Working With Turning Cycles - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | Turning Cycles (software option 50)

Working with turning cycles

You can only use turning cycles in Turning mode
FUNCTION MODE TURN.
In turning cycles the TNC takes into account the cutting geometry
(TO, RS, P-ANGLE, T-ANGLE) of the tool so that damage to the
defined contour elements is prevented. The TNC outputs a warning
if complete machining of the contour with the active tool is not
possible.
You can use the turning cycles both for inside and outside
machining. Depending upon the specific cycle, the TNC detects
the machining position (inside/outside machining) via the starting
position or tool position when the cycle is called. In some cycles
you can also enter the machining position directly in the cycle.
After modifying the machining position, check the tool position and
rotation direction.
If you program M136 before a cycle, the TNC interprets feed rate
values in the cycle in mm/rev., and without M136 in mm/min.
If turning cycles are executed during inclined machining (M144), the
angles of the tool to the contour change. The TNC automatically
takes these modifications into account and thus also monitors the
machining in inclined state to prevent contour damage.
Some cycles machine contours that you have written in a
subprogram. You program these contours with path functions or FK
functions. Before calling the cycle you must program the cycle 14
CONTOUR to define the subprogram number.
You must call turning cycles 880 and 81x - 87x with CYCL CALL or
M99. Before calling a cycle, be sure to program:
Turning mode FUNCTION MODE TURN
Tool call Tool Call
Direction of rotation of turning spindle, e.g. M303
Selection of speed/cutting speed Function Turndata SPIN
If you use feed rate per revolution mm/rev., M136
Tool positioning to suitable starting point e.g. L X+130 Y+0 R0
FMAX
Adaptation of coordinate system and align tool CYCL DEF 800
Adapt rotary coordinate system
HEIDENHAIN | User's manual for cycle programming | 10/2017
12
363