In turning cycles, the control takes the cutting geometry (TO, RS, P-ANGLE, T-ANGLE) of the tool into account in order to prevent damage to the defined contour elements. If it is not possible to machine the entire contour with the active tool, the control will display a warning.
You can use the turning cycles both for inside and outside machining. Depending upon the specific cycle, the control detects the machining position (inside or 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 the direction of rotation.
If you program M136 before a cycle, the control interprets feed rate values in the cycle in mm/rev.; without M136 in mm/min.
If you execute turning cycles with inclined machining (M144), the angles of the tool with respect to the contour change. The control 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 can program these contours with Klartext contouring functions. Before calling the cycle, you must program the cycle 14 CONTOUR to define the subprogram number.
The turning cycles 81x - 87x as well 880, 882, and 883 must be called with CYCL CALL or M99. Before programming a cycle call, be sure to program:
- Turning mode: FUNCTION MODE TURN
- Call a tool with TOOL CALL
- Direction of rotation of turning spindle (e.g., M303)
- Selection of speed or cutting speed: FUNCTION TURNDATA SPIN
- If you use feed rate per revolution mm/rev., M136
- Position the tool to a suitable starting point (e.g., L X+130 Y+0 R0 FMAX)
- Adapt the coordinate system, and align the tool: CYCL DEF 800 ADJUST XZ SYSTEM