.
Danger of collision!
Collision may occur between the tool holder and workpiece
with inside machining. The tool holder is not monitored. If
the tool holder results in a larger rotational diameter than the
cutter does, there is a danger of collision.
Select the tool holder to ensure that it does not result in a
larger rotational diameter than the cutter does
Define a milling tool in the tool table (tool.t) as a milling
tool (for subsequent use as a turning tool)
You can perform interpolation turning with a milling tool. In this
case the following data from the tool table a taken into account
(including delta values): length (L), radius (R), and corner radius
(R2). Orient a cutting edge of the milling cutter to the spindle
center and enter this angle in the parameter Q336. For outside
machining the spindle orientation equals Q336, and for inside
machining the spindle orientation equals Q336+180.
Define a turning tool in the turning tool table (toolturn.trn)
If you are working with option 50, you can define your turning
tool in the turning tool table (toolturn.trn). In this case the
orientation of the spindle to the center of turning takes place
under consideration of tool-specific data, such as the type of
machining (TO in the turning tool table), the orientation angle
(ORI in the turning tool table), parameter Q336, and parameter
Q561.
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
11
337